Allen-Bradley 9/Series CNC Lathe Operation and Programming Manual
Important User Information Because of the variety of uses for the products described in this publication, those responsible for the application and use of this control equipment must satisfy themselves that all necessary steps have been taken to assure that each application and use meets all performance and safety requirements, including any applicable laws, regulations, codes and standards.
9/Series Lathe Operation and Programming Manual October 2000 Summary of Changes New Information The following is a list of the larger changes made to this manual since its last printing. Other less significant changes were also made throughout. Error Message Log Paramacro Parameters Softkey Tree Error Messages Revision Bars We use revision bars to call your attention to new or revised information. A revision bar appears as a thick black line on the outside edge of the page as indicated here.
Chapter
Table of Contents Index (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual Chapter 1 Using This Manual 1.0 Chapter Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1.1 Audience . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1.2 Manual Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
TableIndex of Contents (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual 3.1.3 Setting Tool Offset Tables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3.1.4 Setting Offset Data Using {MEASURE} . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3.1.5 Tool Offset Range Verification . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Table of Contents Index (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual 5.3.5 Selecting a QuickView Plane . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5.4 Digitizing a Program (Teach) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5.4.1 Linear Digitizing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
TableIndex of Contents (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual Chapter 8 Display and Graphics 8.0 Chapter Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8.1 Selection of Axis Position Data Display . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8.2 PAL Display Page . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Table of Contents Index (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual 10.4.1 Leading Zero and Trailing Zero Suppression . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10.4.2 Programming without Numeric Values . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10.4.3 Word Descriptions and Ranges . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10.4.
TableIndex of Contents (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual Chapter 13 Coordinate Control 13.0 Chapter Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13.1 Plane Selection (G17, G18, G19) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13.2 Absolute/Incremental Modes (G90, G91) . . . . . . . . . . . . . . . . . . . . .
Table of Contents Index (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual 16.2 Corner Radius . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16.3 Considerations with Chamfering and Corner Radius . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Chapter 17 Spindles 17.0 Chapter Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
TableIndex of Contents (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual 19.1 Parking a Dual Axis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19.2 Homing a Dual Axis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19.3 Programming a Dual Axis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Table of Contents Index (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual Chapter 22 Single-Pass Turning Cycles 22.0 Chapter Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 22.1 Single-pass O.D. and I.D. Roughing Cycle (G20) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 22.2 Single-pass Rough Facing Cycle (G24) . . . . . . . . . . . . . . . . . . . . . .
TableIndex of Contents (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual (G84.2): Right-Hand Solid-Tapping Cycle . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . (G84.3): Left-Hand Solid-Tapping Cycle . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . (G85): Boring Cycle, No Dwell/Feed Out . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Table of Contents Index (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual Chapter 29 Program Interrupt 29.0 Chapter Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 29.1 Enabling and Disabling Interrupts (M96/M97) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 29.2 Interrupt Request Considerations . . . . . . . . . . . . . . . . . . . . . . . . . . .
TableIndex of Contents (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual G-code Compatibility Considerations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . M-code Compatibility Considerations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Offset Compatibility Considerations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Chapter 1 Using This Manual 1.0 Chapter Overview This chapter describes how to use this manual. Major topics include: Topic On page: Manual organization 1-1 Reading this manual 1-3 Terms and conventions 1-4 Related publications 1-5 1.1 Audience We intend the audience for this manual to be people who program and/or operate an Allen-Bradley 9/Series CNC. This family includes the 9/230, 9/240, 9/260, and 9/290 CNCs.
Chapter 1 Manual/MDI Operation Modes Table 1.A Manual Organization Chapter 1-2 Title Summary 1 Manual Overview Manual overview, intended audience, definition of key terms, how to proceed. 2 Basic Control Operation A brief description of the control’s basic operation including power up, MTB panel, operator panel, access control, and E-STOP. 3 Offset Tables and Setup Basic setup of the offset table, other initial operating parameters.
Chapter 1 Manual/MDI Operation Modes 30 Using a 9/Series Dual-- Processing System Describes dual-- process system. Includes synchronizing multiple part programs and shared spindle configurations. Table 1.A (continued) Manual Organization Appendix Title Summary Appendix A Softkey Tree Describes softkeys and their functions for softkey levels 1 and 2. Also, the softkey tree displaying all levels of softkeys and their location is shown.
Chapter 1 Manual/MDI Operation Modes Explanations and illustrations are presented based on the movement of the cutting tool on a fixed workpiece. The 9/Series control lets you use any alphabetic character for expressing a numerically controlled axis. This manual uses X and Z for the first and second axes on the basic coordinate system, and U and W for the axes parallel to them. The term AMP is an abbreviation for Adjustable Machine Parameters.
Chapter 1 Manual/MDI Operation Modes 1.6 Related Publications HPG Hand Pulse Generator I/O Input/Output MDI Manual Data Input Modal an operating condition that remains in effect on the control until cancelled or replaced MTB Machine Tool Builder ODS Offline Development System PAL Programmable Application Logic RAM Random Access Memory resident on the 9/240 Softkeys the row of keys directly below the screen Super cap A super capacitor.
Chapter 1 Manual/MDI Operation Modes 1-6
Chapter 2 Basic Control Operation 2.0 Chapter Overview This chapter describes how to operate the Allen-Bradley 9/Series control, including: Topic: On page: MTB panel 2-10 {FRONT PANEL} 2-13 Power-up 2-21 Emergency stops 2-22 Access control 2-23 Changing modes 2-30 Display system and messages 2-34 Input cursor 2-37 {REFORM MEMORY} 2-38 Removing an axis 2-40 Time part count 2-40 We also tell you about the control conditions automatically assumed at power up. 2.
Chapter 2 Basic Control Operation Figure 2.1 Monochrome Operator Panel 9/SERIES 7 8 9 4 5 6 1 2 3 _ 0 + = * . % : _ $ ; O N G P X Y Z Q I J K R A B C L # . EOB ] [ ( ) CALC DEL CAN RES F ! E M SHIFT SP D S DISP PROC ? H o T TRANSMIT 19435 Figure 2.2 Color Operator Panel 9/SERIES 7 8 4 5 6 1 2 3 .
Chapter 2 Basic Control Operation 2.1.1 Keyboard Table 2.A explains the functions of keys on the operator panel keyboard. In this manual, the names of operator panel keys appear between [ ] symbols. Table 2.A Key Functions Key Name Function Address and Numeric Keys Use these keys to enter alphabetic and numeric characters. If a key has two characters printed on it, pressing it normally enters the upper left character. Holding down the [SHIFT] key while pressing it enters the lower right character.
Chapter 2 Basic Control Operation Reset Operations If you are using a dual-processing system, refer to page 30-6 for details about reset operations. Block Reset Use the block reset feature to force the control to skip the block execution. To use the block reset function, program execution must be stopped. If program execution stops before the control has completely finished the block execution, a block reset aborts any portion of that block that has not been executed.
Chapter 2 Basic Control Operation Expressions entered on the input line cannot exceed a total of 25 characters. Only numeric or special mathematical operation characters as described below can be entered next to the “CALC:” prompt. Any character that is not numeric or an operation character you enter on the input line generates the error message “INVALID CHARACTER.” The largest number you can enter for a calculate function is 214748367. You cannot enter a number larger than 10 digits.
Chapter 2 Basic Control Operation Example 2.1 Mathematic Expressions Expression Entered Result Displayed 12/4*3 9 12/[4*3] 1 12+2/2 13 [12+2]/2 7 12-4+3 11 12-[4+3] 5 Table 2.C lists the function commands available with the [CALC] key. Table 2.
Chapter 2 Basic Control Operation Example 2.2 Format for [CALC] Functions SIN[2] This evaluates the sine of 2 degrees. SQRT[14+2] This evaluates the square root of 16. SIN[SQRT[14+2]] This evaluates the sine of the square root of 16. Example 2.3 Mathematical Function Examples Expression Entered Result SIN[90] 1.0 SQRT[16] 4.0 ABS[-4] 4.0 BIN[855] 357.0 BCD[357] 855.0 ROUND[12.5] 13.0 ROUND[12.4] 12.0 FIX[12.7] 12.0 FUP[12.2] 13.0 FUP[12.0] 12.0 LN[9] 2.197225 EXP[2] 7.
Chapter 2 Basic Control Operation Example 2.4 Calling Paramacro Variables with the CALC Function Expression Entered 2.1.3 Softkeys Result Displayed #100 Display current value of variable #100 12/#100*3 Divide 12 by the current value of #100 and multiply by 3 SIN[#31*3] Multiply the value of #31 (for the current local parameter nesting level) by 3 and take the sine of that result We use the term softkey to describe the row of 7 keys at the bottom of the CRT.
Chapter 2 Basic Control Operation Softkey level 1 is the initial softkey level the control displays at power-up. Softkey level 1 always remains the same and all other levels are referenced from softkey level 1. The softkeys on opposite ends of the softkey row have a specific use that remains standard throughout the different softkey levels.
Chapter 2 Basic Control Operation To use a softkey function, press the plain, unmarked button directly below the description of the softkey function. Important: Some of the softkey functions are purchased as optional features. This manual assumes that all available optional features have been purchased for the machine. If an option is not purchased, the softkey is blank. 2.1.4 CRT The control can be purchased with a 9-inch monochrome monitor or a 12-inch color monitor..
Chapter 2 Basic Control Operation If you are using a dual-operating system, your MTB panel may operate differently than described here. Refer to page 30-11 for information about your MTB panel. Figure 2.
Chapter 2 Basic Control Operation Table 2.
Chapter 2 Basic Control Operation Table 2.D (continued) Functions of the Buttons on the Push-Button MTB Panel Switch or Button Name How It Works = Default for Push-Button MTB Panel CYCLE STOP The control stops part program execution, MDI execution, or program check when this button is pressed. If pressed during the execution of a program block a cycle suspend state occurs.
Chapter 2 Basic Control Operation The software MTB panel can control these features: Feature 2-14 Description Mode Select Select either Automatic, MDI, or Manual modes as the current operating mode of the control. Rapid Traverse This feature replaces the feedrate when executing a continuous jog move with the rapid feedrate. Feedrate Override Selects a feedrate override percentage for feedrates programmed with an F-word, in 10% increments within a range of 0% to 150%.
Chapter 2 Basic Control Operation Software MTB Panel Screen To use the software MTB panel feature, follow these steps: 1. From the main menu screen, press the {FRONT PANEL} softkey. (softkey level 1) PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD The Software MTB Panel screen displays the current status of the alterable features.
Chapter 2 Basic Control Operation Jog Screen We assumes that you have performed the steps to display the Software Front Panel screen. Make sure that the function selected on the Software Front Panel screen is not the Mirror Image or the Axis Inhibit features. 1. Press the {JOG AXIS} softkey. (softkey level 2) JOG AXIS PRGRAM EXEC This screen appears: E-STOP PROGRAM [mm] F 0.000 MMPM 0.0 Z 0.000 S R X 0.000 T 0 C 359.
Chapter 2 Basic Control Operation Program Execute Screen The following assumes that the steps have been performed to display the Software Front Panel screen (see page 2-15). Make sure that the function selected on the Software Front Panel screen is not the Mirror Image nor the Axis Inhibit feature. 1. Press the {PRGRAM EXEC} softkey. (softkey level 2) JOG AXIS PRGRAM EXEC This screen appears.
Chapter 2 Basic Control Operation 2. Select one of these softkey options: block retrace jog retract cycle start cycle stop 3. To Perform a: Press: Cycle Start the softkey that corresponds to the desired feature. Details on these features are described in chapter 7. Cycle Stop the softkey that corresponds to the desired feature. Details on these features are described in chapter 7. Block Retrace the {BLOCK RETRCE} softkey.
Chapter 2 Basic Control Operation Figure 2.5 Jog Retract Software MTB Panel Screen E-STOP PROGRAM[ MM ] F Z 00000.000 S R X 00000.000 T C 359.99 00000.000 MMPM 0 12 FILENAME SUB NAME MEMORY JOG AXES+ MAN STOP JOG AXES- 2.4 Power Procedures The basic procedure for turning power on and off is described in this section. Refer to the documentation prepared by your system installer for more specific procedures. 2.4.
Chapter 2 Basic Control Operation After power has been turned on, the control displays the power turn-on screen. To activate the main menu, press the [TRANSMIT] key. You see the main menu screen: E-STOP PROGRAM[ MM ] F Z 00000.000 S R X 00000.000 T C 359.99 00000.
Chapter 2 Basic Control Operation 2.5 Control Conditions at Power-Up After powering up the control or performing a control reset operation (see page 2-4), the control assumes a number of initial operating conditions. These are listed below: Initial Password Access is assigned to the level that was active when power was turned off (provided that level is a power-up level selected in access control).
Chapter 2 Basic Control Operation 2.6 Emergency Stop Operations Press the red button on the MTB panel (or any other E-stop switches installed on the machine) to stop operations regardless of the condition of the control and the machine. WARNING: To avoid damage to equipment or hazard to personnel, the system installer should connect the button, so that pressing the button opens the circuit connected to the E-STOP STATUS terminal on the control.
Chapter 2 Basic Control Operation If the E-Stop occurred during program execution, the control may reset the program when E-Stop reset is performed provided AMP is configured to do so. Assuming that a control reset is performed, program execution begins from the first block of the program when is pressed. If the current axis position prohibits this, the operator can manually jog the axes clear, or consider executing a Mid-Program Start. See page 7-12.
Chapter 2 Basic Control Operation 2.7.1 Assigning Access Levels and Passwords This section describes setting or changing the functions assigned to a particular access level, and changing the password used to activate that access level.
Chapter 2 Basic Control Operation 2. Press the {ACCESS CONTRL} softkey. If the {ACCESS CONTRL} softkey does not appear on the screen, the currently active access level is not allowed to use the {ACCESS CONTRL} function. Enter a password that has access to {ACCESS CONTRL}. (softkey level 2) ACCESS CONTRL This screen appears.
Chapter 2 Basic Control Operation 3. Press the softkey that corresponds to the access level that you want to change. The pressed softkey appears in reverse video, and the password name assigned to that access level is moved to the “PASSWORD NAME.” Important: If you attempt to change the functions available to an access level that is equal to or higher than your the current access level, the error message “ACCESS TO THIS LEVEL IS NOT ALLOWED.
Chapter 2 Basic Control Operation 2.7.2 Password Protectable Functions The following section describes the functions on the 9/Series control that can be protected from an operator by the use of a password. If a user has access to a function, the parameter associated with that function is shown in reverse video on the access control screen. Access to these functions can be controlled by passwords. Table 2.
Chapter 2 Basic Control Operation Table 2.E (continued) Password Protectable Functions 2-28 Parameter Name: Function becomes accessible when parameter name is in reverse video: 8) OFFSETS ·{WORK CO-ORD} — Display and alter the preset work coordinate system zero locations and the fixture offset value. ·{TOOL WEAR} Display and alter the tool wear amount tables for the different tools. ·{TOOL GEOMET} — Display and alter the tool geometry tables.
Chapter 2 Basic Control Operation Table 2.E (continued) Password Protectable Functions Parameter Name: Function becomes accessible when parameter name is in reverse video: 22) SI/OEM MESSAGE ·{ENTER MESSAGE} — Enter a new message to be displayed on the control’s power-up screen. ·{STORE BACKUP} — Store an entered message for the power-up screen to backup memory.
Chapter 2 Basic Control Operation E-STOP ENTER PASSWORD: PROGRAM [INCH] F 0.000 MMPM 0 Z 00000.000 S R X 00000.000 T C 359.99 MEMORY MAN 1 STOP ACCESS CONTRL 2.8 Changing Operating Modes 2. Enter the password you want to activate by typing it in on the input line with the keys on the operator panel. The control displays * for the characters you entered. If you make an error entering the password, edit the input line as described on page 2-37. 3.
Chapter 2 Basic Control Operation The control is executing a threading- or multiple-pass turning cycle. Important: Your system installer may have written PAL to disable the use of the {FRONT PANEL} softkey to change modes. If this is the case, then changing modes can be performed by using only on the MTB panel. Manual mode To operate the machine manually, select MAN or MANUAL under or press the {FRONT PANEL} softkey.
Chapter 2 Basic Control Operation MDI mode To operate the machine in MDI mode, select MDI under or press the {FRONT PANEL} softkey Use left/right arrow keys to change mode select options if using {FRONT PANEL}. For details on MDI operation, see page 4-11. Figure 2.7 MDI Mode Screen MDI: E-STOP PROGRAM[ MM ] F Z 00000.000 S R X 00000.000 T C 359.
Chapter 2 Basic Control Operation Automatic mode To operate the machine automatically, select AUTO under or press the {FRONT PANEL} softkey Use left/right arrow keys to select mode options if using {FRONT PANEL}. For details on automatic operation, see chapter 7. Figure 2.8 Automatic Operation Screen E-STOP PROGRAM[ MM ] F Z 00000.000 S R X 00000.000 T C 359.
Chapter 2 Basic Control Operation 2.9 Displaying System and Machine Messages The control has two screens dedicated to displaying messages. The MESSAGE ACTIVE screen displays up to nine of the most current system messages and ten of the most current machine (logic generated) messages at a time. The MESSAGE LOG screen displays a log of up to 99 system messages and a separate log of up to 99 machine messages that occurred since the last time memory was cleared.
Chapter 2 Basic Control Operation Figure 2.9 Message Active Display Screen MESSAGE ACTIVE SYSTEM MESSAGE (The system error messages are displayed in this area) MACHINE MESSAGE (The logic messages are displayed in this area) ERROR LOG CLEAR ACTIVE This is the information displayed on the MESSAGE ACTIVE screen. The control displays up to 9 active system messages and up to 10 machine messages.
Chapter 2 Basic Control Operation Figure 2.10 Message Log Display Screen MESSAGE LOG PAGE 1 of 9 SYSTEM MESSAGE (The logged system error messages are displayed in this area) MACHINE MESSAGE (The logged logic messages are displayed in this area) ACTIVE TIME ERRORS STAMPS This is the information displayed on the MESSAGE LOG screen. The control displays up to 99 system messages and up to 99 machine messages.
Chapter 2 Basic Control Operation 2.9.1 Clearing Active Messages {CLEAR ACTIVE} After the cause of a machine or system message has been resolved, some messages remain displayed on all screens until you clear them. CAUTION: Not clearing the old messages from the screen can prevent messages that are generated later from being displayed. This occurs when the old resolved message has a higher priority than the newly generated message.
Chapter 2 Basic Control Operation 2.11 {REFORM MEMORY} Cursor Operation: Description: Deleting all characters on the input line To delete all entered characters on the input lines press the [DEL] key while holding down the [SHIFT] key. All characters on the input line are deleted. Sending information To send information to the control from input line press the [TRANSMIT] key. All information on the input line is sent to the control.
Chapter 2 Basic Control Operation To reformat control memory and delete all programs stored in memory, follow these steps: 1. Press the {PRGRAM MANAGE} softkey. (softkey level 1) 2. PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD Press the {REFORM MEMORY} softkey.
Chapter 2 Basic Control Operation 2.12 Removing an Axis (Axis Detach) This feature allows the removal of a rotary table or other axis attachment from a machine. When activated, the control ignores messages that may occur resulting from the loss of feedback from a removed axis such as servo errors, etc. Important: This feature removes the selected axis from the control as an active axis. Any attempt to move the removed axis results in an error.
Chapter 2 Basic Control Operation 2. Press the {ACTIVE PRGRAM} softkey. (softkey level 2) ACTIVE EDIT RESTRT DISPLY COPY PRGRAM PRGRAM PRGRAM PRGRAM PRGRAM DELETE VERFY PRGRAM RENAME INPUT PRGRAM PRGRAM COMENT PRGRAM DEVICE REFORM CHANGE MEMORY DIR 3. Press the {TIME PARTS} softkey. This generates the screen shown in Figure 2.11. (softkey level 3) DE-ACT SEARCH MID ST T PATH T PATH PRGRAM PRGRAM GRAPH DISABL TIME PARTS SEQ STOP Figure 2.
Chapter 2 Basic Control Operation Important: Some softkeys shown in Figure 2.11 might not appear on your system due to restricted access. Refer to the beginning of this section and page 2-23 for details. You can modify the values on this screen. Press the {ED PRT INFO}, or the {SET TIME} softkeys as explained in the Screen Field Definitions that follow. {SET DATE}, Press the exit softkey {Ý} to save changes and return to the “Active Program” screen.
Chapter 2 Basic Control Operation Power-on Time/Overall -- indicates the total accumulated time that the control has been ON. This value is saved in backup memory each time the control is powered off, so it is restored at its previous value each time the control is turned ON. To clear this field to zero: 1. Press the {ED PRT INFO} softkey, provided that you have supervisor-level access. 2. Press the up or down cursor keys to move to this field or the next field without changing the current value. 3.
Chapter 2 Basic Control Operation Power-on Time/After Reset -- indicates the total accumulated time that the control has been ON. This value is saved in backup memory each time the control is powered off, so it is restored at its previous value each time the control is turned ON. Use this field with “Run Time” to estimate the utilization ratio of the machine. The value for this field is cleared to zero when the “Run Time” field is cleared to zero; it cannot be changed independently.
Chapter 2 Basic Control Operation Remaining Workpieces -- indicates the number of workpieces that still need to be cut in the lot. The value for this field is automatically set equal to the lot size each time the “Lot Size” value is changed. When the control encounters an M02, M30, or M99 in a main part program, the remaining workpieces field is decremented by one. The control tells the system installers PAL program when the lot remaining size is zero.
Chapter 2 Basic Control Operation 2-46
Chapter 3 Offset Tables and Setup 3.0 Chapter Overview In this chapter we describe the basics for job setup. Major topics include: Topic: 3.
Chapter 3 Offset Tables and Setup Figure 3.
Chapter 3 Offset Table and Setup 3.1.1 Tool Dimensional Parameters Figure 3.
Chapter 3 Offset Tables and Setup Figure 3.3 Tool Length Offsets -Z Gauge point Z tool offset X tool offset (entered as a diameter value) -X The Z offset table value corresponds to the actual Z distance from the tool tip to the gauge point. The X offset value is the distance on the axis from the tool tip to the gauge point. Consequently, when the control activates a tool offset, the Z axis is displaced per the table value, while the X axis is displaced half the table value.
Chapter 3 Offset Table and Setup Figure 3.4 Tool Tip Radius for Typical Lathe Tool .05 Radius Tool Length (Wear Table) The tool length wear compensation offset takes into account the wear that a tool incurs from normal usage. Enter a value in the table that is equal to the difference between the tool tip positions, before and after tool wear.
Chapter 3 Offset Tables and Setup 3.1.2 Tool Orientation Parameters ORNT - Tool Orientation (Tool Geometry Data Table) The control uses the value entered here to determine the orientation of the tool’s cutting edge relative to the surface of the part. This is necessary for the control to perform TTRC correctly. Refer to chapter 21. Figure 3.
Chapter 3 Offset Table and Setup Figure 3.6 Tool Orientations, Rear Turret Lathe (Both A and B Turrets if Two-Turret Lathe) -Z 1 2 6 5 7 9 or 0 -X 8 4 3 Figure 3.
Chapter 3 Offset Tables and Setup 3.1.3 Setting Tool Offset Tables You can set data in the offset tables by using one of six methods. The method described here requires that the offset data is manually measured and then directly keyed into the table.
Chapter 3 Offset Table and Setup Figure 3.8 Tool Offset Screens Tool Wear Table Tool Geometry Table 3. Move the cursor to the offset data to be modified. Use the up, down, left, or right cursor keys to move the block cursor to the tool offset data on the current page. Press the {MORE OFFSET} softkey to change pages. To search all pages for a specific offset number, press the {SEARCH softkey and key in the desired offset number.
Chapter 3 Offset Tables and Setup Diameter or Radius {RADI/DIAM} If the offset value being changed has been selected in AMP as the diameter axis (typically the axis perpendicular to the spindle center line), data may be entered into the offset table as either a radius or diameter value. The current mode for this axis is displayed with an R for radius or a D for diameter mode next to that axes offset. Pressing the {RADI/ DIAM} softkey toggles the offset between these two modes.
Chapter 3 Offset Table and Setup 3.1.4 Setting Offset Data Using {MEASURE} The measure feature offers an easier method of establishing tool offsets. The control, not the operator, computes the tool length and wear offsets, and enters these values into the tool offset tables. The measure feature is used to measure tool length offset values for the wear or geometry tables; it should not be used to modify tool diameter offsets. To enter tool offsets using measure, follow these steps: 1.
Chapter 3 Offset Tables and Setup 3.1.5 Tool Offset Range Verification Tool offset range verification checks: the maximum values entering the tool offset tables the maximum change that can occur in either table To use tool offset range verification, follow this softkey sequence: 1. Press the {SYSTEM SUPORT} softkey. (softkey level 1) 2. PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD Press the {AMP} softkey.
Chapter 3 Offset Table and Setup Your system installer initially sets these values in AMP.
Chapter 3 Offset Tables and Setup Verify for Maximum Value This value represents the absolute maximum value per table for all tool offsets in that table. If you enter: then: a positive number greater than the maximum value the control generates the error message: “OFFSET EXCEEDS MAX VALUE” a negative number less than the negative of the maximum value The control does not modify the value in the table.
Chapter 3 Offset Table and Setup 2. Activate an offset number as follows: Press This softkey: To activate: the {TOOL GEOMET} a tool geometry offset number the {TOOL WEAR} tool wear offset number The tool offset table is displayed. Currently active offset values (if any) are indicated with an * to the right of the offset number. 3. Move the cursor on the offset table until the desired offset is shown in reverse video.
Chapter 3 Offset Tables and Setup External Offset Use the external offset to modify all of the work coordinate system zero points. Use of the external offset is optional. The value entered here offsets all of the work coordinate systems by the specified amount. Enter external offsets in the work coordinate system tables as the external offset value. This offset allows a programmer to use the same set of work coordinate system values in a variety of applications.
Chapter 3 Offset Table and Setup (softkey level 1) (softkey level 1) 2. PRGRAM OFFSET MACRO MANAGE PARAM QUICK CHECK FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD SYSTEM SUPORT Press the {WORK CO-ORD} softkey to display the offset values for the work coordinate systems and the external offset. See Figure 3.9. (softkey level 2) Figure 3.9 Work Coordinate System Setting 3. Move the cursor to the offset data that you want to modify.
Chapter 3 Offset Tables and Setup offset data on the current page. Press the {MORE OFFSET} softkey to change pages. The selected item appears in reverse video. 4. Select data entry type: Unit selection {INCH/METRIC} To select units of “mm” or “inch” for the offset data, press the {INCH/METRIC} softkey. The units used for the currently selected offset G-code or external offset change each time the softkey is pressed.
Chapter 3 Offset Table and Setup 3.4 Backing Up Offset Tables The control can save all of the information that is entered in the tool offset tables and the work coordinate system tables as a backup. This is accomplished by the control generating a program consisting of G10 blocks. These G10 blocks contain the offset numbers and their respective wear and geometry values. Any time your run this program, the set of values contained in these G10 blocks replace the current values in the offset tables.
Chapter 3 Offset Tables and Setup Figure 3.10 Backup Offset Screen 3. Select the offsets to be backed up by moving the cursor to the desired offset by using the up and down cursor keys. The selected offset appears in reverse video. The four options include: TOOL WEAR ---- When wear is selected all data from the tool offset wear tables is stored as a G10 program. TOOL GEOMETRY ---- When geometry is selected all data from the tool offset geometry tables is stored as a G10 program.
Chapter 3 Offset Table and Setup 3.5 Programmable Zone Table The programmable zone feature prevents tool motion from entering or exiting a designated area. For details on programmable zones, refer to chapter 12. This table contains the values for programmable zones 2 and 3. These values define the boundaries for the programmable zones and are referenced from the machine coordinate system. Important: These values may also be entered in AMP by the system installer.
Chapter 3 Offset Tables and Setup Figure 3.11 Programmable Zone Table Important: 4. Use the up or down cursor keys to move the block cursor to the data to be changed. Data located at the cursor appears in reverse video. Press the {MORE LIMITS} softkey to change pages. 5. You can replace data or add to it. 6. 3-22 Depending on the currently active program mode, programmable zone coordinates are displayed in inches or millimeters for a liner axis and in degrees for a rotary axis.
Chapter 3 Offset Table and Setup 3.6 Single- digit Feedrate Table Use this feature to change the values set for the single--digit feedrates. When a single--digit F--word is encountered during block execution, the control looks to the single--digit feedrate table for a feedrate. The feedrate in this table corresponding to the single digit then becomes the active feedrate. For more details on single--digit feedrate F--words, refer to chapter 18.
Chapter 3 Offset Tables and Setup 6. Exit the feedrate parameter screen in two ways: Press This Softkey: To: {UPDATE & EXIT} to save recent changes made to and leave the feedrate parameter screen. {QUIT} to exit the feedrate parameter screen without saving changes.
Chapter 4 Manual/MDI Operation Modes 4.0 Chapter Overview This chapter describes the manual and MDI operating modes. Major topics include: Topic: On page: Mechanical handle feed 4-8 Removing an axis 4-8 Manual machine homing 4-9 MDI mode 4-11 Important: This manual assumes that the rotary or push-button MTB panel is being used and standard PAL to run that MTB panel has been installed.
Chapter 4 Manual/MDI Operation Modes Figure 4.1 Data Display in MANUAL Mode E-STOP PROGRAM[ MM ] F X 00000.000 S Z 00000.000 T U 00000.000 W 00000.000 MEMORY 30000 MDI 00000.000 MMPM 0.0 1 STOP N 99999 (First 4 blocks of program shown here) (PAL messages) PRGRAM OFFSET MACRO MANAGE PARAM 4.1.1 Jogging an Axis PRGRAM SYSTEM CHECK SUPORT In the jog modes, the motion of the cutting tool is controlled by the use of pushbuttons, switches, or hand pulse generators (HPGs).
Chapter 4 Manual/MDI Operation Modes The control can be equipped with an optional offset jogging feature, activated by a switch installed by the system installer. When this feature is active, all jog moves are used to offset the current work coordinate system and no position registers are changed. See page 4-6 for details. Only normal single-axis jogs (one axis at a time in the continuous, incremental, or HPG modes) are permitted during a jog retract operation. See 7-17.
Chapter 4 Manual/MDI Operation Modes 3. Press the button for the axis and direction to jog. The control makes one incremental move each time the button is recognized. Until the control completes the execution of the incremental move, no other jog moves are recognized on that axis. This includes attempts to perform other incremental moves on that axis.
Chapter 4 Manual/MDI Operation Modes Figure 4.2 HPG Feed - 4.1.5 Arbitrary Angle Jog + If desired the system installer can enable a feature that allows control over the angle in which a multi-axis jog move will take through the installation of some optional switches. When this feature is activated, the operator selects two different axes to define a plane for the arbitrary angle jog to take place. Then, an angle is selected (between 0°and 360°) to define a vector for the jog to take place.
Chapter 4 Manual/MDI Operation Modes 4.1.6 Jog Offset The control may be equipped with an optional jog offset feature, activated by a switch installed by the system installer. When this function is active, all jog moves made are added as offsets to the current work coordinate system. Normally, jogging occurs in the manual mode. The system installer has the option to enable a “Jog on the Fly” feature that will allow jogging in automatic or MDI mode for the purpose of jogging an offset.
Chapter 4 Manual/MDI Operation Modes Programmable Zone Overtravel ---- the axes reach a travel limit established by independent programmable areas. Programmable Zones are activated through programming the appropriate G-code. These 3 causes of overtravel are described in detail in chapter 12. When an overtravel condition occurs, all axis motion stops, the control is placed in cycle stop, and one of the following error messages is displayed.
Chapter 4 Manual/MDI Operation Modes 4.2 Mechanical Handle Feed (Servo Off) This feature lets you disable the servo drives, and allows the axes to be moved by external means (such as a hand crank attached to the ball screw) without requiring the control to be in E-Stop. When this feature is enabled, all position displays get updated as the axes are moved. Use this feature in conjunction with the digitize feature described in chapter 5.
Chapter 4 Manual/MDI Operation Modes 4.4 Manual Machine Homing The machine home return operation means the positioning of a specified linear or rotary axis to a machine-dependent fixed position, which is called the machine home. This position is established via a home limit switch mounted on the machine and the encoder marker. The execution of machine home establishes the machine coordinate system.
Chapter 4 Manual/MDI Operation Modes Figure 4.4 Manual Machine Home AXIS/DIRECTION JOG SELECT INCR CONT HAND HOME +X +4 --X +Y TRVRS --Y Cutting tool Machine home +Z --4 --Z To execute the manual return to machine home position: 1. Select HOME under . 2. Place the control in manual mode. See page 4-1. 3. Determine the direction that each axis must travel to reach the home limit switch.
Chapter 4 Manual/MDI Operation Modes This locates the machine home position. When the axis reaches this position, the control resets the position registers to a machine coordinate value specified in AMP. This establishes the zero point of the machine coordinate system. Important: During the machine home operation, softlimits and programmable zones are not active. All active coordinates offsets are cancelled. 4.
Chapter 4 Manual/MDI Operation Modes Figure 4.5 Program Display Screen in MDI Mode E-STOP PROGRAM[ MM ] F X 00000.000 S Z 00000.000 T U 00000.000 W 00000.000 MEMORY 30000 MDI 00000.000 MMPM 0 1 STOP N 99999 (First 4 blocks of MDI shown here) (PAL messages) PRGRAM OFFSET MACRO MANAGE PARAM 4.5.1 MDI Basic Operation PRGRAM SYSTEM CHECK SUPORT Operating procedures in the MDI mode include: 1. When it is in MDI mode, the control accepts standard programming blocks. 2.
Chapter 4 Manual/MDI Operation Modes 3. Pressing the [TRANSMIT] key transmits the blocks to control memory. Once the blocks have been sent to control memory, you cannot send any more MDI blocks until all of the previous set has been executed. The control displays the first 4 blocks of the MDI program entered on lines 17-20 with an ! (exclamation point) just to the left of the blocks.
Chapter 4 Manual/MDI Operation Modes Figure 4.6 MDI Mode Program Screen E-STOP PROGRAM[ MM ] F Z 00000.000 S R X 00000.000 T C 359.99 MEMORY 30000 MDI 00000.000 MMPM 0 1 STOP N 99999 (First 4 blocks of MDI shown here) (PAL messages) PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT Important: Performing a block reset operation causes the control to abort the current MDI program block or skip the following MDI program block. See page 2-4 for details.
Chapter 5 Editing Programs On Line 5.
Chapter 5 Editing Programs On Line 5.1 Selecting the Program To Edit This section provides information on how to select a part program for editing. You can only edit part programs on line that you have stored in control memory. If a part program is on tape or another storage device and you must edit it on line, copy this program to memory as described in chapter 9. Important: You can edit programs that are selected as active for execution.
Chapter 5 Editing Programs On Line The control displays this main part program directory screen: Figure 5.1 Part Program Directory SELECTED PROGRAM: DIRECTORY PAGE NAME SIZE MAIN O12345 RRR TEST 2.3 14.3 9.3 3.9 4 FILES 1 OF 1 COMMENT THIS IS A TEST PROG 120.2 METERS FREE ACTIVE EDIT RESTRT DISPLY COPY PRGRAM PRGRAM PRGRAM PRGRAM PRGRAM 2. Select the part program you want to edit using two methods: Key in the program name of the part program to edit or create.
Chapter 5 Editing Programs On Line 3. Press the {EDIT PRGRAM} softkey. (softkey level 2) ACTIVE EDIT RESTRT DISPLY COPY PRGRAM PRGRAM PRGRAM PRGRAM PRGRAM DELETE VERIFY PRGRAM RENAME INPUT PRGRAM PRGRAM COMENT PRGRAM DEVICE REFORM CHANGE MEMORY DIR 5.2 Editing Programs at the Control (On Line) This section covers how to edit part programs after a program has already been selected to edit as described on page 5-2. CAUTION: Any edit operation that you perform on a part program is permanent.
Chapter 5 Editing Programs On Line Figure 5.2 Program Edit Screen INSERT : EDIT FILE : 000001 N00020 N00025 N00030 N00035 N00040 N00050 POS 1*1 MODE : CHAR WHILE [#1LT 10] DO 1; G01 F1000 X#1; G04 P1 #1 = [#1 + 1]; END 1; M99; MODIFY BLOCK BLOCK INSERT DELETE TRUNC DELETE EXIT CH/WRD EDITOR The maximum number of programs that you can have is 328. In order to store a program, it must use at least 1.3 meters of memory.
Chapter 5 Editing Programs On Line 5.2.1 Moving the Cursor {STRING SEARCH} This section describes moving the cursor in the program display area (lines 7-20 of the CRT). It assumes that you have selected a program to edit as outlined on page 5-2 . Important: The input cursor is the cursor shown on the input lines (lines 2 and 3 on the screen). Refer to page 2-37 for details.
Chapter 5 Editing Programs On Line 4. To end the search operation, press the exit [Ý] softkey. Sometimes you might want to change the cursor size for editing operations such as changing, inserting, or erasing. The control has two cursor sizes available. Cursor Size: Description: single character is automatically assigned to the cursor when you access the edit screen. word encompasses a word and its value for using erasing, inserting, or changing operations.
Chapter 5 Editing Programs On Line 2. Type the program characters to be entered in the input area. Press the [EOB] key (end of block) at the end of each block. If you make a mistake keying in a character before it is sent from the input area, you can edit the input lines as described on page 2-37. 3. Press the [TRANSMIT] key to send data from the input lines to the program display area.
Chapter 5 Editing Programs On Line Example 5.1 Changing Characters To change Z93 to W93 in the following block: Program Block (Program Display Area) Enter (Input Area) G01X93Z93; Notes Move the block cursor to the Z in the program display area and toggle the {MODIFY/INSERT} softkey to “MODIFY:”. G01X93Z93; W G01X93W93; Type this data into the input area, then press the [TRANSMIT] key. This is the block of altered commands shown in the program display area. Example 5.
Chapter 5 Editing Programs On Line Inserting You can insert characters, words, and blocks to the left of the program display cursor within an already existing or newly created part program. Follow these steps to use the insert function. 1. From the edit menu, press the {MODIFY INSERT} softkey until the INSERT: prompt is displayed on the input line. The control toggles between change and insert each time you press the softkey.
Chapter 5 Editing Programs On Line Example 5.5 Inserting Characters To change “X123.0” to “X123.034” when the following is displayed on the input line: Program Block (Program Display Area) Enter (Input Area) N1000X123.0Z45.0; Notes Move the cursor to “Z”and toggle the {MODIFY/INSERT} softkey to “INSERT:”. N1000X123.0Z45.0; 34 Type this data into the input area, then press the [TRANSMIT] key. Result N1000X123.034Z45.0; Example 5.6 Inserting Words To change X93.Z20.; to X93.W31.Z20.
Chapter 5 Editing Programs On Line 3. Press the {DELETE CH/WRD} softkey. (softkey level 3) MODIFY BLOCK BLOCK INSERT DELETE TRUNC DELETE EXIT CH/WRD EDITOR STRING RENUM MERGE QUICK SEARCH PRGRAM PRGRAM VIEW CHAR/ WORD DIGITZ E Erasing Commands to the EOB 1. Move the cursor from the edit menu until the first character or word to be erased is in reverse video. 2. Press the {BLOCK TRUNC} softkey. The control block erases all the information from the cursor to the End of Block character.
Chapter 5 Editing Programs On Line Erasing An Entire Block 1. Move the cursor from the edit menu until it is located on any character in the block that you want to delete. 2. Press the {BLOCK DELETE} softkey. This erases the selected block, including the end of block character. (softkey level 3) MODIFY BLOCK BLOCK INSERT DELETE TRUNC DELETE EXIT CH/WRD EDITOR STRING RENUM MERGE QUICK SEARCH PRGRAM PRGRAM VIEW CHAR/ WORD DIGITZ E Example 5.
Chapter 5 Editing Programs On Line 5.2.5 Sequence Numbers {RENUM PRGRAM} You can assign each block in a part program up to a five-digit numeric value following an N address. Refer to these numbers as sequence numbers. They distinguish one block from another. You can assign sequence numbers at random to specific blocks or to all blocks. Blocks assigned sequence numbers can be called later by designating their sequence number.
Chapter 5 Editing Programs On Line 4. Select the blocks to renumber. There are two choices: If you want to assign sequence numbers to: Press: all blocks from the beginning of the part program {ALL} only the block that already have sequence numbers {ONLY N} Important: Any sequence numbers in a block that are referenced in the current program by a paramacro “GOTO” or “WHILE” or by a roughing cycle are also renumbered.
Chapter 5 Editing Programs On Line 5.2.7 Exiting Edit Mode When you edit a program, all changes and additions that you make are saved immediately in the control’s memory. You don’t execute a formal “save” command. Important: You cannot quit, abandon or abort an edit session and restore the original version of the program. For that reason, we recommend that you copy the program (see page 5-4 ) prior to editing. To exit the edit mode, press the {EXIT EDITOR} softkey.
Chapter 5 Editing Programs On Line How to Select QuickView Features Use these steps to select the QuickView features: 1. Select a program for editing as described on page 5-2 . 2. From the edit menu, press the {QUICK VIEW} softkey. The softkey functions change to those indicated below: (softkey level 4) QPATH+ GCODE DRILL LATHE PLANE PROMPT PROMPT PROMPT PROMPT SELECT Important: If your system is a dual-process lathe, you must select the process to be prompted by QuickView.
Chapter 5 Editing Programs On Line 5.3.1 Using {QPATH+ PROMPT} Sample Patterns With the QuickView functions and the QuickPath Plus section, you can use dimensions from part drawings to create a part program.
Chapter 5 Editing Programs On Line For more information regarding these designations, see chapters 15 and 16. Your system installer can select a different address for angle A in AMP. Refer to your system installer’s documentation. Axis words followed by a (1), (2), or (3) are prompting for the first, second, or third coordinate position respectively. The location of the axis word is shown on the drawing accompanying the prompt screen.
Chapter 5 Editing Programs On Line CIRCLE, ANGLE, POINT ANGLE, CIRCLE, POINT CIRCLE , CIRCLE ANGLE, POINT QUICKPATH PLUS MENU 1 CIR ANG PT 3. CIR CIR ANG CIR PT ANG PT After you select the sample pattern you want, enter values for the parameters as follows: Use the up and down cursor keys to select the parameter you want to change or enter. The selected item appear in reverse video. Type data you want and press the [TRANSMIT] key. 4.
Chapter 5 Editing Programs On Line After you press the {3PT C} softkey, the prompt screen for that sample pattern becomes available. Figure 5.4 is an example of a QuickPath Plus prompting screen. It shows what data must be entered for that prompted screen to generate the necessary tool paths correctly. Figure 5.4 {3PT C} C2 (X2, Z2) (X3, Z3,) C1 (X1, Z1) 5.3.
Chapter 5 Editing Programs On Line Figure 5.5 G-code Prompt Select Screen G CODE PROMPTING MENU DISPLAY G00/01 G02/03 G04 G07/G08 G09/61/62/ 63/64 G10L2 G10L0&11 G10L10-L13 G10.1L20 G14.1/14 G16/15 G16.1/15 G16.
Chapter 5 Editing Programs On Line 6. After you enter all data for the G-code, store the data press the {STORE} softkey. (softkey level 6) STORE CONTNU The control generates the necessary G-code block. The generated block displays in the input area next to the EDIT: prompt. You can edit this block in the input area using the techniques described on page 2-37. 5.3.3 Lathe Cycle Format Prompting 7.
Chapter 5 Editing Programs On Line E-STOP LATHE PROMPT MENU G20: G21: G24: G72: G73: G74: G75: G76: G77: G78: DISPLAY . SINGLE PASS O.D. & I.D. ROUGHING CYCLE SINGLE PASS THREADING CYCLE SINGLE PASS ROUGH FACING CYCLE O.D. & I.D. FINISHING CYCLE O.D. & I.D. ROUGHING CYCLE ROUGH FACING CYCLE CASTING/FORGING ROUGHING CYCLE FACE GROOVING CYCLE O.D. & I.D. GROOVING CYCLE O.D. & I.D. MULTI-PASS THREADING CYCLE SELECT 2.
Chapter 5 Editing Programs On Line 6. After you enter all data for the G-code, store the data by pressing the {STORE} softkey. (softkey level 6) STORE The control generates the necessary G-code block. The generated block is displayed in the input area next to the EDIT: prompt. This block may be edited in the input area using the techniques described on page 2-37. 7.
Chapter 5 Editing Programs On Line DRILL PROMPT MENU DISPLAY G80: CANCEL OR END FIXED CYCLE G81: DRILLING CYCLE, NO DWELL/RAPID OUT G82: DRILLING CYCLE DWELL/RAPID OUT G83: DEEP HOLE DRILLING CYCLE G83.1: DEEP HOLE PECK DRILLING CYCLE, DWELL G84: RIGHT HAND TAPPING CYCLE G84.1: LEFT HAND TAPPING CYCLE G85: BORING CYCLE, NO DWELL/FEED OUT G86: BORING CYCLE SPINDLE STOP, RAPID OUT G86.
Chapter 5 Editing Programs On Line (softkey level 6) STORE The control generates the necessary G-code block. The generated block is displayed in the input area next to the EDIT: prompt. This block may be edited in the input area using the techniques described on page 2-37. 7. To enter the blocks in the program being edited, move the block cursor in the program display area just past the location in the program where it is desired to insert the new blocks.
Chapter 5 Editing Programs On Line 2. Change the plane by pressing the softkey that corresponds to the plane you want to program in (G17, G18, or G19). Refer to documentation prepared by your system installer for details on the planes selected by these G-codes. The display changes to show the selected plane. (softkey level 5) SET 3. G17 G18 G19 If the plane displayed is the plane you want to program the QuickView feature in, press the {SET} softkey.
Chapter 5 Editing Programs On Line 2. From the edit menu, press the {DIGITIZE} softkey. (softkey level 3) MODIFY BLOCK BLOCK INSERT DELETE TRUNC DELETE EXIT CH/WRD EDITOR STRING RENUM MERGE QUICK SEARCH PRGRAM PRGRAM VIEW CHAR/ WORD DIGITZ E 3. Use the following methods to position the cutting tool. The cutting tool should be located at the desired start-point of the new program. Jog the Axes in manual mode. Automatically move the axes by executing a part program or MDI program.
Chapter 5 Editing Programs On Line Table 6.
Chapter 5 Editing Programs On Line If the next move is to be linear, press the {LINEAR} softkey (page 5-31) If the next move is to be circular: Press: If you know: {CIRCLE 3 PNT} three points on the arc (see page 6.42) {CIRCLE TANGNT} the end-point of the arc and the line that is tangent to the start-point of the arc Important: To abort the linear digitize operation, press the exit {Ý} softkey at any time before pressing the {STORE END PT} or {EDIT & STORE} softkeys.
Chapter 5 Editing Programs On Line DIGITIZE: E-STOP TARGET[ MM R ] Z 0.000 X 0.000 C 359.99 F 0.000 MMPM S 00 STORE END PT 2. EDIT & STORE Reposition the tool at the desired end-point of the linear move using any of these methods: Jog the Axes in manual mode. Automatically move the axes by executing a part program or MDI program. Manually move the axes using any means as long as the encoder is still actively recording the tool position (see documentation prepared by the system installer).
Chapter 5 Editing Programs On Line 5.4.2 Digitizing an Arc (3 Points) The following subsection assumes that steps 1-5 in on page 5-28 have been completed to initiate a digitizing operation. To digitize an arc: 1. Press the {CIRCLE 3 PNT} softkey if you know 3 points on the circle. When you press the {CIRCLE 3 PNT} softkey, the control sets the current tool position as the start point (first point of 3 that is necessary to describe an arc) of a circular move.
Chapter 5 Editing Programs On Line 3. After the second point on the arc has been stored reposition the axes at the end point of the arc. Store this block as a circular block by pressing either the {STORE END PT} or the {EDIT & STORE} softkeys. This records the current tool location as the final position for this digitize operation. If you press: It: {STORE END PT} does not return the control to the program display screen.
Chapter 5 Editing Programs On Line Figure 5.6 CIRCLE TANGNT Digitize Screen DIGITIZE: E-STOP TARGET[ MM R F Z - 0.000 X - 0.000 C -359.99 0.000 MMPM S 00 STORE END PT 2. EDIT & STORE Reposition the tool at the end point of the arc using any of these methods: Jog the Axes in manual mode. Automatically move the axes by executing a part program or MDI program.
Chapter 5 Editing Programs On Line If you press: It: {STORE END PT} does not return the control to the program display screen. Pressing this softkey inserts the generated block at whatever location the cursor was last at and allows the operator to immediately begin entering the next block using this same digitize feature. {EDIT & STORE} returns the control to the program display screen.
Chapter 5 Editing Programs On Line 2. Press the {DELETE PRGRAM} softkey. (softkey level 2) ACTIVE EDIT RESTRT DISPLY COPY PRGRAM PRGRAM PRGRAM PRGRAM PRGRAM DELETE VERIFY PRGRAM RENAME INPUT PRGRAM PRGRAM COMENT PRGRAM DEVICE REFORM CHANGE MEMORY DIR 3. Select one of these two choices: Key in the the program name and press the {DELETE YES} softkey Move the block cursor down until the desired program is in reverse video and press the {DELETE YES} softkey.
Chapter 5 Editing Programs On Line 2. Press the {RENAME PRGRAM} softkey. (softkey level 2) ACTIVE EDIT RESTRT DISPLY COPY PRGRAM PRGRAM PRGRAM PRGRAM PRGRAM DELETE VERIFY PRGRAM RENAME INPUT PRGRAM PRGRAM COMENT PRGRAM DEVICE REFORM CHANGE MEMORY DIR 3. Key in the current program name or cursor down until the desired program is in reverse video. Then: Type in a comma, the new program name. Press the {RENAME YES} softkey. To abort the operation press the softkey.
Chapter 5 Editing Programs On Line 2. Select the input device using the {INPUT DEVICE} softkey (as described in chapter 7). This is only necessary if the currently active input device is not the device that the part program to display is currently resident on. The default input device is control memory. 3. Move the block cursor to the program to be displayed (if the program is resident in control memory), or key-in the program name (if reading from an input device attached to port A or port B). 4.
Chapter 5 Editing Programs On Line To assign a comment to a program without using a comment block as the first block of the program, follow the steps below: 1. Press the {PRGRAM MANAGE} softkey. This displays the program directory screen. Any existing comments that have previously been assigned to a program are displayed to the right of the program name. (softkey level 1) PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD 2.
Chapter 5 Editing Programs On Line 5.9 Copying Programs {COPY PRGRAM} This section describes making a duplicate of a part program in control memory. To input or output a part program from/to a peripheral device, see the sections on inputting or outputting programs in chapter 9. To copy part programs stored in memory using different program names: 1. Press the {PRGRAM MANAGE} softkey. (softkey level 1) 2.
Chapter 5 Editing Programs On Line Important: The control displays the active communication parameters if one of the communication ports has been chosen. If the communication port parameters do not match that of the peripheral device, they must be altered for a successful copy to take place. For details on setting communication port parameters, see page NO TAG. 6. Select softkey {COPY YES} or {COPY NO}. {COPY YES} copies the part program, while {COPY NO} aborts the copy operation.
Chapter 5 Editing Programs On Line To access the protectable part program directory: 1. Press the {PRGRAM MANAGE} softkey. (softkey level 1) PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD The control displays the main program directory screen: SELECTED PROGRAM: MAIN NAME MAIN O12345 RRR TEST DIRECTORY SIZE 1 OF 1 COMMENT 2.3 14.3 9.3 3.9 4 FILES PAGE THIS IS A TEST PROG 120.
Chapter 5 Editing Programs On Line 2. Press the {CHANGE DIR} softkey. (softkey level 2) ACTIVE EDIT RESTRT DISPLY COPY PRGRAM PRGRAM PRGRAM PRGRAM PRGRAM VERIFY PRGRAM DELETE RENAME INPUT PRGRAM COMENT PRGRAM PRGRAM DEVICE REFORM CHANGE MEMORY DIR Important: The control does not display the {CHANGE DIR} softkey if your password does not allow you access to it.
Chapter 5 Editing Programs On Line The programs in this directory are protected. This means: they are processed the same as unprotected programs the blocks of protected programs are not displayed during program execution unless you have access to the {CHANGE DIR} softkey (in place of the protected program blocks, the last user non-protected programming block is displayed) you can cycle stop during program execution (but you cannot single block through a program) 5.10.
Chapter 5 Editing Programs On Line To set-up the character encryption/decryption table: 1. Select the protected part program directory. 2. Press the {SET-UP NCRYPT} softkey. (softkey level 2) ACTIVE EDIT RESTRT DISPLY COPY PRGRAM PRGRAM PRGRAM PRGRAM PRGRAM VERIFY PRGRAM DELETE RENAME INPUT PRGRAM COMENT PRGRAM PRGRAM DEVICE REFORM CHANGE NCRYPT SET-UP MEMORY DIR MODE NCRYPT The control displays the set-up encryption screen: ENTER A CHARACTER: = = # % & ( ) * + ’ - = = = = = = = = = .
Chapter 5 Editing Programs On Line To fill in the encryption/decryption table by using the operator panel keys: use the arrow keys to move the cursor to the place where you want to assign an encryption/decryption character enter a character and press the [TRANSMIT] key You must enter a unique character for each character on the set-up encryption screen. To fill in the encryption/decryption table by using the softkey, press the {REVRSE FILL} softkey.
Chapter 5 Editing Programs On Line When you press the {UPDATE & EXIT} softkey, the control does a compile/check of the encryption/decryption table to determine that no duplicate characters exist and that no characters were left blank.
Chapter 5 Editing Programs On Line 3. Press the {STORE BACKUP} softkey. The control displays the message “STORING TO BACKUP -- PLEASE WAIT” on the CRT until the control has finished storing the encryption/decryption table in its backup memory.
Chapter 5 Editing Programs On Line 5-50
Chapter 6 Editing Part Programs Off Line (ODS) 6.0 Chapter Overview This chapter describes how to use the Offline Development System (ODS) to edit part programs. Major sections include: Topic: On page: Selecting the part program application 6-2 Editing off line 6-3 Interfacing with the control 6-6 Downloading from ODS 6-6 Uploading to ODS 6-13 Use the Offline Development System (ODS) to write or edit part programs.
Chapter 6 Editing Part Programs Off Line 6.1 Selecting the Part Program Application Selecting the Part Program application provides access to the part program utilities of ODS. To select the Part Program application: 1. Return to the main menu line of ODS. 2. Press [F3] to pull down the Application menu: The workstation displays this screen: Proj: PALTEST F1 - File 3.
Chapter 6 Editing Part Programs Off Line 6.2 Editing Part Programs Off Line Use the Edit Part Program utility of ODS to edit part programs on a workstation. Programs that already exist on the control can be uploaded to the workstation for editing. These programs or programs created using ODS can be edited using the screen or text editor that is configured in ODS. To edit part programs thorough ODS: 1. Select the Part Program Application. See above. 2.
Chapter 6 Editing Part Programs Off Line 3. Press [E] to select the Part Program option. The workstation displays this screen: Proj: Demo Appl: Part Program F1 - File F2 - Project F3 - Application F4 - Utility Util: File Management F5 - Configuration Editing Part Program ... Selecting New or Existing File Use ARROWS or Type in name. Press ENTER when done or ESC to cancel FILE1 FILE2 FILE3 4. Select a new or existing file. To create a new file, type in the new file name.
Chapter 6 Editing Part Programs Off Line After you select a file, the workstation displays a screen explaining the text editor: Proj: Demo F1 - File Appl: Part Program F2 - Project F3 - Application F4 - Utility Util: File Management F5 - Configuration The configured text editor will now be executed, using the file name selected. Press any key to continue... Use the configured screen or text editor to edit part programs. The editor must be compatible with the ODS operating system.
Chapter 6 Editing Part Programs Off Line 6.3 Interfacing the Workstation with the Control The following sections require that the workstation be connected to the control or storage device. Connect the workstation to the control or storage device with the RS-232 serial interface cable (cable CN25 in the integration/maintenance manual, chapter 4). Use cable CN25 to connect the RS-232 interface port on the rear of the workstation to Port B (CN16F) on the control or the RS-232 port on the storage device.
Chapter 6 Editing Part Programs Off Line To download a part program from ODS to the control’s memory, follow these steps: 1. Interface the workstation with the control. See page 6-6. 2. Return to the main menu line of ODS. 3. Press [F3] to pull down the Application menu. The workstation displays this screen: Proj: PALTEST F1 - File 4.
Chapter 6 Editing Part Programs Off Line 5. Press [F4] to pull down the Utility menu. Proj: Demo F1 - File Appl: Download F2 - Project F3 - Application Util: File Management F5 - Configuration F4 - Utility Send AMP params Send PAL and I/O Send Part Program 6. (A) (P) (R) Use the arrow keys to highlight the Send Part Program option, then press[ENTER], or press [R].
Chapter 6 Editing Part Programs Off Line 7. Use the arrow keys to highlight the download destination or press the letter that corresponds to the download destination. When selected, press [ENTER]. The workstation displays the part program files that are stored in the active project directory of the workstation: Proj: Demo Appl: Download F1 - File F2 - Project F3 - Application Util: File Management F4 - Utility F5 - Configuration Downloading Use ARROW keys or Type in name. FILE1 FILE2 8.
Chapter 6 Editing Part Programs Off Line If the selected part program file name already exists on the control, the workstation displays this screen: Proj: Demo F1 - File Appl: Download F2 - Project F3 - Application Util: Get Part Program F4 - Utility F5 - Configuration File Already Exits Enter Option Rename existing file Overwrite existing file Abort current file (R) (O) (A) Important: The currently active or open part program on the control can not be renamed or overwritten during a download pro
Chapter 6 Editing Part Programs Off Line After selecting the Rename or Overwrite option, or if the file being downloaded did not already exist on the control, the workstation displays this screen: Proj: Demo F1 - File Appl: Download F2 - Project F3 - Application Util: Send Part Program F4 - Utility F5 - Configuration Download In Progress Percent completed 50% The percentage of the download process that has currently been completed is displayed on the screen.
Chapter 6 Editing Part Programs Off Line When the download process is complete, the workstation displays this screen: Proj: Demo Appl: Download F1 - File F2 - Project F3 - Application Util: Send Part Program F4 - Utility F5 - Configuration Download Complete Download Another File? Yes No 9. 6-12 (Y) (N) Select “Yes” or “No.” If you select: Then: Yes the system prompts the programmer through the download procedure again No the workstation returns to ODS the main menu line.
Chapter 6 Editing Part Programs Off Line If the workstation was unable to complete the download procedure in the allotted time frame, it displays this screen: Proj: Demo F1 - File Appl: Download F2 - Project F3 - Application Util: Send Part Program F4 - Utility F5 - Configuration A time-out occurred ... Press any key to continue ... Pressing any key causes the workstation to return to the ODS main menu. 6.
Chapter 6 Editing Part Programs Off Line 3. Press [F3] to pull down the Application menu. The workstation displays this screen: Proj: PALTEST F1 - File 4. Appl: Upload F2 - Project Util: Get PAL I/O F3 - Application F4 - Utility AMP PAL I/O Assignments Part Program Upload Download (A) (P) (I) (R) (U) (D) F5 - Configuration Use the arrow keys to highlight the Upload application, then press or press [U]. [ENTER] 5. Press[F4] to pull down the Utility menu.
Chapter 6 Editing Part Programs Off Line 6. Use the arrow keys to highlight the Get Part Program option, then press[ENTER], or press [R]. The workstation displays this screen: Proj: Demo Appl: Part Program F1 - File F2 - Project F3 - Application Util: Get Part Program F4 - Utility F5 - Configuration Upload Origin Control Storage 7. (C) (S) Use the arrow keys to highlight the upload origin, then press or press the letter that corresponds to the upload origin.
Chapter 6 Editing Part Programs Off Line 8. Use the arrow keys to highlight the name of the part program to be uploaded to the workstation or type in the part program name, then press [ENTER]. When you upload a program from the control, the control does not display a message to indicate that an upload is taking place. If you upload a large program it may take several minutes for the upload to complete.
Chapter 6 Editing Part Programs Off Line If you select the Rename option, the workstation renames the existing file, which has the same name as the file being uploaded, on the workstation. The workstation displays the part program files stored on the workstation: Proj: Demo Appl: Upload F1 - File F2 - Project F3 - Application Enter new name: Util: Get Part Program F4 - Utility F5 - Configuration Rename To.... FILE1 FILE2 FILE3 9.
Chapter 6 Editing Part Programs Off Line If the name of the part program that was entered does not exist on the workstation or the Overwrite option was selected the workstation displays this screen: Proj: Demo F1 - File Appl: Upload F2 - Project F3 - Application Util: Get Part Program F4 - Utility F5 - Configuration Upload In Progress Percent Transferred: 80% The percentage of the upload process that has currently been completed is displayed on the screen.
Chapter 6 Editing Part Programs Off Line After the part program has been uploaded to the workstation, the workstation displays this screen: Proj: Demo Appl: Upload F1 - File F2 - Project F3 - Application Util: Get Part Program F4 - Utility F5 - Configuration Upload Complete Upload Another File? Yes No (Y) (N) Select “Yes” or “No.” If you select: Then: Yes the system prompts the programmer through the upload procedure again No the workstation returns to ODS the main menu line.
Chapter 6 Editing Part Programs Off Line 6-20
Chapter 7 Running a Program 7.0 Chapter Overview This chapter describes how to test a part program and execute it in automatic mode. Major topics include: Topic: On page: Selecting special running condition 7-1 Selecting a part program input device 7-5 Selecting a program 7-6 De-selecting a part program 7-8 Program search 7-9 Program execution 7-17 Jog retract 7-28 Block retrace 7-31 7.
Chapter 7 Running a Program 7.1.2 Miscellaneous Function Lock When the MISCELLANEOUS FUNCTION LOCK is made active, the control displays M-, second auxiliary functions (B-codes), S-, and T-codes in the part program and activates the corresponding Tool Wear Offset, except for M00, M01, M02, M30, M98, M99, and M100-M199. M100-M199 are process synchronization codes for dual-process systems.
Chapter 7 Running a Program 2. Press the {ACTIVE PRGRAM} softkey. (softkey level 2) ACTIVE EDIT RESTRT DISPLY COPY PRGRAM PRGRAM PRGRAM PRGRAM PRGRAM DELETE VERIFY PRGRAM RENAME INPUT PRGRAM PRGRAM COMENT PRGRAM DEVICE REFORM CHANGE MEMORY DIR 3. Press the {SEQ STOP} softkey. (softkey level 3) DE-ACT SEARCH MID ST T PATH T PATH PRGRAM PRGRAM GRAPH DISABL SEQ STOP 4. TIME PARTS Key in the sequence number where you want automatic operation in the part program to stop, then press the [TRANSMIT] key.
Chapter 7 Running a Program 7.1.4 Single Block In single block mode, the control executes the part program block by block. Each time you press the button, the control executes one block of commands in the part program when in single block mode. Figure 7.1 Single Block SINGLE BLOCK CYCLE START When is pressed, one block of commands is executed Cutting tool To activate the single block function, press the button.
Chapter 7 Running a Program 7.2 Selecting a Part Program Input Device Before selecting a part program, you must tell the control where this part program is currently residing.
Chapter 7 Running a Program 3. Press the softkey corresponding to the location where the part program is to be read from, {FROM PORT A}, {FROM PORT B}, or {FROM MEMORY}. (softkey level 3) FROM FROM FROM PORT A PORT B MEMORY To activate a part program, it must be selected as described on page 8.3. 7.
Chapter 7 Running a Program This screen appears: SELECTED PROGRAM: DIRECTORY PAGE NAME TEST O12345 MAIN SHAFT2 XXX SIZE AE 1 OF 1 COMMENT 3.9 1.3 1.3 1.3 1.3 SUB TEST 1 THIS IS A TEST PROGRAM 5 FILES 137.8 METERS FREE ACTIVE EDIT RESTRT DISPLY COPY PRGRAM PRGRAM PRGRAM PRGRAM PRGRAM Important: This screen shows program TEST as active and being edited. Make sure no part program is currently already active.
Chapter 7 Running a Program 3. Press the {ACTIVE PRGRAM} softkey to activate the selected program. The control displays the part program name, followed by the first few blocks of the selected program. Important: The following softkey level 2 indicates that the control is using control memory as an input device. If the input device is some device other than control memory, some of these softkeys are not available.
Chapter 7 Running a Program 2. Press the {ACTIVE PRGRAM} softkey. The control displays the first few blocks of the currently active program. (softkey level 2) ACTIVE EDIT RESTRT DISPLY COPY PRGRAM PRGRAM PRGRAM PRGRAM PRGRAM DELETE VERIFY PRGRAM RENAME INPUT PRGRAM PRGRAM COMENT PRGRAM DEVICE REFORM CHANGE MEMORY DIR 3. If the program selected is not the active program you wanted, press the {DEC-ACT PRGRAM} softkey. The control deactivates the part program and return to the directory screen.
Chapter 7 Running a Program To perform a program search operation: 1. Press the {PRGRAM MANAGE} softkey. The program to search must have been previously selected for automatic execution as described in page 7-6. (softkey level 1) 2. PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD Press the {ACTIVE PRGRAM} softkey.
Chapter 7 Running a Program 4. 5. Choose from the 6 search options: If you are searching for: Press this softkey: a sequence number {N SEARCH} an O-word {O SEARCH} the end of each block {EOB SEARCH} the program one line at a time {SLEW} a specific character string {STRING SEARCH} the beginning of your next program {NEXT PRGRAM} This softkey is available only if your input device has been configured as a tape reader. See chapter 9 on input device selection.
Chapter 7 Running a Program When you press the {NEXT PRGRAM} softkey, the control first searches for a valid program end code. See setting communications, chapter 9. After it finds the program end code, it advances to the program start code of the next program. If the current program is the last program on the tape, the message “SERIAL COMMUNICATION ERROR #5” appears on the screen indicating a time-out error.
Chapter 7 Running a Program Important: Incremental moves that occur during a program search with recall operation, are always referenced from the last known absolute position in the part program. If no absolute position is specified in the searched part program blocks, the control will use the current axis position as the start point for incremental moves. When a search with recall is performed, the control finds a character string or sequence number in a specific block for execution to begin from.
Chapter 7 Running a Program To perform a program search with recall, follow these steps: 1. Press the {PRGRAM MANAGE} softkey. (softkey level 1) 2. PRGRAM OFFSET MACRO MANAGE PARAM QUICK CHECK FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD SYSTEM SUPORT Press the {ACTIVE PRGRAM} softkey.
Chapter 7 Running a Program 5. Key in the desired character string or sequence number to search for and press the [TRANSMIT] key. The control locates an @ symbol to the left of the block immediately before the block that automatic execution begins from. If this is not the block to begin execution from press either the: {CONT} softkey to continue to search for the entered character string or sequence number. {TOP OF PRGRAM} to return to the first block in the program.
Chapter 7 Running a Program {EXIT & MOVE} - Use this softkey if the tool is not at the exact location for execution of the searched block. Be aware that the absolute position of the axes necessary at the start of the searched block is dependant on the previous blocks. There can be offsets activated or incremental moves that can make it difficult for you to determine the exact absolute starting point for the axes.
Chapter 7 Running a Program 7.7 Basic Program Execution After a program is written or loaded into the control, it should be thoroughly tested before a part is mounted and machined. The control offers 3 distinct testing modes in addition to fully automatic operation. These modes are briefly described below in the order in which they would normally be implemented. QuickCheckä (see page 7-18) — This mode is a basic syntax checker for a part program. It checks that proper format and syntax has been followed.
Chapter 7 Running a Program (1) Pressing When you press the button, motion of the cutting tool decelerates and stops, and the control stops automatic operation. If you press the button during a dwell, the dwell is interrupted and any remaining time/revolutions for the dwell are stored for later execution.
Chapter 7 Running a Program To use the QuickCheck feature, follow these steps. 1. Select a program to check as described on page 7-5 and return to softkey level 1. 2. Press the {PRGRAM CHECK} softkey. (softkey level 1) 3. PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD Press the {QUICK CHECK} softkey.
Chapter 7 Running a Program To disable QuickCheck with or without graphics, press the {STOP CHECK} softkey. CAUTION: Note that when a program is run during quick check mode, the control performs all coordinate system offset operations. This means that changes to the coordinate systems or coordinate offset tables are made (G10 blocks, changes to G92 and G52 offsets, and changes to the active work coordinate systems G54-G59.9). All of these changes are discarded at any termination of QuickCheck.
Chapter 7 Running a Program You can activate the Axis Inhibit feature using a switch installed by your system installer (see documentation provided by the system installer) or by using the {FRONT PANEL} softkey (see page 2-13). The control must be in cycle stop or E-Stop to activate or deactivate the Axis Inhibit feature. Any attempt to activate or deactivate the feature during program execution or when in cycle suspend or feedhold states is ignored.
Chapter 7 Running a Program You can use the to modify the cutting feedrate. Your system installer determines in AMP if rapid feedrates are overrides by the switch/button or the switch during Dry Run. CAUTION: When testing a program using Dry Run, the control still recognizes and executes M-, B-, S-, and T-codes. To ignore M-, B-, S-, and T-codes, execute Dry Run in conjunction with miscellaneous function lock. See section 8.1.2.
Chapter 7 Running a Program The Dry Run feature can be activated using a switch installed by your system installer (see documentation provided by your system installer) or by using the {FRONT PANEL} softkey (see page 2-13). 7.7.4 Part Production/Automatic Mode Automatic mode is the normal operating mode of the control. A program that is run in the automatic mode is executed with all of the axes active and all of the programmed feedrates active. Graphics is also available as described in chapter 8.
Chapter 7 Running a Program Command: Process: CYCLE START begins part program execution CYCLE STOP stops part program execution WARNING: Always test a program prior to automatic operation. Always verify that the workspace is clear and all safety features are intact before pressing . Figure 7.
Chapter 7 Running a Program 7.8 Interrupted Program Recover {RESTRT PRGRAM} Use the program recover feature to resume a program that was executing and was interrupted by some means such as a control reset, E-Stop, or even power failure in some cases. This feature will scan the program as it searches for the interrupted block and from within the search area: send to PAL the last programmed modal G--codes from each modal group.
Chapter 7 Running a Program CAUTION: When a program recover is performed the control automatically returns the program to the beginning of the block that was originally interrupted. The beginning of the block is probably not the point that axis motion was interrupted. For absolute linear moves this causes no problem if the tool is still somewhere along the path of the block that program execution was interrupted while cutting.
Chapter 7 Running a Program To perform a program restore operation after automatic program execution has been interrupted follow these steps: 1. Press the {PRGRAM MANAGE} softkey. (softkey level 1) PRGRAM OFFSET MACRO MANAGE PARAM QUICK CHECK FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD SYSTEM SUPORT Important: DO NOT SELECT A PROGRAM AS AN ACTIVE PROGRAM. Do not disable the currently active program (if any).
Chapter 7 Running a Program CAUTION: When you exit a program restart operation (search with memory), M- and S-codes are sent to PAL. If, during normal execution, that program activated a spindle, mid-program start may also start it. 4. Press the {EXIT} softkey if the block selected is the block to begin program execution from. If it not the desired block, it will be necessary to disable the program or perform a search with memory operation to locate the desired block manually.
Chapter 7 Running a Program CAUTION: If the Jog Retract function is deactivated during its execution (performing a control reset, E-Stop, etc.), attempting to return the tool by pressing can cause the Jog Retract function to abort. The program returns to the start point of jog retract along a linear path.
Chapter 7 Running a Program Figure 7.5 Jog Retract Operation Jog retract exit moves Jog retract return moves In Figure 7.5 the control only recognized 6 jog moves upon returning instead of the actual 11 moves that were made to retract the tool. This is because the jog retract feature records consecutive jog moves on the same axis as one move.
Chapter 7 Running a Program Figure 7.6 Jog Retract Moves that Exceed the Maximum Allowed in AMP Return path 4 2 3 7 5 1 6 Figure 7.6 emphasizes the possible problems that can result from exceeding the maximum allowed jog retract moves. In this example, the number of allowed moves set in AMP is four. When you press the cycle start button at the end of the 7th jog move, the control ignores moves 5, 6, and 7 and takes the shortest path to the endpoint of exit move 4.
Chapter 7 Running a Program To perform a block retrace operation: 1. Press the or activate the feature button to stop program execution. 2. Press the button. After you press the button, the control retraces the block that was being executed when the cycle stop occurred or retraces the block just completed if you press the single block button, provided that the block is a legal block for retrace.
Chapter 7 Running a Program The block retrace function is unable to retrace any of these blocks and an attempt to do so results in an error message: Threading Tapping Boring Inch/Metric changes (unit conversion) A block that commands a tool change operation A block that commands a change in the coordinate system Any block that is followed by a Manual Jog Move except a Jog Retract The number of blocks retraced is already equal to the maximum number of retraceable blocks as determined in AMP Certain Paramacr
Chapter 7 Running a Program 7-34
Chapter 8 Display and Graphics 8.0 Chapter Overview The first part of this chapter gives a description of the different data displays available on the control. The second part gives a description of the control’s graphics capabilities. 8.1 Selection of Axis Position Data Display Pressing the [DISP SELECT] key displays the softkeys for selecting the axis position data screens. The control provides 8 different axes position data screens as described in Table 8.A.
Chapter 8 Displays and Graphics The screens described above may also show in addition to axis position: The current unit system being used (millimeters or inches) E-Stop The current feedrate The current spindle speed of the controlling spindle The current tool and tool offset numbers The active program name (if any) The active subprogram name (if any) The current operating mode (MDI, manual or automatic) The current operating status (cycle stop, suspend, start, feedhold) The current block executing (sequen
Chapter 8 Displays and Graphics 3. To return to softkey level 1, press the [DISP SELECT] key again. The most recently selected data position screen will remain in effect for softkey level 1 until either power is turned off or a different position display screen is selected. The default screen selected at power up is the regular size program display. The following figures show the axis position data display that will result when the corresponding softkey is pressed.
Chapter 8 Displays and Graphics {PRGRAM} (Large Display) Axis position in the current work coordinate system displayed in large characters. Figure 8.2 Results After Pressing {PRGRAM} (Large Display) Softkey PROGRAM[ MM E-STOP (ACTIVE PROGRAM NAME) ] X - 7483 .647 Z - 7483 .647 U - 7483 .647 F 0.
Chapter 8 Displays and Graphics {PRGRAM} (Small Display) Axis position in the current work coordinate system displayed for all system axes in the active process (only available when more than 9 axis are AMPed in the system, or more than 8 axis in the process for dual process systems). Figure 8.3 Results After Pressing {PRGRAM} (Small Display) Softkey PROGRAM[ MM X Y Z U V W A B C $X $Y $Z F ] -9999.647 -3333.647 -1111.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.
Chapter 8 Displays and Graphics {ABS} The axis position data in the machine coordinate system. Figure 8.4 Results After Pressing {ABS} Softkey E-STOP ABSOLUTE[ MM ] 0.000 MMPM 00 X 0.000 S Z 0.000 T 0 U -0.
Chapter 8 Displays and Graphics {ABS} (Large Display) Axis position in the machine coordinate system displayed in large characters. Figure 8.5 Results After Pressing {ABS} (Large Display) Softkey E-STOP ABSOLUTE[ MM ] (ACTIVE PROGRAM NAME) X 0.000 Z 0.000 U -0.035 F 0.
Chapter 8 Displays and Graphics Figure 8.6 Results After Pressing {ABS} (Small Display) Softkey ABSOLUTE X Y Z U V W A B C $X $Y $Z F [ MM ] -9999.647 -3333.647 -1111.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 0.
Chapter 8 Displays and Graphics {TARGET} The coordinate values of the end point of the currently executing axis move is displayed at a position in the current work coordinate system. Figure 8.7 Results After Pressing {TARGET} Softkey E-STOP TARGET[ MM ] F X -7483.647 S Z -7483.647 T 0 U -7483.647 MEMORY MAN PRGRAM A B S 0.
Chapter 8 Displays and Graphics {TARGET} (Large Display) The coordinate values in the current work coordinate system, of the end point of commanded axis moves in normal size characters. Figure 8.8 Results after Pressing {TARGET} Softkey TARGET [ MM F E-STOP (ACTIVE PROGRAM NAME) ] X - 7483 . 647 Z - 7483 . 647 U - 7483 . 647 0.
Chapter 8 Displays and Graphics Figure 8.9 Results After Pressing {TARGET} (Small Display) Softkey TARGET X Y Z U V W A B C $X $Y $Z F [ MM ] -9999.647 -3333.647 -1111.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 -2222.647 0.
Chapter 8 Displays and Graphics {DTG} The distance from the current position to the command end point, of the commanded axis in normal size characters. Figure 8.10 Results After Pressing {DTG} Softkey E-STOP DISTANCE TO GO[ MM F X 0.021 S Z 0.000 T 0 U 0.000 MEMORY MAN PRGRAM A B S 8-12 ] 0.
Chapter 8 Displays and Graphics {DTG} (Large Display) The distance from current position to the command end point of the commanded axis move in large characters. Figure 8.11 Results After Pressing {DTG} (Large Display) Softkey E-STOP DISTANCE TO GO[ MM ] (ACTIVE PROGRAM NAME) X 0.021 Z 0.000 U 0.000 F 0.
Chapter 8 Displays and Graphics Figure 8.12 Results After Pressing {DTG} (Small Display) Softkey Distance to Go X Y Z U V W A B C $X $Y $Z F ] 0000.000 0000.000 0000.000 0000.000 0000.000 0000.000 0000.000 0000.000 0000.000 0000.000 0000.000 0000.000 0.
Chapter 8 Displays and Graphics {AXIS SELECT} Important: {AXIS SELECT} is available only during a large character display or when more than 9 axes are displayed on a normal size display. When you press {AXIS SELECT}, the control displays the axis names in the softkey area. Press a specific axis letter softkey to toggle the position display of that axis on and off.
Chapter 8 Displays and Graphics {M CODE STATUS} The currently active M--codes are displayed. This screen indicates only the last programmed M--code in the modal group. It is the PAL programmers responsibility to make sure proper machine action takes place when the M--code is programmed. Figure 8.
Chapter 8 Displays and Graphics {PRGRAM DTG} This screen provides a multiple display of position information from the program screen and the distance to go screen. Figure 8.15 Program, Distance to Go Screen E-STOP PROGRAM DISTANCE TO GO X - 7483.647 X 0.031 Y - 7483.647 Y 0.000 Z - 7483.647 Z 0.000 F 0.
Chapter 8 Displays and Graphics {PRGRAM DTG} (Small Display) This screen provides a multiple display of position information from the program screen and the distance to go screen. It displays all system axes in the active process (only available when more than 9 axis are AMPed in the system, or more than 8 axis in the process for dual process systems). Figure 8.16 Program, Distance to Go Screen (Small Display) PROGRAM X Y Z U V W A B C $X $Y $Z F Distance to Go -9999.647 -3333.647 -1111.647 -2222.
Chapter 8 Displays and Graphics {ALL} This screen provides a multiple display of position information from the program, distance to go, absolute, and target screen. The all display is only available on systems with 6 or less axes. On systems with more than 6 axes, other combination screens are available which display a subset of the data available on the ALL display. Figure 8.17 Result After Pressing {All} Softkey E-STOP PROGRAM DISTANCE TO GO X Y Z X Y Z - 7483.647 - 7483.647 - 7483.647 0.000 0.
Chapter 8 Displays and Graphics {G CODE STATUS} The currently active G-codes are displayed. Figure 8.18 Results After Pressing {G CODE} Softkey PROGRAM STATUS PAGE 2 OF 2 G50.1 MIRROR IMAGE CONTROL G64 G67 CUTTING MODE MACRO CALL CANCEL G70 G80 G90 G94 G97 G98 INCH PROGRAMMING CANCEL OR END FIXED CYCLE ABSOLUTE FEED/MIN CSS PROGRAMMING OFF FIXED CYCLE INITIAL LEVEL RETURN PROGRAM STATUS G01 G07 G12.
Chapter 8 Displays and Graphics {SPLIT ON/OFF} The split screen softkey is only available if your system installer has purchased the dual-process option. When you press the {SPLIT ON/OFF} softkey, you can view information for both processes. The screen displays two 40-column screens on one 80-column screen. Process 1 is displayed on the left, and process 2 is displayed on the right. The active process appears in reverse video.
Chapter 8 Displays and Graphics A large screen display makes it easier for you to see the axes. E-STOP PROGRAM [MM] PROGRAM [MM] X 0.000 Z 0.000 F 0.000 IPM S O X 0.000 F 0.000 PRGRAM 8.2 PAL Display Page ABS IPM S O TARGET DTG AXIS SELECT If desired the system installer has the option of configuring custom screens that will show up on the CRT.
Chapter 8 Displays and Graphics If the parameter altered is used in the currently executing program block, that value will not be activated until the following block (unless a cutter compensation value is being altered). If the parameter is altered in a block that is within the controls look ahead range (refer to chapter 22 for details on block look ahead) then the look ahead blocks are re-setup and the new parameter value is incorporated in them (unless a cutter compensation value is being altered).
Chapter 8 Displays and Graphics 9/240 CNCs The 9/240 control is equipped to display four languages. The languages available and the order they are displayed are fixed in this order: English Italian Japanese German 8.4 Graphics QuickCheck and active program graphics function similarly. They both plot tool paths. The following section describes how to use both types of graphics and distinguishes how they differ.
Chapter 8 Displays and Graphics 2. Select a program. Press {SELECT PRGRAM}. (softkey level 2) SELECT QUICK PRGRAM CHECK 8.4.2 Running Graphics STOP CHECK T PATH T PATH GRAPH DISABL 3. Use the up and down cursors to select a program. 4. Press {ACTIVE PRGRAM} to return to level 2 and activate the program. Follow these steps to run graphics: 1. Press the {PRGRAM CHECK} softkey. (softkey level 1) 2.
Chapter 8 Displays and Graphics The control for both QuickCheck and active graphics continues to plot tool paths, even if the graphics screen is not displayed. Actual display of the tool paths is only possible on the graphics screen. When the graphics screen is displayed again, any new tool motions appear on the screen. While on the graphics screen only the currently executing block is displayed. The currently executing block is displayed on line 22 of the CRT, and it is limited to 80 characters.
Chapter 8 Displays and Graphics 8.4.3 Disabling Graphics In some cases, you may want to operate without graphics. For example, you cannot edit a part program using QuickView while in graphics, or you may want to speed up processing by disabling graphics.
Chapter 8 Displays and Graphics You may want to change the parameters to alter your graphics. If you want to view a different graphics screen, you must change the default values for the parameters.
Chapter 8 Displays and Graphics 2. Set Select Graph. Use the up and down cursor keys to select the axes. Then set them by pressing the left or right cursor keys. The data for the selected axes change each time you press the left or right cursor key. A pictorial representation of the selected graph, which is determined by the selected axes, is displayed on the screen. You have three fields that you can adjust. The axes are shown as horizontal and vertical axes.
Chapter 8 Displays and Graphics 4. Set Auto Size. Use the up and down cursor keys to select the parameter. Set auto size by pressing the left or right cursor keys. The value for the selected parameter changes each time you press the left or right cursor key. If you turn this parameter “ON”, the control re-sizes the graphics screen to the size of the programmed part. To use this feature, turn this parameter “ON”, then run the part program.
Chapter 8 Displays and Graphics 7. Set the Main Program Sequence Starting #: parameter. It is only available with QuickCheck. Use the up and down cursors to select this parameter. Set it by typing in the new value for that parameter using the keys on the operator panel. Press the [TRANSMIT] key when the new value has been typed in. The old value for the sequence number is replaced with the new value.
Chapter 8 Displays and Graphics 9. Set the Process Speed parameter. It is only available with QuickCheck. Use the up and down cursors to select this parameter. Set it by pressing the left or right cursor keys. The data for the selected parameter changes each time you press the left or right cursor key. Use this parameter to select the speed for the control to draw graphics.
Chapter 8 Displays and Graphics 8.4.5 Graphics in Single-Block 8.4.6 Clearing Graphics Screen The active and QuickCheck graphics features can run in single-block or continuous mode as described in chapter 8. In: This happens: Single block one block of a part program executes each time you press the . Continuous mode the control continues to execute blocks sequentially as they are read.
Chapter 8 Displays and Graphics Figure 8.19 Zoom Window Graphic Display Screen. 20.0 15.6 11.1 6.7 2.2 -2.2 -6.7 X -11.1 -15.6 -20.0 -20.0 -10.3 Z -0.5 9.2 INCR DECR WINDOW WINDOW 18.9 27.7 ZOOM ABORT 38.4 48.1 57.9 ZOOM This screen resembles the regular QuickCheck graphics screen with the exception that it includes a window and different softkeys. Use the window to define a new size and location for the tool path graphic display. The area within the window will become your next screen.
Chapter 8 Displays and Graphics To use the zoom window feature: 1. Press the {ZOOM WINDOW} softkey. This changes the display to the zoom window display. (softkey level 3) CLEAR MACHNE ZOOM GRAPHS INFO WINDOW 2. ZOOM BACK GRAPH SETUP Use the cursor keys on the operator panel to move the center of the window around the screen. To move the window center at a faster rate, press and hold the [SHIFT] key while pressing the cursor keys.
Chapter 8 Displays and Graphics 3. To change the size of the window, use the {INCR WINDOW} or softkeys. To change the window size at a faster rate, press and hold the [SHIFT] key while pressing the {INCR WINDOW} or {DECR WINDOW} softkeys. {DECR WINDOW} 4. Each time you press: The Zoom Window : {INCR WINDOW} increases in size. {DECR WINDOW} decreases in size. Once the size and the location of the window are correct, press the {ZOOM} softkey to return to the regular QuickCheck graphics screen.
Chapter 8 Displays and Graphics 8.5 Power Turn-on Screen When power is turned on, the control displays the power turn-on screen . The following section discusses how to modify information displayed on this screen at power up. Editing the System Integrator Message Lines To edit the system integrator message lines of the power turn-on screen, do the following: 1. Press the [SYSTEM SUPORT] softkey.
Chapter 8 Displays and Graphics 4. Press the {ENTER MESAGE} softkey. This highlights the softkey, and the control displays the input prompt “PTO MESSAGE:” at the top of the screen. Also, the current text, if any, of the selected message line is shown on the input line next to the prompt. (The text may be edited like any other input string.) (softkey level 3) ENTER MESAGE 5. STORE BACKUP Once the line has been edited, press the key. This transfers the edited line to the PTO screen.
Chapter 8 Displays and Graphics In the event that a system error or warning, PAL display page, PAL message, or E-Stop condition occurs while the screen saver is active, the horizontal scrolling line is replaced with a scrolling message “MESSAGE PENDING, PRESS A KEY TO DISPLAY.” The operator should press any keyboard key or softkey to return to the normal 9/Series screen and view the condition. The system installer can write PAL to disable the screen saver automatically when one of these conditions occur.
Chapter 8 Displays and Graphics The screen saver setup screen appears. SCREEN SAVER ACTIVATION TIMER : 05 MINUTES SAVER ON/OFF INCR TIMER DECR TIMER Press This Softkey To: SAVER ON/OFF toggle between enabling and disabling the screen saver. When the softkey name is shown in reverse video, the screen saver is enabled. Note the system installers PAL program can override this softkey setting. INCR TIMER increase the duration of the Activation Timer by five minute increments.
Chapter 9 Communications 9.0 Chapter Overview This chapter covers: Topic 9.1 Setting Communications On page: Communication port parameters 9-3 Inputting part programs from a tape reader 9-9 Outputting part programs to a tape punch 9-13 Verifying saved materials 9-17 Error conditions for inputting and outputting part programs 9-18 This section covers the communication port parameters that are available with the control.
Chapter 9 Communications 2. Press the {DEVICE SETUP} softkey to display the device setup screen as shown in Figure 9.1. (softkey level 2) PRGRAM PARAM DEVICE MONISETUP TOR AMP TIME PARTS PTOM SI/OEM The 9/230 CNC does not support port A. It uses only port B. Figure 9.
Chapter 9 Communications 3. Use the up or down cursor keys to move the cursor to the parameter to be changed. The current value for each parameter will be shown in reverse video. Important: Select both the SERIAL PORT (A or B) and the DEVICE being set first (see Figure 9.1) since all other parameters are device dependent. 4. To change a value after a parameter has been selected, press the left or right cursor keys.
Chapter 9 Communications All of the following parameters can be set independently for each communication port (A or B). DEVICE (setting type of peripheral) Select your peripheral device immediately after selecting your serial port. The devices with default communication parameters stored in the control are listed in Table 9.A. If the device that you are using is not listed, select either USER PUNCH, USER PRINTER, or USER READER. Important: You cannot select the same device for both peripheral ports.
Chapter 9 Communications PORT TYPE Port type options differ depending on the port you select.
Chapter 9 Communications PROTOCOL Select the protocol for communications from the following options. LEVEL_1 LEVEL_2* DF1 RAW PARITY (parity check) Select the parity from the following parity check schemes: Parity Parity Check NONE No parity check EVEN Even parity ODD Odd parity STOP BIT (number of stop bits) Select the number of stop bits with this parameter. You can select: 1, 1.5, or 2 bits DATA LENGTH Select the number of bits that constitute one character with this parameter.
Chapter 9 Communications OUTPUT CODE Select either EIA (RS-244A) or ASCII (RS-358-B) as output codes for 8 bit data lengths. Selecting 7 bit data length sets this output code to “N/A” since EIA and ASCII do not apply to this type. AUTO FILENAME This parameter is valid only if you are inputting part programs to the control from a tape reader (refer to DEVICE for details). This parameter is used only if your tape contains more than one part program.
Chapter 9 Communications STOP PRG END This parameter is available only if you are reading a tape and have selected a tape reader as your device (refer to DEVICE for details). It determines if the tape reader is to stop at the end of each program or continue reading until the end-of-tape code is reached. Refer to the PROGRAM END section to determine what defines the end-of-program for your system. Setting Result Yes the tape reader stops every time it encounters a program end code.
Chapter 9 Communications If “%” is set to “yes”, making it a valid program end-code, no program end-code other than PRGRM NAME can be set to “yes”. If another program end-code is set to “yes”, the “%” option is automatically set to “no”. Refer to the descriptions for M-codes in chapter 10 for details. M02, M30 -- refer to the descriptions for M-codes in chapter 10 for details M99 -- refer to the descriptions for M-codes in chapter 10 for details % -- also used as end-of-tape code.
Chapter 9 Communications Figure 9.2 Program Directory Screen SELECTED PROGRAM: DIRECTORY NAME O12345 TEST MAIN TTTE XXX PAGE SIZE 1.3 3.9 1.3 1.3 1.3 5 FILES 1 OF 1 COMMENT SUB TEST 1 NEW THIS IS A TEST PROGRAM 120.7 METERS FREE ACTIVE EDIT RESTRT DISPLY COPY PRGRAM PRGRAM PRGRAM PRGRAM PRGRAM 3. Press the {COPY PRGRAM} softkey.
Chapter 9 Communications 5. Select the device to copy from by using this table. If the peripheral device is connected to: Press this softkey: Port A {FROM A TO MEM} Port B {FROM B TO MEM} The screen is changes to the “COPY PARAMETERS” screen (Figure 9.3) and displays the current device and setup parameters for that communication port. If the device displayed on the screen is not correct, select the correct device using the procedure described on page 9-1. Figure 9.
Chapter 9 Communications Input Multiple Programs Press {MULTI PRGRAM} to copy multiple programs from the tape into memory. If STOP PRG END was set to the tape reader “yes” stops each time it encounters a program end or tape end code. “no” continuously reads programs until it encounters a tape end code. For details on how multiple programs are input and named, refer to the AUTO FILENAME, STOP PRG END, and PROGRAM END parameters discussed beginning on page 9-7.
Chapter 9 Communications 9.3 Outputting Part Programs to a Tape Punch If a program is in control memory and you want to send a copy of that program to a peripheral device, follow these steps: 1. Verify that the peripheral device is connected to the correct serial port and that the port is configured for that device (refer to page 9-1). 2. Press the {PRGRAM MANAGE} softkey. The control displays the screen shown in Figure 9.4.
Chapter 9 Communications 3. Press the {COPY PRGRAM} softkey. (softkey level 2) ACTIVE EDIT RESTRT DISPLY COPY PRGRAM PRGRAM PRGRAM PRGRAM PRGRAM VERIFY PRGRAM DELETE RENAME INPUT PRGRAM COMENT PRGRAM PRGRAM DEVICE REFORM MEMORY 4. Enter the program name to output from memory. There are two ways to do this: Type in the program name using the alphanumeric keys on the key board. The control displays program name on the input line (line 2 of the screen) next to the prompt “FILENAME”.
Chapter 9 Communications 6. Specify if you want to output one, multiple, or all programs onto tape. Output Single Program Press {SINGLE PRGRAM} to output the program selected in step 4. Output Multiple Programs Press {MULTI PRGRAM} to output more than one program. After you pressed the {MULTI PRGRAM} key, the program selected in step 4 is output. The Program Directory Screen (see Figure 9.
Chapter 9 Communications All programs are copied to the peripheral device and stored using the same program name as the original, in the order that they appear on the Program Directory Screen. (softkey level 3) SINGLE MULTI OUTPUT PRGRAM PRGRAM ALL Figure 9.
Chapter 9 Communications 9.4 Verifying Part Programs Against Source Programs To verify that a part program stored in memory matches a source program stored in memory or on a peripheral device: 1. If one of the programs to either verify or verify against is on a peripheral device, make sure that the peripheral device is connected to the correct serial port and that the port is configured for that device (refer to page 9-1). 2. Press the {PRGRAM MANAGE} softkey. (softkey level 1) 3.
Chapter 9 Communications 5. To verify a part program in memory against a part program stored on a peripheral device, press the {VERIFY PORT A} or {VERIFY PORT B} softkey depending on where the peripheral device is connected. To verify a part program in memory against another part program in memory, press the {VERIFY MEMORY} softkey. (softkey level 3) VERIFY VERIFY VERIFY PROT A PORT B MEMORY 6. Press the {VERIFY YES} softkey. To abort the verify operation press the {VERIFY NO} softkey.
Chapter 10 Introduction to Programming 10.0 Chapter Overview The 9/Series control performs machining operations by executing a series of commands that make up a part program. These commands are interpreted by the control which then directs axis motion, spindle rotation, tool selection, and other CNC functions. Part programs can be executed from the control’s memory or from a CNC tape. This chapter begins with an explanation of CNC tape format.
Chapter 10 Introduction to Programming Tape with Program End = M02, M30, M99 This particular tape format allows single- or multi-program format on a tape. It also lets you enter either M02, M30, or M99 as a program end code. See chapter 10 for details on legal program end codes. Figure 10.1 shows a typical configuration for a multiple program tape with M30 and M99 as program end codes.
Chapter 10 Introduction to Programming Tape with Program End = % (ASCII), ER (EIA) Unlike the previous tape type mentioned, this type of tape accepts only the “%” (ER) field as the program end code. See Figure 10.2. See chapter 10 for details on legal program end codes and the effect of STOP PRG END. Figure 10.
Chapter 10 Introduction to Programming (2) Leader Section The information between the tape start and the program start is called the tape leader section. The leader section is a tape indexing section. On punched tape, the holes punched in the leader section can be configured to show alphanumeric characters. The control ignores information within the leader section and does not perform a parity check on this information. Important: A program start code must not appear within the leader section.
Chapter 10 Introduction to Programming This section should include a program name, program blocks, comments, and end-of-program. Each block in the part program is separated by an EOB code. The control displays a semicolon “;” to indicate the presence of an EOB code. Important: When performing an EOB search, the search is executed from the beginning of the part program, NOT from the point of display.
Chapter 10 Introduction to Programming (8) Tape End (Rewind, Stop Code) The tape end code, indicating the end of a tape, is designated with either: 10.2 Program Configuration Code: Description: % ASCII format ER EIA format Each individual machining operation performed by the control is determined by the control’s interpretation of a group of words or codes (commands) called a “block.” Individual blocks in a part program define each machining process.
Chapter 10 Introduction to Programming A block is a set of words and characters that defines the operations of the control. For example: / N3 G00 X10. Z10. M3 ; end of block character miscellaneous function word (spindle on forward) axis movement words preparatory function word (rapid positioning mode) sequence number word optional block delete character The 9/Series control sequentially executes blocks in a part program to conduct the required machining operation.
Chapter 10 Introduction to Programming 10.2.1 Program Names You can enter up to 8 alphanumeric characters for program names. Subprograms are designated with the letter O followed by 5 numbers. If you enter a new program name with 5 numeric characters, the control assumes that it is a subprogram and automatically inserts the letter O as the first character in the name. The control does not consider programs with more than 5 numeric characters as subprograms.
Chapter 10 Introduction to Programming 10.2.2 Sequence Numbers Each block in a part program can be assigned a sequence number to distinguish one block from another. Sequence numbers begin with an N address, followed by a one to five digit numeric value. Sequence numbers can be assigned at random to specific blocks or to all blocks. If you assign sequence numbers to locks, you can designate their sequence numbers.
Chapter 10 Introduction to Programming 10.2.4 Block Delete and Multi Level Delete When you program a slash “/” followed by a numeric value (1-9) anywhere in a block, the control skips (does not execute) all remaining programmed commands. The block delete feature is turned on with the {FRONT PANEL} softkey or with an optionally installed switch on the MTB panel. If the {FRONT PANEL} softkey is used, only block delete /1 is available.
Chapter 10 Introduction to Programming 10.2.5 End of Block Statement All program blocks must have an end of block statement as the last character in the block. This character tells the control how to separate data into blocks. The control uses the “;” to mark the end of a block. Important: When performing an EOB search, the search is executed from the beginning of the part program, NOT from the point of display.
Chapter 10 Introduction to Programming 10.3.1 Subprogram Call (M98) Generally, programs are executed sequentially. When you enter an M98Pnnnnn command (“nnnnn” representing a subprogram number) in a program, the control merges the subprogram (designated by the address P) before the block that immediately follows the M98 command. The control issues the error message “CANNOT OPEN SUBPROGRAM”, if it cannot find the subprogram designated by the M98 command.
Chapter 10 Introduction to Programming 10.3.
Chapter 10 Introduction to Programming Example 10.7 Subprogram Calls and Returns MAIN PROGRAM SUBPROGRAM 1 SUBPROGRAM 2 (MAIN PROGRAM); (SUBPROGRAM 1); (SUBPROGRAM 2); N00010...; N00110; N00210; N00020...; N00120...; N00220...M99; N00030M98P1; N00130M99; N00040...; N00140...; N00050...; N00150M30; N00060M98P2L2; N00070M30; This path of execution results when you select the main program in Example 10.7 as the active program: (MAIN PROGRAM); N00010...; N00020...
Chapter 10 Introduction to Programming 10.3.3 Subprogram Nesting We use the term nesting to describe one program calling another. The program called is a nested program. When a subprogram is called from the main program it is on the first nesting level or nesting level 1. If that subprogram in turn calls another subprogram, the called subprogram is in nesting level 2. Subprograms can be nested up to a maximum of 4 levels. Figure 10.
Chapter 10 Introduction to Programming 10.4 Word Formats and Functions Words in a part program consist of addresses and numeric values. Component: Description: Address A character to designate the assigned word function. Numeric value A numeral to express the event called out by the word. Figure 10.4 Word Configuration Word G 0 Address Word 1 X 1 .
Chapter 10 Introduction to Programming Table 10.A shows the effects of leading zero suppression (LZS) and trailing zero suppression (TZS). It presumes that your system installer has set a format of X5.2 (integer 5 digits, decimal 2 digits) in AMP. Different formats would result in different decimal point placement compared to those shown below, but the end result would be comparable. Table 10.
Chapter 10 Introduction to Programming Important: If backing up a table using a G10 program (such as the offset tables or coordinate system tables), keep in mind the G10 program output is generated in the current format of the control (LZS or TZS). If you intend to transport this table to a different machine it must also be using the same format. 10.4.
Chapter 10 Introduction to Programming Table 10.B Word Formats and Descriptions Address Valid Range inch Valid Range metric Function A 8.6 3.3 8.5 3.3 Rotary axis about X (AMP assigned) Angle in QuickPath Plus programming B 3.0 3.0 Second miscellaneous function (AMP assigned) C 8.6 8.6 8.5 8.5 Rotary axis about Z (AMP assigned) Chamfer length in QuickPath Plus programming D 8.6 8.5 Fixed cycle parameter E 2.6 3.7 Thread lead F 8.6 8.5 Feedrate function (F-word) G 2.1 2.
Chapter 10 Introduction to Programming 10.4.4 Minimum and Maximum Axis Motion (Programming Resolution) The maximum programmable value accepted by the control is 99,999,999. The minimum is .000001 inch or .00001mm. The actual range of programmable values depends on specifications determined by your system installer. By using AMP to establish the format of numeric values for words, your system installer sets the “programming resolution” for axis motion, the smallest programmable distance of axis motion.
Chapter 10 Introduction to Programming 10.5.2 A_L_,R_,C_ (QuickPath Plus Words) To simplify programming an angle, corner radius, or chamfer between two lines, all that is necessary is the angle between the lines and the radius or chamfer size connecting them. This method of programming can be used to simplify the cutting of many complex parts. QuickPath words are made up of the addresses below followed by the desired numeric value.
Chapter 10 Introduction to Programming Feedrates are expressed by the distance of movement per interval. Depending on the mode of the control and the results you want, the distance can be millimeters, inches, meters, or revolutions. The interval can be minutes or revolutions. Table 10.
Chapter 10 Introduction to Programming Important: G-codes can also be expressed in terms of a parametric expression (for example G[#12+6]). For details, see chapter 28. Example 10.8 explains execution of modal G-codes, using G00 and G01, both classified into the same G-code group. Example 10.8 Programming Modal G-codes G00 X1. Z2.; G00 mode is effective Z3. ; G00 mode is effective G01 X2. Z1. ; G01 mode is made effective X3. Z3. ; G01 mode is in effect G00 X1.Z2.
Chapter 10 Introduction to Programming Table 10.E G-code Table A B C G00 Modal 01 Rapid Positioning G01 Linear Interpolation G02 Circular Interpolation (Clockwise) G03 00 Dwell 18 Send Command and Wait for Return Status (used with 9/Series Data Highway Plus Communication Module) Send Command without Waiting for Return Status (used with 9/Series Data Highway Plus Communication Module) Programming Using Radius Values G05 G05.1-G05.
Chapter 10 Introduction to Programming Table 10.E (continued) G-code Table A B C G27 Modal 00 Function Machine Home Return Check G28 Automatic Return to Machine Home G29 Automatic Return from Machine Home G30 Return to Secondary home G31 External Skip Function 1 G31.1 External Skip Function 1 G31.2 G31.3 External Skip Function 2 External Skip Function 3 G31.
Chapter 10 Introduction to Programming Table 10.E (continued) G-code Table A B C Modal G59.2 Type Preset Work Coordinate System 8 G59.3 Preset Work Coordinate System 9 G61 13 Exact Stop Mode G62 Automatic Corner Override G63 Tapping Mode G64 Cutting Mode Modal G65 00 Paramacro Call Non-Modal G66 14 Paramacro call Modal G66.1 Paramacro call G67 Paramacro call cancel G20 G20 G70 G21 G21 G71 G70 G70 G72 G71 G71 G73 O.D. and I.D.
Chapter 10 Introduction to Programming Table 10.E (continued) G-code Table A B C G99 G95 G95 G96 Modal Function Type Feed per revolution mode 17 CSS ON G97 Modal RPM Spindle Speed Mode -- G98 G98 -- G99 G99 10 Initial level return drilling cycles Modal R-point level return drilling cycles A set of default G-codes becomes effective at power up, when the control is reset,or an emergency stop condition is reset. These default G-codes are selected by your system installer in AMP.
Chapter 10 Introduction to Programming execute after the axis motion is completed This order of execution can also be altered by using the paramacro feature, system parameter #3003. See chapter 28. Your system installer determines in AMP if M- and G-codes get reset every time the control executes an M02 or M30 end of program command. If the control does reset M- and G-codes, modal M- and G-codes default back to their power up condition, and non-modal M- and G-codes are reset to their default values.
Chapter 10 Introduction to Programming Table 10.F M-codes M-code Number Modal or Non-modal Group Number Function M00 NM 4 Program stop M01 NM 4 Optional program stop M02 NM 4 Program end M30 NM 4 Program end and reset (tape rewind) M03 M 7 Spindle positive rotation (cw) M04 M 7 Spindle negative rotation (ccw) M05 M 7 Spindle stop M19 M 7 Spindle orient PRIMARY SPINDLE SPINDLE 2 M03.2 M 11 Spindle positive rotation (cw) M04.
Chapter 10 Introduction to Programming (1) Program Stop (M00) When you execute M00, execution stops after the block containing the M00 is executed. At this time, the CRT displays the “PROG STOP” message. To restart the operation, press the button. (2) Optional Program Stop (M01) The optional program stop function has the same effect as the program stop function, except that it is controlled by an external switch.
Chapter 10 Introduction to Programming (5) Overrides Enabled (M48) When your execute M48, the feedrate override, rapid feedrate override, and the spindle speed override functions become effective. These are enabled on power up without requiring this M code to be executed. An M48 cancels an M49 and your system installer can choose which is active upon power-up. (6) Overrides Disabled (M49) Use the override cancel M--code (M49) to ignore any override set by the operator on the MTB panel.
Chapter 10 Introduction to Programming (10) End of Subprogram or Main Program Auto Start (M99) M99 End of Subprogram or Paramacro program When you execute M99, subprogram execution is completed and program execution returns to the calling program. This word is not valid in an MDI command, but it can be contained in a subprogram called by an MDI command. For details on programming an M99, see page 10-11 or chapter 28.
Chapter 10 Introduction to Programming (12) Synchronization with Setup (M150-M199) M150 - M199 — Synchronization with Setup (dual-process system only) This set of M-codes cancels any information already in block look ahead and re-setup the blocks before process execution is resumed. This re-setup is only essential when shared information is being changed from one process to another, as in the case of the dual processing paramacro parameters. See page 30-7.
Chapter 10 Introduction to Programming 10.5.9 O-Words (Program Names) The O-word is used to define a program name. To use an O word as a program name it must be the first block entered in a program. This block can be used to identify a program when reading from a tape (when program name is selected as “automatic” from the device setup menu). This is useful when many programs are placed together on a single tape. An O-word can have up to 5 numeric characters following it. 10.5.
Chapter 10 Introduction to Programming Important: Your system installer sets a maximum speed in AMP for each gear range for each spindle configured in AMP. If an S-word is programmed requesting a spindle speed that exceeds this limit. The spindle speed holds at the AMP-defined maximum. A new value may be set for this maximum RPM by programming a G92 code followed by an S-word. See chapter 17.
Chapter 10 Introduction to Programming 10.5.12 T-Words (Tool Selection and Tool Length Offset) Modern machining processes usually require a machine that is capable of selecting different tools. Typically tools are mounted in a turret and assigned tool numbers as illustrated in Figure 10.6. Figure 10.
Chapter 10 Introduction to Programming Table 10.G T-word Formats Format Type Wear Offset # Geometry Offset # (1) 1 DGT GEOM + WEAR last digit same as wear (2) 2 DGT GEOM + WEAR last two digits same as wear # (3) 3 DGT GEOM + WEAR last three digits same as wear # (4) 1 DGT WEAR last digit same as tool # (5) 2 DGT WEAR last two digits same as tool # (6) 3 DGT WEAR last three digits same as tool # For details on programming a T-word discussing tool length offsets, see chapter 20.
Chapter 10 Introduction to Programming 10-38
Chapter 11 Coordinate System Offsets 11.0 Chapter Overview This chapter covers the control of the coordinate systems on the 9/Series control. G-words in this chapter are among the first programmed because they define the coordinate systems of the machine in which axis motion is programmed. This chapter describes: On page: Information about: Machine coordinate system 11-1 Preset Work coordinate systems G54-59.
Chapter 11 Coordinate System Offsets Once you establish, the machine coordinate system is not affected by a control reset operation or any other programming or operator operation. Figure 11.1 Machine Coordinate System, Home Coordinate Assignment +X 10 Mechanically fixed Machine Home point Chuck 15 +Z Machine Coordinate System zero point In Figure 11.1, your system installer defined the machine coordinate system zero point by assigning the machine home point to have the coordinates X=10 and Z=15.
Chapter 11 Coordinate System Offsets 11.1.1 Motion in the Machine Coordinate System (G53) Although axis motion is usually commanded in the work coordinate system, axis motion is possible when a G53 is programmed in a block if you reference coordinate values in the machine coordinate system. G90G53X___Z___; The X- and Z-words above specify coordinate positions in the machine coordinate system. These coordinate values indicate the end point of the next move in the machine coordinate system.
Chapter 11 Coordinate System Offsets Figure 11.2 Results of Example 12.1 X X Axis motion in machine coordinate system 30 Axis motion in work coordinate system N1 50 20 N3 40 30 20 Work coordinate system N2 30 Z 50 10 Machine coordinate system 10 11.2 Preset Work Coordinate Systems (G54-59.
Chapter 11 Coordinate System Offsets Figure 11.3 Work Coordinate System Tool position at machine coordinate zero point Zero point on the work coordinate system Zero point on the part drawing Chuck Workpiece Workpiece Z Distance to be designated X Distance to be designated There are 7 preset work coordinate systems selected using G54 - G59.3. The required work coordinate system can be selected by specifying any of these G-codes in the program. Work coordinate systems called out by G54 - G59.
Chapter 11 Coordinate System Offsets Figure 11.4 Work Coordinate System Definition X X G54 Work coordinate system 2 Z -3 Z 3 -2 Machine coordinate system Machine home In Figure 11.4, the machine coordinate system was defined by declaring the fixed position machine home as the point X=-3., Z=-2. Then the G54 work coordinate system zero point was defined by the coordinates X=2, Z=3 in the machine coordinate system.
Chapter 11 Coordinate System Offsets To change work coordinate systems, specify the G-code corresponding to the work coordinate system you want in a program block. Any axis motion commands in a block that contains a change from one work coordinate system to another is executed in the work coordinate system specified in that block. Example 11.2 Changing Work Coordinate Systems Comment Program Block G54; G00X20.Z20.; axis motion in the G54 work coordinate system. G55X10.Z10.
Chapter 11 Coordinate System Offsets The third method, and the one described in this section, alters the work coordinate system table through G10 programming. Changing the values in the table using any of these methods does not cause axis motion. It does immediately shift the active coordinate system by the amount entered. The format for altering the work coordinate systems using G10 is: G10 L2 P__ O__ X__ Z__; Important: The order of the words in this program block is important.
Chapter 11 Coordinate System Offsets Example 11.3 Work Coordinate System Shift Using G10 Program block Work coordinate Position Absolute coord. Position G54G01X25.Z25.; G91; G10L2P1O2X10.Z10.; X25 Z25 X50 Z45 X15 Z15 X50 Z45 X25 Z25 X50 Z45 X15 Z15 X50 Z45 or G54G01X25.Z25.; G90; G10L2P1O2X35.Z30.; Important: This modification is permanent. The new table values for the work coordinate systems are saved even when control power is turned off. Figure 11.7 Results of Example 12.
Chapter 11 Coordinate System Offsets 11.3 Work Coordinate System External Offset The external offset allows all work coordinate system zero points to be shifted simultaneously, relative to the machine coordinate system. This offset can compensate for part positioning shifts that result when a different chuck is installed. It can also compensate for tool position shifts that result from a different tool turret.
Chapter 11 Coordinate System Offsets 11.3.1 Altering External Offset (G10L2) There are 3 methods to change the value of an external offset in the work coordinate system table. Two methods can be found in the following sections: Method: Chapter: manually alter the external offset value in the work coordinate system table 3 alter the paramacro system parameter values 5201- 5206 28 The third method, and the one described in this section, alters the external system table through G10 programming.
Chapter 11 Coordinate System Offsets Example 11.4 Changing the External Offset Through G10 Programming Program Block Comments G10L2P1O1X-15.Z-10.; defines work coordinate system zero point to be at X-15, Z-10 from the machine coordinate system zero point G90; G10L2P0O1X-15.Z-20.; sets external offset of X-15, Z-20 moving work coordinate system zero point to be at X-30, Z-30 from the machine coordinate system zero point G90; G10L2P0O1X-30.Z-30.
Chapter 11 Coordinate System Offsets 11.4 Offsetting the Work Coordinate Systems This section describes the more temporary ways of offsetting the work coordinate systems. These offsets are activated through programming, and they are canceled when you remove power to the control. They may also be cancelled by an M02, M30, or control reset, depending upon the selections made in AMP by your system installer. Important: All of these offsets are global in nature.
Chapter 11 Coordinate System Offsets For example specifying values of zero for all axes in a G92 block causes the current tool position to become the zero point of the current work coordinate system. Execution of a G92 block does not produce any axis motion. Important: Any axis not specified in the G92 block is not offset, and the current coordinate position for that axis remains unchanged.
Chapter 11 Coordinate System Offsets Figure 11.10 Results of Example 12.5 X X Tool position 10 30 Z 20 10 New zero point established by the G92 block Z 20 30 Zero point for the G54 work coordinate system Machine coordinate system zero point CAUTION: G92 offsets are global. Changing from one coordinate system to another does not cancel the offset. Do not specify a change in coordinate systems (G54-G59.3) unless the effects of the offset have been considered. Example 11.
Chapter 11 Coordinate System Offsets Example 11.6 Changing Work Coordinate Systems With Offset Active Program Comment N1 G10L2P1X0Z0; Define G54 work coordinate system zero point to be positioned X0, Z0 away from the machine coordinate system N2 G10L2P2X20.Z25.; Define G55 work coordinate system zero point to be positioned X20, Z25 away from the machine coordinate system N3 G55X10.Z5.; Move to X10, Z5 in the G55 work coordinate system N4 G54X10.Z5.
Chapter 11 Coordinate System Offsets 11.4.2 Offsetting Coordinate Zero Points (G52) To offset a work coordinate system an incremental amount from its zero point, program a G52 block that includes the axis names and distances to be offset. G52 X___ Z___ ; This command offsets the current work coordinate system by the axis values that follow the G52 command. Example 11.7 Work Coordinate System Offset by G52 Program Block Machine Coordinate Position Work Coordinate Position G01X25.Z25.
Chapter 11 Coordinate System Offsets A G52 offset can also be canceled by executing a G92 or G92.1, performing a control reset or an E-STOP reset operation, or executing an end of program M30 or M02. A G92 command only cancels a G52 offset if one is active when the G92 block is executed. A G52 offset can be activated at some time after the G92 block is executed even if a G92 offset is still in effect. CAUTION: G52 offsets are global.
Chapter 11 Coordinate System Offsets Example 11.8 Typical Set Zero Offset Application Operation -Manual jog- Comment axes are manually jogged to a location where the operator has determined that a special operation must be performed.
Chapter 11 Coordinate System Offsets To use this feature, follow these steps: 1. Press or on the MTB panel to interrupt automatic or MDI operation. 2. Turn on the switch to activate the jog offset feature (refer to documentation provided by your system installer). 3. Change to manual mode, unless the control is equipped for the “Jog-on-the-Fly” feature which allows jogging in automatic or MDI modes (refer to documentation prepared by your system installer). 4.
Chapter 11 Coordinate System Offsets Example 11.9 demonstrates the G92.1 offset cancel. Example 11.9 G52 Offset Cancelled By a G92.1 Program Blocks Comment N1 G01Y25.X25.; move to Y25, X25 N2 G52Y10.X10.; work coordinate system is offset by Y10, X10 N3 Y25.X25.; move to Y25, X25 in the offset coordinate system N4 G92.1; G52 offset is cancelled, program position displays axis position at X35Y35. Figure 11.13 Results of Example 12.
Chapter 11 Coordinate System Offsets The G92.2 block must be programmed with no axis words. Axis words in a G92.2 block generate an error. When you execute the G92.2 block, all G92, {SET ZERO}, and Jog offsets are canceled on all axes. You cannot cancel the offsets on only one or more of the axes. No axis motion takes place during execution of a G92.2 block. Axes remain at their last programmed position while the work coordinate system adjusts to remove these offsets. 11.
Chapter 12 Overtravels and Programmable Zones 12.0 Chapter Overview Overtravels and programmable zones define areas that restrict the movable range of the cutting tool. The 9/Series control is equipped to establish two overtravel areas and two programmable zones as illustrated in Figure 12.1. On page: Topic: Hardware overtravels 12-2 Software overtravels 12-3 Programmable zone 2 12-5 Programmable zone 3 12-7 Figure 12.
Chapter 12 Overtravels and Programmable Zones There are two types of overtravels: Hardware overtravels ---- Established by your system installer by mounting mechanical limit switches on the movable range of the axes Software overtravels ---- Established in AMP by your system installer designating coordinate values in the machine coordinate system There are two types of Programmable Zones. Zone: Description: Programmable Zone 2 Established by the operator, or person in charge of job setup.
Chapter 12 Overtravels and Programmable Zones 12.2 Software Overtravels The coordinate values of the points defining the software overtravels are set in AMP by your system installer. This overtravel can only be disabled by your system installer in AMP. If your system installer has enabled the software overtravels, the control is not allowed to exit the area defined by the software overtravels. Figure 12.
Chapter 12 Overtravels and Programmable Zones Figure 12.
Chapter 12 Overtravels and Programmable Zones 12.3 Programmable Zone 2 Programmable zone 2 defines an area which the tool cannot enter. Generally, zones are used to protect some vital area of the machine or part located within the software overtravels. Important: Programmable zones are defined using coordinates in the machine coordinate system. They are not affected by any changes in the work coordinate system, including external offsets.
Chapter 12 Overtravels and Programmable Zones Programming this G-code: turns Zone 2: turns Zone 3: G22 On On G22.1 Off On G23 Off Off G23.1 No Change* Off * A G23.1 turns on programmable zone 2 if it is the default power up condition configured in AMP (also activated at a control reset). G23.1 does not turn on programmable zone 2 when it is activated in a part program. G23 is normally automatically made active at power up, though this is ultimately determined by the system installer in AMP.
Chapter 12 Overtravels and Programmable Zones Figure 12.5 Programmable Zone 2 Software overtravel Programmable Zone 2 Tool tip can not enter zone 2 For details on how the control reacts to entry into a prohibited area, see page 12-13. 12.4 Programmable Zone 3 Programmable zone 3 can define an area which the tool cannot enter or an area the tool cannot exit. The current tool location determines when programmable zone 3 is made active.
Chapter 12 Overtravels and Programmable Zones Values for programmable zone 3 are entered either in the programmable zone table (described on page NO TAG) or through a G22 program block. A maximum and a minimum coordinate value (in the machine coordinate system) are assigned for each axis. The resulting coordinates define the boundaries for programmable zone 3. Figure 12.
Chapter 12 Overtravels and Programmable Zones Figure 12.7 Programmable Zone 3 This area becomes Programmable Zone 3 if the zone is enabled when tool is inside of this area Programmable Zone 3 if enabled when tool is outside of this area Programmable zone 3 becomes active when either the G22 or G22.1 code is executed. It is made inactive when the G23 or G23.1 code is executed. Program G-code: To turn on these zones: these zones: To turn off G22 2 and 3 not applicable G22.
Chapter 12 Overtravels and Programmable Zones If you program other commands other than a G-code in the same modal group in a G22, G22.1, G23, or G23.1 block, this error message appears: “UNNECESSARY WORDS IN ZONE BLOCK” Programming zone 3 values (3 or less axes) You can reassign values for the parameters that establish programmable zone 3 by programming axis words in a G22 program block. Two methods are available.
Chapter 12 Overtravels and Programmable Zones If a value for a maximum axis parameter is less than the value set for an axis current minimum parameter, or if a value for a minimum axis parameter is set greater than the value set for an axis current maximum value, the control displays the message: “INVALID VALUE (MAX < MIN) FOR ZONE 3 AXIS (X)” This message displays the name of the axis that has been set incorrectly. It does not indicate if it is the minimum or maximum value that is incorrect.
Chapter 12 Overtravels and Programmable Zones Using this method, the same integrand word assigned in AMP to more than one axis correspond only to the absolute axis words programmed in the G22 block. Integrand words cannot be programmed alone (without a absolute axis word in the G22 block). The following example assumes a machine with axes configured as shown above.
Chapter 12 Overtravels and Programmable Zones 12.5 Resetting Overtravels Tool motion stops during overtravel conditions that occur from 3 causes: Cause: Description: Hardware overtravel the axes reach a travel limit, usually set by a limit switch or sensor mounted on the axis. Hardware overtravels are always active. Software overtravel commands cause the axis to pass a software travel limit.
Chapter 12 Overtravels and Programmable Zones 12-14
Chapter 13 Coordinate Control 13.0 Chapter Overview This chapter describes 9/Series coordinate control. For information about: 13.1 Plane Selection (G17, G18, G19) See page: Plane selection G17, G18,G19 13-1 Absolute/Incremental modes G90, G91 13-2 Inch/Metric modes G70, G71 13-4 Radius/Diameter modes G07, G08 13-5 Scaling G14, G14.1 13-7 The 9/Series control has a number of features that operate in specific planes.
Chapter 13 Coordinate Control Example 13.1 Altering Planes for Parallel Axes Assuming the system installer has made the following assignments in AMP: G18 -- the ZX plane.
Chapter 13 Coordinate Control In the above block, the control moves the cutting tool away from the current axis position, a distance of 40 units on the X axis and 20 units on the Z axis. G91 is a modal G-code and remains active until cancelled by a G90. Example 13.2 Absolute vs Incremental Commands Incremental Command Absolute Command G90X20.Z10.; G91X10.Z-25.; Figure 13.
Chapter 13 Coordinate Control To program incremental moves using G-code system A, call out axis positions using U, W, and V. Incremental command, G code system A U20.W-25.; The above commands are not modal. Incremental and absolute commands can be programmed at any time, even in the same block. Table 13.A shows the typical command addresses for absolute and incremental programming in G-code system A. See the documentation provided by your system installer for axis names in your system. Table 13.
Chapter 13 Coordinate Control 13.4 Radius/Diameter Modes (G07, G08) Usually, workpieces on CNC lathes are cylindrical. The control allows workpiece dimensions programming as either radius or diameter values. G08 places the control in diameter programming mode. This mode remains active until cancelled by a G07. G07 places the control in radius programming mode. This mode remains active until cancelled by a G08.
Chapter 13 Coordinate Control Figure 13.2 Diameter/Radius Programming X 15 Diameter Programming Mode (G08) Radius Programming Mode (G07) G90G08X12.; G90G07X6 or or G91G08X-8.; G91G07X-4.; 10 5 10 6 20 12 Z Important: The following must always be programmed as radius value, regardless of whether G07 or G08 is active: Most of the X axis infeed amounts or similar values (addresses D, I, K) used in Simple and Compound fixed cycles (G70 - G78).
Chapter 13 Coordinate Control 13.5 Scaling Use the scaling feature to reduce or enlarge a programmed shape. Enable this feature by programming a G14.1 block as shown below: G14.1 X__ Z__ P__; Where : Is : X and Z the axis or axes to be scaled and the center of scaling for those axes. P the scaling magnification factor for the specified axes. The axes programmed in the G14.1 block determine which axes are scaled. The corresponding axis word values specify the center of scaling for each axis.
Chapter 13 Coordinate Control Figure 13.3 Results of Example 13.4 Original part contour X Contour after scaling X axis only by .5 in G90 absolute mode 30 20 10 6 20 40 Z 60 When incremental mode (G91) is active, the control ignores the programmed centers of scaling. The control performs scaling on the axes programmed in the G14.1 block, but the scaling moves are referenced from their current axis positions, not the programmed center of scaling or the active coordinate zero point.
Chapter 13 Coordinate Control Figure 13.4 Results of Example 13.5 Original part contour Contour after scaling X axis only by .5 in G91 incremental mode X 30 -9 20 10 Z 20 40 60 G14 disables scaling on all axes. When you disable scaling, the center of scaling and any scaling magnification factors are cleared. The next time you enable scaling, these values must be reset. In addition to G14, M99 in the main program, M02, M30, and a control reset operation disables scaling.
Chapter 13 Coordinate Control 13.5.1 Scaling and Axis Position Display Screens When you enable scaling for a particular axis, the letter “P” is displayed next to the axis name on all axis position display screens. Figure 13.5 shows scaling enabled on all axes. Figure 13.5 Axis Position Display Screen Showing Scaling Enabled E-STOP PROGRAM[ MM ] F PR X 1234.567 S P Z 9876.000 T 0.000 MMPM 00 0 (ACTIVE PROGRAM NAME) MEMORY MAN STOP PRGRAM OFFSET MACRO MANAGE PARAM 13.5.
Chapter 13 Coordinate Control To access the scaling magnification data screen, follow these steps: 1. Press the {OFFSET} softkey on the main menu screen. (softkey level 1) 2. PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD Press the {SCALNG} softkey to display the scaling magnification data screen. See Figure 13.6. (softkey level 2) WORK TOOL CO-ORD WEAR TOOL TOOL RANDOM GEOMET MANAGE TOOL COORD SCALNG BACKUP ROTATE OFFSET Figure 13.
Chapter 13 Coordinate Control Important: If an axis is configured as a rotary axis, the scaling magnification display screen displays dashes instead of numbers for that axis. Rotary axes cannot be scaled. The left column lists the current center of scaling for each axis. When scaling is cancelled, the current center of scaling for each axis is set to zero. The format of this value is determined by the word format of the selected axis.
Chapter 13 Coordinate Control When changing work coordinates (G54-G59.3), the center of scaling is transferred from the old work coordinate system to the new work coordinate system. The offset distance from the tool position in the old work coordinate system to the tool position in the new work coordinate system is not scaled. Scaling is applied to G52 and G92 offsets. The center of scaling shifts when the work coordinate systems are shifted by a G92 offset or by changing coordinate offset values.
Chapter 13 Coordinate Control G37, G37.1 - G37.4 Gxx Z__ Z (scaled) G73, G74, G76, G82, G83, G84 G85, G86, G87, G88, G89 Gxx X__ Y__ Z__R__I__Q__K__P__F__L__ X Y Z R I Q K P F L (scaled) (scaled) (scaled) (scaled) (not scaled) (not scaled) (not scaled) (not scaled) (not scaled) (not scaled) Important: R uses the scale factor associated with the axis that is perpendicular to the active plane.
Chapter 13 Coordinate Control G78 G78 X__Z__K__D__F__E__A__P__I__ X (scaled) Z (scaled) K (not scaled) D (not scaled) F (not scaled) E (not scaled) A (not scaled) P (not scaled) I (scaled) G33 G33 Z_F_E_Q G33 X_Z_F_E_Q G33 X_F_E_Q X Z E F Q (scaled) (scaled) (not scaled) (not scaled) (not scaled) G34 G34 Z_F_E_Q K G34 X_Z_F_E_Q K G34 X_F_E_Q K X Z E F Q K (scaled) (scaled) (not scaled) (not scaled) (not scaled) (scaled) G20 G20 X_Z_I_ X (scaled) Z (scaled) I (scaled) 13-15
Chapter 13 Coordinate Control CAUTION: This cycle cuts more metal when scaling is enabled. G21 G21 X_Z_F_E_ X Z F E (scaled) (scaled) (not scaled) (not scaled) G24 G24 X_Z_K_ X (scaled) Z (scaled) K (scaled) CAUTION: This cycle cuts more metal when scaling is enabled. G81 G81 X_Z_R F_L_ X Z R F L (scaled) (scaled) (scaled) (not scaled) (not scaled) Important: R uses the scale factor associated with the axis that is perpendicular to the active plane.
Chapter 14 Axis Motion 14.0 Chapter Overview This chapter covers the group of G-words that generates axis motion or dwell data blocks. Major topics include: Information about: 14.
Chapter 14 Axis Motion Your system installer determines the feedrate for the rapid positioning mode in AMP, individually for each axis. The feedrate of a positioning move that drives more than one axis is limited by the rapid rate set for the slower axis. The slower axis is driven at its rapid rate, while the feedrate for other axes is reduced to maintain a linear move. This also assures that all axes start and stop at the same time.
Chapter 14 Axis Motion 14.1.2 Linear Interpolation Mode (G01) The format for linear interpolation mode is: G01X ____ Z ____ F ____ ; Where : Is : G01 G01 establishes the linear interpolation mode. In linear interpolation mode, the cutting tool is fed along a straight line at the currently programmed feedrate. XZ This is the location of the end point of the linear move in the current work coordinate system.
Chapter 14 Axis Motion Once the feedrate, F, is programmed it remains effective until another feedrate is programmed (F is modal). You can override programmed F-words. For details, see chapter 18. Example 14.3 Modal Feedrates Program Block Comment G91G01X10.Z20.F.1; F.1 is effective until Z35.; another feedrate is X40.Z35.; programmed Z44.F.3; F.3 is effective The feedrate for a multi-axis move is specified as the vectorial feedrate.
Chapter 14 Axis Motion You must establish a plane before the control performs the correct arc. This should have been done by your system installer, typically assigning the Z and X axes to the G18 plane. This becomes the default plane that the control assumes when: power is turned on E-Stop is reset the control is reset Circular interpolation can be performed in the absolute (G90) or incremental (G91) mode. Important: S--Curve Acc/Dec mode is not available with circular interpolation mode.
Chapter 14 Axis Motion Example 14.4 Circular Interpolation G18 (ZX Plane) Absolute Mode Incremental Mode G08G02; X30.Z-15.I15.K0F.1; G08G02; X50.Z45.I15.K0F.1; or or G08G02; X50.Z45.R15.F.1; G08G02; X30.Z-15.R15.F.1; In Example 14.4, the K-word can be omitted. If either I or K is omitted from the circular block, the control assumes they have a value of 0, unless an R-word is present. Figure 14.4 Results of Circular Interpolation, Example 14.
Chapter 14 Axis Motion Example 14.5 Arc Programmed Using Radius Arc 1 Arc 2 center angle less than center angle greater than 180 degrees 180 degrees G90G02X25.Z40.R18.F.1; G90G02X25.Z40.R-18.F.1; Figure 14.5 Results of An Arc Programmed with Radius Command, Example 14.5 X Arc 2 R-18 start point 25 Arc 1 R18 end point Z 40 Important: Any axis that is not specified when programming a circle remains at its current axis position value.
Chapter 14 Axis Motion Example 14.6 Arc End Points Same As Start Points Arc 1-Full Circle Arc 2-No Motion G02I-5.K5.F.1; G02R7.07F.1; or or G02X15.Z5.I-5.K5.F.1; G02X15.Z5.R7.07F.1; Figure 14.6 Results of An Arc with End Point Equal To Start Point, Example 14.
Chapter 14 Axis Motion 14.1.4 Positioning Rotary Axes This section describes how to program a rotary axis. A rotary axis is a non-linear axis that typically rotates about a fixed point. A rotary axis is not the same as a spindle which uses an M19 to orient to a specific angle. A spindle orient (M19) cannot move simultaneously with the other axes in the system. A rotary axis is capable of rotating when other axes are being moved.
Chapter 14 Axis Motion In incremental mode (G91), the rotary axis is programmed to move in an angular distance (not to a specified angle as in absolute). The maximum incremental departure depends on the programming format selected in AMP by your system installer. The sign of the angle determines what direction the rotary axis rotates. For example, if the current C axis position is 25°and this block is programmed: G91C50; the C axis would rotate 50°in the positive direction.
Chapter 14 Axis Motion Determining Rotary Axis Feedrates The feedrate for a rotary axis is determined in much the same way as linear axes. When the control is in rapid mode (G00), the feedrate for the rotary axis is the rapid feedrate for that axis as set in AMP. Remember that if other axes are moving in the same block, the feedrate for the block is limited by the axis that takes the longest time to complete its programmed move at its rapid speed. (see chapter 18 for details).
Chapter 14 Axis Motion 14.2 Automatic Motion To and From Machine Home 14.2.1 Automatic Machine Homing (G28) Machine tools have a fixed machine home position that is used to establish the coordinate systems. The 9/Series control offers two methods for homing a machine after power up. Operation: Description: Manual machine home uses switches or buttons on the MTB panel provided solely for this purpose. Manual homing is described in detail in chapter 4.
Chapter 14 Axis Motion 2. When the output command equals 0 (i.e., the axis stops), the control will determine the absolute position. Refer to your AMP manual for more information about DCM Homing for Absolute Position. If your axis is already homed, refer to the Automatic Return to Home (G28) section later in this chapter. Important: DCM axis homing must be performed manually or by programming a G28.
Chapter 14 Axis Motion Figure 14.7 Automatic Return to Machine Home (G28) Machine home Intermediate point Z Usually a G28 is followed by a G29 (automatic return from machine home) in a part program; however, the control stores the intermediate point in memory for use with any subsequent G29 block executed before power down. Only one intermediate point is stored for each axis. When a G28 is programmed with a new intermediate point, any axis not programmed in that block remains at the old value.
Chapter 14 Axis Motion 14.2.3 Automatic Return from Machine Home (G29) When a G29 is executed in a part program (or through MDI), the axis or axes move first to the intermediate point, and then to the position indicated in the G29 block. If a G28 was just executed, then this has the effect of returning the axis from machine home. For example, executing the block: G29 X7.0 Z1.5; in absolute mode would move the axes to (7.0, 1.5) after passing through the intermediate point stored in control memory.
Chapter 14 Axis Motion Figure 14.8 Automatic Return From Machine Home, Results of Example 14.7 X Machine home 200 N30 150 N40 N30 N10 N20 100 50 Z 50 100 150 200 Important: When a G29 is executed, tool offsets and/or cutter compensation are deactivated on the way to the intermediate point, and they are re-activated when the axis moves from the intermediate point back to the point indicated in the G29 block. 14.2.
Chapter 14 Axis Motion If an attempt is made to execute a G27 before the axes have been homed, the control goes to cycle stop and displays this error message: “MACHINE HOME REQUIRED OR G28” 14.2.5 Move To Alternate Home (G30) The G30 command is similar to the G28 command. The main difference is the axis or axes move to an alternate home position instead of machine home. The command format determines whether the axes return to a second, third, or fourth alternate home position.
Chapter 14 Axis Motion Important: When the control executes a G28 or G30 block, it temporarily removes any tool offsets and cutter compensation during the axis move to the intermediate point. The offsets and/or cutter compensation are automatically re-activated during the first block containing axis motion following the G28 or G30, unless that block is a G29 block.
Chapter 14 Axis Motion 14.3.2 Dwell - Number of Spindle Revolutions In the G95 mode (feed per revolution), G04 suspends execution of commands in the next block for the time it takes the controlling spindle to turn a designated number of revolutions. G95G04 P__; X__; U__; Specify the required dwell length by either a P-, X-, or U-word in units of spindle revolutions. It does not matter which of these three words you use, as long as only one appears in the same block. The allowable range is 0.
Chapter 14 Axis Motion The control only cancels the mirror feature for those axes that are programmed in the G50.1 block. Axes not programmed in the G50.1 block remain mirrored. There is no significance to the values programmed with the axis words in a G50.1 block. Axis values might not be required, depending on how the way AMP was configured by your system installer. In either case, the control ignores these values. Example 14.
Chapter 14 Axis Motion Figure 14.9 Programmable Mirror Image, Results of Example 14.8 X 120 90 75 Start point End point 60 30 0 30 60 75 90 120 Z When the mirror image function is active on only one of a pair of axes, the control: executes a reverse of programmed G02/G03 arcs. G02 becomes counterclockwise and G03 becomes clockwise activates a reverse of programmed G41/G42 cutter compensation.
Chapter 14 Axis Motion Your system installer can install a switch for each of the 4 available axes. What axes are mirrored with what switches depends on the PAL program in your system. You can mirror about more then one axis using more then one manual mirror image switch at the same time or one switch can control more than one axis. Refer to documentation prepared by your system installer for details. Important: You can use programmable mirror image at the same time as manual mirror image.
Chapter 15 Using QuickPath Plusä 15.0 Chapter Overview The QuickPath Plus feature offers a convenient programming method to simplify programming with the 9/Series control. We discuss some QuickPath Plus features in this chapter. Major topics include: On page: Topic: Programming 15-2 Linear QuickPath 15-3 Circular QuickPath 15-7 This method of programming can prove useful in simplifying the programming of a part directly from a part drawing.
Chapter 15 Using QuickPath Plus 15.1 Programming QuickPath Plus When programming QuickPath Plus, remember: Any axis words that are programmed must be in the current plane, and angles are measured from the first axis defining that plane. All examples in this section assume that the ZX plane is active (angles are measured relative to the Z axis). QPP always uses “,A” as the angle word. When you create new programs, always program the QPP angle with ,A.
Chapter 15 Using QuickPath Plus If an angle is programmed in a circular QuickPath Plus block, an error is generated. If an L-word is programmed in a G13, or G13.1 block an error is generated. 15.2 Linear QuickPath Plus One End Coordinate Many times part drawings give a programmer only one axis dimension for a tool path and require that the other axis dimension be calculated by the angle. This QuickPath Plus feature eliminates the need for this calculation. This must be a linear block. See section 15.
Chapter 15 Using QuickPath Plus Example 15.1 Angle Designation: N10 GO1 X0.0 Z25.0 F.1.; N20 X15. ,A90; N30 Z5.,A165; Figure 15.1 Results of Angle Designation, Example 15.1 X 165° 15 10 5 Z 0 5 10 15 20 25 Important: Circular QuickPath Plus can also use an angle (,A) in a program block. This is described in section 15.3. No End Coordinate Known (L) This feature of QuickPath Plus allows the programmer to define a tool path using only the start point angle and length of a tool path.
Chapter 15 Using QuickPath Plus Important: If any axis word from the current plane is designated in the block, the L-word is ignored and the control calculates the end point from the angle and the axis word. If an angle (,A) or a length (L) is programmed in a block that also contains both axis words in the current plane, then QuickPath Plus is not performed and the control ignores the ,Aand the L-words in the block. Example 15.2 Angle with Length Designation: N10 GO1 X0. Z25. F.1.
Chapter 15 Using QuickPath Plus The format for these blocks is: N1 ,A__; N2 ,A__Z__X__; Where : Is : ,A Angle This word is used to define the angle of a tool path. This manual assumes that the ,A-word is used. The angle is a positive value when measured counterclockwise from the first axis defining the currently active plane and a negative value when measured clockwise. The angle is in units of degrees.
Chapter 15 Using QuickPath Plus 15.3 Circular QuickPath Plus (G13, G13.1) The programmer uses the Circular QuickPath when a drawing does not call out the actual intersection of two consecutive tool paths and at least one of the tool paths is circular. This prevents the programmer from having to do any complex calculations to determine end points and start points when an arc is involved. For most cases of circular QuickPath Plus there may be two possible intersection points for the two defined blocks.
Chapter 15 Using QuickPath Plus Linear to Circular blocks When the coordinates of the intersection of a linear path into a circular path are unknown, use the following format. G13 or G13.1 must be programmed. These blocks must be programmed in absolute.
Chapter 15 Using QuickPath Plus Circular to Linear blocks When the coordinates of the intersection of a circular path into a linear path are unknown, use the following format. G13 or G13.1 must be programmed in the first of the two blocks. These blocks must be programmed in absolute. Format: G13G02I__K_; or G01,A__Z__X__; G13G02R__; G01,A__Z__X__; Important: K values are the normal integrand values when you use this format (measured from start point of arc to arc center). Example 15.
Chapter 15 Using QuickPath Plus Circular to Circular blocks When the coordinates of the point of intersection of a circular path into a circular path are unknown, use the following format. G13 or G13.1 must be programmed. If using this format, the R-word cannot be used to specify the radius of an arc in either of the circular blocks. These blocks must be programmed in absolute.
Chapter 16 Chamfering and Corner Radius 16.0 Chapter Overview During cornering, the 9/Series control has the option of performing either a chamfer (a linear transition between the blocks) or a corner radius (an arc transition between blocks). ,C Chamfer size This word is used to define a chamfer length that connects two intersecting tool paths. This word determines the distance that the chamfer begins and ends from the tool paths intersection.
Chapter 16 Chamfering and Corner Radius There is a limit of 4 non-motion blocks allowed between the first and second motion blocks defining the corner transition. A non-motion block is any block that does not generate axis motion in the currently active plane. The control generates an error if more than 4 non-motion blocks are programmed between the cornering plane. Use the chamfering and corner radius features are often used in conjunction with QuickPath Plus.
Chapter 16 Chamfering and Corner Radius Figure 16.1 Results of Chamfering Using ,C from Example 16.1 X 2.0 20.0 Z Example 16.2 Linear to Circular Motions with Chamfer N10X0.Z0.F.1; N20X10.Z10.,C5; N30G02X20.Z20.R10; Figure 16.2 Results of Linear to Circular Motions with Chamfer, Example 16.
Chapter 16 Chamfering and Corner Radius 16.2 Corner Radius Use the ,R command to program a radius between two intersecting tool paths. The R command must be programmed after a comma (,). Program the ,R followed by the radius size in the block where the first path is programmed. The control looks ahead to the block commanding the second path and automatically inserts the circular rounding bock to meet that path. This inserted circular block is always tangent to both programmed tool paths.
Chapter 16 Chamfering and Corner Radius Figure 16.3 Results of Radius for a Circular Path into a Linear path, Example 16.3 X 30 25 20 N20 Actual end point of block N20 and start point of corner block Corner block 15 R 10 5 N30 Actual start point of block N30 and end point of corner block Programmed end point of block N20 Z 5 10 15 20 25 Example 16.4 Radius and Chamfer with QuickPath Plus N10Z25.X0.F.1; N20G01A90,C2.; N30Z15.X20.A180,R5.; N40X40.; N50Z5.
Chapter 16 Chamfering and Corner Radius Figure 16.4 Results of Radius and Chamfer, Example 16.4 X 5.0 20.0 10.0 R 5.0 2.0 40.0 20.0 Z 16.3 Considerations with Chamfering and Corner Radius When using chamfering and corner radius, remember: If the control is executing in single block mode, the control enters the cycle stop state after executing the first block and the adjacent chamfer or corner radius.
Chapter 16 Chamfering and Corner Radius You must program ,C and ,R in blocks that contain axis motion in the current plane. If they are programmed in a block that does not contain axis motion in the currently active plane, the control generates an error.
Chapter 16 Chamfering and Corner Radius 16-8
Chapter 17 Spindles 17.0 Chapter Overview This chapter describes spindle speed control, orientation, and direction, and the virtual C axis. See page: Topic: Spindle Speed Control 17-1 Controlling Spindles (G12.1, G12.2, G12.3) 17-9 Spindle Orientation (M19, M19.2, M19.3) 17-10 Spindle Direction (M03, M04, M05) 17-12 Virtual C Axis 17-13 Synchronized Spindles 17-23 If you are using a dual-processing system, spindle control is different. Refer to page 30-13 for details. 17.
Chapter 17 Spindles In this case, cutting speed V is expressed with this equation: V = (3.14159)(D)(N)/1000 To cut a 150-mm-diameter workpiece at a cutting speed of 200 m/min, the spindle speed to provide the required cutting speed is calculated to be approximately 1325 rpm using the above equation. This means that by designating “S1325;” in a part program, cutting is conducted at a cutting speed of 200 m/min.
Chapter 17 Spindles The S-word units represent revolutions per minute (RPM) in most cases. Only during CSS programming are the S-word units different. While CSS mode is active, the S-word units represent surface feet per minute. Only the controlling spindle can change its S-word mode from RPM to CSS. 17.1.
Chapter 17 Spindles Each P-word corresponds to a specific axis assigned to it in AMP. Any CSS axis changes made by programming a P-word in the G96 block remain in effect regardless of what mode the control is in. The default CSS axis is assigned to P0 and is active on power-up and after a control reset. Use this equation to calculate constant surface speed: N = K V/D RPM = Surface speed per minute / (.262 x diameter) Where : Is : N Spindle speed (rpm) K Constant 318.
Chapter 17 Spindles Figure 17.2 Constant Surface Speed Mode (G96) 1. Chuck 2. 3. Æ 200 Æ 100 CAUTION: During the blocks when CSS mode (G96) is active, the programmed S-word units are surface speed per minute. For systems allowing multiple spindles, when CSS is active, the S-word units for all spindles is surface speed per minute. To maintain RPM units on the non-controlling spindles, do not program them while CSS is active on the controlling spindle.
Chapter 17 Spindles Important: If it is desirable to prevent the spindle speed from reaching a maximum RPM a ceiling can be placed on the spindle speed at a rate below the maximum AMP setting. For details, see the CSS notes on page 17-6. Relationships between spindle speeds and cutting diameters are shown in Table 17.A for different surface speeds. Table 17.A Spindle RPM as related to cutting diameter and programmed CSS Programmed Surface Speed, Feet/min. (meters/min.
Chapter 17 Spindles In G96 mode, spindle speeds increase as the workpiece diameter decreases. When the spindle speed reaches the upper limit, it is held at this value even if the theoretical spindle speed exceeds that value. This maximum RPM may also be affected by the maximum gear speed set for a specific gear in AMP. Important: The G92s command to set a new max spindle RPM in CSS may not be programmed while CSS is active.
Chapter 17 Spindles When programming M58, the M59 code is cancelled and the G96 mode becomes active again. The spindle maintains the same surface speed that was in effect prior to the execution of M59 unless an S-code was specified in the M59 block. CAUTION: Restoring the constant surface speed mode might cause the spindle speed to change rapidly depending on the cutting tool position. Displayed spindle speed during CSS The CRT display normally shows the current spindle speed in RPM following the S-word.
Chapter 17 Spindles 17.1.2 RPM Spindle Speed Mode (G97) In the G97 mode, the spindle revolves at the programmed RPM regardless of the position of the cutting tool. For example, to revolve the spindle at 500 rpm, program: G97 S500 M03; The G97 code is modal and remains active until it is cancelled by the G96 code. Important: If an S-word is specified in the G97 block when you change from G96 to G97 mode, the control uses the S-word as the new RPM value.
Chapter 17 Spindles For systems with no spindle configured, simulated spindle feedback is provided for the primary spindle. This allows all control features that require spindle feedback, i.e., IPR feedrate, threading, CSS, to simulate the feedback from a spindle even through the AMPed system configuration contained no spindle. The default is 4000 count-per-rev device.
Chapter 17 Spindles Important: A spindle orient is also sometimes automatically requested by the control when performing some of the drilling cycles described in chapter 26. This drilling cycle orient orients to either the AMP-defined position if using a closed-loop orient type or to the position defined as the open-loop orient position. Important: In systems allowing multiple spindles (9/260 ad 9/290), only one M19 code can be in a block. If two or more M19 codes appear in one block, e.g., M19.
Chapter 17 Spindles To cancel spindle orient: 17.4 Spindle Direction (M03, M04, M05) Program: Meaning: Spindle 1 code M19 M03 M04 M05 Spindle 1 clockwise Spindle 1 counterclockwise Spindle 1 stop Spindle 2 code M19.2 M03.2 M04.2 M05.2 Spindle 2 clockwise Spindle 2 counterclockwise Spindle 2 stop Spindle 3 code M19.3 M03.3 M04.3 M05.
Chapter 17 Spindles Example 17.1 9/290 Control with 3 Spindles Configured in AMP N0001 M05 Spindle 1 stop N0002 M05.2 M05.3 Spindles 2 & 3 stop N0003 M03 M04.2 S150 Spindle 1 clockwise 150 rpm Spindle 2 counterclockwise 150 rpm N0004 M03.2 M03.
Chapter 17 Spindles To function as a virtual C axis, the lathe spindle must have a precision encoder that provides position data to the control. There can be only one encoder marker per revolution of the spindle. When the virtual C axis feature is activated, the control switches spindle operation from an open-loop spindle to a closed-loop virtual C positioning axis.
Chapter 17 Spindles Only the primary spindle (selected with G12.1) can be used in coordination with virtual C. On systems allowing auxiliary spindles, if the auxiliary spindle is the controlling spindle when virtual C is activated, this error message appears, “ILLEGAL CODE DURING VIRTUAL C.” 17.5.
Chapter 17 Spindles Where: Is: R the radius at which the feed axis (typically the X axis) is positioned at the start of cylindrical interpolation. Can be used to alter the feed axis depth if programmed in a G16.1 block during cylindrical interpolation. C the angular coordinate (if in G90 absolute mode) or the angular distance (if in G91 incremental mode) to which the virtual C axis is to move.
Chapter 17 Spindles If G02 or G03 circular interpolation is made active while in G16.1 cylindrical interpolation mode, a circular cut can be made around the circumference of the part (such as the shape cut in Figure 17.3). This is accomplished by programming the C and Z axis endpoints along with the desired circle radius R as described in chapter 14. The R parameter now defines the radius of the circular path to be cut, not the feed axis position. Important: When programming circular interpolation in G16.
Chapter 17 Spindles mode. If the AMP parameter Automatic Home on Virtual C Entry is set to “NO” (refer to the documentation provided by your system installer), you need to home the virtual C axis, typically by programming a M19S0. The control positions the tool on the cylindrical work surface with two distinct moves. In the first move, all programmed axis moves in the initial G16.1 block (including the C axis) are executed. This move takes place at the rapid feedrate for the axes.
Chapter 17 Spindles Where : Is : q The angle to be programmed for the virtual C axis. L The length of the arc along the circumference of the cylinder, as required to define a legal endpoint for the arc programmed in the G02/G03 block. R The radius at which the feed axis is positioned. This is the active R value programmed in the initial G16.1 block, not the R radius for the G02/G03 block. Figure 17.4 Results of Cylindrical Interpolation, Example 17.
Chapter 17 Spindles 17.5.2 Virtual C Axis, End Face Milling End face milling coordinates the motion of the virtual C axis with that of the linear machine axes to machine contours on the end face of a workpiece as shown in Figure 17.5. Virtual C axis end face milling is turned on using a G16.2 block and turned off with a G15 block (or a G16.1 block requesting cylindrical interpolation). A G15 block can not contain any axis words. Figure 17.
Chapter 17 Spindles End Face Milling Block Format The block used to activate virtual C axis end face milling has this format: G16.2 X__ Y__ Z__ R__ F__ Where : Is : X The coordinate (if in G90 absolute mode) or the linear distance (if in G91 incremental mode) to which the X axis is to move. Be aware that this value is affected by diameter (G08) or radius (G07) programming mode.
Chapter 17 Spindles When end face milling is activated, the circle plane is set to XY. The X axis becomes the primary axis of the circle plane and remains so, as long as the G16.2 mode is active. If the active plane is changed, the change does not become effective until the G16.2 mode is cancelled, and is superseded if the G16.2 plane is reactivated.
Chapter 17 Spindles 17.6 Synchronized Spindles Use this feature to synchronize the position and/or velocity between two spindles with feedback using your 9/440, 9/260, or 9/290 control. Two types of synchronization are available: Velocity — synchronizes only the speed between two spindles Velocity and Position — synchronizes the speed and angular position between two spindles Prior to activation, you are responsible for selecting the proper gear ranges and ratios.
Chapter 17 Spindles 17.6.1 Using the Spindle Synchronization Feature Use these three G--codes to manipulate the spindle synchronization feature: Set spindle positional synchronization (G46)— sets the follower spindle speed/direction and relative position offset to match the controlling spindle. Set active spindle speed synchronization (G46.1)— sets the follower spindle speed/direction to match the controlling spindle.
Chapter 17 Spindles The following example assumes that the controlling and follower spindles were defined as spindle 2 and spindle 1, respectively, by your system installer. Example 17.4 Spindle Synchronization M03 S200; Spindle 1 clockwise 200 rpm M04.2 S400; Spindle 2 counterclockwise at 400 rpm G12.2; Spindle 2 as controlling spindle G46 S90; Spindle 1 changes direction and accelerates to spindle 2’s speed; spindle 1 synchronizes angular position with spindle 2 (offset 90 degrees) Example 17.
Chapter 17 Spindles Activate Spindle Speed Synchronization (G46.1) Use the “Activate Spindle Speed Synchronization” to synchronize speed and direction only. Using G46.1 does not guarantee a consistent positional offset between the two spindles. During a G46.1, the follower spindle attempts to synchronize speeds with the controlling spindle.
Chapter 17 Spindles 17.7 Special Considerations for Spindle Synchronization When using the synchronized spindle feature, remember: you cannot retrace through a synchronization block (G45, G46, or G46.1). However, you can retrace through blocks where synchronization was already active. in dual--process systems, both spindles used for synchronization must be configured in the process that is programming spindle synchronization.
Chapter 17 Spindles When synchronization is active, any part program commands destined for the follower spindle (i.e., M03, M03.2, M03.3...G12.1, G12.2, and G12.3) will cause an error. On a multiprocess configuration, this is true of either process. On a multiprocess 9/Series, the process controlling the controlling spindle also controls the follower spindle when spindle synchronization is active. If it is unable to obtain control, an error results: UNABLE TO SYNCH IN CURRENT MODE.
Chapter 18 Programming Feedrates 18.0 Chapter Overview This chapter describes 9/Series control feedrates, including special AMP assigned feedrates and automatic acceleration/deceleration. For information about: 18.1 Feedrates See page: Feedrates 18-1 Special AMP-assigned Feedrates 18-8 Automatic Acceleration/Deceleration 18-10 Feedrates are programmed by an F-word followed by a numeric value. You can enter feedrates in a part program block or through MDI.
Chapter 18 Programming Feedrates Figure 18.1 Programming a Tangential Feedrate X X Linear interpolation end point Circular interpolation programmed feedrate programmed feedrate X axis feedrate Z axis feedrate end point X axis feedrate start point Z axis feedrate start point Z Z For example, if a feedrate is programmed as F100.0 millimeters per minute, and a linear move is made from X0, Z0 to X10, Z10, the feedrate along that 45 degree angular path would be 100.0 mmpm.
Chapter 18 Programming Feedrates For outside arc paths, the speed of the tool tip relative to the part surface can be determined using the following formula: Tool tip speed = F x Rp ---Rc Is : Where : F programmed feedrate Rc radius of the arc measured to the center of the tool radius Rp programmed radius of the arc Figure 18.
Chapter 18 Programming Feedrates 18.1.2 Feed Per Minute Mode (G94) In the G94 mode (feed per minute), the numeric value following address F represents the distance the axis or axes move (in inches or millimeters) per minute. If the axis is a rotary axis, the F-word value represents the number of degrees the axis rotates per minute. To program a feedrate of 55 mm of tool motion per minute program: G94 F55.; Figure 18.
Chapter 18 Programming Feedrates Since the G95 code is modal any F-word designated in any block after the G95 is considered a feed distance per spindle revolution until a G94 is executed. Figure 18.4 Feed Per Revolution Mode (G95) Cutting tool Chuck Workpiece “F”is the distance the tool moves per revolution of the workpiece. F Cutting tool B Chuck Workpiece 20.0 A If G95 F.2 is the feedrate, the tool moves from A to B in 100 revolutions of the workpiece.
Chapter 18 Programming Feedrates 18.1.4 Rapid Feedrate Rapid feedrate drives all active axes at a speed which creates a linear move. The control determines which axis must travel the furthest and drives that axis at its maximum feedrate assigned in AMP. Use rapid feedrate to position the tool to a specified point at a high speed. It is called during the execution of a G00 code followed by an axis motion command and in many of the canned cycles for positioning.
Chapter 18 Programming Feedrates Use on the MTB panel to override the rapid feedrate for G00 mode in four increments: F1 ---- percent value set in AMP by your system installer 25% 50% 100%. Important: Normally this override is not active for any dry run motions (see chapter 7) unless otherwise specified in PAL by your system installer.
Chapter 18 Programming Feedrates 18.1.6 Feedrate Limits (Clamp) The maximum allowable speed for each axis is set in AMP. If any axis feedrate exceeds the maximum allowable speed for that axis the control automatically adjusts the feedrate to a value that does not cause axis speed to exceed its set limit. Figure 18.5 Feedrate Clamp X FXMAX Fp F FXMAX : maximum X axis feedrate FZMAX : maximum Z axis feedrate FZMAX Fp : programmed feedrate F : actual feedrate Z In Figure 18.
Chapter 18 Programming Feedrates Important: Single-digit feedrates are always entered as per minute feedrates (IPM or MMPM) regardless of the control’s current feedrate mode. When a single-digit feedrate is programmed, the control automatically switches to the IPM or MMPM mode. The control automatically switches back to the previously active feedrate mode when the next feedrate is programmed that is not a single-digit feedrate. If there are no feedrates set in the tables that correspond to F1-F9.
Chapter 18 Programming Feedrates If you use this feature simultaneously with the Dry Run feature, the feedrates that are assigned to the External deceleration feature are used. The feedrates for this feature are not related to the Dry Run feedrates, although the operation of this feature is similar to Dry Run. This feedrate is unaffected by the switch and the settings, and it operates as if the switches are set at 100 percent.
Chapter 18 Programming Feedrates Refer to the table below to determine the type of acceleration/deceleration performed for manual motion and programmed moves. Table 18.B Acc/Dec Type Performed with Manual Motion and Programmed Moves Motion Type Hand-- pulse generator Always Uses Exponential Acc/Dec Configurable in AMP by System Installer via Manual Acc/Dec Mode Always Uses Linear Acc/Dec Linear or S- Curve Acc/Dec per G- code n Arbitrary angle moves (i.e.
Chapter 18 Programming Feedrates 18.3.1 Exponential Acc/Dec To begin and complete a smooth axis motion, the 9/Series control uses an exponential function curve to automatically accelerate/decelerate an axis. Your system installer sets the acceleration/deceleration time constant “T” for each axis in AMP. Figure 18.6 shows axis motion using exponential Acc/Dec. Figure 18.
Chapter 18 Programming Feedrates Axis motion response lag can be minimized by using Linear Acc/Dec for the commanded feedrates. The system installer sets Linear Acc/Dec values for interpolation for each axis in AMP. Figure 18.7 shows axis motion using Linear Acc/Dec. Velocity Figure 18.7 Linear Acc/Dec Acceleration Time Time Jerk 18.3.
Chapter 18 Programming Feedrates 18.3.3 S- Curve Acc/Dec When S--Curve Acc/Dec is enabled, the control changes the velocity profile to have an S--Curve shape during acceleration and deceleration when in Positioning or Exact Stop mode. This feature reduces the machine’s axis shock and vibration for the commanded feedrates. Figure 18.8 shows axis motion using S--Curve Acc/Dec. Figure 18.
Chapter 18 Programming Feedrates 18.3.4 Programmable Acc/Dec Programmable Acc/Dec allows you to change the Linear Acc/Dec modes and values within an active part program via G47.x and G48.x codes. You cannot retrace through programmable acc/dec blocks (G47.x and G48.x). However, you can retrace through blocks where programmable acc/dec was already active. Selecting Linear Acc/Dec Modes (G47.x - - modal) Programming a G47.x in your part program allows you to switch Linear Acc/Dec modes in nonmotion blocks.
Chapter 18 Programming Feedrates Selecting Linear Acc/Dec Values (G48.n - - nonmodal) Programming a G48.x in your part program allows you to switch Linear Acc/Dec values in nonmotion blocks. Axis values in G48.n blocks will always be treated as absolute, even if the control is in incremental mode. Below is the format for calling G48 commands. Use this format with the axis names assigned by your system installer: G48.
Chapter 18 Programming Feedrates 18.3.5 Precautions on Corner Cutting When Acc/Dec is active, the control automatically performs Acc/Dec to give a smooth acceleration/deceleration for cutting tool motion. However, there are cases in which Acc/Dec can result in rounded corners on a part during cutting. In Figure 18.9, this problem is obvious when the direction of cutting changes from the X axis to the Z axis. In this case, the X axis decelerates as it completes its move, while the Z axis is at rest.
Chapter 18 Programming Feedrates Exact Stop Mode (G61 - - modal) G61 establishes the exact stop mode. The axes move to the commanded position, decelerate and come to a complete stop before the next motion block is executed. To cancel this mode, program G62, or G63. Cutting Mode (G64 - - modal) G64 establishes the cutting mode. This is the normal mode for axis motion and is generally selected by your system installer as the default mode active on power up.
Chapter 18 Programming Feedrates When the corner angle, A, is larger than the value set for “min. angle for corner override” in AMP, the programmed feedrate is overridden from point “a” to point “b,” and from point “b” to point “c.
Chapter 18 Programming Feedrates Figure 18.11 Programmed Feedrate Not Reached Z Programmed feedrate F100 F E F60 E D R A T E Feedrate clamped here to allow time for deceleration Linear Deceleration Linear Accel Z4.8 Z4.9 Z5.0 DISTANCE Z5.1 12162-I Normally this causes no problem. However, in cases where a series of very short axis moves in separate blocks exist, this limitation to the feedrate can cause finish problems as well as increased cycle time. Figure 18.
Chapter 18 Programming Feedrates To avoid this feedrate limitation, the short block Acc/Dec clamp can be disabled by programming a G36.1. In this mode, the control assumes that no rapid decelerations are required and allows axis velocities to go higher than they otherwise would. Activate G36.
Chapter 18 Programming Feedrates G36 and G36.1 are modal. The control should only be in short block check disable mode (G36.1) when executing a series of fast short blocks that contain only slight changes in direction and velocity. What constitutes a slight change in direction and velocity depends on the Acc/Dec ramp configured for your machine. G36 -- Short Block Acc/Dec clamp Enable G36.
Chapter 19 Dual Axis Operation 19.0 Chapter Overview The Dual Axes feature lets the part programmer simultaneously control multiple axes while programming commands for only one. It differs from the split axis feature of the 9/Series control in that the split axis feature is used to control a single axis positioned by two servo motors.
Chapter 19 Dual Axis Operation Figure 19.1 Dual Axis Configuration Lead screw Axis 1 Encoder Servo motor Dual Axes - two completely separate axes responding to the same programming commands. Encoder Servo motor Axis 2 Lead screw The 9/Series control can support two dual axis groups. A dual axis group consists of two or more axes coupled through AMP and commanded by a master axis name.
Chapter 19 Dual Axis Operation Figure 19.2 shows the position display for a system that contains a dual axis group containing two axes with a master axis name of X. Whether or not all axes of a dual group show up on the position display is determined in PAL by your system installer. Figure 19.2 Axis Position Display for Dual X Axis E-STOP PROGRAM[ MM ] F X1 -7483.647 S Z -0219.550 T U -2345.673 X2 -7483.647 MEMORY MAN 00 0 (ACTIVE PROGRAM NAME) STOP PRGRAM OFFSET MACRO MANAGE PARAM 19.
Chapter 19 Dual Axis Operation CAUTION: Be careful when an axis is unparked. Any incremental positioning requests you make to the dual axis group are referenced from the current location of all axes in the dual group. This includes any manual jogging or any incremental part program moves. When an axis is unparked, we recommend you make the next command the dual axis group be an absolute command to realign the axes in the dual group to the same position. Perform an axis park in a dual group through PAL.
Chapter 19 Dual Axis Operation Homing Axes Simultaneously This method allows a request for all axes in the dual group to be homed at the same time. This does not mean that all axes reach home at the same time. Keep in mind that your system installer can define different feedrates and different home positions for each axis in the dual group. With proper PAL programming, your system installer can configure all axes in the dual axis group to home when the request is made to the master axis.
Chapter 19 Dual Axis Operation Important: You can use the PAL axis mover feature if it is necessary to position dual axis group members separately without requiring any parking. Refer to the PAL manual and the system installer’s documentation for details. Invalid Operations on a Dual Axis Table 19.A lists the features that are not compatible with dual axes. If you must execute one of these features on a dual axis, only the AMP master axis can be used. All other axes in the dual group must be parked.
Chapter 19 Dual Axis Operation 19.4 Offset Management for a Dual Axis Give consideration to offsets used for a dual axis. In most cases, each axis can have independent offset values assigned to it. This section describes the difference in dual axis operation when it concerns offsets. How to activate/deactivate and enter these offset values is not described here unless some change specific to a dual axis occurs. See chapter 3 for implementation details about the offset you are using.
Chapter 19 Dual Axis Operation Set Zero You can perform a set zero operation on the axes in a dual group on an individual basis. For example, if you have a dual axis named X and it consists of two axes, X1 and X2, when the set zero operation is executed through PAL, you must specify which axis in the dual group to set zero. When the set zero operation is performed on an axis, the current axis location becomes the new zero point of the coordinate system.
Chapter 20 Tool Control Functions 20.0 Chapter Overview This chapter describes these tool control functions: Topic: On page: Programming a T-word 20-3 Entering tool offset data 20-6 Tool management 20-14 Programming a T-word ---- Different formats available for selecting a tool number and tool offsets Tool length offsets ---- Compensate for the difference between the tool length assumed while programming, and the actual length of the tool used for cutting. This feature can offset up to 4 axes.
Chapter 20 Tool Control Functions 20.1 T-words and Tool Length Offsets Modern machining processes usually require a machine that is capable of selecting different tools. Typically tools are mounted in a turret and assigned tool numbers as illustrated in Figure 20.1. The tool length offset data, tool tip radius data, tool wear compensation data and tool orientation data are set in the offset table corresponding to different offset numbers See chapter 3. Figure 20.
Chapter 20 Tool Control Functions 20.1.1 Programming a T-word and Tool Offsets Important: If tool life management is being used on the system, see the tool management section in this chapter for details on programming a T-word. This section assumes that the tool life management feature is not being used. Your system installer determines the format for a T-word in AMP. Table 20.A shows the 6 available format selections. Table 20.
Chapter 20 Tool Control Functions Example 20.2 Using T-word Format #3 T2013; This example first calls for tool number 2 to be rotated into position, then data is accessed from the offset tables (chapter 3) for values under tool geometry offset number 13, and tool wear offset number 13. From these simple examples translation to the other formats should be relatively easy. The tool number is always the digits closest to the T-word.
Chapter 20 Tool Control Functions 20.1.2 Activating Tool Length Offsets Your system installer has the option in AMP to determine exactly when the geometry and wear offsets take effect and when the tool position changes to the new shifted location. This manual makes the assumption that the system is configured to immediately shift the coordinate system by the geometry and wear amounts, and delay the move that re-positions the tool to the same coordinate position in the current work coordinate system.
Chapter 20 Tool Control Functions 20.2 Entering Tool Offset Data Using (G10L10, G10L11) You can enter data in the tool offset tables by programming the correct G10 command. This section describes the use of the G10 commands for the lathe tool offset table. Important: Only the value in the offset table value changes when a G10 code modifies a tool offset table value.
Chapter 20 Tool Control Functions Example 20.5 Using G10 to Change The Tool Offset Table N00001 G90; N00002 G10 L10 P4 Z2.1 Q1; Offset number 4 has a new value of 2.1 for tool offset in the Z direction and new orientation value of 1 in geometry table. The current value for any axis not specified and for the tool radius remain unchanged. N00003 G10 P4 L11 Z1.1; Offset number 4 has a new value of 1.1 for tool offset in the Z direction in the wear table.
Chapter 20 Tool Control Functions Manually Entering Random Tool Data Data can be entered into the random tool table either manually, as described here, by programming, or by running a backup program of the tool data. These other methods are described later in this section. To manually enter the random tool data, follow these steps: 1. Press the {OFFSET} softkey. (softkey level 1) 2.
Chapter 20 Tool Control Functions POCKET ASSIGNMENT TABLE PKT 001 004 007 010 013 016 019 022 025 028 031 034 037 TOOL 0002 0007 0006 PKT 002 005 008 011 014 017 020 023 026 029 032 035 038 TOOL 0003 XXXX XXXX RAPLCE CLEAR VALUE VALUE PAGE 1 OF 2 PKT 003 006 009 012 015 018 021 024 027 030 033 036 039 TOOL 0001 XXXX XXXX CUSTOM ACTIVE BACKUP The columns labeled PKT give the tool changer pocket numbers. The columns labeled TOOL give the tool number of the tool in the corresponding pocket.
Chapter 20 Tool Control Functions To enter a custom tool (a tool that requires more than one tool pocket) enter the tool number of the custom tool in the pocket that is to be used as the “shaft pocket”. The shaft pocket is where the tool changer is positioned when the particular custom tool is to be used. Enter the number of pockets needed (to a max of 9), a comma, followed by the position of the shaft pocket in this group of pockets. Press the [TRANSMIT] key enters the data into the table.
Chapter 20 Tool Control Functions Format for Programming Random Tool Table Use this block to set data for the random tool pocket assignment table: G10.1 L20 P__ Q__ O__ R__; Where : Is : G10.1 L20 This tells the control that the block will be setting data for the random tool pocket table. The G10.1 L20 is not modal, it must be programmed in every block that sets data for the random tool pocket assignment table. P__ The value following the P-word determines the pocket number that is being set.
Chapter 20 Tool Control Functions Backup Random Tool Table The control has a feature that allows you to back up (save) the information in the random tool table. The control generates a G10.1 program from the information already in the table. To do this follow these steps: 1. Press the {OFFSET} softkey. (softkey level 1) 2. PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD Press the {RANDOM TOOL} softkey.
Chapter 20 Tool Control Functions Starting a Program with a Tool Already Active You can begin a part program with a tool already active in the chuck. In order for random tool to be able to properly handle that tool, it must enter information about that tool in the random tool table. Important: If you use random tool when the tool was loaded into the chuck, it do not need to enter any data since random tool remembers what tool is loaded even after power is turned off.
Chapter 20 Tool Control Functions 20.4 Automatic Tool Life Management Use the automatic tool management feature to monitor the life of a tool, determine when the tool should be replaced, and provide a replacement tool when that tool is requested in a program. Tool are assigned to selected groups. Instead of calling a specific tool in a program, the programmer calls a tool group. The control then selects the first tool assigned to that group.
Chapter 20 Tool Control Functions Tool Life Measurement Type The control can measure the life of a tool using one of three possible methods: Tool Life Type 0 Method Selected time Meaning This is selected by choosing 0 as the type of tool life measurement. Time measures tool life as the length of time that a cutting tool is operated at a cutting feedrate. The value for the expected tool life is entered in units of minutes.
Chapter 20 Tool Control Functions Tool life Threshold Percentage A threshold level may also be assigned to a tool group. The threshold level is assigned as a percentage of the total expected life of the tool. When a tool reaches this threshold level, it is classified as old for that tool group. A tool is classified as old only to allow the operator to see that a tool is close to expiration.
Chapter 20 Tool Control Functions Figure 20.2 Typical Tool Group Directory Screen ENTRY GROUP NO: TOOL GROUP DIRECTORY PAGE 1 0F 1 (FILE NAME) GROUP 1 2 TOOL NUMBER 1 2 44 55 63 90 EDIT GROUP 88 99 DELETE DELETE GROUP ALL At this point, you can delete any or all tool groups that already exist for some reason follow these steps: To delete: Press: select tool group the {DELETE GROUP} softkey. Key in the desired group number to delete and press the [TRANSMIT] key.
Chapter 20 Tool Control Functions Figure 20.3 Typical Tool Group Data Screen ENTER DATA: EDIT TOOL GROUP 1 (FILE NAME) ENTRY NO 1 2 3 4 PAGE 1 OF 1 THRESHOLD RATE =80% TOOL NUMBER OFF NO 2 4 6 8 LIFE TYPE = TIME CHANGE INSERT DELETE CHANGE CHANGE TOOL TOOL TOOL TYPE T RATE 5. From this screen, you can: Operation: Description: Change tools Alter one of the tool numbers that has already been entered in the group.
Chapter 20 Tool Control Functions 20.4.2 Assigning Detailed Tool Data This section assumes that tools have already been assigned to their specific groups. This section describes specific information that is to be entered into the tool life management tables for the individual tools. This information may also be entered into the tool management tables using the programming method described on page 20-22.
Chapter 20 Tool Control Functions If tool life is measured by the number of uses (1 is selected as tool life type), then the units for the expected tool is the number of programs that the tool may be selected as an active tool in. The accumulated life of a tool is increased by one if that tool is selected in a program as the active tool. Remember that the same tool may be active more than once in a program, however its accumulated life only increments by one.
Chapter 20 Tool Control Functions 2. Press the {TOOL MANAGE} softkey. (softkey level 2) WORK TOOL CO-ORD WEAR TOOL TOOL RANDOM GEOMET MANAGE TOOL COORD BACKUP SCALNG ROTATE OFFSET 3. Press the {TOOL DATA} softkey. The control displays the prompt “EDIT GROUP:”. (softkey level3) TOOL DIR 4. TOOL DATA BACKUP DATA Key in the group number to edit using the keys on the operator panel and press the [TRANSMIT] key. Figure 20.4 shows all of the information for that tool group that is displayed. Figure 20.
Chapter 20 Tool Control Functions 5. From this screen it is possible to perform the following operations. The application of these operations was described in detail earlier in this section. Operation: Description: Enter or alter the tool length offset number To enter or alter a value for the tool length offset number, move the cursor to the tool number of the tool to alter and press the {EDIT LN OFF} softkey.
Chapter 20 Tool Control Functions Important: G10 blocks may not be programmed when TTRC is active. CAUTION: Any time that a G10L3; block is executed the control automatically clears all information that is in the management tables for all tools and tool groups. Any time after the G10L3 command, parameters may be programmed to enter what tool group is being entered, the type of tool life measurement that is being used, and the tool life threshold percentage.
Chapter 20 Tool Control Functions The following program blocks assign tools to groups, length and cutter compensation offset numbers, and expected tool life to specific tools. This information is assigned to the last group number programmed in a block using the P-word. The format for these blocks is: T__ H__ D__ L__; Where : Is : T__ The value entered with the T-word is the tool number of the tool to be assigned to that group.
Chapter 20 Tool Control Functions Example 20.6 Programming Tool Life Management Data Program Block Description G10L3; Starts loading tables. P1I1Q60; Begins loading data for tool group 1. Type 1 (number of uses) measurement. Threshold 60%. T1H5D7L25; Places tool 1 in group 1 with length offset number of 5, cutter radius offset number 7, and expected life of 25 uses. T2H2; Places tool 2 in group 1 with length offset number of 2, no cutter radius offset number and expected life of 25 uses.
Chapter 20 Tool Control Functions 2. Press the {TOOL MANAGE} softkey. (softkey level 2) WORK TOOL CO-ORD WEAR TOOL TOOL RANDOM GEOMET MANAGE TOOL COORD BACKUP SCALNG ROTATE OFFSET 3. Press the {BACKUP DATA} softkey. The prompt “BACKUP FILENAME:” is displayed on the input line. (softkey level 3) TOOL DIR 4. 20.4.4 Programming a T-word Using Tool Management TOOL DATA BACKUP DATA Key in any legal program name and press the [TRANSMIT] key.
Chapter 20 Tool Control Functions Example 20.7 Assume your system installer has set the following constraints in AMP: - the tool group boundary is set as 100 - the T-word format is configured as 2-digit geometry and wear (see section 20.
Chapter 20 Tool Control Functions Example 20.8 Programming Tool Changes Using Tool Life Management. Example 20.8 assumes that: - your system installer has configured in AMP the boundary for tool life management at 100 - the tool changer is located at the secondary machine home point called by a G30; this is not necessarily true for different machine applications - the T-word format is configured as 3 digit geometry + wear - the maximum allowable T-word format has been set to allow 6-digit T-words.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function 21.0 Chapter Overview This chapter describes Tool Tip Radius Compensation function.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.1 Taper and Arc Cutting Without TTRC Without TTRC active, control assumes tool has a perfect point Cutting tool Actual tool tip radius Part profile Material left uncut due to radius of tool tip Put the radius of the tool and tool orientation data into the offset tables in advance. This function lets the control use the same program to produce the same workpiece, regardless of the radius of the tool that does the cutting.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function outside ---- Refer to an angle between two intersecting programmed tool paths outside if, in the direction of travel, the angle measured clockwise from the second tool path into the first is greater than 180°. See Figure 21.2. If one or both of the moves are circular, the angle is measured from a line tangent to the tool path at their point of intersection.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function This table highlights the differences between the two types: Type of Move Entry Move Into TTRC Tool Path Exit Move From TTRC Type A Type B - The tool takes the shortest possible path to its offset position. - The tool stays at least one radius away from the start-point of the next block at all times. - Extra motion blocks can be generated to attempt to prevent gouging of the part as may occur in Type A. - Same as Type B. - Same as Type A.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.3 TTRC Direction G42; Compensation right G40; Compensation cancel Programmed tool path and direction G41; Compensation left Important: The TTRC function is not available during any of the thread cutting cycles. TTRC must be canceled before any threading routine can be performed.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function You can program TTRC in various ways. Example 21.1 shows 1-, 2-, and 3-block programs activating TTRC with entry moves. Example 21.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Important: The TTRC feature is not available for any motion blocks that are programmed in MDI mode. See page 21-30. The TTRC mode can be altered by programming either G41, G42, or G40, or the tool radius can be changed in an MDI program. However, none of the tool paths executed in MDI will be compensated. Any changes made to TTRC are not applied until the next block executed in automatic mode. Figure 21.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.5 Results of TTRC Program Example Cutting tool center path X N2 N4 N3 N5 N1 N6 start point 21.2 TTRC Generation Blocks G39, G39.1 Z In certain instances, TTRC creates a non-programmed move called a generated block. These blocks improve cycle time and corner-cutting quality.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function The generated block between the two tool paths can be programmed as linear or circular with these G-codes: G39(or G39.1); Where : Causes: G39 linear transition blocks. If neither G39 or G39.1 is programmed, G39 is the default. This command is modal. G39.1 circular transition blocks. When cutting straight line-to-arc or arc-to-straight line moves, the generated block will always be linear, and the G39.1 will be ignored. This command is modal.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function 21.3 TTRC Tool Paths (Type A) The easiest way to demonstrate the cutting tool’s the actual tool paths when using TTRC type A is by pictorial representation. The following subsections describe the cutter path along with a figure to clarify the description 21.3.1 TTRC Type A Entry Moves An entry move is defined as the path that the cutting tool takes when the TTRC function first becomes activated in a program. Figure 21.7 shows a typical entry move.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function If the next programmed move is circular (an arc), position the tool at right angles to a tangent line drawn from the start-point of that circular move. Figure 21.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Example 21.3 Sample Entry Move After Non-Motion Blocks Assume current compensation plane is the ZX plane. N01X0Z0; N2G41T1; This block commands compensation left N3M02; This is not the entry block since no axis motion takes place in the current plane. N4...; No axis motion in current plane. N5...; No axis motion in current plane. N6...; No axis motion in current plane.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.10 Results of Example 21.4 Programmed path r r Too many non-motion blocks here TTRC reinitialized here G41 r r r 21.3.2 TTRC Type A Exit Moves Cancel the TTRC feature by programming G40. Refer to the path that is taken when the tool leaves TTRC as the exit move. The path that the tool follows during an exit move is dependant on: The direction of compensation (G41 or G42).
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Example 21.5 gives some sample exit move program blocks. Example 21.5 Type A Sample Exit Moves Assume the current plane is the XZ plane and TTRC is already active before the execution of block N100 in these program segments. N100X1.Z1.; N110X3.Z3.G40; Exit move. N100X1.Z1.; N110G40; N120X3.Z3.; Exit move. N100X1.Z1.; N110G40; N120; No axis motion in the current plane. N130...; No axis motion in the current plane. N140...
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.11 through Figure 21.15 show examples of typical exit moves using type A TTRC. All examples assume that the number of non-motion blocks before the designation of the G40 command have not exceeded the number allowed as determined by your system installer in AMP. Figure 21.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function If the last programmed move is circular (an arc), positioning the tool at right angles to a tangent line drawn from the end-point of that circular move. Figure 21.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function The I- and K-words in the exit move block define a vector that is used by the control to redefine the end-point of the previously compensated move. I- and K-words are always programmed as incremental values regardless of the current mode (G90 or G91).
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.14 Results of Example 21.6 Compensated path using I, K vector Compensated path if no I, K in G40 block N11 Compensated path Programmed path r N10 r r I, K Intercept line If the vector defined by I and/or K is parallel to the programmed tool path, the resulting exit move is offset in the opposite direction of the I and/or K vector by one radius of the tool. Figure 21.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function 21.4 TTRC Tool Paths (Type B) We demonstrate the actual tool paths taken by the cutting tool when using TTRC type B by pictorial representation. The following subsections describe the cutter path along with a figure to clarify the description. 21.4.1 TTRC Type B Entry Moves An entry move is defined as the path that the cutting tool takes when the TTRC function first becomes activated in a program. Figure 21.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.17 and Figure 21.18 show examples of typical entry moves using type B TTRC. Figure 21.17 Tool Path for Entry Move Straight Line-to-Straight Line G39 (Linear Generated Blocks) 0 £q £90 D E r r C r q r r q B G42 Start-point B A C r 180 £q £270 Start-point G41 r q Start-point A 90 £q £180 Programmed path r G41 r G42 q G39 (Linear Generated Blocks) 270 £q £360 A r r C G42 G39.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function If the next programmed move is circular (an arc), position the tool at right angles to a tangent line drawn from the start-point of that circular move. Figure 21.18 Tool Path for Entry Move Straight Line-to-Arc G39 (Linear Generated Blocks) 0 £q £90 r r r r r q r G39.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function There is no limit to the number of blocks that can follow the programming of G41 or G42 before an entry move takes place. The entry move is always the same regardless of the number of blocks that do not program motion in the current plane for compensation. Example 21.7 Sample Entry Move After Non-Motion Blocks Assume current compensation plane is the ZX plane. N01X0Z0; N2G41; This block commands compensation left.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.19 Too Many Non-Motion Blocks Programmed path r r Too many non motion blocks here TTRC reinitialized here G41 r r r 21.4.2 TTRC Type B Exit Moves Program a G40 to cancel the TTRC feature. Refer to the path that is taken when the tool leaves TTRC is referred to as the exit move. The path that the tool follows during an exit move is dependant on: The direction of compensation (G41 or G42).
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Example 21.9 gives some sample exit move program blocks. Example 21.9 Sample Exit Move Segments Assume the current plane to be the ZX plane. N100X1Z1; N110X3Z3G40; Exit move. N100X1Z1; N110G40; N120X3Z3; Exit move. N100X1Z1; N110G40; N120...; No axis motion in the current plane. N130...; No axis motion in the current plane. N140...; No axis motion in the current plane. ” ” ” ” N200X3Z3; Exit move. N100X1Z1; N110...
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.20 and Figure 21.21 show examples of typical exit moves using type B TTRC. All examples assume that the number of non-motion blocks before the designation of the G40 command has not exceeded the number allowed as determined by your system installer in AMP. Figure 21.20 Tool Path for Exit Move Straight Line-to-Straight Line G39 (Linear Generated Blocks) 0 £q £90 G39.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function If the last programmed move is circular (an arc), the tool is positioned at right angles to a tangent line drawn from the end-point of that circular move. Figure 21.21 Tool Path for Exit Move Arc-to-Straight Line G39 (Linear Generarated Blocks) 0 £q £90 End-point G39.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.20 and Figure 21.21 assume that the number of blocks that do not contain axes motion in the currently selected plane, following G40 before the exit move takes place, do not exceed an amount selected in AMP by your system installer. If the number of non-motion blocks following G40 exceeds the limit, the control generates its own exit move.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Example 21.10 Exit Move Defined By An I, K Vector But Limited To Tool Radius Assume T1 radius is 3. N10 Z10.G41T1; N11 X10.Z2.I3K-10.G40; Figure 21.23 Results of Example 21.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function 21.5 Tool Path During TTRC Except for entry and exit moves, the basic tool path generated during TTRC is the same for types A and B TTRC. Whether tool left or tool right is specified, the path taken is a function of the angle between tool paths (G41 or G42) and the radius of the cutting tool.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.25 through Figure 21.28 illustrate the basic motion of the cutting tool as it executes program blocks during TTRC. Figure 21.25 TTRC Tool Paths Straight Line-to-Straight Line G39 (Linear Generated Block) Linear 0 £q £90 generated block r G41 G42 r Programmed path r q r Circular generated block G41 r Programmed path G39.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.26 TTRC Tool Paths Straight Line-to-Arc G39.1 (Circular Generated Block) 0 £q £ 90 G39 (Linear Generated Block) 0 £q £ 90 Linear generated blocks r Circular generated block r r r q r q Programmed path Programmed path G41 G41 G42 90 £q £180 G42 180 £q £270 G41 Linear generated block r Programmed path r r r G41 G42 q r Programmed path Linear generated block G42 G39.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.27 TTRC Tool Paths Arc-to-Straight Line G39.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.28 TTRC Tool Paths Arc-to-Arc G39 (Linear Generated Block) 0 £q £90 r r r r r r r q G41 G39.1 (Circular Generated Block) 0 £q £90 q G41 r r r Programmed path Programmed path G42 G42 180 £q £270 90 £q £180 q q r G41 Programmed path G41 Programmed path Programmed path r G42 G42 G39 (Linear Generated Block) 270 £q £360 G42 Programmed path G41 G41 r G39.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function 21.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function The control generates the motion block that connects point 1 to point 2 as shown in these examples: Example 21.11 Linear-to-Linear Change in TTRC Direction (Reversing Tool Path) N10 Z10.G41; N11 Z20.; N12 Z10.G42; N13 Z0.; Figure 21.29 Results of Example 21.11 Point 1 & 2 Compensated N10 Programmed G41 N11 N13 Programmed G42 N12 Example 21.12 Linear-to-Linear Change in TTRC Direction (Continuing Tool Path) N10 Z10.G41; N11 Z20.; N12 Z30.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Example 21.13 Linear-to-Linear Change in TTRC Direction (With Generated Blocks) N10 X15.Z10.G41; N11 X-5.Z8.; N12 X0.Z35.G42; Figure 21.31 Results of Example 21.13 r r r r N11 Compensated path N10 Programmed path N12 G41 G42 r Point 2 r Point 1 Example 21.14 Linear-to-Linear Change in TTRC Direction (No Generated Blocks) N20 X5Z10.G41; N21 X-5.Z7.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.32 Results of Example 21.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.34 Change in Compensation With No Possible Tool Path Intersections Compensated path r2 r1 r1 Programmed path G41 G42 r1 Programmed path G42 r2 r1 Compensated path G41 Compensated path r Programmed path G41 G42 r 21.6.2 Too Many Non-Motion Blocks The control always looks ahead to the next motion block to determine the actual tool path for a motion block in TTRC.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function When scanning ahead, if the control does not find a motion block before the number of non-motion blocks has been exceeded, it does not generate the normal TTRC move. Instead the control sets up the compensation move with an end-point one-tool radius away from and at right angles to, the programmed end-point. In many cases this may cause unwanted overcutting of a work piece. In many cases, this can cause unwanted overcutting of a work piece. Figure 21.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.36 Too Many Non-Motion Blocks Following a Circular Move Programmed path G42 Programmed path G42 Compensated path Compensated path + r Programmed path G42 Compensated path r Too many non-motion blocks here Too many non-motion blocks here 21.6.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.37 Compensation Corner Movement for Two Generated Blocks This block is eliminated if both hX1-X2h and hZ1-Z2h are less than AMP parameter X1Z1 New block if block is eliminated X2Z2 Compensated Programmed When the control generates 3 motion blocks, the length of the second generated block is checked against a minimum allowable length, determined in AMP by your system installer.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function 21.6.4 Changing Cutter Radius During Compensation If a tool becomes excessively worn, broken, or for any other reason requires the changing of the programmed tool tip radius, TTRC should be cancelled and re-initialized after the tool has been changed. See page NO TAG on changing the tool offset and page on changing the active tool offset number.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.39 Linear-to-Linear Change in Cutter Radius During Compensation With control generated motion blocks No control generated motion blocks N10 N11 D_ N12 N10 N11 D_ N12 r1 Compensated path r1 r1 r1 r2 N10 r1 N10 Compensated path r2 N11 Programmed path r1 Generated blocks Programmed path N12 r2 r2 N11 N12 Figure 21.40 describes the tool path when the programmed moves are linear-to-circular. Figure 21.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.41 describes the tool path when the programmed moves are circular-to-circular. Figure 21.41 Circular to Circular Change in Cutter Radius During Compensation No control-generated motion blocks With control-generated motion blocks Programmed path Programmed path Compensated path Compensated path r1 r2 r1 r1 r2 r2 Generated blocks Change in Cutter Radius During Jog Retract.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function The new offset is activated. TTRC is able to compensate for this new diameter by modifying the saved jogged path. This path is modified so that the new tool cuts the same part as the old tool. The absolute position of the machine will, therefore, be different on the return path from what it was when jogging away from the part. This jogged path is adjusted when you press the button to return from the jog retract.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.42 shows an example of a typical change in tool radius during jog retract with TTRC active: Figure 21.42 Change in Cutter Radius During a Jog Retract Programmed path . . Compensated path Original tool radius . . . Difference in tool radius DR . . . Jog retract return moves . Tool radius changed here 21.6.5 MDI or Manual Motion During TTRC . . 90° . . .
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.43 TTRC Interrupted with MDI Blocks 3 MDI blocks (no compensation applied) Programmed path G42 r Compensation reinitializes here r End-point of MDI Important: If during cutter compensation, you switch out of automatic mode and either: generate axis motion in manual mode on an axis in the cutter compensation plane, or execute any block in MDI mode, cutter compensation is re-initialize when you return to automatic mode.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Figure 21.44 Cutter Compensation Re-Initialized after a Manual or MDI Operation. Manually jog axes (or any MDI execution) and return to the compensated path. Cutter Compensation is re-initialized here. The control assumes that the current position is a programmed position at the point of re-initialization. Consequently, after the initialization, tool compensation is offset by twice the tool radius.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function specified, the control executes the move prior to the return to home operation as an exit move. This can cause undesired overcutting of the part. If compensation was not cancelled using a G40 command before returning to machine or secondary home points, the control automatically re-initializes TTRC for the return from machine or secondary home points.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function 21.6.7 Changing or Offsetting Work Coordinate System in TTRC We recommend that you cancel TTRC by using a G40 command before any modifications to the current work coordinate system are made, including any offsets or any change of the coordinate system (G54-G59.3). If compensation is not cancelled using a G40 command, the control automatically, temporarily cancels compensation for the change in work coordinate system.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function 21.6.8 Block Look-Ahead During normal program execution, the control is constantly scanning ahead several blocks to set up the necessary motions to correctly execute the current block. This is called Block Look-Ahead. The 9/Series control has 21 set-up buffers. Different features require the use of some of these setup buffers. One is always used for the currently executing block. TTRC requires at least 3 of these buffers.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Backwards Motion Detection The compensated tool path is parallel to but in the opposite direction of the programmed tool path. Figure 21.47 Typical Backwards Motion Error Compensated Path Programmed Path A C’ Compensated path motion opposite of programmed path D D’ A’ B B’ C Circular Departure Too Small No intersection can be generated between two consecutive compensated tool paths. Figure 21.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Interference This error occurs when compensation vectors intersect. Normally when this intersection occurs, a backwards motion error is generated; however, a few special cases exist that are caught only by interference error detection. Figure 21.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function Error detection M-codes are only functional when TTRC is active. TTRC is active when the control is in G41 or G42 mode and has already made the entry move into compensation. If an M800 or M801 is programmed in G40 mode or before the entry move into TTRC takes place, the M code is ignored. If error detection is disabled in TTRC, and TTRC is exited (G40 programmed), the next time TTRC is re-activated error detection will be re-activated automatically.
Chapter 21 Tool Tip Radius Compensation (TTRC) Function 21-56
Chapter 22 Single-Pass Turning Cycles 22.0 Chapter Overview Single-pass turning cycles consist of these cycles: G20 Single-pass O.D. and I.D. roughing cycle G24 Single-pass rough facing cycle G21 Simple threading cycle This chapter describes the following major topics: Topic: On page: G20 22-1 G24 22-8 These cycles are called single-pass cycles because each time the cycle is executed, it makes only one cutting pass over the workpiece.
Chapter 22 Single-Pass Turning Cycles Important: Descriptions in this chapter are written assuming the control is in the G18 plane and that plane has been defined as the ZX plane. If your system has a different plane active, operation of these features is different. Parameters are defined here assuming Z is the first axis in the plane, and X is the second axis in the plane. If, for example, the XZ plane is the currently active plane, descriptions in this document should be interpreted accordingly (i.e.
Chapter 22 Single-Pass Turning Cycles CAUTION: When programming the single-pass cycle, the first move to the depth of cut is a rapid move. Make sure that the tool does not contact the part on this initial move. The feedrate used in the single-pass cycle is the currently active programmed cutting feedrate. If desired, a different cutting feedrate may be specified in the single-pass cycle block.
Chapter 22 Single-Pass Turning Cycles Example 22.1 Straight Cutting Cycle G90G00X40.Z60.; G20X28.Z25.F10. X24.; X20.; G00; Figure 22.2 Results of Example 22.
Chapter 22 Single-Pass Turning Cycles G20 Taper O.D. and I.D. Roughing A G20 block that includes an I-word generates a turning pass that produces a taper. Figure 22.3 G20 Taper Cutting Cycle X Cutting feed Rapid feed I Z The format for the G20 single-pass cycle to cut a taper is: G20X__Z__I__; Where : Is : X__ the depth of cut for the X axis at the end point of the cutting move into the part.
Chapter 22 Single-Pass Turning Cycles After the G20 block is executed, the control re-executes the cycle for any following block that commands axis motion (until the cycle is cancelled). The value of the axis word in that block is used to replace the parameter determined with that axis word in the original G20 block and the cycle is re-executed using these new parameters. Figure 22.4 applies only if programming X and Z as incremental values.
Chapter 22 Single-Pass Turning Cycles Example 22.2 Taper Cutting G90G00X50.Z106.; G20X38.Z46.I-11.F.5; X32.; X26.; X20.; Figure 22.5 Results of Example 22.
Chapter 22 Single-Pass Turning Cycles 22.2 Single-pass Rough Facing Cycle (G24) G24 calls either a straight or a tapered facing cycle. This cycle is a single-pass cycle (makes only one cutting pass over the workpiece each time it is called). Use the G24 cycle to cut along the face of a workpiece (in this manual that means it cuts along the X axis). The G24 cycle basically consists of the moves shown in Figure 22.6. Figure 22.6 G24 Straight Facing Cycle 1. Rapid approach to the part 2.
Chapter 22 Single-Pass Turning Cycles The feedrate used in the single-pass cycle is the currently active programmed cutting feedrate. If desired, a different cutting feedrate may be specified in the single-pass cycle block. The rapid feedrate (for the axis in motion as assigned in AMP) is used for the approach to the part and the return to start point. G24 Straight Facing The format for the G24 straight facing cycle is: G24X__ Z__; Where : Is : X__ the length of cut along the X axis.
Chapter 22 Single-Pass Turning Cycles Example 22.3 Straight Facing Cycle G90G00X30.Z22.; G24X10.Z15.F10. Z13.; Z11.; G00; Figure 22.7 Results of Example 22.
Chapter 22 Single-Pass Turning Cycles G24 Tapered Facing A G24 block that includes a K-word generates a facing pass that produces a taper. Figure 22.8 G24 Face Taper Cutting Cycle X K Z Cutting feed Rapid feed The format for the G24 single-pass cycle to cut a taper on a face is: G24X__Z__K__; Where : Is : X__ the length of cut along the X axis. In incremental mode specify the amount of feed across the part, in absolute mode specify the coordinate position of the end point of the cutting stroke.
Chapter 22 Single-Pass Turning Cycles After the G24 block is executed the control re-executes the cycle for any following block that commands axis motion (until the cycle is cancelled). The value of the axis word in that block is used to replace the parameter determined with that axis word in the original G24 block and the cycle is re-executed using these new parameters. Figure 22.9 applies only if programming X and Z as incremental values.
Chapter 22 Single-Pass Turning Cycles After this G24 block is executed, the control re-executes the cycle for any following block that contains an axis word (until the cycle is cancelled). The value of this axis word is used to replace the parameter determined with that axis word in the original G24 block and the cycle is re-executed using these new parameters. Example 22.4 Tapered Face Cutting G90G00X43.Z55.; G24X10.Z50.K-10.F10.; Z45.; Z40.; G00; Figure 22.10 Results of Example 22.
Chapter 22 Single-Pass Turning Cycles 22-14
Chapter 23 Grooving/Cutoff Cycles 23.0 Chapter Overview These two cycles are provided to perform grooving or cutoff operations: G76 Face Grooving Cycle G77 O.D. & I.D. Grooving Cycle This chapter reviews the following major topics: Topic: On page: Face grooving cycle 23-3 O.D. & I.D. cycle 23-6 Important: Descriptions in this chapter are written assuming the control is in the G18 plane and that plane has been defined as the ZX plane.
Chapter 23 Grooving/Cutoff Cycles Figure 23.
Chapter 23 Grooving/Cutoff Cycles Figure 23.2 Tool Path during a G77 O.D. Grooving Cycle Tool path, cutting feedrate Tool path, rapid feedrate No motion, for drawing clarification X Z K I I+e e I I+e X e I+e X e I+e I+e e D X e I+e I+e e e e I+e e I+e I e e e D D Z These cycles may also be used as cut off cycles. The tool infeeds into a piece of stock, as in grooving, except that it cuts all the way through the part.
Chapter 23 Grooving/Cutoff Cycles The format for this cycle is: G76X__Z__I__K__F__D__; Where : Is : X__ the location where the last groove is cut. If only one groove is to be cut do not program X. This may be programmed as either an incremental or absolute value. Remember that its value is also affected by diameter or radius modes (G07 and G08). Z__ the total depth of the groove from the Z coordinate position of the tool prior to the execution of the G76 block.
Chapter 23 Grooving/Cutoff Cycles Figure 23.3 G76 Face Grooving Cycle Parameters X K e X inc. X abs. Z abs. I Z inc. Z The retraction amount e is set in AMP by the system installer. Example 23.1 G76 Grooving Cycle Absolute Programming Incremental Programming G00X7.6Z5.3; G00X-1.8Z-1.2 G76X2.0Z3.6I-2.8K-0.8D0; G76X-5.6Z1.7I-2.8K-0.
Chapter 23 Grooving/Cutoff Cycles Figure 23.4 Results of G76 Grooving Cycle Example X 9.4 7.6 K=-0.8 e 4.8 I=-2.8 2.0 Z 3.6 23.2 O.D. & I.D. Grooving Cycle (G77) 5.3 6.5 The G77 O.D. & I.D. grooving cycle is typically used to cut multiple grooves in a workpiece or as a cut off cycle. When the cycle is performed the groove or cutoff is cut by infeeding the tool into the workpiece in steps to allow the removal of chips.
Chapter 23 Grooving/Cutoff Cycles The format for this cycle is: G77X__Z__I__K__F__D__; Where : Is : Z__ the location where the last groove is cut. If only one groove is to be cut do not program Z. This may be programmed as either an incremental or absolute value. X__ the total depth of the groove from the X coordinate position of the tool prior to the execution of the G77 block.
Chapter 23 Grooving/Cutoff Cycles Figure 23.5 G77 O.D. & I.D. Grooving Cycle Parameters X e I K Z abs. X inc. Z inc. X abs. Z Example 23.2 G77 O.D. & I.D. Grooving Cycle Used As a Cutoff Cycle 23-8 Absolute Programming Incremental Programming G00G90X42.Z56.; G00G91X-36.Z-9.; G77X19.Z21.I-8.K-14.D2.; G77X-23.Z-35.I-8.K-14.D2.
Chapter 23 Grooving/Cutoff Cycles Figure 23.
Chapter 23 Grooving/Cutoff Cycles 23-10
Chapter 24 Compound Turning Routines 24.0 Chapter Overview Compound turning routines are routines that make multiple passes across the workpiece to cut a specific contour into the workpiece. A set of blocks, called contour blocks, define the final contour shape of the workpiece. A calling block, containing one of the following G-codes, sets the parameters for the execution of the routine and defines what blocks are used as the contour blocks. Topic: On page: G73 O.D. and I.D.
Chapter 24 Compounding Turning Routines 24.1 O.D. and I.D. Roughing Routine (G73) The G73 contour turning routine is used to rough out the contour of a workpiece by making repetitive cuts parallel to the Z axis. A final pass may be made with this routine to cut parallel to the final contour of the workpiece. A finish allowance may be left on the workpiece to be removed later by a G72 finishing routine. This routine may be used in conjunction with Tool Tip Radius Compensation (TTRC).
Chapter 24 Compound Turning Routines Case 1: A Case 1 G73 roughing routine is defined when the workpiece contour has no pockets. The following constraints must be met in order to successfully perform a Case 1 contouring routine: The first block of the contour program must command motion in only the X axis. No Z axis motion is permitted in the first block of the contour program.
Chapter 24 Compounding Turning Routines Figure 24.2 Workpiece Finish Contour Case 1 and Case 2 (G73) Case 2 Case 1 X X Start Point Z Start Point Z The G73 block is programmed with this format: G73P__Q__U__W__I__K__D__R__F__S__T__; Where : Is : P__ the sequence number (N-word) of the first block in the set of contour blocks that define the final contour. Q__ the sequence number (N-word) of the last block in the set of contour blocks that define the final contour.
Chapter 24 Compound Turning Routines Where : Is : I K determine the amount of stock to be removed on the final pass of the routine. The actual amount of material removed on this final pass is equal to the average of the I and K parameters ((I+K)/2). It is not necessary to enter both of these parameters in the calling block. If only one is entered the control uses half of the entered parameter value. The final pass is optional and does not need to be programmed.
Chapter 24 Compounding Turning Routines Figure 24.3 Parameters for G73 Roughing Routine X Start Point (I+K)/2 D Shape after roughing Shape after roughing and final pass Workpiece finished shape R (U+W)/2 Z In Figure 24.3, the contour blocks for this routine must define all motions that would cut the workpiece finished shape. The first block of the contour blocks must be the tool path from the start point to the point where the initial roughing pass begins (point A to B in Figure 24.3).
Chapter 24 Compound Turning Routines The G73 roughing routine activates the Tool Tip Radius Compensation (TTRC) function regardless of whether it was active prior to the roughing routine. If TTRC was not active, the roughing routine uses the tool tip radius data of the previously programmed T-word. At the end of the roughing routine, TTRC is cancelled unless it was active prior to the roughing routine. In Example 24.1, the workpiece contour blocks are blocks N11 - N14. Example 24.
Chapter 24 Compounding Turning Routines Figure 24.4 Effect of Positive and Negative Finish Allowance Parameters C A A B U(+), W(+) C B X B A U(-), W(+) C U(+). W(-) Z B A C U(-), W(-) The workpiece contour in Figure 24.5 is illegal for the G73 roughing routine and may not be cut. When this routine is used to cut a contour the Z axis motion must either continuously increase or continuously decrease. No reversal is allowed on the Z axis. Figure 24.
Chapter 24 Compound Turning Routines G73 Tool Paths, Case 1 When the control executes a Case 1 G73 contouring path, these tool paths are generated: Figure 24.6 Tool Paths for Case 1 G73 Roughing Routine Cutting feed Rapid feed X (start point) D R D R D R Shape defined by workpiece contour blocks (I+K)/2 (U+W)/2 Final pass (Optional) Z In Figure 24.6: 1. The tool is moved from the start point parallel to the X axis, at a feedrate F, a distance D as programmed in the G73 block. 2.
Chapter 24 Compounding Turning Routines Figure 24.7 Tool Retraction in Case 1 G73 45° R X Z 45° R 4. Rapid traverse back along the X and Z axes to the coordinate that the last rough cut started from in step 2. 5. Move parallel to the X axis, at a feedrate F, a distance D as programmed in the G73 block. Steps 2 - 5 continue to repeat until the operation is aborted or the rough contour shape is completed.
Chapter 24 Compound Turning Routines Example 24.2 Case 1 G73 Roughing Routine N011 G00X80.Z150.; N012 G73P14Q18U.8W.8I.6K.6D18.R7.F100; N013 M30; N014 X20.; N015 Z110.; N016 X40.Z80.; N017 Z50.; N018 X70.Z40.; Figure 24.8 Results of Example 24.2 Start Point X 18 (D) 70 1.4 40 Z 20 Cutting feed Rapid feed 0 40 50 80 110 140 In Figure 24.8, the final pass over the workpiece does not remove all material from the final contour.
Chapter 24 Compounding Turning Routines Figure 24.9 Tool Paths for Case 2 G73 Roughing Routine (with pockets) Cutting feed Start Point Rapid feed R D (U+W+I+K)/2 Important: Figure 24.9 does not show the optional final pass being made. This is for drawing clarity. In Figure 24.9, after the roughing passes of one pocket have been completed, the control does not perform a normal retract move out of the pocket.
Chapter 24 Compound Turning Routines Figure 24.10 Tool Motion in Case 2 G73 Cutting feed Rapid feed Start point 8 6 R 5 4 D 1 7 2 3 8 8 8 In Figure 24.10, these tool paths are made: 1. The tool is moved from the start point to first contour point at feedrate F. This move must generate motion in both the X and Z axes. 2.
Chapter 24 Compounding Turning Routines 7. A rough cut is made at feedrate F, into the workpiece parallel to the X axis to the X coordinate of the last rough cut. Steps 2 - 7 continue to repeat until the operation is aborted or the rough contour shape is completed. The rough contour shape is completed when the thickness of the remaining material to be removed from the contour is equal to the sum of the finish allowance (U+W)/2 and the final pass allowance (I+K)/2.
Chapter 24 Compound Turning Routines Figure 24.11 Results of Example 24.3 Cutting feed X Rapid feed Start Point 100 80 10 60 40 (I+K+U+W)/2 1.4 20 20 24.2 Rough Facing Routine (G74) 40 60 80 100 120 140 Z The G74 rough facing routine is used to rough out the contour of a workpiece by making repetitive cuts parallel to the X axis. A final pass may be made with this routine to cut parallel to the final contour of the workpiece.
Chapter 24 Compounding Turning Routines Figure 24.12 Stock Removal in G74 Rough Facing Tool paths determined automatically Start point X Shape after roughing and final pass Workpiece finished shape Finishing allowance Z The G74 block has a P and Q parameter that call the sequence numbers (N-words) of the first and last blocks defining the final contour to be cut into the workpiece.
Chapter 24 Compound Turning Routines Case 2: A Case 2 G74 rough facing routine is defined when a workpiece contour contains a pocket. The following constraints must be met in order to successfully perform a Case 2 rough facing routine: The first block of the contour program must contain motion in both the X and Z axis (the move from the start point to the first contour point must have motion in both axes). The workpiece contour may increase or decrease along the Z axis after the first contour block.
Chapter 24 Compounding Turning Routines Where : Is : P__ the sequence number (N-word) of the first block in the set of contour blocks that define the final contour. Q__ the sequence number (N-word) of the last block in the set of contour blocks that define the final contour. U W determine the finishing allowance that is left on the part when the routine is completed. This finish allowance is typically removed later in the program when a G72 finishing routine block is executed.
Chapter 24 Compound Turning Routines Where : Is : R__ used to program the retract amount made after each rough facing pass. This retract amount is an incremental, radius value measured parallel to the Z axis. Case 1 operations retract at a 45 degree angle to the Z axis and Case 2 operations retract parallel to the Z axis. This does not affect the programmed value of R, as R is always measured parallel to Z.
Chapter 24 Compounding Turning Routines In Figure 24.14, the contour blocks for this routine must define all motions that would cut the workpiece finished shape. The first block of the contour blocks must be the tool path from the start point to the point where the initial roughing pass begins. The first block of the contour blocks may not be a rapid move (G00).
Chapter 24 Compound Turning Routines Figure 24.15 Effect of Positive and Negative Finish Allowance Parameters A B A U(+), W(+) B U(+), W(-) X C C C C Z U(-), W(+) B A U(-), W(-) A B In Figure 24.16, the workpiece contour is illegal for the G74 roughing routine and may not be cut. When this cycle is used to cut a contour the X axis motion must either constantly increase or constantly decrease. No reversal is allowed on the X axis. Figure 24.
Chapter 24 Compounding Turning Routines G74 Tool Paths, Case 1 When the control executes a Case 1 G74 rough facing routine the following tool paths are generated: Figure 24.17 Tool Paths for Case 1 G74 Rough Facing (I+K) 2 D D D X D start point Cutting feed R Rapid feed R Shape defined by workpiece contour blocks Final Pass (optional) (U+W)/2 Z In Figure 24.17: 1. The tool is moved from the start point parallel to the Z axis, at a feedrate F, a distance D as programmed in the G73 block. 2.
Chapter 24 Compound Turning Routines Figure 24.18 Tool Retraction in Case 1 G74 R 45° X R 45° Z 4. Rapid traverse back along the X and Z axes to the coordinate that the last rough cut started from (in step 2). 5. Move parallel to the Z axis, at a feedrate F, a distance D as programmed in the G74 block. Steps 2 - 5 continue to repeat until the operation is aborted or the rough contour shape is completed.
Chapter 24 Compounding Turning Routines Example 24.5 Case 1 G74 Rough Facing Routine N011 G00X80.Z130.; N012 G74P14Q19U6.W6.I10.K10.D10.R8.F10.S60; N013 M30; N014 Z40.; N015 X60.; N016 X40.Z60.; N017 Z80.; N018 X30.Z90.; N019 Z110.; N020 X20.Z130.; Figure 24.19 Results of Example 24.5 (D) 20 (K) 10 X (D) 20 (D) 20 (start point) Cutting feed 8 Rapid feed 8 80 60 40 0 40 60 30 80 90 20 110 Z 130 In Figure 24.
Chapter 24 Compound Turning Routines G74 Tool Paths, Case 2 If a pocket or multiple pockets are present in a workpiece face, it requires a Case 2 G74 rough facing routine. For Case 2, the control cuts each pocket separately, starting with the pocket closest to the beginning of the operation. Figure 24.20 shows the tool paths for a typical multiple pocket contour. The retract path used after each roughing pass is different than for Case 1 rough facing. Figure 24.
Chapter 24 Compounding Turning Routines Figure 24.21 Tool Motion in Case 2 G74 Start point 1 2 8 Cutting feed 7 Rapid feed D 8 6 3 R 8 4 5 8 In Figure 24.21, these tool paths are made: 1. The tool is moved from the start point to the first contour point at feedrate F. This move must generate motion in both the X and Z axes. 2.
Chapter 24 Compound Turning Routines 6. A rapid traverse is made back along the X and Z axes to the X coordinate that the last rough cut started from (in step 3) and a Z coordinate that is D distance above the Z coordinate of the last rough cut. 7. A rough cut is made at feedrate F, into the workpiece parallel to the Z axis to the Z coordinate of the last rough cut. Steps 2 - 7 continue to repeat until the operation is aborted or the contour shape is completed.
Chapter 24 Compounding Turning Routines Figure 24.22 Results of Example 24.6 X Cutting feed Rapid feed Start point 10 120 A (I+K+U+W)/2 1.
Chapter 24 Compound Turning Routines 24.3 Casting/Forging Roughing Routine (G75) In the G75 casting/forging roughing routine (also called pattern repeating routine), the control generates multiple cuts, each parallel to the workpiece final shape. Each cut is offset from the other an amount determined by the I, K and D parameters. Through this process, a shape similar to the finished contour is obtained when the routine is completed.
Chapter 24 Compounding Turning Routines The G75 block is programmed with this format: G75 P__ Q__ I__ K__ U__ W__ D__ F__ S__ T__; Where : Is : P__ The sequence number of the first block in the set of contour blocks that defines the finished workpiece shape. Q__ The sequence number of the last block in the set of contour blocks that defines the finished workpiece shape. U W Finish allowance. These parameters determine the finishing allowance that is left on the part when the routine is completed.
Chapter 24 Compound Turning Routines Figure 24.24 Pattern Repeating Routine Parameters Cutting feed Rapid feed X (start point) Note: Tool paths not to scale. Shape defined by workpiece contour blocks (I+K)/2 Finishing pass (U+W)/2 Z In Figure 24.24, the contour blocks for this routine must define all motions that would cut the workpiece finished shape and the tool path that connects the start point of the routine to the first block of the workpiece finished shape.
Chapter 24 Compounding Turning Routines Prevent this invalid cycle profile error by keeping the right portion of the following equation less than the radius of any arcs in your cycle profile. R ² p (I+U)2 + (K+W)2 + (tool radius) The same basic equation can apply to other contours. If the length of a block in the contour is less than the right portion of the above equation, you can get an “INVALID CYCLE PROFILE” error depending on your part contour.
Chapter 24 Compound Turning Routines The G75 routine can be programmed while the tool tip radius compensation mode (G41 or G42) is active. If tool tip radius compensation is active prior to the G75 block it remains active throughout the execution of the routine. The G75 roughing routine activates the Tool Tip Radius Compensation (TTRC) function regardless of whether it was active prior to the roughing routine.
Chapter 24 Compounding Turning Routines When the G75 routine is executed in single block mode, the execution of the routine stops after each complete iteration of the routine (a total of D iterations are made). Example 24.8 G75 Casting/Forging Roughing Routine N11 G00X100.Z175.; N12 G75P14Q20I8.K12.U5.W5.D3F.1S100; N13 M30; N14 G00 X20.Z125; N15 G01 Z85.; N16 G02X30.Z75.R10.; N17 G01X50.; N18 Z55.; N19 G02X60.Z35.R20.; N20 G01X80.; Figure 24.
Chapter 24 Compound Turning Routines 24.4 O.D. and I.D. Finishing Routine (G72) The G72 finish routine is normally executed after the completion of a contouring routine (G73, G74 or G75). With the G73, G74, and G75 routines a finish allowance is left on the workpiece if a U- and/or K-word is specified in the routine. The G72 routine is used to remove this finish allowance and cut the workpiece to within the specified tolerance of the actual workpiece finished shape.
Chapter 24 Compounding Turning Routines In Example 24.9, the workpiece contour blocks are blocks N11 - N14. Example 24.9 Typical G72 Block Followed by Blocks Defining Final Contour N005 G72P11Q14; . . . N010 M30.; N011 X24.; N012 X55.Z40.; N013 X65.Z35.; N014 X70.Z5.; The G72 routine can be programmed while the tool tip radius compensation mode (G41 or G42) is active. If tool tip radius compensation is active prior to the G72 block, it remains active throughout the execution of this routine.
Chapter 25 Thread Cutting 25.0 Chapter Overview The 9/Series control provides two methods of thread cutting: Single-pass thread cutting G33 and G34 blocks generate a single thread cutting pass. G33 can cut straight, tapered, face, multistart, and multiblock threads. G34 can cut thread passes of increasing or decreasing leads.
Chapter 25 Thread Cutting 25.1 Considerations for Thread Cutting When performing threading operations, remember: Emergency Stop - Pressing the emergency stop during threading causes all axes to come to a rapid stop. This likely causes damage to the part or tool and resuming the threading moves is not possible.
Chapter 25 Thread Cutting Axis feedrates - When threading, the speed of the cutting axis is determined by the controlling spindle speed and the thread lead through this equation: axis feedrate = (S) / (F inches per revolution) = (S) / (E threads per inch) = (S)(E inches per thread) Where : Is : S the actual speed of the controlling spindle (programmed spindle speed times the spindle speed override switch setting in percent) F threads per revolution or degree depending on the current active mode E
Chapter 25 Thread Cutting Figure 25.1 Angular versus Plunge Infeed Angular Infeed Cutting tool Plunge Infeed Cutting tool The G78 threading pass allows the selection of different infeed types by programming a P-word. If you use any of the other threading methods, it is necessary to insert a small Z move to generate an angular feed. Form Cut Threading - The auto threading cycles (G21 and G78) assume a sharp triangular tool. If you use a shaped-tip tool, the tool loading is affected.
Chapter 25 Thread Cutting Important: This feature may only be used with the G78 or G21 threading cycle. It is ignored if a G33 or G34 threading pass is being made. Using Thread Retract Enabled in PAL, thread retract lets you interrupt a thread cutting operation without damaging the thread by pressing . When the operation is interrupted, the control automatically performs a retract (by cutting a chamfer) out of the thread to prevent damage to the thread due to ringing.
Chapter 25 Thread Cutting 25.3 Single Pass Threading Mode (G33) The G33 thread cutting mode can cut straight, tapered, face, and multistart threads that have constant thread leads (use G34 to cut threads that do not have a constant lead). The G33 thread cutting mode is a mode, not a cycle and does not generate any extra motion blocks. This mode synchronizes the thread cutting tool motion with the spindle to allow programming multiple passes over the same threads. Figure 25.
Chapter 25 Thread Cutting Where : Is : X This parameter is the end point of the thread cutting move in the X axis. This parameter may be an incremental or absolute and radius or diameter value. If not present there must be a Z parameter. If an X parameter is present, it indicates either a face, tapered, or lead-in thread. When used in a G33 block without a Z parameter, a facing thread is made parallel to the X-axis at the Z axis position prior to the G33 block.
Chapter 25 Thread Cutting Example 25.1 Parallel Thread Cutting Thread lead: 5 threads/inch (.20 inch pitch) Depth of cut: .7 inch (after final pass) Number of cutting passes: 2 N1 M03 S50; N2 G00 X1.5 Z2.2; N3 X.9; N4 G33 Z.8 F.2; N5 Z.5 X1.2 N6 G00 X1.5; N7 Z2.2; N8 X.7; N9 G33 Z.8 F.2; N10 Z.5 X1.2 N11 G00 X1.5; N12 Z2.2; Figure 25.5 Parallel Thread Cutting Results from Example 25.1 X 1.5 1.2 N7 N12 N11 N6 N5 0.9 0.7 N2 N3 N4 N8 N10 N9 Z 0.5 0.8 2.2 1.
Chapter 25 Thread Cutting The programmed lead remains in effect until another thread lead value is programmed, the control is reset, or an M02 or M30 end of program block is executed. For tapered threads, the thread lead (determined by the F- or E-word) is applied along the axis that travels the greatest distance when cutting the thread. See Figure 25.6. Figure 25.
Chapter 25 Thread Cutting Example 25.2 Tapered Thread Cutting Thread lead: .125 threads/mm (8 mm pitch) Depth of cut: 1 mm (X direction) Number of cutting passes: 2 N1 M03 S30; N2 G77 G00 X20. Z4.; N3 G33 X48. Z-47. F8; N4 X52 Z-55; N5 G00 X60.; N6 Z4.; N7 X12.; (second pass) N8 G33 X40. Z-47.; N9 X52 Z-55; N10 G00 X60.; N11 Z4.; Figure 25.7 Results of Tapered Thread Cutting Example 25.
Chapter 25 Thread Cutting Example 25.3 Multistart Thread Cutting Thread lead: 2 threads/inch (.50 inch pitch) Depth of cut: .7 inch (after final pass) Number of cutting passes: 2 at 180 degrees apart N1 M03 S50; N2 G00 X1.5 Z2.2; N3 X.9; N4 G33 Z.8 E2. Q0; N5 Z.5 X1.2 N6 G00 X1.5; N7 Z2.2; N8 X.9; N9 G33 Z.8 E2. Q180; N10 Z.5 X1.2 N11 G00 X1.5; N12 Z2.2; Figure 25.8 Multistart Thread Cutting Results from Example 25.
Chapter 25 Thread Cutting 25.4 Single Pass Variable Lead Thread Cutting (G34) The G34 code programs the variable lead thread cutting mode. It is programmed almost identically to the G33 thread cutting mode with the addition of a K-word used to program the amount of lead variation per revolution. Figure 25.9 Variable Lead Thread Important: Do not re-program the G34 command in consecutive threading blocks.
Chapter 25 Thread Cutting Where : Is : E F This parameter may be entered by using either an E- or F-word. It represents the thread lead along the axis with the largest programmed distance to travel to make the thread cut. It is mandatory when cutting any threads. If the E-word is programmed, its value (sign ignored) is equal to the number of threads per inch or inches per thread (determined in AMP) regardless of whether inch or metric mode is active at the time.
Chapter 25 Thread Cutting Metric and inch Lead variation limits are indicated below: +/- 0.0001 to +/- 0.000001 to +/- 100.0000 mm/rev +/- 1.000000 inch/rev Example 25.4 Variable Lead Face Threading Using G34 N1G00G07X57.Z37.5F100; N2G91; N3G34X-47.5F.1K.071; N4G00Z10.; N5X47.
Chapter 25 Thread Cutting Figure 25.11 Results of Variable Lead Face Threading Example X 57.0 .1 mm/rev .171 mm/rev .526 mm/rev 57.0 Z 37.5 .171 mm/rev 47.5mm 9.5 Z 37.
Chapter 25 Thread Cutting 25.5 Single Pass Threading Cycle (G21) The G21 single pass threading cycle can be programmed to cut parallel or tapered fixed lead threads (variable lead threads may only be cut using a G34 block). This threading cycle performs a predetermined series of machining steps designated by a single program block. The two chamfering features (threading retract and threading chamfer) described on page 25-4 can also be used with this threading cycle.
Chapter 25 Thread Cutting When this cycle is executed: 1. The cutting tool rapids to the depth programmed with the X-word. 2. The thread cutting pass is made to the position programmed with the Z-word using a feedrate that generates the required lead programmed with the E- or F-word. If the Thread Chamfering feature was enabled before the cycle began executing, the control performs a chamfer just before reaching the programmed Z position. 3.
Chapter 25 Thread Cutting Figure 25.12 Results of G21 Straight Thread Cutting Example X 10.0 0.5 lead 4.8 4.3 Z 5.0 10.0 Taper Thread Cutting This format is for programming a single pass tapered threading cycle: G21X__Z__I__ F__ ; E Where : Is : X This parameter is the end point of the thread cutting move in the X axis. This parameter may be an incremental or absolute and radius or diameter value. This is the depth that the X axis moves to before starting the thread cutting pass.
Chapter 25 Thread Cutting Figure 25.13 G21 Taper Thread Cutting Parameters X X Inc. I X Abs. Z F Z Abs. Z Inc . When this cycle is executed: 1. The cutting tool rapids to the depth programmed with the X-word added to the I value. 2. The thread cutting pass is made to the position programmed with the X- and Z-words using a feedrate that generates the required lead programmed with the F- or E-word.
Chapter 25 Thread Cutting 4. The cutting tool is returned along the Z axis at a rapid feedrate to the Z axis position prior to the G21 block. 5. Program execution continues on to the next block. G21 is modal. Following passes need to contain only a new value for the infeed (X value). The other parameters programmed in the G21 block remains in effect. 25.6 O.D. & I.D.
Chapter 25 Thread Cutting Programming Multipass Thread Cutting Before programming the G78 threading routine, the cutting tool must be positioned to the point from which the routine is to be executed. This point is the end-point of each complete cycle of the threading routine’s execution. Use this format to program a multipass thread cutting routine: G78X__Z__K__D__ F__ E A__P__I__; Where : Is : X: This parameter is the coordinate value of the root (depth) of the thread.
Chapter 25 Thread Cutting If a straight thread is desired: enter a value of zero for this parameter or do not program the I-word in the block The control performs threading in either radius or diameter mode. Be aware that X values entered as a radius or a diameter value when entered. Z, I, K, and D, parameters are always entered as radius values regardless of the current mode. X and Z may also be programmed as incremental or absolute values.
Chapter 25 Thread Cutting Tool Infeed This multipass threading routine provides 4 different types of cutting tool infeed determined by a P-word in the threading block. These different infeeds are provided to allow operation with different types of cutting tools and materials. These different infeed types all move the end-point of the cutting tool when infeeding an amount referenced from the infeed reference point. P1 - Constant cutting volume, angular infeed along thread face.
Chapter 25 Thread Cutting Figure 25.
Chapter 25 Thread Cutting Figure 25.
Chapter 25 Thread Cutting 25-26
Chapter 26 Drilling Cycles 26.0 Chapter Overview This chapter covers the G-word data blocks in the drilling cycle group. The operations of the drilling cycles are explained on these pages: Page: Topic: Drilling cycles 26-1 Positioning and Hole Machining Axes 26-4 Parameters 26-7 Drilling Cycle Operations 26-8 Altering Drilling Cycle Operating Parameters 26-38 Fixed Drilling Cycle Examples 26-40 WARNING: The cycles described in this chapter can be used with live tooling.
Chapter 26 Drilling Cycles Table 26.A Drilling Cycles 26-2 G-code Application Tool Movement Operation At Hole Bottom Retraction Movement G80 Cancel Or End Fixed Cycle N/A N/A N/A G81 Drilling Cycle, No Dwell/Rapid Out Feed Retract Rapid Traverse G82 Drilling Cycle, Dwell/Rapid Out Feed Dwell / Retract Rapid Traverse G83 Deep Hole Drilling Cycle Intermittent Feed Retract Rapid Traverse G83.
Chapter 26 Drilling Cycles In general, drilling cycles consist of the following operations (see Figure 26.1): Figure 26.
Chapter 26 Drilling Cycles 26.2 Positioning and Hole Machining Axes This section assumes that the programmer can determine the hole machining axis using the plane select G-codes (G17, G18, G19). Refer to the system installer’s documentation to make sure that a specific axis has not been selected in AMP to be the hole machining axis. G-codes G17, G18, or G19 determine the plane, the hole machining axis, and the positioning axes. The two axes that define the selected plane are used as positioning axes.
Chapter 26 Drilling Cycles Figure 26.2 shows typical drilling cycle motions in absolute (G90) or incremental (G91) mode. Note the changes in how the R point and Z level are referenced. Figure 26.
Chapter 26 Drilling Cycles Figure 26.3 shows the two different modes available for selecting the return level in the Z axis after the hole has been drilled. These two modes are selected with G98 (which returns to the same level the cycle started at) and G99 (which returns to the level defined by the R point). Figure 26.
Chapter 26 Drilling Cycles 26.3 Parameters This section provides a detailed explanation of each parameter you can program for the drilling cycles. Some parameters are not valid with all cycles; see the specific description of each cycle. To alter drilling cycle operation parameters, see section 26.5. These drilling cycle parameters are described below: X__Y__Z__R__ I__J__K__ P__F__L__Q__D__S__; Where : Is : X specifies the location of the hole position in the selected plane.
Chapter 26 Drilling Cycles 26.4 Drilling Cycle Operations Drilling cycles G83.1, G84.1, G86.1 and G81-G89 are modal, which means they remain active until you program a G-code that cancels the drilling cycle. Certain drilling cycles can, therefore, be repeated at different positions without having to re-program all the parameters associated with a given operation.
Chapter 26 Drilling Cycles (G81): Drilling Cycle, No The format for the G81 cycle is: Dwell/Rapid Out G81X__Z__R__F__L__; Where : Is : X specifies location of the hole. Z defines the hole bottom. R defines the R point level. F defines the cutting feedrate. L defines the number of times the drilling cycle is repeated. See page 26-7 for a detailed description of these parameters. Important: The programmer or operator must start spindle or live tool rotation. Figure 26.
Chapter 26 Drilling Cycles In the G81 drilling cycle, the control moves the axes in this manner: 1. The tool rapids to the initial point level above the hole location. 2. The drilling tool then rapids to the R point level, slows to the programmed cutting feedrate and begins the drilling operation. 3. The drilling tool continues to drill at the programmed feedrate until it reaches the depth of the hole as programmed with the Z-word. 4.
Chapter 26 Drilling Cycles Figure 26.5 G82: Drilling Cycle, Dwell/Rapid Out Cutting feed Rapid feed R point level initial point level Hole bottom 1 4 3 2 Z R Dwell at hole bottom 5 In the G82 drilling cycle, the control moves the axes in this manner: 1. The tool rapids to initial point level point above the hole location. 2. The drilling tool then rapids to the R point level, slows to the programmed cutting feedrate and begins the drill operation. 3.
Chapter 26 Drilling Cycles (G83): Deep Hole Drilling Cycle The format for the G83 cycle is: G83X__Z__R__Q__F__L__; Where : Is : X specifies location of the hole. Z defines the hole bottom. R defines the R point level. Q defines the infeed amount for each step into the hole. F defines the cutting feedrate. L defines the number of times the drilling cycle is repeated. See page 26-7 for a detailed description of these parameters.
Chapter 26 Drilling Cycles In the G83 drilling cycle, the control moves the axes in this manner: 1. The tool rapids to initial point level above the hole location. 2. The drilling tool then rapids to the R point level, slows to the programmed cutting feedrate and begins the deep hole drilling operation. 3. During the drilling operation, the control infeeds the drilling tool by an amount Q, as programmed in the G83 block. 4. The drilling tool retracts at a rapid feedrate to the R point level. 5.
Chapter 26 Drilling Cycles Figure 26.7 G83.1: Deep Hole Peck Drilling Cycle with Dwell R point level Initial point level 1 Hole bottom 2 Q 3 4 Q d R 5 6 d 7 Moves to hole bottom when Q is larger than remaining depth In the G83.1 peck drilling cycle, the control moves the axes in this manner: 26-14 1. The tool rapids to the initial point level above the hole location. 2.
Chapter 26 Drilling Cycles 6. After the drilling tool retracts an amount d, it then resumes drilling at the cutting feedrate to a depth d + Q. This retraction and extension continues until the drilling tool reaches the depth of the hole as programmed with the Z-word in the drilling cycle block. 7. The drilling tool then retracts at a rapid feedrate to the initial point level as determined by G98.
Chapter 26 Drilling Cycles Figure 26.8 G84: Right-Hand Tapping Cycle Cutting feed Rapid feed R point level Initial point level 1 4 Hole bottom Spindle or live tool rotation direction reversed at hole bottom 3 Z 5 R 2 6 7 Spindle or live tool rotation in the forward direction In the G84 right-hand tapping cycle, the control moves the axes in this manner: CAUTION: The programmer or operator must set the direction of spindle rotation for tap-in.
Chapter 26 Drilling Cycles 4. If a value was programmed for the P parameter, the threading tool dwells after it reaches the bottom of the hole, and after the spindle has been commanded to reverse. The spindle or live tool reverses to the counterclockwise direction. 5. The threading tool retracts at the cutting feedrate to the R point. 6. If a value was programmed for the P parameter, the threading tool dwells after it reaches the R point.
Chapter 26 Drilling Cycles Important: When programming a G84 tapping cycle, remember: the programmer or operator must start spindle or live tool rotation override usage - the control ignores the feedrate override switch and clamps override at 100 percent during tapping, the feedrate override switch and the feedhold feature are both disabled; cycle stop is not acknowledged until the end of the return operation Figure 26.9 G84.
Chapter 26 Drilling Cycles CAUTION: The programmer or operator must set the direction of spindle rotation for tap-in. The control forces the proper spindle direction for the tap-out, but uses the programmed spindle direction for the tap-in. 1. The tool rapids to the initial point level above the hole location. 2. The threading tool then rapids to the R point level, slows to the programmed cutting feedrate and begins the tapping operation. 3.
Chapter 26 Drilling Cycles (G84.2): Right-Hand Solid-Tapping Cycle Use this cycle to cut right-handed threads. The format for the G84.2 cycle is: G84.2X__Z__R__F__L__Q__D__S__; Where : Is : X specifies location of the hole. Z defines the hole bottom. R defines the R point level. F defines the thread lead along the drilling axis (Z in this manual). It is mandatory and modal in any subsequent solid tapping cycle blocks until a new F-word is programmed.
Chapter 26 Drilling Cycles on a dual-process lathe, both processes can be in solid-tapping mode at the same time assuming that they have separate controlling spindles you must disable CSS before performing solid tapping; an attempt to execute the tap phase of a solid-tapping cycle with CSS results in a decode error cycle stop and feedrate override are acknowledged throughout the cycle, but can be disabled by G63 you can use active reset to abort the cycle after the cycle stop request has been acknowledged
Chapter 26 Drilling Cycles In the G84.2 right-hand solid-tapping cycle, the control moves the axes in this manner: 1. The tool rapids to the tapping position above the hole location. 2. The threading tool then rapids to the R point. 3. The control either orients or stops the spindle. If a Q-word was programmed: the control: yes orients the spindle no stops the spindle 4.
Chapter 26 Drilling Cycles (G84.3): Left-Hand Solid-Tapping Cycle Use this cycle to cut left-handed threads. The format for the G84.3 cycle is: G84.3X__Z__R__F__L__Q__D__S__; Where : Is : X specifies location of the hole. Z defines the hole bottom. R defines the R point level. F defines the thread lead along the drilling axis (Z in this manual). It is mandatory and modal in any subsequent solid tapping cycle blocks until a new F-word is programmed.
Chapter 26 Drilling Cycles on a dual-process lathe, both processes can be in solid-tapping mode at the same time assuming that they have separate controlling spindles you must disable CSS before performing solid tapping; an attempt to execute the tap phase of a solid-tapping cycle with CSS results in a decode error cycle stop and feedrate override are acknowledged throughout the cycle, but can be disabled by G63 you can use active reset to abort the cycle after the cycle stop request has been acknowledged
Chapter 26 Drilling Cycles In the G84.3 left-hand solid-tapping cycle, the control moves the axes in this manner: 1. The tool rapids to the tapping position above the hole location. 2. The threading tool then rapids to the R point. 3. The control either orients or stops the spindle. If a Q-word was programmed: the control: yes orients the spindle no stops the spindle 4.
Chapter 26 Drilling Cycles See page 26-7 for a detailed description of these parameters. Important: The programmer or operator must start spindle or live tool rotation. Figure 26.10 G85: Boring Cycle (Without Dwell, Feed Out) Cutting feed Rapid feed R point level Initial point level Hole bottom 1 3 2 4 5 In the G85 boring cycle, the control moves the axis in this manner: 1. The tool rapids at the initial point level, to the hole location. 2.
Chapter 26 Drilling Cycles (G86): Boring Cycle, Spindle Stop/Rapid Out The format for the G86 cycle is: G86X__Z__R__P__F__L__; Where : Is : X specifies location of the hole. Z defines the hole bottom. R defines the R point level. P defines the dwell period at hole bottom. F defines the cutting feedrate. L defines the number of times the drilling cycle is repeated. See page 26-7 for a detailed description of these parameters.
Chapter 26 Drilling Cycles In the G86 drilling cycle, the control moves the axis in this manner: 1. The tool rapids to the initial point level above the hole location. 2. The cutting tool then rapids to the R point level, slows to the programmed cutting feedrate and begins the boring operation. 3. The cutting tool bores at the programmed feedrate until it reaches the depth of the hole as programmed with the Z-word. 4.
Chapter 26 Drilling Cycles Figure 26.12 G86.1: Boring Cycle, Tool Shift Hole bottom Bored hole R point level Shift Q Spindle orient after dwell at Z point level to position tool for removal Initial point level Cutting feed 1 Rapid feed 4 Shift 3 2 Spindle or live tool oriented and tool shifted 8 Shift Q 7 5 6 In the G86.1 boring cycle, the control moves the axes in this manner: 1. The tool rapids to the initial point level above the hole location. 2.
Chapter 26 Drilling Cycles The shift direction is determined by two possible methods: Method I This shift method is a single-axis shift. The direction and axis for the shift is set in AMP by your system installer or can be altered using the drilling cycle parameter table. See page 26-38. the direction of the axis is specified as + or -. the feedrate using this shift method is always rapid traverse. the Q-word shift amount is always interpreted as a positive value; a negative Q-word is not allowed.
Chapter 26 Drilling Cycles When using Method II, remember: the generated move is a single linear move and executes at (G87): Back Boring Cycle The format for the G87 back boring cycle is: G87X__Z__ I__J__K__ Q__ R__F__L__; Where : Is : X specifies location of the hole. Z defines the Z point level. The Z point level in this case is the top of the hole that is being cut by the back boring operation. Q or I, J, K defines the tool shift amount.
Chapter 26 Drilling Cycles Figure 26.13 G87: Back Boring Cycle Cutting feed Rapid feed Hole bottom Z point level Initial point level Spindle or live tool rotation forward 5 1 Spindle or live tool orientation 6 8 7 Spindle or live tool orientation 2 4 3 In the G87 back boring cycle, the control moves the axes in this manner: 1. The tool rapids to the initial point level above the hole location. 2.
Chapter 26 Drilling Cycles Method I This shift method is a single axis shift. The direction and axis for the shift is set in AMP by the system installer or can be altered using the drilling cycle parameter table. See page 26-38.
Chapter 26 Drilling Cycles 6. After reaching the Z depth, the spindle or live tool rotation stops so that the control can re-orient the back boring tool to the position specified in AMP. The back boring tool is shifted a third time, in the same manner as in step 2, so that it is again “off-center” and can be removed through the existing hole. (G88): Boring Cycle, Spindle Stop/Manual Out 7.
Chapter 26 Drilling Cycles Figure 26.14 G88: Boring Cycle, Spindle Stop/Manually Out Cutting feed Rapid feed Manual operation R point level Initial point level Hole bottom 1 Z 3 4 Spindle or live tool stops at hole bottom after dwell 5 Cycle start 2 R 6 7 Spindle rotation in the forward direction In the G88 boring cycle, the control moves the axis in this manner: 1. The tool rapids to the initial point level above the hole location. 2.
Chapter 26 Drilling Cycles 6. The boring tool is then retracted at a rapid feedrate to initial point level, as determined by G98. 7. At this point, the rotation of the spindle or live tool changes to the clockwise direction. When the single block function is active, the control stops axis motion after steps 1, 2 and 5. (G89): Boring Cycle, Dwell/Feed Out The operations in G89 are identical to as those of the G85 boring cycle with the exception that the control executes a dwell at hole bottom.
Chapter 26 Drilling Cycles Figure 26.15 G89: Boring Cycle, Dwell/Feed Out Cutting feed Rapid feed R point level Initial point level Hole bottom 1 4 3 Z 2 R Dwell 5 6 In the G89 boring cycle, the control moves the axes in this manner: 1. The tool rapids to initial point level above the hole location. 2. The boring tool then rapids to the R point level, slows to the programmed cutting feedrate and begins the boring operation. 3.
Chapter 26 Drilling Cycles 26.5 Altering Drilling Cycle Parameters The system installer determines many parameter for the drilling cycles in AMP. For details on these cycles, see page 26-4 or chapters 22 -- 25. These 3 parameters may also be changed by the operator by using the Drilling Cycle Parameter screen: G83.1 Deep Hole Peck Drilling Cycle retract amount - This parameter determines the value of “d.
Chapter 26 Drilling Cycles 2. Press the {PRGRAM PARAM} softkey. (softkey level 2) 3. PRGRAM AMP PARAM DEVICE MONISETUP TOR PTOM SI/OEM SYSTEM TIMING TIME PARTS Press the {DRLCYC PARAM} softkey. The Drilling Cycle Parameter screen is displayed. Figure 26.16 shows a typical Drilling Cycle Parameter screen. (softkey level 3) ZONE F1-F9 LIMITS DRLCYC PARAM INTERF CHECK Figure 26.16 Drilling Cycle Parameter Screen ENTER VALUE: DRILLING CYCLE PARAMETERS G83.
Chapter 26 Drilling Cycles 4. From this screen select the parameter that it is desired to change by pressing the up or down cursor keys. The selected parameter is shown in reverse video. 5. There are two options: To replace the current value of the parameter with a new value, key in the new value on the input line of the CRT and press the {REPLCE VALUE} softkey. The new value replaces the old value.
Chapter 26 Drilling Cycles Example 27.3 Programming G83, Deep Hole Drilling Cycle in Absolute Mode N10 G90 G00 X5 Y12 Z0 G17 F200; N20 G83 X1 Y10 Z-5 R-2 Q1.5; N30 X5 Y5 Z-8; N40 X9 Y10 Z-5; N50 M30; Figure 26.17 Result of Example 27.2 and Example 27.
Chapter 26 Drilling Cycles 26-42
Chapter 27 Skip and Gauge Probing Cycles 27.0 Chapter Overview This chapter describes the external skip and gauging functions available on the 9/Series control. External skip functions are motion generating G-code blocks that can be aborted when the control receives an external signal through the PAL program. Gauging functions are similar to the external skip functions except that the axis coordinates (at the time the external signal is received) can be used to modify the tool offset table.
Chapter 27 Skip and Gauge Probing Cycles CAUTION: We do not recommend using a skip block from any fixed cycle block (such as drilling or turning). If you do choose to execute a skip block in a fixed cycle mode, be aware that the block that is skipped when the trigger occurs can be a cycle generated block. If this is the case the cycle will continue normal execution skipping only the portion of the cycle that was executing when the trigger occurred.
Chapter 27 Skip and Gauge Probing Cycles Important: The move that immediately follows a G31 series external skip block cannot be a circular move. The coordinates of the axes when the external skip signal is received are available as the paramacro system parameters #5061--#5066 (work coordinate system) and #5071--#5076 (machine coordinate system). These values will have been adjusted to compensate for the probe tip radius if a radius compensation value was entered.
Chapter 27 Skip and Gauge Probing Cycles The format for any G37 skip blocks is: G37 Z__ F__; Where : Is : G37 Corresponds to any of the G-codes in the G37 series. Use the one that is configured to respond to the current skip signal device that is being used. X, Z The axis on which the length offset measurement is to be taken is specified here as either X or Z. Only one axis may be specified in a G37 block.
Chapter 27 Skip and Gauge Probing Cycles Important: The move that immediately follows a G37 series skip block cannot be a circular move. The system installer determines in AMP if the new value is added to or replaces the old value in the table. The system installer also determines in AMP what gauge cycles alter which tool offset tables, geometry, or wear. The control automatically compensates for probe radius and length when calculating tool offset changes if these probe parameters have been entered.
Chapter 27 Skip and Gauge Probing Cycles Figure 27.1 Typical Tool Gauging Configurations Tool Tool Tool -X -X +Z Probe radius Probe Probe Probe radius Case 1 Case 2 Probe length Probe radius Probe Case 3 Figure 27.1 illustrates 3 typical tool gauging configurations. All 3 cases assume that the probe is at a known, fixed point on the machine. In Case 1, the Z axis tool offset length is being gauged, while in Case 2, the X axis tool offset length is being gauged.
Chapter 28 Paramacros 28.0 Chapter Overview The Paramacrost feature is similar to a subprogram with many added features.
Chapter 28 Paramacros 28.1 Parametric Expressions It may be necessary for mathematical expressions to be evaluated in a complex paramacro. This requires that some form of mathematical equation be written in a paramacro block. The following is a discussion of the operators and function commands available for use on the control. These operators and function commands are valid in any block within a program, subprogram, paramacro, or MDI program. 28.1.
Chapter 28 Paramacros Example 28.1 Mathematical Operations Expression entered Result 12/4*3 9 12/[4*3] 1 12+2/2 13 [12+2]/2 7 12-4+3 11 12-[4+3] 5 All logical operators have the format of: A logical operator B where A and B are numerical data or a parameters with a value assigned. If B is negative in the above format, an error will occur. If A is negative, the absolute value of A is used in the operation and the sign is attached to the final result.
Chapter 28 Paramacros 28.1.2 Mathematical Function Commands This subsection lists the basic mathematical functions that are available on the control and their use. Use these functions to accomplish mathematical operations that are necessary to evaluate the trigonometric and other complex mathematical equation such as rounding off, square roots, logarithms, exponent, etc. NO TAG lists the basic functions that are available and their meanings. Table 28.
Chapter 28 Paramacros Example 28.3 Format for Functions SIN[2] This evaluates the sine of 2 degrees. SQRT[14+2] This evaluates the square root of 16. SIN[SQRT[14+2]] This evaluates the sine of the square root of 16. LN[#2+4] This evaluates the logarithm of the value of parameter #2 plus 4. Example 28.4 Mathematical Function Examples Expression Entered Result SIN[90] 1.0 SQRT[16] 4.0 ABS[-4] 4.0 BIN[855] 357 BCD[357] 855 ROUND[12.5] 13.0 ROUND[12.4] 12.0 FIX[12.7] 12.0 FUP[12.
Chapter 28 Paramacros 28.1.3 Parametric Expressions as G- or M- Codes You can use parametric expressions to specify G-codes or M-codes in a program block. For example: G#1 G#100 G#500 M#1 M#100 M#500; G#520 G[#521-1] G[#522+10] M#520 M[#522+1] M[#522+10]; When using a parametric expression to specify a G-- or M-code, remember: When specifying more than one G-- or M-code in a block from the same modal group, the G-- or M-code closest to the End-of-Block of that block is the one activated.
Chapter 28 Paramacros 28.2 Transfer of Control Commands Use transfer of control commands to alter the normal flow of program execution. Normally the control executes program blocks sequentially. By using control commands, the programmer can alter this normal flow of execution and transfer execution to a specific block or begin looping (executing the same set of blocks repetitively). Important: Transfer of control commands call a block by its N number.
Chapter 28 Paramacros Program a condition between the [ and ] brackets in this format: [A EQ B] where A and B represent some numerical value. The values for A and B can be in the form of some mathematical equation or in the form of a paramacro parameter. Example 28.6 Evaluation of Conditional Expressions Expression Evaluation [6.03 EQ 6.0301] FALSE [6.03 NE 6.0301] TRUE [2.5 GT 2.5] FALSE [2.5 LT 2.51] TRUE [2.51 GE 2.5] TRUE [2.5 LE 2.5] TRUE [[2.
Chapter 28 Paramacros Example 28.7 Unconditional GOTO N1...; N2...; N3GOTO5; N4...; N5...; N6...; /N7GOTO1; In Example 28.7, execution continues sequentially until block N3 is read; then execution transfers to block N5 and again resumes sequential execution to block N6. If optional block skip 1 is off, block N7 will transfer execution back to block N1. Conditional IF-GOTO The conditional IF-GOTO command is dependent on whether a mathematical condition is true.
Chapter 28 Paramacros When block N2 is read, parameter #3 is compared to the value -1.5. If the comparison is true, then blocks N3 and N4 are skipped, and execution continues on from block N5. If the comparison is false, then execution continues to block N3. When block N6 is read, parameter #4 is compared to the value 3. If the comparison is true, then execution is transferred to block N1; if it is false, execution continues to block N7. 28.2.
Chapter 28 Paramacros Use this format for the WHILE-DO-END command: WHILE [ (condition) ] DO m; ; ; ; END m; Where : Is : (condition) some mathematical condition. This condition is tested by the control to determine if it is true or false. m an identifier used by the control to relate a DO block with an END block. The value of m must be the same for the DO as it is for the corresponding END. This value can be either 1, 2, or 3.
Chapter 28 Paramacros Example 28.10 Nested WHILE DO Commands N1#1=1; N2WHILE[#1LT10]DO1; N3#1=[#1+1]; N4WHILE[#1EQ2]DO2; N5...; N6END2; N7END1; N8...; In Example 28.10, blocks N2 through N7 are repeated until the condition in block N2 becomes false. Within DO loop 1, DO loop 2 will be repeated until the condition in block N4 becomes false. 28.3 Parameter Assignments The following subsections describe assigning different paramacro parameter values and how these parameters are used in a paramacro.
Chapter 28 Paramacros Local parameters are used in a specific macro to perform calculations and axis motions. After their initial assignment, these parameters can be modified within any macro at the same nesting level. For example macro O11111 called from a main program has 33 local parameter values to work with (#1 to #33). All macros called from the main program, and nested at the same level, use the same local parameters with the same values unless they are initialized in that macro.
Chapter 28 Paramacros Example 28.11 Assigning Using More Than One I, J, K Set G65P1001K1I2J3J4J5; The above block sets the following parameters: parameter #6 = 1 parameter #7 = 2 parameter #8 = 3 parameter #11 = 4 parameter #14 = 5 If the same parameter is assigned more than one value in an argument, only the right-most value is stored for the parameter. Example 28.12 Assigning the Same Parameter Twice G65P1001R3.1A2R-0.5 The above block sets the following parameters: parameter #1 = 2.
Chapter 28 Paramacros 28.3.2 Common Parameters The common parameters refer to parameter numbers 100 to 199 and 500 to 999 for all 9/Series controls except for the 9/240, which allows 100 to 199 and 500 to 699. The common parameters are assigned through the use of a common parameter table as described on page 28-38. Common parameters are global in nature. This means that the same set of parameters can be called by any program, macro, subprogram, or MDI program.
Chapter 28 Paramacros Table 28.
Chapter 28 Paramacros Table 28.D (continued) System Parameters System Parameter Parameter # Page 5731 to 5743 Home Marker Distance 28-31 5751 to 5763 Home Marker Tolerance 28-31 1 These parameters may only have their value received (read-only) 2 These parameters may only have their value changed (write-only) #2001 to 9499 Tool Offset Tables These parameters may be changed or simply read through programming.
Chapter 28 Paramacros When the control executes this block, a cycle stop is performed and the message “SEE PART PROGRAM FOR MACRO STOP MESSAGE” is displayed on line 1 of the CRT. This is intended to point out to the operator an important comment in the program block that assigns a value to parameter 3000 (see chapter 10 on comment blocks). For example, programming #3000=.
Chapter 28 Paramacros #3003 Block Execution Control 1 Use this parameter to control whether the control ignores single-block mode and to control when M-codes are executed in a block. The value of this parameter ranges from 0 to 3, and it is a write-only parameter.
Chapter 28 Paramacros #3006 Program Stop With Message Use this parameter to cause a cycle stop operation and display a message on line 1 of the CRT. Any block that assigns a new value to the parameter 3006 will result in a cycle stop. Any decimal value may be assigned to this parameter the value of which is not used. When the control executes this block, a cycle stop is performed and the message “SEE (MESSAGE) IN PART PROGRAM BLOCK” is displayed on line 1 of the CRT.
Chapter 28 Paramacros This parameter reflects both the programmed and front-panel (external mirror) status of mirroring on the axes. #4001 to 4120 Modal Information These are read-only parameters. They indicate the value of a modal program word. NO TAG shows the modal program word that applies to the given parameter number. Table 28.
Chapter 28 Paramacros #5001 to 5012 Coordinates of End Point These parameters are read-only. They correspond to the coordinates of the end point (destination) of a programmed move. These are the coordinates in the work coordinate system.
Chapter 28 Paramacros #5041 to 5052 Machine Coordinate Position These parameters are read-only. They correspond to the coordinates of the cutting tool in the machine (absolute) coordinate system.
Chapter 28 Paramacros #5071 to 5079 or #5561 to 5562 Skip Signal Position Machine Coordinate System These parameters are read-only. They correspond to the coordinates of the cutting tool when a skip signal is received to PAL from a probe or other device such as a switch. These are the coordinates in the machine (absolute) coordinate system.
Chapter 28 Paramacros #5081 to 5089 or #5581 to 5592 Active Tool Length Offsets These are read-only parameters. They correspond to the currently active tool length offsets (see chapter 20). 5081 Current axis 1 tool length offset. 5087 Current axis 7 tool length offset. 5082 Current axis 2 tool length offset. 5088 Current axis 8 tool length offset. 5083 Current axis 3 tool length offset. 5089 Current axis 9 tool length offset. 5084 Current axis 4 tool length offset.
Chapter 28 Paramacros The system installer determines in AMP the name (or word) that is used to define the axis. The following error of a system constantly changes. You can use this parameter to take a “snapshot” of the following error, but the value that is read may not the current following error of the system. #5201 to 5212 External Offset Amount These parameters are read or write. They correspond to the current value set in the work coordinate table for the external offset (see chapter 3).
Chapter 28 Paramacros 5241 G55 Axis 1 Coordinate 5341 G59.1 Axis 1 Coordinate 5242 G55 Axis 2 Coordinate 5342 G59.1 Axis 2 Coordinate 5243 G55 Axis 3 Coordinate 5343 G59.1 Axis 3 Coordinate 5244 G55 Axis 4 Coordinate 5344 G59.1 Axis 4 Coordinate 5245 G55 Axis 5 Coordinate 5345 G59.1 Axis 5 Coordinate 5246 G55 Axis 6 Coordinate 5346 G59.1 Axis 6 Coordinate 5247 G55 Axis 7 Coordinate 5347 G59.1 Axis 7 Coordinate 5248 G55 Axis 8 Coordinate 5348 G59.
Chapter 28 Paramacros 5301 G58 Axis 1 Coordinate 5302 G58 Axis 2 Coordinate 5303 G58 Axis 3 Coordinate 5304 G58 Axis 4 Coordinate 5305 G58 Axis 5 Coordinate 5306 G58 Axis 6 Coordinate 5307 G58 Axis 7 Coordinate 5308 G58 Axis 8 Coordinate 5309 G58 Axis 9 Coordinate 5310 G58 Axis 10 Coordinate 5311 G58 Axis 11 Coordinate 5312 G58 Axis 12 Coordinate The system installer determines in AMP the name (or word) that is used to define the axis.
Chapter 28 Paramacros #5651 to 5662 Deceleration Ramps for Linear Acc/Dec Mode These parameters are read only. They correspond to the active deceleration ramps in Linear Acc/Dec mode. You can set these parameters by programming a G48.2 in your part program block. Control Reset, Program End (M02/M03), or G48 will reset these values to their default AMP values. For more information about programming G48.x codes, refer to chapter 18 in your 9/Series CNC Operation and Programming Manual.
Chapter 28 Paramacros #5691 to 5702 Deceleration Ramps for S- Curve Acc/Dec Mode These parameters are read only. They correspond to the active deceleration ramps in S--Curve Acc/Dec mode. You can set these parameters by programming a G48.4 in your part program block. Control Reset, Program End (M02/M03), or G48 will reset these values to their default AMP values. For more information about programming G48.x codes, refer to chapter 18 in your 9/Series CNC Operation and Programming Manual.
Chapter 28 Paramacros #5731 to 5743 Home Marker Distance These parameters are read only. They correspond to the current home marker distance. These parameters will contain the distance to marker calculated when the axis stopped after the home switch went false during the last homing operation.
Chapter 28 Paramacros Input Flags: There are 4-integer or 3-integer and 32-bit pattern input parameters available. The part program may only read the values assigned to these parameters; it may not write values to them. The paramacro input parameters available to the part programmer are: #1000 -- #1031 and #1040 -- #1071 These paramacro PAL parameters are used to display the binary equivalent of the integer assigned to #1032.
Chapter 28 Paramacros Output flags should not be used as Input flags unless absolutely necessary. This is because the operator/programmer has the ability to inadvertently write data to the Output flags, whereas the Input flags cannot be written to from the control. Output flags are broken into four 32-bit words. The part programmer can only assign or read the values of to these flags as integers with the exception of parameter #1132 which may be assigned as an integer or as a bit pattern.
Chapter 28 Paramacros All shared dual-process parameters are saved at power-down. This means that they retain their value even after power to the control is lost. Synchronization Problems with Shared Dual-Process Parameters The programmer must concern himself with timing when changing dual process paramacro parameters that are used in more than one process.
Chapter 28 Paramacros Table 28.
Chapter 28 Paramacros To enter a value for a parameter # using an argument, enter the word corresponding to the desired parameter number in a block that calls a paramacro (for legal argument locations, see specific formats for calling the macro) followed by the value to assign that parameter. For example: G65P1001A1.1 B19; assigns the value of: 1.1 to local parameter #1 in paramacro 1001 19 to local parameter #2 in paramacro 1001 You can specify arguments as any valid parametric expression.
Chapter 28 Paramacros Example 28.15 Assigning Parameters: #100=1+1; #100=5-3; #100=#3; #100=#7+1; #100=#100+1; You can also assign multiple paramacro parameters in a single block. In a multiple assignment block, each assignment is separated by a comma. For example: #1=10,#100=ROUND[#2+#3],#500=10.0*5; If you use multiple assignments in the same block, remember: You can enter as many assignments as can be typed into one block (127 characters maximum).
Chapter 28 Paramacros Direct Assignment Through Tables Use this feature to view or set common parameters and view local parameters. Assignment through tables is generally used to edit common parameters. To edit the values of the common parameters or view the local parameters, follow these steps. 1. Press the {MACRO PARAM} softkey. (softkey level 1) 2.
Chapter 28 Paramacros If viewing the local parameter table, do not continue to step 3. If editing one of the common parameter tables, move on to step 3. (softkey level 3) LOCAL PARAM 3. COM-1 PARAM COM-2A COM-2B PARAM PARAM Select a parameter to change by moving the cursor to the desired parameter number. Note that the selected parameter is shown in reverse video. Move the cursor by an entire page by pressing the up or down cursor key while holding down the [SHIFT] key.
Chapter 28 Paramacros 5. If the {COM-2A PARAM} softkey has been pressed (in step 2), additional softkeys will be available to alter the parameter name. Select and complete the appropriate step to alter the common parameter names. The 3 options include: To edit an existing parameter name or enter a parameter name for the first time for a local parameter, press the {REPLCE NAME} softkey. Key in a parameter name for the parameter.
Chapter 28 Paramacros Addressing Assigned Parameters Once you assign a parameter you can address it in a program: Example 28.16 Addressing Assigned Parameters #100=5; #105=8; G01X#100+5 ; Axis moves to 10. G01x[#100+5] Axis moves to 8 You can also indirectly address parameters with other parameters Example 28.17 Indirectly Addressing Parameters #100=101 #101=2.345 G01 X#[#100]; X axis moves to the contents of #100 which is #101. #101 has the value of 2.345.
Chapter 28 Paramacros 2. Enter a name for the backup file and press [TRANSMIT]. The system verifies the file name and backs up the selected parameters into a part program. You can restore these parameters by selecting and executing that part program. Important: If part program calculations cause an overflow value, then the generated backup file contains an M00 and the parameter number followed by the word “OVERFLOW” as a comment. 28.
Chapter 28 Paramacros CAUTION: Any edits that are made to a subprogram, or to a paramacro program (as discussed in chapter 5) that has already been called for automatic execution, are ignored until the calling program is disabled and reactivated. Subprograms and paramacros are called for automatic execution the instant that the calling program is selected as active (as discussed in chapter 7). 28.5.
Chapter 28 Paramacros 28.5.2 Modal Paramacro Call (G66) Use this format for calling a paramacro using the G66 command: G66 P_ L_ A_ B_; Where : Is : P Indicates the program number of the called macro. P ranges from 1 - 99999. L Programs the number of times the macro will be executed after each motion block that follows the G66. L ranges from 1 - 9999, and may be expressed as any valid parametric expression. If not specified, the control uses a default value of 1. A-Z Optional argument statements.
Chapter 28 Paramacros Unlike nonmodal macro calls, the G66 macro call repeats automatically after any axis move until cancelled by a G67 block. This also applies to nested macros. When the control begins execution of the nested macro 1002 in the program below, each axis move in the nested macro also calls for the execution of the macro 1001. Example 28.18 Modal Macro Call N0100G66P1001; N0200G65P1002; In Example 28.18, after the complete execution of the macro 1002, the macro 1001 is called.
Chapter 28 Paramacros Important: When the control executes block N040, the original value as set in block N020 for parameter number 1 is ignored, and the most current value (1.7) is used. The first time macro 1001 is executed, Z moves 1.1 units. The second time macro 1001 is executed, Z moves 1.7 units. 28.5.3 Modal Paramacro Call (G66.1) Use this format for calling a paramacro using the G66.1 command: G66.1 P_ L_ A_ B_; Where : Is : P Indicates the program number of the called macro.
Chapter 28 Paramacros The L--word or any optional argument statements following a G66.1 can contain any valid mathematical expression. For example: G66.1 P1002 L[#1+1] A[12*6] B[SIN[#101]]; Example 28.20 G66.1 Macro Operation N0100G90G17G00; N0110G66.1P9400; Macro 9400 is executed. N0120G91G18G01; G91 and G18 become effective, 01 is assigned to parameter #10, macro 9400 is executed. N0130G03X1.; 03 is assigned to parameter #10, 1. is assigned to parameter #24, macro 9400 is executed.
Chapter 28 Paramacros 28.5.4 AMP-defined G-Code Macro Call Use this format for calling an AMP-defined macro: G_ A_ B_; Where : Is : G_ Programs an AMP-defined G-code command (from G1 to G255.9). A-Z Optional argument statements. May be programmed using any letter from A to Z excluding G, L, N, O, or P. Used to assign numeric values to parameters in the paramacro (see NO TAG). Arguments may be specified as any valid parametric expression.
Chapter 28 Paramacros 28.5.5 AMP-Defined M-Code Macro Call Use this format for calling an AMP-defined M-code macro: M255 A_B_ Where : Is : M255 Programs an AMP-defined M-code command. A-Z Optional argument statements. May be programmed using any letter from A to Z excluding G, L, N, O, or P. Used to assign numeric values to parameters in the paramacro (see NO TAG). Arguments may be specified as any valid parametric expression. These macros are executed only as non-modal macro.
Chapter 28 Paramacros These macros are executed only as non-modal macro. The execution of the T--, S--, or B--code macro calls is the same as M-code macro calls with the following exceptions: the parameter # referenced when called the macro program called T calls macro 9000 S calls macro 9029 B calls macro 9028 In order for the T--, S--, or B--words to call up a macro program, these prerequisites must be met: 1. The value following the word must be equal to the value stored for the specified parameter #.
Chapter 28 Paramacros Precautions must be taken when attempting to nest AMP assigned macro calls since many combinations of these calls may not be valid. The system installer determines in AMP the functionality of the AMP-defined macro call when nested.
Chapter 28 Paramacros Table 28.J Works as the System-defined Code TYPE OF MACRO NESTED 1 CALLING PROGRAM G65, G66,or G66.1 AMP-G AMP-M AMP-T S or B G65, G66 or G66.1 Yes Yes Yes Yes AMP G-code Yes No No No AMP M-code Yes No No No AMP-T-- , S-- , or B-- code Yes No No No 1 What Yes/No means: Yes - - the macro type across the top row may be called from the macro type down the left column.
Chapter 28 Paramacros POPEN This command affects a connection to the output device by sending a DC2 control code and a percent character “%” to the RS-232 interface. This command must be specified prior to outputting any data. After this command, the control outputs any following program blocks including the parameter values that are used in them.
Chapter 28 Paramacros Example 28.22 would yield an output equal to the character strings with the * symbols being converted to spaces and the parameter values for parameters #123 and #234. The value of the parameter is output in binary as a 32-bit string with the most significant bit output first. Negative values are output in 2’s complement. Example 28.23 BPRNT Program Example #123=0.40936; #124=-1638.4; #10=12.
Chapter 28 Paramacros There may be as many S and #P in a block as desired provided that the length of the block does not exceed the maximum block size. Example 28.24 Sample of a DPRNT Block DPRNT[INSTALL*TOOL*#123[53]*PRESS*CYCLE*STOP**#234[20]]; Example 28.24 would yield an output equal to the character strings with the * symbols being converted to spaces and the parameter values for parameters #123 and #234. The value of the parameter is output as a string of decimal digits.
Chapter 28 Paramacros 28-56
Chapter 29 Program Interrupt 29.0 Chapter Overview This chapter describes the program interrupt feature. This feature lets you execute a subprogram or paramacro program while some other program is executing. This subprogram or paramacro is executed when PAL receives an interrupt signal (usually through the use of some switch triggered by the operator or one of the axes). The interrupt program can be executed even mid-block during a program’s execution.
Chapter 29 Program Interrupt An error is generated if anything other than an N-word, a P- or L-word, a block delete /, or a comment character is programmed in the M96 or M97 block. An interrupt M-code M96 or M97 may also be programmed within a interrupt program. If this is the case the interrupt does not become enabled/disabled until the interrupt currently being executed is completed and execution is returned to the main program.
Chapter 29 Program Interrupt The subprogram or paramacro program is assigned to a particular type of interrupt by programming a P-word in the M block that enables the interrupt (M96 in this manual). When selecting a program with a P-word, only the numeric value of the program name is entered; the letter O is omitted. For example, programming: M96L0P11111; would enable the program O11111 as a type 1 interrupt and allow it to be executed when switch 0 sends a signal to PAL.
Chapter 29 Program Interrupt 29.2 Interrupt Request Considerations The system installer determines: - in AMP, if a signal to execute an interrupt program is delayed until the end of a currently executing block, or executed immediately. - in AMP, whether an interrupt program request is recognized when an interrupt switch is turned on, or only when the switch makes the transition from off to on. This helps prevent the accidental execution of an interrupt program.
Chapter 29 Program Interrupt An Interrupt: - requested when the control is in E-Stop is ignored, regardless of whether the interrupt is enabled or not. - can only be executed when the control is in the state. If a request for an interrupt is made when the control is in or cycle suspend, the interrupt request is still recognized. The interrupt program will be executed when a state becomes active again.
Chapter 29 Program Interrupt Type 1 Interrupts If the Interrupt Program: Then the Control: Does not generate axis motion executes the interrupt program and then continues executing the part program as normal regardless of the location that the interrupt program was executed. Generates axis motion returns the tool to the endpoint of the next fully unexecuted block and continues executing the part program from this point. Figure 29.
Chapter 29 Program Interrupt Type 2 Interrupts The control returns the tool to the point in the program where it was when the interrupt was performed by using type 2 interrupts. Normally the first 4 linear moves (G00 or G01) in the interrupt program are remembered. This may be altered by programming a specific M-code.
Chapter 29 Program Interrupt You can alter the number of blocks that the control re-executes in reverse when returning to the start position of the interrupt. The number of return blocks is normally 4; however, it can be altered by these codes: M-code: Number of Blocks Retraced: M900 zero M901 one M902 two M903 three M904 four These M-codes can be programmed in any block in the main program before the interrupt program is executed.
Chapter 29 Program Interrupt The system installer determines if an interrupt program is to be called as a paramacro or a subprogram when it executes. If it is Called: Then: A Paramacro This assigns a new set of local parameters for the interrupt A Subprogram The same set of local parameters that applied to the interrupted program apply to the subprogram.
Chapter 29 Program Interrupt 29-10
Chapter 30 Using a 9/Series Dual-Processing System 30.0 Chapter Overview Read this chapter to learn general information related to programming and operating a dual-processing system. Major topics in this chapter cover: Topic: 30.
Chapter 30 Using a 9/Series Dual--Processing System 30.2 Operating a Dual-Processing System Dual-process systems operate almost exactly the same as their single-process counterparts. Each process functions as an independent 9/Series control. With the exception of shared dual-processing paramacro parameters, there is little shared data between processes. Each process has its own offset tables, programmable zone tables, and paramacro parameters.
Chapter 30 Using a 9/Series Dual--Processing System You cannot switch the active process while you use the digitize feature, a tool path or QuickCheck graphic display, or within an active program search operation. If you attempt to switch the active process, the control displays an error message. Select an active process by using one of these methods: Method: Description: [PROC SELECT] key found on the operator panel next to the [TRANSMIT] key.
Chapter 30 Using a 9/Series Dual--Processing System Editing a Part Program An “E” next to the program name on the part program directory screen indicates that the program is currently being edited. Only one program can be open for editing at a time. You cannot edit programs in more than one process at the same time. You cannot edit a program that is currently active (selected to run) in a different process.
Chapter 30 Using a 9/Series Dual--Processing System You can use QuickCheck as a program “syntax only” checker (no graphics) in both processes at the same time. Error Messages The control displays error messages on the screen for only the currently active process (except on split-screens). The name of the currently active process flashes in reverse video if an error occurs in another process. Change to the appropriate process to display the current errors for that process.
Chapter 30 Using a 9/Series Dual--Processing System Reset Operations Dual-process systems have a process reset operation, in addition to the normal block reset and control reset functions. These reset operations work as follows: If you want to perform a: Press: The control will: Block Reset [RESET] Skip the currently active block in the currently selected process (see chapter 2).
Chapter 30 Using a 9/Series Dual--Processing System 30.3 Synchronizing Multiple Part Programs On some machines or systems, it is often necessary to synchronize the operations of 9/Series dual processes. For example, on a dual-turret lathe, if one turret must rough a shaft down to size before another turret begins cutting a thread, it is extremely important that the turret roughing the shaft completes this task before the threading turret begins cutting the thread. Figure 30.
Chapter 30 Using a 9/Series Dual--Processing System Synchronization M-codes are not allowed in the last block in the part program. This can cause the part program to pause indefinitely, waiting for the next part program block (which does not exist) to become active. Synchronization M-codes are ignored during QuickCheck execution and during a Mid-Program Start operation. Example 30.1 Example of Synchronization for Threading (see Figure 30.3) Process 1 Comment N1 G90 S500 G00 X40. Z60.
Chapter 30 Using a 9/Series Dual--Processing System Example 30.2 Incorrect Use of Simple Synchronization with Shared Paramacro Parameters Process 1 Comment N17 #7100=100; Paramacro parameter 7100 is set to 100 Process 2 Comment N32 M100; Process pauses waiting for M100 in process 1. Block N33 is set up in buffer prepared for execution. N33 X#7100; Destination of this block is dependent on when this block was read into the setup buffer.
Chapter 30 Using a 9/Series Dual--Processing System Coordinating Synchronization Between Processes Remember that both processes are executing coordinated part programs. Failing to coordinate part programs correctly can result in the processes executing different synchronization codes and mutually locking each other out. Example 30.4 Mismatched Synchronization Codes Process 1 Comment Process 2 Comment N32 M101 Process 2 paused, waiting for M101 in process 1.
Chapter 30 Using a 9/Series Dual--Processing System Synchronization in MDI Mode Synchronization M-codes can be programmed in MDI mode. These can prove useful when attempting to manually start multiple programs from some point other than the beginning or when it is necessary to execute MDI programs on both processes simultaneously.
Chapter 30 Using a 9/Series Dual--Processing System For example, press to place process 1 in cycle suspend mode, while process 1 is waiting for process 2 to execute an M101. Later, when you request for process 1, the synchronization M-code is re-activated and process 1 is again paused, waiting for process 2 to execute an M101. If, while process 1 is in cycle suspend mode, process 2 executed an M101, process 2 will pause at that synchronization block.
Chapter 30 Using a 9/Series Dual--Processing System 30.4.1 Shared Spindle Configurations Shared spindle configurations are for those dual-processing systems that have one spindle that must be controlled by both processes. See Figure 30.4. As a general rule for this type of machine, spindle control is given to the process currently requesting spindle control. WARNING: It is the programmer’s responsibility to watch for conflicting overlap of spindle control between the two processes.
Chapter 30 Using a 9/Series Dual--Processing System Use the synchronization M-codes to properly dictate which process has control of the spindle at any given time. Adding a synchronization M-code to the above program segments would remedy the problem of process 1 cutting at the wrong RPM and in the wrong direction.
Chapter 30 Using a 9/Series Dual--Processing System An error is generated and the process enters cycle stop if you attempt to activate one of these features while one is already active in another process. For example, if process 1 is currently performing virtual C on the shared spindle and process 2 attempts to execute a G84 right hand tapping block, process 2 will generate an error and enter cycle stop. Process one will continue until completion or until it encounters a synchronization M-code.
Chapter 30 Using a 9/Series Dual--Processing System Figure 30.5 Multi-Start Thread When Same Start Point Is Used Process 2 2nd Threading Pass If both processes key off same marker pulse, then multi-start thread results.
Chapter 30 Using a 9/Series Dual--Processing System Figure 30.6 Identical Thread Is Cut When Start Point Is Shifted Using Equation Process 2 2nd Threading Pass .025 Marker Process 1 1st Threading Pass 12601-I Example 30.6 Threading on Both Processes with a Shared Spindle Process 1 Comment N1 G00 X10. Z10 S500. M03; Move to process 1 start point and start spindle rotation N3 G21 X4.8 Z5. E2.; N2 M100; Process 2 Comment N1 G00 X10. Z11.
Chapter 30 Using a 9/Series Dual--Processing System Figure 30.7 Cutting a Thread Using Both Processes Process 2 2nd Threading Pass Process 1 1st Threading Pass 12602-I Spindle Orient on a Shared Spindle Both processes can request a spindle orient. If one process requests a spindle orient while the other process’s spindle orient command has not completed, the control generates an error. The process that requested the second spindle orient is forced into cycle stop mode. 30.4.
Chapter 30 Using a 9/Series Dual--Processing System 30.5 Using Interference Checking with a Dual-Process Lathe The Interference Checking feature is designed to help prevent collisions by the axes of a dual-processing machine. Interference checking provides an area (usually around the cutting tool or tool turret for each process) that defines a boundary that moves with the tool. The other process cannot enter into this boundary. This helps prevent collisions.
Chapter 30 Using a 9/Series Dual--Processing System Activating Interference Checking The interference boundaries for each process are entered into the interference checking tables. These tables relate the boundaries to specific tool or offset geometries. The system installer selects the number of boundaries that are available (from 1-32) for each process. Each process can have a different interference boundary number active at the same time.
Chapter 30 Using a 9/Series Dual--Processing System Using Interference Checking to Prevent Collisions When two protected areas are about to collide, the control suspends motion, stopping one or both of the processes and preventing a collision. In Example 30.7, process 1 will collide with process 2. Since process 2 is stationary, the control puts process 1 in cycle suspend to prevent a collision. Once the control detects the collision, it suspends the action. Interference checking operates in real time.
Chapter 30 Using a 9/Series Dual--Processing System 30.5.1 Measuring Interference Boundaries The control can store as many as 32 different boundaries for each process. Two separate areas make up each of these boundaries. Both axes are activated when the boundary is activated through PAL. Figure 30.10 illustrates the use of two areas to make up interference boundary 01. Figure 30.10 Using Two Areas to Define an Interference Checking Boundary Area 2 These areas define an interference boundary.
Chapter 30 Using a 9/Series Dual--Processing System Important: Your system installer determines the relationship of the machine coordinate systems between processes (relative location of zero points and direction of positive travel) in AMP and through hardware. This manual assumes the machine coordinate systems of both processes are as shown in Figure 30.11. Refer to your system installer’s documentation for details on how your machine coordinate systems are configured. Figure 30.
Chapter 30 Using a 9/Series Dual--Processing System Important: These areas are measured from the machine coordinate zero point to the extremes of the fixture encompassed by the zone when the machine is at home. The machine coordinate system zero point and machine home are frequently not the same point on the machine. Machine home is a fixed mechanical position established by the homing sequence off hardware homing switches.
Chapter 30 Using a 9/Series Dual--Processing System Figure 30.12 Protecting Additional Axes with Interference Checking Though only X and Z define this interference area, some protection is also offered to W since an X or Z collision would be detected anytime W would collide. This protection, however, will cause the control to detect a collision even if sufficient clearance exists on the W axis. Disable interference checking when it is necessary to overlap a third axis.
Chapter 30 Using a 9/Series Dual--Processing System 3. Press the {INTERF CHECK} softkey to display the interference checking data entry screen shown in Figure 30.13. (softkey level 3) ZONE F1-F9 LIMITS INTERF CHECK DRLCYC PARAM Figure 30.13 Interference Checking Data Table INTERFERENCE TABLE PAGE TOOL NO *1 X X Z Z PLUS MINUS PLUS MINUS AREA 1 [INCH] 1.5000 -.5000 1.5000 0.0000 1 OF 32 AREA 2 [INCH] 1.5000 -1.0000 6.0000 1.
Chapter 30 Using a 9/Series Dual--Processing System This boundary number should be the same as the tool geometry number (T-word) that will be active when the tool and/or fixture is being controlled. Refer to your system installer’s documentation for details on which tool or fixture corresponds to which interference boundary number (1-32). 6. Use the up or down cursor keys to move the block cursor to the interference area parameter to be changed. The selected field appears in reverse video. 7.
Chapter 30 Using a 9/Series Dual--Processing System This is a representation of the basic format for modifying the tables. G10 L{ Where : L(5-6) 5 } P__ X___ Z___ I___ K___; 6 Is : The definition of which area in the table is being modified. L5 - Modifies the Area 1 values L6 - Modifies the Area 2 values P The boundary number of the interference boundary that is having its values changed is specified following the P address.
Chapter 30 Using a 9/Series Dual--Processing System Example 30.9 Resulting Boundary from Example 30.8 +X 23” Process 1 19.5” 13” Area 1 Area 2 Machine Home Process 1 19” 18.5” 15” Machine Coordinate System Zero Point (Both Processes) 11” +Z 12608-I 30.5.4 Backing Up Interference Tables The control can save all of the information that is entered in the interference tables as a backup. This is done by the control generating a program consisting of G10 blocks.
Chapter 30 Using a 9/Series Dual--Processing System 2. Press the {PRGRAM PARAM} softkey. (softkey level 2) PRGRAM AMP PARAM DEVICE MONISETUP TOR TIME PARTS PTOM SI/OEM 3. Press the {INTERF CHECK} softkey to display the interference checking data entry screen as shown in Figure 30.13. (softkey level 3) ZONE F1-F9 LIMITS 4. DRLCYC PRBCYC INTERF PARAM PARAM CHECK Press the {BACKUP INTERF} softkey. Figure 30.14 shows the backup interference boundary screen.
Chapter 30 Using a 9/Series Dual--Processing System Figure 30.14 Backup Interference Boundary Screen STORE TO BACKUP INTERFERENCE TABLE TO TO TO PORT A PORT B FILE 5. Determine the destination for the G10 program: To Send the G10 Program To: Press This Softkey: Go to Step: peripheral attached to port A {TO PORT A} 7. a peripheral attached to port B {TO PORT B} 7. to control memory {TO FILE} 6. 6. Press the {TO FILE} softkey. The control asks for a program name.
Chapter 30 Using a 9/Series Dual--Processing System 30.6 Shared Axes on Dual- Processing Systems Your system installer can configure an axis to be shared by different processes. With this feature multiple processes can execute part program commands or perform manual operations on the same shared axis. A shared axis can not be commanded by more than one process simultaneously. Control of the shared axis must be changed from process to process thru the system installer’s PAL program. 30.6.
Chapter 30 Using a 9/Series Dual--Processing System Block Retrace Any part program blocks prior to an axis process switch can not be retraced. If you attempt to retrace beyond the point that an axis switch occurred, the control generates an error. Also an axis process switch can not be performed if you are currently performing a block retrace. Scaling Scaling is performed on a per process basis. If you switch processes for a scaled axis, scaling is removed in the new process.
Chapter 30 Using a 9/Series Dual--Processing System 30.6.2 Switching a Shared Axis to a Different Process The system installer determines what axes are shared and how a shared axis is changed from process to process. Using AMP and PAL the system installer determines the process for a shared axis at power up, control reset, and E-Stop reset. Refer to your system installer’s documentation for details.
Chapter 30 Using a 9/Series Dual--Processing System 30.6.3 Setting up a Shared Axis Your system installer performs the majority of set up operations in PAL and AMP to define a shared axis configuration. This section covers operations you should perform on the control to properly operate the shared axis.
Chapter 30 Using a 9/Series Dual--Processing System You can not change the offset for an axis that is not currently assigned to the process through a part program (G52, and G92). You can however change coordinate system tables without the shared axis being in the process using PAL or by manually inputting the data through the {OFFSET} softkey. If the shared axis is not in the process activating the new work coordinate system (G54-G59.
Chapter 30 Using a 9/Series Dual--Processing System Example 30.10 Changing Processes with Tool Offsets Process One Activates this Tool Process Two Activates this Tool Shared Axis T1010; (controls shared axis) T000; Process one activates tool offset on shared axis as defined in AMP (delayed/immediate shift/move). When process two takes control of the shared axis, the shared axis tool offset is canceled on the shared axis until it is returned to the process.
Chapter 30 Using a 9/Series Dual--Processing System Figure 30.15 Dual- Axis Configuration Lead screw Axis 1 Encoder Servo motor Dual Axes - two completely separate axes responding to the same programming commands. Encoder Servo motor Axis 2 Lead screw The 9/Series control supports two groups of dual axes. This is the total number of groups allowed on the system for both processes (i.e. two groups in one process or one group in each process).
Chapter 30 Using a 9/Series Dual--Processing System Coupling/Decoupling is a dual group function. All axes must be in the dual groups default process before they can be either coupled or decoupled. When a coupling or decoupling occurs a re-setup occurs of any part program blocks read into the controls block look ahead buffer. This may causes a slight hesitation in program execution while the control sets up the new look ahead buffer.
Chapter 30 Using a 9/Series Dual--Processing System Other restrictions are as follows: If the dual- axis is currently: Then: performing a manual motion (including continuous, incremental, or handwheel jog, homing, jog on the fly, or angled jogs) the request to decouple that axis is ignored until the manual motion is completed¶ being positioned by the PAL axis mover the request to decouple that axis is ignored until the PAL axis mover has completed moving the dual-- axis¶ in the active plane and cutte
Chapter 30 Using a 9/Series Dual--Processing System An axis that is decoupled from its dual group can have an integrand letter assigned to it in AMP by the system installer. This integrand is used with that axes originally assigned AMP axis name to perform functions such as circular interpolation. Plane dependant operations (such as circular interpolation or cutter compensation) are available to a dual axes while coupled (provided the dual--axis is defined in the active plane).
Chapter 30 Using a 9/Series Dual--Processing System 30-42
Appendix A Softkey Tree Appendix Overview This appendix explains softkeys and includes maps of the softkey trees. Understanding Softkeys We use the term softkey to describe the row of 7 keys at the bottom of the CRT. The function of each softkey is displayed on the CRT directly above the softkey. Softkey names are shown in this manual between the { } symbols. Softkeys are often described in this manual as being on a certain level, for example, softkey level 3.
Appendix A Softkey Tree For example : (softkey level 1) PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT When softkey level 1 is reached, the previous set of softkeys is displayed. Press the continue softkey {Þ } to display the remaining softkey functions on softkey level 1. (softkey level 1) FRONT PANEL ERROR PASSMESAGE WORD SWITCH LANG On softkey level 1, the exit softkey is not displayed since the softkeys are already on softkey level 1.
Appendix A Softkey Tree Describing Level 1 Softkeys (softkey level 1) PRGRAM OFFSET MACRO MANAGE PARAM PRGRAM SYSTEM CHECK SUPORT FRONT PANEL SWITCH LANG ERROR PASSMESAGE WORD If you want to: Press: Edit, activate, or copy a program from a peripheral or control memory {PRGRAM MANAGE} Display or enter tool offset data, the work coordinate system offset data, etc.
Appendix A Softkey Tree AXIS POSITION DISPLAY FORMAT SOFTKEYS PRGRAM A B S TARGET D T G AXIS SELECT M CODE STATUS PRGRAM D T G A L L G CODE STATUS SPLIT ON/OFF A-4 NOTE: The first 4 softkeys (from PRGRAM to DTG) toggle between small and large screen display.
Appendix A Softkey Tree THE FUNCTION SELECT SOFTKEYS LEVEL 1 WITH POWER UP (AXIS POSITION) DISPLAY SCREEN Optional PAL flag set to display “front panel” when MTB is not part of the total CNC system PRGRAM MANAGE see page A-6 OFFSET see page A-7 MACRO PARAM see page A-9 PRGRAM CHECK see page A-10 SYSTEM SUPORT see page A--11 FRONT PANEL see page A-13 ERROR MESAGE see page A-13 PASSWORD see page A-14 SWITCH LANG PAL Display Page Option: Five softkeys available on third screen.
Appendix A Softkey Tree PRGRAM MANAGE level 1 level 2 PRGRAM MANAGE ACTIVE PRGRAM EDIT PRGRAM level 3 level 4 see page A-15 see page A-16 EXEC RESTRT PRGRAM QUIT EXIT DISPLY PRGRAM MEM TO PORT A COPY PRGRAM FROM A TO MEM MEM TO PORT B FROM B TO MEM MEM TO MEM DELETE YES DELETE PRGRAM VERIFY PORT A VERIFY PORT B VERIFY MEMORY PRGRAM COMENT RENAME YES RENAME PRGRAM RENAME NO FROM PORT A FROM PORT B FROM MEMORY INPUT.
Appendix A Softkey Tree OFFSET (Lathe & Mill) level 1 level 2 level 3 level 4 level 5 REPLCE VALUE OFFSET WORK CO-ORD ADD TO VALUE INCH/ METRIC RADI/ DIAM (lathe only) MORE OFFSET SEARCH NUMBER REPLCE VALUE ADD TO VALUE ACTIVE OFFSET TOOL WEAR MORE.
Appendix A Softkey Tree OFFSET (Grinder) level 1 level 2 level 3 level 4 REPLCE VALUE OFFSET WORK CO-ORD ADD TO VALUE INCH/ METRIC RADI/ DIAM (cylindrical only) MORE OFFSET MODIFY LABEL SEARCH NUMBER REPLCE VALUE WHEEL GEOM ADD TO VALUE CHANGE OFFSET MORE.
Appendix A Softkey Tree MACRO PARAM level 1 level 2 level 3 SEARCH NUMBER MACRO PARAM LOCAL PARAM REFRSH SCREEN SEARCH NUMBER COM-1 PARAM REPLCE VALUE ZERO VALUE 0 ALL VALUES REFRSH SCREEN SEARCH NUMBER REPLCE VALUE ZERO VALUE REPLCE NAME COM-2A PARAM CLEAR NAME CLEAR ALL NM COM-2B PARAM SHARED PARAM 0 ALL VALUES REFRSH SCREEN A-9
Appendix A Softkey Tree PRGRAM CHECK level 1 PRGRAM CHECK level 2 level 3 SELECT PRGRAM ACTIVE PRGRAM DE-ACT PRGRAM QUICK CHECK level 4 CLEAR GRAPH MACHIN INFO GRAPH ZOOM WINDOW SYNTAX ONLY ZOOM BACK GRAPH SETUP STOP CHECK T PATH GRAPH T PATH DISABL A-10 level 5 DEFALT PARAM SAVE PARAM
Appendix A Softkey Tree SYSTEM SUPPORT level 1 level 2 level 3 level 4 level 5 REPLCE VALUE SYSTEM SUPORT PRGRAM PARAM (lathe only) DRLCYC PARAM ZONE LIMITS ADD TO VALUE MORE LIMITS F1-F9 UPDATE & EXIT MILCYC PARAM PROBE PARAM QUIT REPLCE VALUE ADD TO VALUE UPDATE & EXIT (mill only) QUIT REVERS ERROR AMP AXIS PARAM HOME CALIB AXIS CALIB SERVO PARAM SPNDL PARAM PATCH AMP REPLCE VALUE SEARCH NUMBER UPDATE & EXIT UPDATE BACKUP TO BACKUP FROM BACKUP REPLCE VALUE INSERT POINT DELETE PO
Appendix A Softkey Tree SYSTEM SUPPORT level 1 level 2 level 3 level 4 level 5 Continued from previous page DISPLY RING I/O SYSTEM SUPORT MONI-TOR REMOTE I/O FAST I/O AXIS MONITOR SERIAL I/O DATA SCOPE SEARCH MONITR RECOVR ENABLE @ AXIS RECV PORT A START STOP XMIT PORT B REPEAT XMIT PORT A PORT B ED PRT INFO PTOM SI/OEM SYSTEM TIMING SCREEN SAVER ENTER MESAGE STORE BACKUP RESET MAXMUM SAVER ON/OFF INCR TIMER DECR TIMER A-12 SINGLE XMIT FREEZE UN FREEZE CLEAR SELECT RUNG FORWD SEARC
Appendix A Softkey Tree FRONT PANEL level 1 FRONT PANEL level 2 JOG AXIS level 3 level 4 SET ZERO JOG AXES+ JOG AXES-- PRGRAM EXEC BLOCK RETRCE JOG AXES+ JOG RETRCT JOG AXES-- CYCLE START CYCLE STOP ERROR MESAGE level 1 ERROR MESAGE level 2 ERROR LOG CLEAR ACTIVE level 3 ACTIVE ERRORS FULL MESAGE TIME STAMPS This softkey toggles between [TIME STAMPS] and [FULL MESAGE] A-13
Appendix A Softkey Tree PASSWORD level 1 PASSWORD level 2 ACCESS CONTRL level 3 UPDATE & EXIT 01 (NAME) 02 (NAME) 03 (NAME) 04 (NAME) UPDATE & EXIT 05 (NAME) 06 (NAME) 07 (NAME) 08 (NAME) STORE BACKUP A-14 (NAME) = PASSWORD NAME
Appendix A Softkey Tree ACTIVE PRGRAM level 2 level 3 level 4 level 5 level 6 FORWRD ACTIVE PRGRAM REVRSE DE-ACT PRGRAM TOP OF PRGRAM CANCEL N SEARCH SEARCH EXIT O SEARCH EOB SEARCH FORWRD SLEW REVRSE STRING SEARCH TOP OF PRGRAM CANCEL EXIT CONT MID ST PRGRAM SEQ # SEARCH TOP OF PRGRAM STRING SEARCH QUIT EXIT T PATH GRAPH CLEAR GRAPHS MACHNE INFO ZOOM WINDOW ZOOM BACK T PATH DISABL GRAPH SETUP INCR WINDOW DECR WINDOW ZOOM ABORT ZOOM DEFALT PARAM SEQ STOP TIME PARTS SAVE PARAM
Appendix A Softkey Tree EDIT PRGRAM level 2 EDIT PRGRAM level 3 level 4 level 5 MODIFY INSERT BLOCK DELETE FORWRD BLOCK TRUNC DELETE CH/WRD REVRSE EXIT EDITOR TOP OF PRGRAM BOT OF PRGRAM STRING SEARCH ALL RENUM PRGRAM MERGE PRGRAM QUICK VIEW ONLY N see page A-17 EXEC CHAR/ WORD LINEAR DIGITZ E CIRCLE 3 PNT CIRCLE TANGNT MODE SELECT STORE END PT EDIT & STORE RECORD MID PT STORE END PT EDIT & STORE INCH/ METRIC ABS/ INCR PLANE SELECT DIA/ RADIUS A-16 (lathe only)
Appendix A Softkey Tree QUICK VIEW level 3 MILL QUICK VIEW level 4 QPATH+ PROMPT level 5 level 6 see page A-18 G CODE PROMT SELECT MILL PROMPT SET PLANE SELECT G17 STORE G18 G19 LATHE QUICK VIEW QPATH+ PROMPT G CODE PROMT SELECT DRILL PROMPT SET LATHE PROMPT PLANE SELECT G17 STORE G18 G19 A-17
Appendix A Softkey Tree QPATH+ PROMPT level 4 level 5 level 6 QPATH+ PROMPT CIR ANG PT STORE CIR CIR ANG CIR PT ANG PT 2ANG PT 2ANG PT R 2PT R 2ANG PT C 2PT C 2ANG 2PT 2R 3PT 2R 2ANG 2PT 2C 3PT 2C 2ANG 2PT RC 3PT RC 2ANG 2PT CR 3PT CR END OF APPENDIX A-18
Appendix B Error and System Messages Overview This appendix serves as a guide to error and system messages that can occur during programming and operation of the 9/Series control. We listed the messages in alphabetical order along with a brief description. Important: To display both active and inactive messages, press the {ERROR MESAGE} softkey found on softkey level 1. For details, see chapter 2. Important: This appendix covers only error and system messages.
Appendix B Error and System Messages Message Description 2 2MB RAM IS BAD/MISSING The control has discovered the RAM SIMMs for the two megabyte extended storage option are either damaged or missing. The RAM SIMMs must be installed or replaced. Contact your Allen Bradley sales representative for assistance. 9 9/SERIES LATHE - CANNOT USE MILL AMP The control was powered up with a lathe software option chip installed, when the AMP file that was downloaded was configured for a mill.
Appendix B Error and System Messages Message Description AMP WAS MODIFIED BY PATCH AMP UTILITY This message always appears after changes have been made to AMP using the patch AMP utility. Its purpose is to remind the user that the current AMP has not been verified by a cross-reference check normally performed by ODS. It is meant as a safety warning.
Appendix B Error and System Messages Message Description AXIS INVALID FOR G24/G25 The programmed axis was not AMPed for software velocity loop operation, and can not be used in a G24 or G25 block. To use these features the axis programmed must be configured for tachless operation (or be a digital servo).
Appendix B Error and System Messages Message Description BAD RAM DISC SECTOR CHECKSUM ERROR A RAM disk sector error was detected during the RAM checksum test at power-up. Attempt to power-up again. If the error remains, contact Allen-Bradley customer support services. BAD RECORD IN PROGRAM This indicates a serious problem with the program. Attempt to open the program a second time. If retry doesn’t work, you may have to delete the program.
Appendix B Error and System Messages Message Description CANNOT COPY The requested copying task cannot be performed due to an internal problem in the file or RAM disk. Contact Allen-Bradley customer support service. CANNOT DELETE - OPEN PROGRAM The selected program is either active or open for editing and cannot be deleted.
Appendix B Error and System Messages Message Description CANNOT RENAME When performing a rename of a program name, the new program name has not been correctly entered. The format is OLD PROGRAM NAME,NEW PROGRAM NAME. CANNOT REPLACE START POINT An illegal attempt was made to change the axis calibration start-point using the online AMP feature. CANNOT RESTART G24 HARD STOP An attempt was made to restart a part program on a block which would have an axis at the hard stop.
Appendix B Error and System Messages Message Description CHARACTERS MUST FOLLOW WILDCARD You have used incorrect search string syntax in the PAL search monitor utility. CHECKSUM ERROR IN FILE The file (AMP, PAL) being downloaded from a storage device has a checksum error. The file cannot be used. CIRCLE MID-POINT NOT ENTERED The center-point of an arc is not entered in a circular programming block. Circular blocks require programming either an R or an I, J, K in the block.
Appendix B Error and System Messages Message Description CPU #2 HARDWARE ERROR #4 The 68030 main processor has detected an illegal address. Consult Allen-Bradley customer support services (9/290 only). CPU #2 HARDWARE ERROR #6 The 68030 main processor has detected a privilege violation. Consult Allen-Bradley customer support services (9/290 only). CPU #2 HARDWARE ERROR #8 CPU #2 has detected an unassigned vector interrupt. Consult Allen-Bradley customer support services (9/290 only).
Appendix B Error and System Messages Message CYLIND/VIRTUAL CONFIGURATION ERROR Description An axis configuration error was detected by the control when cylindrical interpolation or end face milling was requested in a program block. Some examples would include: A cylindrical/virtual axis is named same as a real axis or is missing (for example on a lathe A, the cylindrical axis may have been named the same as a incremental axis name).
Appendix B Error and System Messages Message Description DEPTH PROBE TRAVEL LIMIT The adaptive depth probe has moved to its AMPed travel limit. Note the value entered in AMP is the adaptive depth probe deflection from the PAL determined probe zero point. It may not be the actual total probe deflection. DEPTH PROBE NOT SUPPORTED A depth probe axis has been AMPed on an axis located on a servo card or a 9/230 that does not support the adaptive depth feature. (analog servo rev < rev 0.
Appendix B Error and System Messages Message Description DRESSER WARNING LIMIT REACHED The axis specified as the dresser axis has been dressed smaller than the dresser warning limit value as specified on the dresser status page. DRILL AXIS CONFIGURATION ERROR The drilling axis is not a currently configured machine axis. On dual processing controls this message may result when the drilling axis is in another process.
Appendix B Error and System Messages Message Description ENCODER QUADRATURE FAULT An error has been detected in the encoder feedback signals. Likely causes are excessive noise, inadequate shielding, poor grounding, or encoder hardware failure. END OF FILE When transferring a file over the serial port, the control has reached the last block in the program. END OF PROGRAM When displaying a part program on the CRT, the control has reached the last block in the program.
Appendix B Error and System Messages Message EXTRA KEYBOARD OR HPG ON I/O RING Description The control detected a keyboard or HPG on the 9/Series fiber optic ring that was not configured as a ring device. The I/O ring will still function and the control will NOT be held in E-Stop. You may also use the keyboard or HPG by selecting it as the active device via the corresponding PAL flags.
Appendix B Error and System Messages Message Description FLASH SIMMS CONTAIN INVALID DATA Flash SIMMs have become corrupted probably from a communication error during a system update. Retry the system executive update utility. If the situation persists, contact Allen-- Bradley support. FLASH SIMMS U10 AND U14 ARE EMPTY OR MISSING Make sure your flash SIMMs are installed in the correct tracks.
Appendix B Error and System Messages Message GRAPHICS ACTIVE IN ANOTHER PROCESS Description Graphics can only be active in one process at a time. You must turn graphics off in one process before you can activate them in another process. H HARD STOP ACTIVATION ERROR An attempt was made to (G24) hard stop an axis while a different axis was already holding against a hard stop.
Appendix B Error and System Messages Message Description HIPERFACE PASSWORD FAILURE During the SINCOS device’s alignment procedure, the logic used to set the passwords detects an incorrect password. A section of the code will repeatedly attempt various combinations of each of the passwords to correct the error condition. HOME REQUEST ON A PARKED AXIS An attempt was made, while using dual axes, to do a homing operation on a parked axis.
Appendix B Error and System Messages Message Description ILLEGAL DUAL CONFIGURATION Both dual master axes names have the same letter OR when assigning dual groups in AMP, dual groups must be assigned in contiguous order, starting with group 1, 2, 3, 4, and 5. You can not assign axes to dual group 3 without axes having been assigned to dual groups 1 and 2. ILLEGAL DUAL LINEAR/ROTARY CONFIGURATION The dual group cannot contain a mixture of linear and rotary axes.
Appendix B Error and System Messages Message Description INCOMPATIBLE TOOL ACTIVATION MODES This message is displayed and the control is held in E-Stop at power up when the tool geometry offset mode is “Immediate Shift/Immediate Move”and the tool wear offset mode is “Immediate Shift/Delay Move” or when the tool geometry offset mode is “Immediate Shift/Delay Move”and the tool wear offset mode is “Immediate Shift/Immediate Move”. These modes are incompatible.
Appendix B Error and System Messages Message Description INVALID CHECKSUM DETECTED This error is common for several different situations. Most typically it results when writing or restoring invalid data to flash memory. For example if axis calibration data is being restored to flash and there was an error or invalid memory reference in the axis calibration data file. Typically this indicates a corrupt or invalid file. INVALID CNC FILENAME An error occurred in G05 DH+ communications block.
Appendix B Error and System Messages Message Description INVALID FIXED DRILLING AXIS The axis selected as the drilling axis is an invalid axis for a drilling application. INVALID FORMAT SPECIFIED IN B/DPRNT CMD Improper format was used in the paramacro command (BPRNT or DPRNT) that outputs data to a peripheral device. INVALID FUNCTION ARGUMENT An invalid paramacro argument was used in a paramacro function. The argument contains either bad syntax or an illegal value.
Appendix B Error and System Messages Message Description INVALID PROGRAM NUMBER (P) A program number called by a sub-program or paramacro call is invalid. A P-word that calls a sub-program or paramacro can only be an all-numeric program name as many as 5 digits long. The O-word preceding the numeric program number in control memory cannot be entered with the P-word. INVALID REMOTE NODE NAME An error occurred in G05 DH+ communications block.
Appendix B Error and System Messages Message Description INVALID TOOL LENGTH OFFSET NUMBER An attempt was made to enter a tool length offset number in the tool life management table that is larger than the maximum offset number allowed. If the tables are being loaded by a G10 program, the length offset number is entered with a H-word in the block. INVALID TOOL LIFE TYPE An attempt was made to enter an invalid tool life type for a tool group in the tool management tables.
Appendix B Error and System Messages Message Description LARGER MEMORY - REFORMAT This message typically occurs after a new AMP or PAL has just been downloaded to the control. There is now more memory available for the RAM disk, but you need to reformat to use it. If desired, you do not have to reformat RAM and can continue to run the control with the RAM disk at its current size.
Appendix B Error and System Messages Message Description MAXIMUM BLOCK NUMBER REACHED A renumber operation was performed to renumber block sequence numbers (N-words), and the control has exceeded a block number of N99999. Either the program is too large to renumber, or the parameters for the first sequence number, or the sequence number increment, are too large. When this error occurs, the renumber operation stops renumbering at the last block within the legal range of N-words.
Appendix B Error and System Messages Message Description MINIMUM RPM LIMIT AUXILIARY SPINDLE 2 The commanded aux spindle 2 speed requested by the control is less than the AMPed minimum aux spindle 2 speed for the current gear being used. This requires a gear change operation or a change in the programmed aux spindle 2 speed. In some cases, the switch may be sufficient.
Appendix B Error and System Messages Message Description MISSING I/O RING DEVICE The I/O assignment file that was compiled and downloaded with PAL defines an I/O ring device that is not physically present in the I/O ring. Verify that all device address settings are correct. MISSING INTEGRAND/RADIUS WORD A circular or helical block has been programmed with axis data and no radius (R) or integrand (I, J, or K) values.
Appendix B Error and System Messages Message Description MULTIPLE FUNCTIONS NOT ALLOWED Multiple functions are not allowed. MULTIPLE SPINDLE CONFIGURATION ERROR Each multiple spindle must have a servo board identified in AMP to indicate to which board the spindle is connected. The spindle must be included in the number-of-motors AMP parameter for the board the spindle is on. MUST ASSIGN TOOL NUMBER FIRST In random tool, an attempt was made to customize a tool before the tool number was assigned.
Appendix B Error and System Messages Message Description N NEED SHADOW RAM FOR ONLINE SEARCH Your system contains the DH+ module and you have not installed the extra RAM SIMMS that are required to run the PAL online search monitor with the DH+ module installed. You must buy additional RAM for a system equipped with both of these features. Contact your Allen-Bradley Sales representative to purchase these SIMMS. Refer to your 9/Series integration manual for details on installing additional SIMMS.
Appendix B Error and System Messages Message Description NO PROGRAM TO RESTART There is no program to restart. The previous program was either completed or cancelled. NO RECIPROCATION DISTANCE A reciprocation interval of zero (0) was programmed for a grinder reciprocation fixed cycle. NO RECIPROCATION FEEDRATE The reciprocation feedrate, E-word, required during a grinder reciprocation fixed cycle was not programmed.
Appendix B Error and System Messages Message Description O OBJECT NOT FOUND IN PROGRAM The object you are searching for in the search monitor utility does not exist in the current module, or does not exist in the program in the direction you are searching. OCI ETHERNET CARD NOT INSTALLED An OCI dual-- process system has a standard CRT installed. The OCI Ethernet card has not been installed. This may happen if a dual-- process OCI executive is loaded into a non-- OCI system.
Appendix B Error and System Messages Message Description OVER SPEED IN POCKET CYCLE The programmed feedrate for an irregular pocket cycle (G89) was too high for the cycle to keep up. The part program stops at the endpoint of the block in which the error occurred. The cycle must be executed with a lower feedrate. OVERTRAVEL (+) The indicated axis has reached the positive software overtravel limit during an axis jog. This message can appear prior to reaching the overtravel limit in certain instances.
Appendix B Error and System Messages Message Description PAL SOURCE REV. MISMATCH - CAN’T MONITOR PAL source code in the control does not match the revision of the CNC executive. The PAL code may execute if all of the PAL system flags exist but the monitor cannot be used. PAL USING MEMORY - REFORMAT The AMP parameter allowing PAL to be stored in RAM memory has been enabled. This changes the amount of RAM memory available for part program storage, requiring the RAM disk to be reformatted.
Appendix B Error and System Messages Message Description POCKET IS PART OF CUSTOM TOOL An attempt was made to assign a tool to a tool pocket that is already used by a custom tool. Custom tools are assigned to tool pockets that are shown with an XXXX next to the pocket number on the random tool table. POCKET MILLING SHAPE IS INVALID A parameter is missing in the G88 programming block. POINT ALREADY EXISTS The point that you are trying to enter is already in the axis calibration table.
Appendix B Error and System Messages Message Description PROGRAM NOT FOUND The program cannot be located in memory. Check to make sure the program name was correctly entered. PROGRAM OPEN FOR EDIT IN ANOTHER PROCESS On a dual-processing system, you cannot edit a program that is active in another process. You will need to switch processes if you want to edit the other program. PROGRAM REWIND ERROR An attempt to rewind the tape was not successful.
Appendix B Error and System Messages Message Description RECIP AXIS IN WRONG PLANE The reciprocation axis specified in a G81 or a G81.1 programming block is not in the currently selected plane. RECIP AXIS NOT PROGRAMMED No reciprocation axis was specified in a G81 or a G81.1 programming block. RECIPROCATION NOT STOPPED An attempt was made to deactivate the current part program while reciprocation is still active. You must deactivate reciprocation before deactivating the current part program.
Appendix B Error and System Messages Message Description REMOTE I/O USER FAULT OCCURRED The RIO module detected that the user fault bit was set. The interboard communications fault LED is flashing. REMOTE I/O WATCHDOG TIMEOUT The watchdog mechanism on the RIO module timed out, indicating that the RIO module has not operated in an expected manner for possibly 17ms. The processor fault LED is turned ON.
Appendix B Error and System Messages Message Description S-- CURVE OPTION NOT INSTALLED An attempt was made to select S-- Curve Acc/Dec (G47.1) when the S-- Curve option bit was set to false. Make sure your system includes the S-- Curve option. S NOT LEGAL PROGRAMMING AXIS NAME This is displayed at power-up when the letter “S”is assigned to linear or rotary axis. Only the spindle(s) can be AMPed with “S”as the name; it cannot be assigned to a programmable axis.
Appendix B Error and System Messages Message SERVO AMP C LOOP GAIN ERROR Description One of the following AMP parameter errors exist:: Current Prop. Gain + Current Integral Gain < 4096 or Current Prop. Gain - Current Integral Gain > 0. SERVO AMP ERROR There is an error in one or more of the AMP parameters relative to servo control or an absolute feedback encoder failed to initialize.
Appendix B Error and System Messages Message Description SERVO PROCESSOR OVERLAP The analog version of the servo sub-system provides fine iteration overlap detection. This message is displayed if the fine iteration software on the DSP does not execute to completion in one fine iteration. SERVO PROM CHECKSUM ERROR The checksum test on the servo processor software stored in PROM memory has failed. This test is performed on power-up and periodically while the system is running.
Appendix B Error and System Messages Message Description SPINDLE IS CLAMPED An attempt was made to program a block containing a spindle code other than an M05 while the PAL servo clamp request flag for the spindle was set. SPINDLE MODES INCOMPATIBLE An attempt was made to enter virtual mode when the spindle that is used for this mode is synchronized as the follower spindle or an attempt was made to perform end face milling during synchronization.
Appendix B Error and System Messages Message Description SYSTEM MODULE GROUND FAULT The 1394 system module has detected a ground fault. The system generates a ground fault when there is an imbalance in the DC bus of greater than 5A. This drive error can be caused by incorrect wiring (verify motor and ground wiring), motor malfunction, or an axis module IGBT malfunction. SYSTEM MODULE OVER TEMP The 1394 contains a thermal sensor which senses the internal ambient temperature.
Appendix B Error and System Messages Message Description THREAD LEAD IS ZERO No thread lead has been programmed in a block that calls for thread cutting. Thread lead is programmed with either an F- or an E-word. THREAD PULLOUT DISTANCE TOO LARGE The programmed threading pullout distance is larger than the programmed distance of the thread departure.
Appendix B Error and System Messages Message Description TOO MANY NONMOTION CHAMFER/RADIUS BLOCKS Too many non-motion blocks separate the first tool path that determines the chamfer or radius size (programmed with a ,R or ,C) from the second tool path. A maximum number of non-motion blocks is set in AMP by the system installer. A non-motion block is defined as any block that does not generate axis motion in the current plane.
Appendix B Error and System Messages Message Description UNABLE TO SYNCH IN CURRENT MODE The control can not perform the request to synchronize spindles. Possible causes are: synchronization is already active; virtual/cylindrical programming or a threading operation is active on the primary or follower spindle when the synchronization request is made; or on a dual-- process system, one of the requesting processes cannot gain control over both spindles.
Appendix B Error and System Messages Message Description Z Z-WORD CANNOT BE GREATER THAN R-WORD The depth (Z-word) of a pocket formed using a G88.5 and G88.6 hemispherical pocket cycle cannot be greater than the radius (R-word) of that pocket. ZONE 2 PROGRAM ERROR The next block in the program or MDI entry would cause the specified axis to enter the restricted area of programmable zone 2.
Appendix C G-code Tables Appendix Overview This appendix lists the G-codes for 9/Series turning center. This table is presented numerically by G--code system B along with a brief description of their use. These G-codes are discussed in detail in the sections within this manual that refer to their specific use. The group numbers given in the table refer to modality. Group 00 is not modal and independent of other G-codes. The remaining G-code groups are modal with other G-codes with the same group number.
Appendix C G-code Tables A B C G12.1 Modal 21 G12.2 Spindle 1 Controlling 00 G13 QuickPath Plus (Use First Intersect.) 19 G14.1 Scaling (Disable) 15 G16.1 Virtual C (Cancel) Virtual C Cylindrical Interpolation G16.2 Virtual C End Face Milling G17 02 G18 Plane Selection Plane Selection G19 Plane Selection G90 G77 G20 G92 G78 G21 G94 G79 G24 G22 01 Single Pass O.D. and I.D.
Appendix C G-code Tables A B C G45 Modal 23 G46 Function Disable Spindle Synchronization Type Modal Set Spindle Positional Synchronization G46.1 Set Active Spindle Speed Synchronization G47 24 G47.1 Linear Acc/Dec in All Modes S-- Curve Acc/Dec for Positioning and Exact Stop Mode G47.9 Infinite Acc/Dec (No Acc/Dec) (AMP-- selectable only) G48 00 Reset Acc/Dec to Default AMPed Values G48.1 Acceleration Ramp for Linear Acc/Dec Mode G48.2 Deceleration Ramp for Linear Acc/Dec Mode G48.
Appendix C G-code Tables A B C G75 G75 G77 O.D. and I.D. Grooving Cycle G76 G76 G78 O.D. and I.D. Multi-Pass Threading Routine G80 Modal 09 Function Cancel or end fixed cycle G81 Drilling cycle (no dwell, rapid out) G82 Drilling cycle (dwell, rapid out) G83 Deep hole peck drilling cycle G83.1 Deep hole peck drilling cycle (dwell) G84 Right hand tapping cycle G84.1 Left hand tapping cycle G84.2 Right hand solid tapping cycle G84.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility Appendix Overview The 7300 Series CNC tape compatibility feature has been developed for customers with an existing library of standard 7320 and 7360 CNC tapes. This feature allows those 7300 tapes to be read and executed by the control. If desired, these 7300 tapes can be copied into the control’s memory to allow editing and execution, or they can be executed directly from tape, with the exception of 7300 pattern repeat subprograms.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility Table D.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility G28 and G29 Automatic Thread Cutting or Roughing Cycle G28 and G29 are not standard 7300s Lathe G-codes, but have been provided to enable automatic thread cutting or roughing. Both G28 and G29 are used for the Automatic Thread Cutting cycle. This Automatic Thread Cutting feature simplifies part programming of multiple-pass thread cutting operations for straight or tapered constant-lead threads.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility The format for the G28 block is: G28__D__X__Z__F Where: Specifies: D final threading depth or roughing depth. For Absolute Programming mode (G90), this parameter is programmed as an X axis position. For Incremental Programming mode (G91), this parameter is programmed as a distance measured parallel to the X axis from the initial work surface. X depth of first thread cutting pass or first roughing pass.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility The format for the G29 block is: G29__D__K__I__Z__L__F Where: Specifies: D return pass clearance, which is the distance between the initial work surface and the starting point. D value must always be programmed as an incremental distance, regardless of the current operating mode. K thread lead, which is the distance the thread cutting tool is to move along the Z axis per revolution of the spindle.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility CAUTION: The feedrate of any thread cutting pass is lead-limited to 100 inches per minute (IPM). If the values of the programmed thread lead and the currently active spindle speed generate a feedrate that exceeds 100 IPM, the control automatically reduces the value of the programmed thread lead to limit the thread cutting feedrate at 100 IPM. The lead of the resulting thread, therefore, is less than the programmed thread lead. Figure D.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility M-code Compatibility Considerations Table D.B lists all of the 7300 M-codes that the control can execute in 7300 mode. See the System 7360 Programming Manual for details on these M-codes and their operation. Table D.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility Offset Compatibility Considerations Tool Length Offset When the control is in 7300 mode, tool length offsets are activated in the same manner as on the 7300. The control supports 1- through 4-digit T-words, and through AMP configuration, you have the flexibility of specifying how the control activates offsets.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility The control has two offset tables: geometry and wear table. The sum from these two tables is used to generate tool length data when the tool offset number is programmed. When in 7300 mode, the active offset is also computed as the sum of the geometry and wear offsets. Refer to chapter 3 for details. When changing from inch to metric (or vice versa) in 7300 mode, the control does automatic conversion on tool offset values.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility Pattern Repeat A pattern repeat is a series of blocks of information repeated a specified number of times for a specified function. A pattern repeat is called in 7300 mode with the following format: (CP, name, r)# where: Name: Indicates: CP a pattern repeat is called. name the pattern blocks being called (part program name). r the number of times the pattern blocks get executed. # end of block.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility Executing 7300 Part Programs The system installer has to write PAL program for the control to execute in 7300 tape compatibility mode. Refer to the PAL manual for details. The control allows the Power-Turn-On mode (PTO) of the control to be specified in AMP with respect to inch/metric (G70/G71) mode and absolute/incremental (G90/G91) programming mode. For 7300 tape compatibility, we recommend that you select G70 and G90 for PTO mode.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility The main program, which has the pattern repeat call block “(CP, name, r),” can be executed from tape or from the control memory. However, if you want to make minor editing to your main program, you must copy the program into the control memory. Refer to section 10.2, “Inputting Part Programs,” for details on how to copy a program from tape. Important: To execute a program from tape, the tape must be positioned at the start of the main program.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility Table D.
Appendix D Allen-Bradley 7300 Series CNC Tape Compatibility D-14
Index Index (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual Numbers 7300 Series CNC Tape Compatibility Automatic Mode, 7-23 Automatic Return from Machine Home (G29), 14-15 Automatic Tool Management, 20-14 9/240 G--Codes Applicable, D-12 Automatic MultiPass Roughing, D-3 Automatic Thread Cutting (G28, G29), D-3 Features Not Supported on 9/240, D-13 G--Code Considerations, D-1 M--Code Considerations, D-7 Overview, D-1 Tool Length Offset, D-8 Tool Life Management, D-
Index 9/Series Lathe Operation and Programming Manual C C Axis, Virtual, 17-13 C-Word, 10-21 Cancel Fixed Cycle (G80), 26-8 Casting/Forging Roughing Cycle Routine (G75), 24-29 Chamfering and Corner Radius, 16-1 Changing Languages, 8-23 Changing Parameters Auto Erase, 8-32 Auto Size, 8-30 Grid Lines, 8-30 Overtravel Zone Lines, 8-30 Process Speed, 8-32 Rapid Traverse, 8-29 Select Graph, 8-29 Sequence Starting #:, 8-31 Sequence Stopping #:, 8-31 Changing parameters, {GRAPH SETUP}, 8-28 Chinese, Language Dis
Index Index (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual Displaying Position ABS, 8-6 ABS (Large Display), 8-7 absolute (Small Display), 8-7 ALL, 8-19 distance to go (Small Display), 8-13 DTG, 8-12 DTG (Large Display), 8-13 G Code Status, 8-20 M Code Status, 8-16 PRGRAM, 8-3 PRGRAM (Large Display), 8-4 PRGRAM (Small Display), 8-5 PRGRAM DTG, 8-17 program/DTG (Small Display), 8-18 Target, 8-9 Target (Large Display), 8-10 target (Small Display), 8-10 Distance to Go
Index 9/Series Lathe Operation and Programming Manual Changing and Inserting, 5-8 Entering Characters and Blocks, 5-7 Erasing Characters and Blocks, 5-11 EIA (RS-244), 9-7 Emergency Stop Operations, 2-12, 2-22 Emergency Stop Reset, 2-12, 2-22 End Face Milling, 17-20 Energizing the Control, 2-19 English, Language Display, 8-23 Entering Characters and Blocks, 5-7 Entering Interference Values Manually, 30-25 Entering Interference Values Through Programming, 30-27 Entering Part Programs Offline, 6-1 Erasing C
Index Index (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual G31, 27-2 G31.1, 27-2 G31.2, 27-2 G31.3, 27-2 G31.4, 27-2 G33, 25-6 G34, 25-12 G36, 18-19 G36.1, 18-19 G37, 27-3 G37.1, 27-3 G37.2, 27-3 G37.3, 27-3 G37.4, 27-3 G39, 21-9 G39.1, 21-9 G40, 21-4 G41, 21-4 G42, 21-4 G47, 18-15 G48, 18-16 G52, 11-17 G53, 11-3 G54-59.3, 11-4 G61, 18-18 G62, 18-18 G63, 18-18 G64, 18-18 G65, 28-43 G66, 28-44 G66.
Index 9/Series Lathe Operation and Programming Manual Groups, for dual axes, 30-38 H Hardware Installed, 8-37 Hardware Overtravel, 12-2 Hole Machining Axes, 26-4 Index (General) 9/Series PAL Reference Manual Enabling, 29-1 Program, 29-8 Request, 29-4 Types, 29-5 Italian, Language Display, 8-23 J Homing a Dual Axis, 19-4 Japanese, Language Display, 8-23 Homing, Manual Machine, 4-9 Jog Offset, 11-19 Homing, the Axis Automatic Homing, 14-12 Automatic Return from Machine Home (G29), 14-15 Machine Ho
Index Index (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual M M --Code Status Display, 8-16 M Codes, M00 program stop, 28-42 M-Codes, 10-27 M00 Program Stop, 10-30 M01 Optional Program Stop, 10-30 M02 End of Program, 10-30 M03 Primary Spindle Clockwise, 17-12 M04 Primary Spindle Counterclockwise, 17-12 M05 Primary Spindle Stop, 17-12 M19 First Spindle Orient, 17-10 M19.2 Spindle 2 Orient, 17-10 M19.
Index 9/Series Lathe Operation and Programming Manual O O.D. & I.D. Finishing Routine (G72), 24-35 O.D. & I.D. Grooving Cycle (G77), 23-6 O.D. & I.D. Multipass Threading Routine (G78), 25-20 O.D. & I.D.
Index Index (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual Single--Pass Turning Cycles, 22-1 Power Up Display, 8-37 Parametric Expressions, 28-2 Power--Up Conditions, 2-21 Parity, for communications, 9-6 Preparatory Functions, 10-22 Parking a Dual Axis, 19-3 Preset Work Coordinate Systems, 11-4 Part Production/Automatic Mode, 7-23 Probing Applications (G31), 27-3 Applications (G37), 27-5 Skip Function (G31), 27-2 Tool Gauging, 27-3 Part Program Error Cond
Index 9/Series Lathe Operation and Programming Manual Index (General) 9/Series PAL Reference Manual R Programmable Zones, 12-1 Programming Configuration, 10-6 R-Word, 10-21 Programming Data and Backing up Tool Management Tables, 20-22 Radius Mode (G07), 13-5 Programs Inputting from Peripheral, 9-9 outputting to peripheral, 9-13 verifying against source, 9-17 Rapid Feedrate, 18-6 Prompting Format Drill Cycle, 5-25 G--Codes, 5-21 Lathe Cycle, 5-23 QuickPath Plus, 5-18 Protectable Directory Protec
Index Index (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual Moving the Cursor, 5-6 Program Search, 7-9 Search With Recall, 7-12 Select Graph, 8-29 Selecting a Part Program Input Device, 7-5 Selecting Linear Acc/Dec Modes, Using G47, 18-15 Selecting Linear Acc/Dec Values, Using G48, 18-16 Separate Spindle Configuration, 30-18 Sequence Numbers, 10-9, 10-33 Sequence Stop, {SEQ STOP}, 7-2 Servo Firmware Revision, 8-37 Servo Modules Installed, 8-37 Setting Communications
Index 9/Series Lathe Operation and Programming Manual MERGE PRGRAM, 5-15 MID ST PRGRAM, 7-12, 7-25 MODIFY INSERT, 5-8 MORE LIMITS, 3-22 MORE OFFSET, 3-9 NCRYPT MODE, 5-45 PASSWORD, 2-24 PLANE SELECT, 5-27, 5-30, 13-1 PRGRAM, 8-1, 8-3 PRGRAM CHECK, 7-19, 8-24 PRGRAM DTG, 8-17 PRGRAM MANAGE, 5-43 PRGRAM PARAM, 26-39 PROGRAM DTG, 8-1 PTOM SI/OEM, 8-37 QPATH+ PROMPT, 5-18 QUICK CHECK, 7-18, 8-24 QUICK VIEW, 5-16 RANDOM TOOL, 20-7 REFORM MEMORY, 2-38 RENAME, 5-37 RENUM PRGRAM, 5-14 SAVE PARAM, 8-32 SCREEN SAVE
Index Index (General) 9/Series Lathe 9/Series PAL Reference Manual Operation and Programming Manual Synchronization Coordinating, 30-10 Cycle Stop, 30-11 M-codes, 30-7 MDI Mode, 30-11 Multiple Part Programs, 30-7 Program Interrupts, 30-11 Simple, 30-8 With Setup, 30-8 Synchronized Spindle, 17-23, 17-24, 17-26 System A, G Code, 13-3 System Error Messages, B-1 System Integrator Message, 8-37 System Startup Screen, 8-37 System Timing Screen, 8-37 T T-Word, 20-2 Programming T-word, 20-3 Thread Cutting, 25-1
Index 9/Series Lathe Operation and Programming Manual Linear Transition (G39), 21-9 Linear Transition (G39), 21-8 Machine Home (To/From), 21-49 MDI or Manual Motion, 21-47 Minimum Block Length, 21-9 Non--Motion Blocks, 21-39 Overview, 21-1 Programming Instruction, 21-4 Special Cases, 21-35 Work Coordinate System, Offsetting, 21-51 TRVRS, 2-13 Turing Cycle Operations, O.D. & I.D.
Publication 8520-- UM511A-- EN-- P - November 2000
Publication 8520-- UM511A-- EN-- P - November 2000 Supercedes Publication 8520--5.1.1 -- August 1998 Publication 8520-- UM511A-- EN-- P - November 2000 PN 176953 Copyright 2000 Allen-Bradley Company, Inc.
