CENTURION 7 CNC Operation Manual Version 3.2 June 2003 MILLTRONICS MANUFACTURING COMPANY 1400 Mill Lane Waconia, MN 55387 952- 442-1410 952-442-1401 Technical Support 952-442-1418 Parts http://www.milltronics.
Copyright 2003 Milltronics Manufacturing All Rights Reserved
PREFACE This manual describes the operation of the Centurion 5, 6 and 7 CNC controls. From the operator’s standpoint there is no visible difference. Functionality is the same in all controls. The Centurion 7 hardware offers enhanced performance, larger memory, and faster processing. When this manual makes reference to Centurion 7, it implies Centurion 5 and 6 also. The Centurion 7 has five controllable axes in its basic configuration: X, Y, Z, A, and B.
TABLE OF CONTENTS PREFACE ...................................................................................................................................... iii AXIS DEFINITIONS ..................................................................................................................... 1 INTRODUCTION .......................................................................................................................... 3 SECTION ONE - PROGRAM CONFIGURATION ....................................
TABLE OF CONTENTS F6 (Displ) Main-Displ............................................................................................................... 34 F7 (Parms) Main-Parms............................................................................................................ 34 F1 (Setup) Main-Parms-Setup .................................................................................................. 35 F2 (Prec) Main-Parms-Setup-Prec................................................................
TABLE OF CONTENTS F2 (Conv) Main-Prog-Conv...................................................................................................... 84 F1 (Edit) Main-Prog-Conv-Edit................................................................................................ 84 Definitions of the Edit Keys ..................................................................................................... 85 Definitions of the Store/Input Keys .................................................................
TABLE OF CONTENTS F3 (Tool) ................................................................................................................................. 105 F4 (Cont)................................................................................................................................. 105 F9 (Skip) ................................................................................................................................. 105 F10 (Mirr) ....................................................
TABLE OF CONTENTS F3 (Rect) Mill-Frame-Rect ..................................................................................................... 148 F5(Poly) Mill-Frame-Poly ...................................................................................................... 148 F7 (3dPkt) Mill-3dPkt............................................................................................................. 149 F1 (Start) Mill-3dPkt-Start....................................................................
TABLE OF CONTENTS End of Program ....................................................................................................................... 190 SECTION FOUR - PREPARATORY FUNCTIONS (G CODES)............................................ 191 G Codes................................................................................................................................... 191 Interpolation functions .............................................................................................
TABLE OF CONTENTS Work coordinate systems (G54 - G59)(G5#0…G5#9)........................................................... 257 Local coordinate system (G52)............................................................................................... 257 Single direction or one shot rapid positioning (G60).............................................................. 259 Exact stop mode (modal) (G61)..............................................................................................
TABLE OF CONTENTS SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) ........................................ 303 Program stop (M00)................................................................................................................ 305 Optional stop (M01)................................................................................................................ 305 Block skip ( / ).................................................................................................................
TABLE OF CONTENTS MOD ....................................................................................................................................... 342 ORIGIN................................................................................................................................... 342 SECTION SEVEN - SAMPLE PROGRAMS............................................................................ 347 APPENDIX........................................................................................
AXIS DEFINITIONS All directions are referenced with respect to the tool. The following illustrates the X, Y, and Z directions.
INTRODUCTION A group of commands given to the CNC for operating the machine is called a program. By specifying commands the tool is moved along a straight line or an arc, and machine functions such as coolant on/off, tool change, or spindle on/off are performed. The function of moving the tool along straight lines and arcs is called interpolation.
INTRODUCTION The following types of coordinate systems are available. 1. Machine system 2. Work coordinate system 3.
INTRODUCTION The position to be reached by the tool is commanded with a coordinate value referenced to one of the above coordinate systems. The coordinate value consists of one component for each axis, X, Y, and Z. Coordinate values may be given in either absolute or incremental mode. In absolute mode, the tool moves to a point the programmed distance from the zero point of the coordinate system. In incremental mode, the tool moves to a point the programmed distance from the current tool position.
SECTION ONE - PROGRAM CONFIGURATION By definition, a program is a group of commands given to the CNC for operating a machine. By specifying commands, the tool is moved along a straight line or an arc, or the spindle motor is turned on and off. In a program, specify the commands in the sequence of actual tool movements. Block Block Block Program Block Tool movement sequence . . . Block A group of commands at each step of the sequence is called the block.
SECTION ONE – PROGRAM CONFIGURATION Program Normally a program number is specified at the beginning of a program, and a program end code (M99, M02, M30) is specified at the end of the program. Neither is required; however, it may be advantageous to omit the program end code from programs that are used as subprograms. An end program code is assumed when the end of the main program is encountered.
SECTION ONE – PROGRAM CONFIGURATION Subprograms can be used to build part libraries of commonly used patterns and can reside anywhere in memory. Command format ranges The basic address and command value ranges are listed in the table below. Note these figures give the maximum numerical limit for the control. These limits will always be greater than or equal to the physical limits of the machine. The machine limits are set via parameters in the machine setup section of the control.
SECTION ONE – PROGRAM CONFIGURATION Command formats for axes: M and G codes Axis commands can be programmed in a calculator format. No leading or trailing zeros are necessary. Whole numbers may be programmed without the decimal point. A decimal point may be used with mm, inches, or second values. The location of the decimal point is as follows. Z15.0 F10.0 G04 P1 Z15 millimeters or Z15 inches 10 mm/min., or 10 inch/min.
SECTION TWO - FRONT PANEL OPERATION The Centurion 6 front panel has two 16-key keypads and 12 function keys. The keypads are used to enter the alphanumeric data requested by the CNC. The upper keypad is used primarily to enter alpha characters. To enter one of the shifted characters simply press and release the Shift key then the character. After the character has been entered, the control automatically returns to the non-shifted character set.
SECTION TWO - FRONT PANEL OPERATION Centurion 7 Front Panel 12
SECTION TWO - FRONT PANEL OPERATION Diagram of Main Screen 1 2 3 4 5 6 7 8 RunTime When you are verifying a program the runtime displays the calculated time to make the parts. When you are running a program it shows the elapsed time since the program was started. The total of all program run times are kept in the “Job Time” parameter (F7 Parms – F9 Ctrl). History Line History Line shows you where you are in the software and where you came from.
SECTION TWO - FRONT PANEL OPERATION Diagram of Status Window 1 2 3 4 5 6 7 8 9 10 11 12 13 14 The \ changes back and forth to / and \ each time the status window is updated. Comp: Tool Radius Compensation (Left, Right or Cancelled) Tool: The first two digits indicate the active tool number. The second two digits in parentheses indicate the pending tool number. If you execute a T14 without the M6 the pending tool number will be 14. The tool length. The tool radius.
SECTION TWO - FRONT PANEL OPERATION 15 16 17 18 Spindle override and direction: The position of the spindle override and the resulting rpm (if there is no spindle encoder) or the actual rpm (if there is a spindle encoder). This line also displays whether the spindle is off or running CW or CCW. The spindle load meter will show the load on the spindle. It becomes longer and changes color from blue to green to yellow to red as the load increases.
SECTION TWO - FRONT PANEL OPERATION F2 (JOG) Main-Jog The machine must be homed prior to jogging. F2 (Jog) is used to move the machine around in a manual mode to pick up zeros and align parts. Upon pressing F2 (Jog) the following screen appears. Note: F5 and F6 can be changed to store the positions in the G92 floating zero offset. The function keys across the bottom of the screen select the desired jogging mode. The F1 (Slow) key selects slow jog.
SECTION TWO - FRONT PANEL OPERATION F3 (HDW) Main-HDW The machine must be homed prior to handwheeling. The handwheel mode is used to move the machine around using the electronic handwheel. Its main use is for setting tool length offsets, setting work offsets, and aligning parts. Upon pushing F3 (HDW) the following screen will appear. Note: F8 can be changed to store the positions in the G92 offset.
SECTION TWO - FRONT PANEL OPERATION Procedure for Setting Tool Length Offset Note: there is an alternative method for setting tool lengths on 31. A tool length offset is used to compensate for the difference between Z axis home and part surface (part zero). Setting floating zero in Z axis is not recommended. To set tool length offset, load tool #1 in the spindle by doing an MDI→ T1M6. Use handwheel or jog to touch the tool on the part at a known location. Select F6 (ZTool).
SECTION TWO - FRONT PANEL OPERATION Procedure for Setting a Work Offset A work offset shifts the X and Y axis zero positions to a desired place (edge of the part). Thus a part can be programmed from its part zero. To find and set a work offset, refer to the example. Using a ½" diameter edge finder in the X axis, handwheel or jog to the edge of the part and depress F8 (G54-X). Establish whether the edge finder is positive or negative from the desired zero. Enter -.25 for the X position.
SECTION TWO - FRONT PANEL OPERATION F4 (Run) Main-Run (The machine must be homed prior to running a program) The F4 (Run) key is used to execute the active program. Upon depressing the F4 (Run) key, the following screen appears. After the above screen appears, F1 (Start) must be pushed and the following screen will appear.
SECTION TWO - FRONT PANEL OPERATION pushed, the control will request that the desired block or sequence number be typed in, followed by Enter. If Cycle Start is depressed, the active program will start running from the selected block number. If F3 (Tool) is depressed, the control will request a tool number. After typing the tool number followed by an Enter, Cycle Start is pressed, and the active program will start running at the desired tool number and the following screen will appear.
SECTION TWO - FRONT PANEL OPERATION axes can be jogged or handwheeled away from the work, the spindle may be turned on/off, and F9 (Resum) remains active. As long as the Resume is active, the F9 key on the Run screen will show a Resume function. If the Resume function is selected, the active program will be resumed at the halted point. First, Z will retract to the tool change position–all the way up–when a Resume Cycle Start is executed. Second, X and Y will rapid to the halted point.
SECTION TWO - FRONT PANEL OPERATION F6 (Displ) Main-Run-Displ The F6 (Displ) key can be accessed from a number of screens. The following screen is shown as though the F6 (Displ) was entered from the RUN screen. All the display functions and screens are identical, independent of the entry point. Only the return point differs based on the original entry point. When the F6 (Displ) key is depressed, the following screen will appear. Note: F7 and F9 only come up in protected modes.
SECTION TWO - FRONT PANEL OPERATION F2 (Error) Main-Run-Displ-Error The Following Error refers to the lag in the servo system. The F2 (Error) key changes the display to read current position, next position, and Following Error. The Following Error display is intended to help in machine setup or troubleshooting an axis problem. When F2 (Error) is pressed, the following screen will appear.
SECTION TWO - FRONT PANEL OPERATION The graphics on this control are full 3D and will be displayed in the graphics area as long as the control remains in the Graph mode. When other displays are requested, windows will appear in the graphics area showing the requested data. When these functions are finished, the windows will disappear and the graphic display will be reinstated. The scales at the bottom and left side of the screen are to be used as a reference for the part size.
SECTION TWO - FRONT PANEL OPERATION Note: The display is auto-scaled when the new orientation is displayed. F2 (Pan) Main-Run-Displ-Graph-Pan The F2 (Pan) key selects the pan function, which allows the operator to pan around a part. The following display will appear. The crosshair which appears on the screen can be moved around using the numerical keys or arrow keys F7 thru F10.
SECTION TWO - FRONT PANEL OPERATION F3 (Wind) Main-Run-Displ-Graph-Wind The F3 (Wind) key selects the window function which allows the operator to window in on a particular area of the part. The following display will appear when F3 (Wind) is selected. The crosshair which appears on the screen can be moved around using the numeric keys or arrow keys F7 thru F10 (the same as pan). To zoom in using a window, move the cursor to the first corner of the window area and depress F5 (Enter) or Enter.
SECTION TWO - FRONT PANEL OPERATION F6 (Zoom+) Main-Run-Displ-Graph-Zoom+ The F6 (Zoom) key selects the zoom+ function which doubles the size of the part being displayed on the screen. Generally, this function is used to enlarge a specific area of a part enabling the operator to see greater detail. F7 (Limit) Main-Run-Displ-Graph-Limit The F7 (Limit) key draws a box on the screen which corresponds to the axis limits of the machine. This allows viewing of the part in relation to the machine's overtravels.
SECTION TWO - FRONT PANEL OPERATION The following screens represent the displayed information for the various axis selections. Note: The diagnostic screens will differ for machines that have varying options. The text that shows up on the screen is from the files INP.XXX and OUT.XXX, where XXX is the extension for the desired language to display on the screen. The INP.XXX and OUT.XXX files for a basic machine with no options are present in the ROM directory.
SECTION TWO - FRONT PANEL OPERATION F7 (Menu) Main-Run-Menu The F7 (Menu) key selected from the Run or Verify screen brings up a window containing a listing of all the available programs, which may be run. The screen shown below will be displayed when the program menu is requested. To activate one of the programs listed in the window, use the arrow and page keys to move the cursor to the desired program and press F5 (Enter), or Enter on the keyboard.
SECTION TWO - FRONT PANEL OPERATION F10 (HDW) Main-Run-HDW When the F10 (HDW) key is activated, the axis moves in the program will relate to turning the electronic handwheel. The feedrates (feed/rev. or feed/min.) will effect the distance moved per click of the handwheel. The four miscellaneous parameters that effect the distance moved per click of the handwheel are listed below. 1. Handwheel Encoder PPU Pulses per rev of the electronic handwheel. This should be 400 for our current systems. 2.
SECTION TWO - FRONT PANEL OPERATION During the tool setting routine, the tool table is loaded with the appropriate values. After all the tool offsets are loaded, the operator can press ESC (Halt) to exit the tool setting routine. Note: This routine can be modified for specific applications (auto tool setters, different tool changers etc.). F5 (MDI) Main-MDI The F5 (MDI) key on the Main menu selects the MDI (manual data input) function.
SECTION TWO - FRONT PANEL OPERATION 20 English 22 Safe zone check off 24 Circ Pocket Clear 26 Circ Finish Outside 29 Return From Ref 31 Z to Clearance 33 Facing Cycle 35 Rect Finish Inside 39 Threading Cycle 41 Left CutterComp On 43 + H Offset Dir 45 Left Auto Comp On 47 Auto Comp Off 50 Scaling Off 52 Local Coordinate 54 Worksystem 1 56 Worksystem 3 58 Worksystem 5 60 One-Shot Rapid Move 63 Tapping Mode On 65 Move Lockout Block 69 Rotation Off 71 Mirror Image On 73 Woodpecker Drill 76 Fine Bore 80 Canned C
SECTION TWO - FRONT PANEL OPERATION 08 Flood On 30 Spindle Off, End of Program 91 Graph On 94 3D Sweep On 96 Rounded Wall 98 Call Jump 09 Coolant Off 90 Graph Off 93 3D Sweep Off 95 Tapered Wall 97 Pocket Clear 99 End of Program Note: The text file that displays the legal M codes on the screen is Mcodes.XXX, where XXX is the extension for the corresponding language. The control first looks for Mcodes.XXX in the RAM directory. If not found, it then searches the ROM directory for the file.
SECTION TWO - FRONT PANEL OPERATION F1 (Setup) Main-Parms-Setup The F1 (Setup) selection brings up the parameters, which make the control unique to a particular machine or application. When F1 (Setup) is selected the following screen appears. Note: F2 (Prec) through F9 (DOS) are only displayed if the control is in the protected mode set by a validation code. The CNC requires a VALIDATION CODE and an ACCESS LEVEL number to allow the machine setup parameters to be displayed or changed.
SECTION TWO - FRONT PANEL OPERATION Note: The parameters in the setup sections are normally set by the machine tool builder. Changing these parameters can affect a large number of machine functions and machine performances and should only be modified by experienced service personnel. Assuming the proper codes have been entered, the following screens can be selected. F2 (Prec) Main-Parms-Setup-Prec If the F2 (Prec) selection for Machine Precision is made, the following screen will be displayed.
SECTION TWO - FRONT PANEL OPERATION Note: When editing or entering parameter values (or any other numeric value on the control), you can use the built in calculator. Example: Instead of entering .3750 you may enter 3/8 Instead of entering 1.3750, you may enter 1 + 3/8 If you want to modify the current value, you may use “.” as the current value. If the current value is .358 and you want to add .002, type .+.002 (instead of entering .360).
SECTION TWO - FRONT PANEL OPERATION recognize commands over either the RS-232 or CLK/DATA interface. Whenever a valid command with no error is received over the RS-232 interface, it will start transmitting over the RS-232 interface and not the CLK/DATA interface. In like fashion, it is possible to switch back to the CLK/DATA interface. Whenever a valid command with no error is received over the CLK/DATA interface, it will start transmitting over the CLK/DATA interface and not the RS-232 interface.
SECTION TWO - FRONT PANEL OPERATION Alternatively, the CNC program will use the serial keyboard interface if the serial keyboard parameter is set to Yes and the letter "s" appears as an option on the command line. The serial keyboard is enabled in the following examples if the serial keyboard parameter is also set to yes.
SECTION TWO - FRONT PANEL OPERATION 100% Rapid in Dry-Run: No means the feedrate override will affect rapid moves in the dry run mode. Yes means the feedrate override will not affect rapid in the dry run mode. Rapid moves are 100%. Spindle on in Dry-Run: No means the spindle will not come on in the dry run mode. Yes means the spindle will come on in the dry run mode. Tool Tables by: Radius or Diameter Don't Load Canned Cycles: No means Canned Cycles will be loaded.
SECTION TWO - FRONT PANEL OPERATION Put Pot down on swing arm tool changers: Yes means the pot will be down for the pending tool. No means it will be up. Check drawbar switch: Yes for newer machines with drawbar switches.
SECTION TWO - FRONT PANEL OPERATION Parameter file version: Should always be 1 Use Small Soft keys: Should be set to no for 12" CRT monitors Notes on Parameters Note 1: To change a parameter, press F1 (Edit) and type in the new number. Note 2: After changing any power parameter, return to the main menu before cycling power. Note 3: After any power parameter is changed, the machine must be powered down, then up again. These parameters are only read on power up.
SECTION TWO - FRONT PANEL OPERATION may then recommence. Some parameters can be related to the machine position. To edit or load these parameters, use F4 (Mach) to load the X, Y, and Z positions into the parameters. Use the F5 (M-XY) for the X and Y axis or the F6 (M-Z) key for the Z axis. The following is a list of all the selectable parameters displayed in this mode and a description of their functions. Axis Address Label X 88.0000 Y 89.0000 Z 90.0000 Pulses Per Unit X 10000.0000 Y 10000.0000 Z 10000.
SECTION TWO - FRONT PANEL OPERATION Home Sequence X 02.0000 Y 02.0000 Z 01.0000 These numbers determine the order the axes will home in: #1 first, #2 next, etc. Axes with the same number home together. 0 will cause that axis to not home. Positive Limit X 00.0000 Y 00.0000 Z 00.0000 Dimension from machine zero where the positive software limit occurs Negative Limit X -31.0000 Y -18.0000 Z - 6.5000 Dimension from machine zero where the negative software limit occurs Maximum Feed X 200.0000 Y 200.
SECTION TWO - FRONT PANEL OPERATION Rapid Acc/Dec X 20.0000 Y 20.0000 Z 20.0000 The Rapid Acc/Dec is a number that determines the rate at which the axis velocity is increased or decreased for rapid moves. The smaller the number the longer the Acc/Dec times will be. Acceleration and deceleration in this control are linear ramp units and are in inches per sec². Feed S-Curve Acc (Cent 7 and up) The units are identical to the (linear) acc/dec. These ramps are used when the s-curves are enabled in feed moves.
SECTION TWO - FRONT PANEL OPERATION G60 Unidirectional X 00.0000 Y 00.0000 Z 00.0000 Same as G00 unidirectional except only active in a G60 block Backlash X 00.0000 Y 00.0000 Z 00.0000 Sets the distance in inches or mm. The control will compensate for lost motion whenever an axis reversal takes place. Active in all modes. Excess Error X 00.2500 Y 00.2500 Z 00.2500 Sets the distance in inches or mm. The machine can lag behind the CNC. The CNC will shut the system down due to an excess following error.
SECTION TWO - FRONT PANEL OPERATION Home Switch=0 Marker=1 X 00.0000 Y 00.0000 Z 00.0000 Sets whether an axis will seek a home limit switch and then the marker pulse, or just seek the nearest marker pulse. Max Handwheel Error X 01.0000 Y 01.0000 Z 01.0000 When the excess error reaches this value, pulses from the handwheel are ignored. Error is specified in inches or mm. Tool Change X + 00.0000 Y + 00.0000 Z + 00.0000 Z moves to this location on a G32 (Z to toolchange) or M6 (toolchange) command.
SECTION TWO - FRONT PANEL OPERATION F5 (Misc) Main-Parms-Setup-Misc The F5 (Misc) key brings up various miscellaneous setup parameters dealing with the spindle and M codes. When F5 (Misc) is selected, the following screen appears. Miscellaneous parameters are edited similarly to the Power parameters. The following is a list and short description of the miscellaneous parameters. Basic Machine Info Machine Type Type in VMD30, etc.
SECTION TWO - FRONT PANEL OPERATION Spindle Encoder PPU1 Pulses per rev of spindle, used for hard tapping option and displaying the RPM in gear 1 Spindle encoder PPU2 Pulses per rev of spindle, used for hard tapping option and displaying the RPM in gear 2 Handwheel Encoder PPU Pulses per rev of the handwheel, should be 400 for current systems Spindle Range 1 Max spindle speed for gear 1 Spindle Range 2 Max spindle speed for gear 2 . . .
SECTION TWO - FRONT PANEL OPERATION Hard Tap Fudge Factor Used to adjust the depth of rigid tapping cycle. Higher numbers will decrease the amount of overshoot at the bottom of the hole. Feed Back on Mitutoyo Scale Yes will enable the Z axis feedback from the Mitutoyo scale options. Feed Back on Quill Scale Yes enables the glass scale for Z axis quill options. Quill Epsilon If the value is zero no error checking is done for quill movement.
SECTION TWO - FRONT PANEL OPERATION Door Open Override Axis Door Open Override Input See notes on European code (page 55) at the end of this section. Check Tool Door Open If Yes, Z input 10 is checked before tool changer arm is commanded. If the input is not seen in 15 seconds, a timeout error is displayed. Check Processor Temperature If Yes and the over temperature Z input 4 is made, an over temp message will be displayed. Cool-Down Time (Min) (Cent 6 and up) Used on spindle air-purge systems.
SECTION TWO - FRONT PANEL OPERATION rapids. This parameter should be approximately 100 for our current systems. Sharp Corners Yes will cause all corners to be rounded to a maximum specified by the max corner deviation parameter. No will round the corners proportionally to the feed rate. Full feed rate will round the corners by the max corner deviation parameters. Slower federates will reduce the deviation. Max Corner Deviation This number sets the maximum deviation allowed on a corner. A value of .
SECTION TWO - FRONT PANEL OPERATION Software Options Security Code # 0 Secret code to enable S-curves Use S-curves (Cent 7 and up) Yes to enable S-curves for acceleration and deceleration. Look Ahead (Cent 6 and up) Specifies the number of axis moves the control can see ahead, which enables the control to prepare for sharp corners or features that could otherwise be rounded off when feedrates are increased. Note: Look Ahead is only active in DNC-fast mode. Valid values are between 10 and 255.
SECTION TWO - FRONT PANEL OPERATION Use FLZ instead of G54 Used for setting work offset in jog and handwheel mode. Yes means use FLZ (G92 offsets). No means use G54 offsets. Tool Setting If set to any tool the jog and handwheel tool setting routines will prompt the operator for the tool # being set. If it is set to current tool the control will assume the active tool # is the one that is being set. Tool Setting Use Work Offsets If set to No, the position given by the operator is relative to home.
SECTION TWO - FRONT PANEL OPERATION Post M codes Table Post M code #0 Post M code #1 Post M code #2 Post M code #3 Post M code #4 Post M code #5 Post M code #6 Post M code #7 Post M code #8 Post M code #9 M codes listed here will be executed after all other operations within the block. Report File DOS file names to write DPRINT text to when using POPEN P0 Command Name Any string in this parameter will show up on the F10 (Util) key.
SECTION TWO - FRONT PANEL OPERATION Max Feed with Door Open The maximum speed the machine can move with the door open with the Door-Override Button pressed Soft Start Delay (secs) Time delay before allowing axis movement after the machine is reset. The software that relates to European codes concerns a safety door open switch. Below is a description of how the software operates relating to the Set Up button and the software parameters.
SECTION TWO - FRONT PANEL OPERATION If the door is open and Setup is held in, the machine will handwheel up to the 70% rate on the feedrate override switch, which is 2mm per click of the handwheel. (It is difficult to generate speeds greater than 1000 mmpm in this mode). Modifying the distance per click of the handwheel also requires a password available only to the machine builder. If the doors are opened while the machine is running: 1 2 3 4 The spindle will shut off. The axis will stop moving.
SECTION TWO - FRONT PANEL OPERATION Keys displayed in the Edit Mode: F5 (HwOvr) Main-Parms-Setup-OVRs- HwOvr The F5 (HwOvr) key brings up the handwheel switch settings for the feedrate override switch. These settings determine how far an axis will move for one increment of the handwheel (001=1 pulse). Editing is performed in the same fashion as feedrate override parameters. The following screen displays the handwheel override settings.
SECTION TWO - FRONT PANEL OPERATION F6 (SpOvr) Main-Parms-Setup-OVRs-SpOvr The F6 (SpOvr) key brings up the 16 spindle override switch settings. These settings are the percentages a spindle command will be overridden at each switch position. The spindle override parameters are changed in the same fashion as the feedrate override parameters. The spindle override screen is displayed below.
SECTION TWO - FRONT PANEL OPERATION F7 (BSC) Main-Parms-Setup-BSC Ballscrew Compensation Table Creation Help Type X, Y, Z (A,B,C) to select the axis. F1 (New) creates a new, zero ballscrew table. F2 (On) turns ballscrew comp on for given axis. F3 (Off) turns ballscrew comp off for given axis. F4 (Load) loads the ballscrew table into the axis. F5 (Gap) changes the spacing in the ballscrew file generated from F1 (New). F6 (Edit) jumps into editor with ballscrew table.
SECTION TWO - FRONT PANEL OPERATION F2 (Coord) Main-Parms-Coord The F2 (Coord) key of the parameter screen brings up the parameters dealing with the various coordinate systems in the control. To edit the work coordinate parameters, use the PgUp, PgDn, and arrow keys to position the cursor to the correct parameter, then push the F1 (Edit) key and arrow to the desired axis. Type in the new values and press Enter, then ESC (Exit).
SECTION TWO - FRONT PANEL OPERATION Keys displayed in the Edit Mode: Operation of the work coordinate systems G92 and G52 are discussed in Section 4 page 294 (G92) and page 257 (G52). These parameters are positions relative to the machine zero and will become the new zero point when they are used. The F4 (Mach) key in the edit mode enters the current machine position as the work coordinate zero point for X, Y, and Z axes. The F5 (M-XY) enters the coordinates for X and Y axis only.
SECTION TWO - FRONT PANEL OPERATION F4 (D Off) Main-Parms-D Off The F4 (D Off) key displays the 99 D radius or diameter offsets available on the CNC. These offsets are accessed and edited in the same manner as all other parameters. Following is the D offset screen. The cursor will default to the active tool number.
SECTION TWO - FRONT PANEL OPERATION F5 (H Off) Main-Parms-H Off The F5 (H Off) key displays the 99 H tool length offsets available on the control. These offsets are accessed and edited in the same manner as all other parameters. The H offset screen follows. The cursor will default to the active tool number. F6 (Save) Main-Parms-Save F6 (Save) saves all files in the RAM directory to a floppy. You will be informed that duplicate files on the floppy will be overwritten.
SECTION TWO - FRONT PANEL OPERATION F8 (Prog) Main-Parms-Prog This set of parameters gives the machine programmer access to all the internal parameters the CNC is using to execute a program. Normally these parameters would be used for display purposes only as an aid to program debugging. However, it is possible to read and change these parameters in a parametric program.
SECTION TWO - FRONT PANEL OPERATION P232 thru P239 Contains the work coordinate offset relative to the machine zero of the enabled axis P232=X P233=Y P234=Z . . . etc P240 thru P247 Contains the active tool length (H) parameter for the enabled axis P240=X P241=Y P242=Z . . .
SECTION TWO - FRONT PANEL OPERATION P304 Status if control is in data mode or normal programming (o=off, 1=on) P305 H offset direction or sign P306 Status of 0=G0, 1=G1, 2=G2, 3=G3 mode P307 Not used P308 Number of active plane 0=G17 (X4), 1=G18 (ZX), 2=G19 (YZ), 3=G18 (XZ) P309 Cutter comp.
SECTION TWO - FRONT PANEL OPERATION P320 thru P322 Gives the primary, secondary, and tertiary axis based on plane selection X=1 Y=2 Z=3 . . . etc For G17 XY pri=1 sec=2 ter=3 For G18 ZX pri=3 sec=1 ter=2 For G19 YZ pri=2 sec=3 ter=1 For G18 XZ pri=1 sec=3 ter=2 P323 0 = Return to R-plane (G99), 1 = initial level (G98) P324 Tapping mode (0 = off, 1 = on) P369 Job time (sum of run times) P370 True tool number used for tool changers Block Rate Block per second for the last program executed.
SECTION TWO - FRONT PANEL OPERATION Auto Rotary Brake Yes will control the rotary brake on A and B axis automatically. This parameter shuts off before rotary moves, and it turns the brake back on when the move is complete. Rotary Brake Delay (Secs) This is the delay in seconds after an M11 (A axis brake release) and M13 (B axis brake release). It is also the delay time after autobrake release in Home, Jog, and Handwheel. The default is .25 seconds. Max is 2.55 seconds.
SECTION TWO - FRONT PANEL OPERATION Message Only The message shown appears below: and perform an alternate operation, change to a different tool, etc. The operator can also view the state (or change the state) of the flag in the CTRL parameters. The parameter "Tool Load Flag" has two states: Limit Exceeded or Limit not Exceeded. If the Limit is exceeded only the message is displayed. Sampling is done only in feed moves (G1, G2 and G3). Sampling is not done in rapid moves (G0).
SECTION TWO - FRONT PANEL OPERATION Only tools 1 through 25 are monitored and will have these parameters available. The spindle load bar will also have a number associated with it. Serial Port Data Note: Com port, baud rate, parity, data bits and stop bits are communications parameters. See page 100, Section 4 on F4 (RS232) for more information.
SECTION TWO - FRONT PANEL OPERATION Digitizing Parameters P100 Digitizing Proportional gain P101 Digitizing Integral gain P102 Digitizing Differential gain P103 Digitizing Subscan increment P104 Digitizing Detail angle P105 Digitizing Probe backlash P106 Digitizing Probe radius P107 Digitizing Feed 1 - sampling P108 Digitizing Feed 2 - searching P109 Digitizing Feed 3 - retract P110 Digitizing Probe vibration P111 Digitizing Wall seek activate P120 thru P139 Used by 3D pocket P140
SECTION TWO - FRONT PANEL OPERATION P150 Circular auto-routines radius, rectangular auto-routine, corner radius P151 X rectangular pocket dimension P152 Y rectangular pocket dimension P153 XY finish stock for autoroutines P154 Z finish stock for autoroutines P155 Cut width on pocket clearing autoroutines P156 Radius of bolt hole cycles P157 Bolt hole start angle P158 Bolt hole number of holes in 360° P159 Bolt hole number of holes to be drilled P160 thru P171 Scratch P172 thru P179 Co
SECTION TWO - FRONT PANEL OPERATION F10 (User) Main-Parms-User This set of 100 parameters is reserved for the parts programmer to use when writing parametric programs. These parameters are undefined and can be edited, displayed, or loaded from this screen. The editing and displaying formats are identical to the parameters discussed in this section. See Section 5 for information on parameter programming.
SECTION TWO - FRONT PANEL OPERATION F8 (Prog) Main-Prog There are two modes of program file creation/editing available on the Centurion 6 control: text and conversational. Pressing the F8 (Prog) key will enable the soft keypad to allow selection of the type of programming desired. It also allows the transfer of programs to or from the floppy disk drive. Text and conversational programs are stored in the control in different file formats and have different prefixes to distinguish them.
SECTION TWO - FRONT PANEL OPERATION F1 (Text) Main-Prog-Text Upon entering the text programming mode, the upper right-hand box containing the active program number will display the last text program edited. F1 (Edit) Main-Prog-Text-Edit The F1 (Edit) key will select the program shown in the upper right corner as the active text edit program.
SECTION TWO - FRONT PANEL OPERATION another string using the F7 (Chang) command. And, in most cases, you can even undo your last few changes with the F2 (Rest) restore line or F1 (UnDo) commands. These commands, and many more, are described briefly in the following sections. The first screen you will see when entering the text editor is the edit screen with the first 16 lines of the program displayed. The main edit soft keys are located at the bottom of the screen.
SECTION TWO - FRONT PANEL OPERATION F2 (End) Marks the end of a block. Like the begin-block marker, the end-block marker is invisible, and the block itself will not be displayed unless both markers are set. F3 (Word) Marks a single word as a block, combining the functions of the beginblock and end-block commands. If the cursor is positioned within a word, that word will be marked. If it is not within a word, then the word to the right of the cursor will be marked.
SECTION TWO - FRONT PANEL OPERATION F3 (Words) Main-Prog-Text-Edit-Words The F3 (Words) soft key represents reserved words that may be used for programming the control. Pressing a key will cause that word to be printed on the screen. See Section 6 on parametric programming. Note: F6 (RETRN) will print RETURN. F4 (Misc) Main-Prog-Text-Edit-Misc This section discusses a number of commands that do not readily fit into any of the other category.
SECTION TWO - FRONT PANEL OPERATION F8 (Find) Lets you search for a string of up to 67 characters. When you enter this command you will be asked for a search string. The last search string entered, if any, will be displayed. You can select the string again by pressing Enter, or you may edit it or enter a new search string. After the search string is entered you must specify your search options. The options you used last, if any, are displayed.
SECTION TWO - FRONT PANEL OPERATION With the "N" option, no prompt is displayed before it changes the string or strings. F9 (FNext) Repeats the last search operation. If the last search command called for a Find Operation, the same search string and options will be repeated; for a Find-and-Replace Operation, the replacement string will be reused as well. F5 (Ins) Main-Prog-Text-Edit-Ins If the F5 (Ins) key is on, the editor is in insert mode and characters will be inserted at the cursor position.
SECTION TWO - FRONT PANEL OPERATION Notes: When the program is being verified, it will ignore M6s, M0s, M1s, INPUT statements, etc. The program is copied to a file in the parts directory called “TEXTVER”. No checks are done for out-of-parts space when the file is copied. The “TEXTVER” file is deleted when you return to the edit screen. This is done so that it will not automatically save the program you are working on (it will still prompt you with the “Program was Modified. Accept changes? (Y/N)” message.
SECTION TWO - FRONT PANEL OPERATION F7 (Menu) Main-Prog-Text-Menu The F7 (Menu) key will display a list of all text programs currently in the parts directory. By using the F7 - F10 keys, file selection arrows are positioned at the program to edit, and the F5 (Enter) key is pressed to make a selection. See Section 4 for information on changing drives and paths to other text programs. The edit window will appear displaying the first 16 programs.
SECTION TWO - FRONT PANEL OPERATION F2 (Conv) Main-Prog-Conv The following discussion will deal with selecting conversational programs. Upon entering the conversational programming mode, the active window in the upper right-hand corner will change to show the last conversational program edited. Five options are available from which to choose the conversational program that is to be edited.
SECTION TWO - FRONT PANEL OPERATION While programming or editing in the conversational system, three types of soft key configurations will be encountered. They are: - Soft key configuration 1: Edit Keys These function keys are available whenever the edit menu system has not been entered. It is possible to step through the program, edit events, and insert or delete events. Definitions of the Edit Keys F1 (Edit): Pressing the F1(Edit) key will position the cursor at the first field of the current event.
SECTION TWO - FRONT PANEL OPERATION F2 (View): Allows viewing of the entire program and lets the operator position to any of the events in the program. A window similar to the following will be displayed. F7 ( ↑ ), F8 ( ↓ ), F9 (PgUp), and F10 (PgDn) can be used to move to the desired event. Then press ESC or Enter to display that event.
SECTION TWO - FRONT PANEL OPERATION F9 (Prev) Displays the previous event in the program file. F10 (Next) Displays the next event in the program file. Help (Verf) When editing a conversational file, you can verify the program you are editing. The Help key will show Verf when it is active. The HELP (Verf) key will not be active if you are currently running or verifying a program.
SECTION TWO - FRONT PANEL OPERATION - Soft key configuration 2: Store/Input Keys These soft keys will be available whenever input is expected. At this time, a screen containing any number of fields will be displayed and the cursor will be positioned in one of the fields. There are two types of fields, which may be displayed on an input screen: data and toggle. Data fields are fields in which data is entered using the keypad. Fields that are red require entries.
SECTION TWO - FRONT PANEL OPERATION F2 (New) Main-Prog-Conv-New Pressing the F2 (New) key will allow entry of the number for a new conversational program. After the number has been entered, the control will check the conversational programs currently in the parts directory to see if a program by that number already exists.
SECTION TWO - FRONT PANEL OPERATION Pressing a function key will either bring up an input screen [e.g. F1 (Pos)] much like the following. or another menu [e.g. F2 (Mill)] like this: Notice that on all levels except level 1 there is an ESC (Back) key. This key will return you to the previous level menu keys. Pressing the F10 (Exit) key will exit the menu subsystem and display the level 1 Edit keys. When an input screen is encountered the following Store/Input keys appear.
SECTION TWO - FRONT PANEL OPERATION F7 (Menu) Main-Prog-Conv-Menu The F7 (Menu) key will display a list of all conversational programs currently loaded in the parts directory. By using F7 - F10 keys, file selection arrows are positioned at the program to edit, and the F5 (Enter) key is pressed to make the selection. The edit window will appear displaying the program setup screen.
SECTION TWO - FRONT PANEL OPERATION Verify is used to verify the active program. Upon pressing the F9 (Verf) key, the following screen appears. After the above screen appears, push F1 (Start) and the following screen will appear. The F1 (First) key is automatically selected when entering this screen from the Verf screen. Therefore, if it is desired to verify the active program from the beginning, you need only to press the Cycle Start button.
SECTION TWO - FRONT PANEL OPERATION Cycle Start button is pressed. The active program will start verifying at the desired tool number and the following screen will appear. The F4 (Path) key will show the tool path on the graphics screen, which is the default. The F5 (Part) key will show the part path on the graphics screen. The F6 (Both) key will show both the part path and then the tool path on the graphics screen.
SECTION TWO - FRONT PANEL OPERATION F6 (Displ) Main-Verf-Displ The F6 (Display) key can be accessed from a number of screens. The following screen is shown as if the F6 (Displ) was entered from the F9 (Verf) screen. All the display functions and screens are identical, independent of the entry point. Only the return point differs based on the original entry point. When the F6 (Disp) key is pressed, the following screen will appear. F1 (Next) Main-Verf-Displ-Dist See page 23, Section 2.
SECTION TWO - FRONT PANEL OPERATION F3 (Graph) Main-Verf-Displ-Graph If the F3 (Graph) key is activated, the control switches from displaying text to a graphic display of the active part program. The following screen will appear. The graphics on this control are full 3D and will be displayed in the graphics area as long as the control remains in the F3 (Graph) mode. When other displays are requested, windows will appear in the graphics area showing the requested data.
SECTION TWO - FRONT PANEL OPERATION F8 (Dry) Main-Verf-Dry F8 (Dry) run in the verify mode will run the program as fast as possible. For feedrate override positions 100% and greater – verify speeds are progressively slower for overrides 0-90%. F9 (Halt) Main-Verf-Halt F9 (Resum) Main-Verf-Resum Once a program has been F9 (Halt)ed, the resume feature of the control becomes active. The F9 (Resum) key will now be displayed on the verify screen. A program can be resumed as long as the resume is active.
SECTION TWO - FRONT PANEL OPERATION F1 (Probe) Main-Util-Probe Note: For machines with the Digitizing option. If Digitizing is an option and F1 (Probe) is pressed, the following screen will be displayed. Note: F1 (Probe) is used for XZ or YZ digitizing only. F1 (Begin) If the input file and output mode have been selected, digitizing will begin. If not, error message 808 “set up not selected” is displayed.
SECTION TWO - FRONT PANEL OPERATION F2 (XyDig) Main-Util-XyDig Note: For machines with the Digitizing option. If Digitizing is installed and F2 (XyDig) is pressed, the following will be displayed. F1 (Begin) If the input file and output mode have been selected, digitizing will begin. If not, error message 808 “set up not selected” is displayed. F3 (In) Displays a menu from which to select a file that contains the guidance information for digitizing.
SECTION TWO - FRONT PANEL OPERATION F1 (Load) Main-Util-Files-Load The F1 (Load) function is used to load programs from the floppy disk into the control's program memory. When this function is selected the following screen is displayed. The edit window will display a list of the programs on the floppy drive. The selection cursor ( > < ) is positioned at the first program. F1 (Start) Pressing this key will begin the transfer of the selected programs from floppy disk to program memory.
SECTION TWO - FRONT PANEL OPERATION The help key will be used to either select a new drive or to verify a program (based on the control parameter) Help (Drive) Displays a list of available drives for a new menu. Help (Verf) Will graphically verify the part that the cursor is on. Note: If the parameter to extract files is set, a single file on the floppy separated by 0#### can be loaded and separated into several files.
SECTION TWO - FRONT PANEL OPERATION F5 (Send) Main-Util-RS232-Send When F5 (Send) is depressed, the following keys appear. After selecting F1 (Text) or F2 (Conv), select which programs you want to send to the off-line computer from the menu. These actions will display the following menu. F1 (Begin) starts transmission of the active send program that is shown in the upper right-hand corner. F7 (Menu) allows selection of programs from a menu to send.
SECTION TWO - FRONT PANEL OPERATION Note: If the program number being received already exists, the operator will be prompted. If the parameter to extract files is set, several files can be sent from an off-line computer; the control will extract them to the correct #### file if they are separated by 0####'s. When extracting, no checking is done for files that already exist. F7 (8Ram) Main-Util-RS232-8Ram This function is used to load programs from RS-232 to the ram drive and later DNC'ed from the ram drive.
SECTION TWO - FRONT PANEL OPERATION F1 (Edit) allows you to modify the tool number in each pocket. F3 (Dflt) loads the default tool numbers (tool 1 in pocket 1, tool 2 in pocket 2, etc). F7 also zeroes the tool number in the spindle. F6 (DNC) Main-Util-DNC The F6 (DNC) mode is used for running large programs. These programs are not loaded into the control's memory, therefore they cannot have GO-TO's, WHILE-WEND loops, GO-SUB's, or CALLS. Note: CALLS are allowed in fast DNC fast.
SECTION TWO - FRONT PANEL OPERATION F3 (Fast) Main-Util-DNC-Fast After pressing F3 (Fast), the following screen will appear. F1 (RS232) Depressing F1 (RS232) will wait for data from the Com port, then request a cycle start to begin the program. F2 (File) F2 (File) selects a program from a menu of the programs in the control. F3 (Disk) F3 (Disk) selects a program from a menu of the programs on the floppy disk or from local area network.
SECTION TWO - FRONT PANEL OPERATION F1 (First) F1 (First) starts from the beginning. F2 (Block) F2 (Block) starts from a sequence number. F3 (Tool) F3 (Tool) starts from a tool number. F4 (Cont) F4 (Cont) allows starting from a location where DNC was aborted earlier. When a file is aborted the file position is saved. No checking is performed if the operator has switched file numbers or modified the DNC file. F4 (Cont) will continue from the file position that was aborted on any file.
SECTION TWO - FRONT PANEL OPERATION This mode should be used for large programs where a fast block rate is required, for example when making short moves at fast feedrates. No trig help, cutter comp, rotating, scaling, or other non-standard commands, can be done in this mode. Valid data for the fast mode are: X, Y, Z, A, B, I, J, K, F and N Valid G codes are: G0, G1, G2, G3, G17, G18, G19, G70, G71, G90, G91 If a code that is not in these groups is executed, the block time for that block will slow down.
SECTION TWO - FRONT PANEL OPERATION F7 (Chart) Main-Util-Chart The F7 (Chart) key will display help charts created by the end user specific to their applications. If there is a file called charts.dat in the RAM directory, it will be displayed. The format of this file allows an indexing system to other files and data available to the operator. The following is a sample listing of charts.dat. Note: The first 16 lines of chart.dat are not displayed.
SECTION TWO - FRONT PANEL OPERATION Memory Avail displays the system memory available in bytes. Parts Storage displays the amount of parts storage in bytes. Front Panel displays the front panel version code. Controller Card displays the controller card version (v0206 is 2.06) and an error count (should be zero). Acroloop information for X, Y, and Z axis for Centurion 5 systems is as follows. version, (v0214=2.
SECTION TWO - FRONT PANEL OPERATION This screen gives internal information about the system. Lines 1 through 5 show memory allocations to DOS, CNC overlays, and the heaps. Line 6 shows the MS-DOS version and whether the CPU is an 80286, 80386, 80486, or 80586. Lines 11 & 12 show the compiler and blocks pre-allocated for canned cycles, text cycles, and custom M and G codes. Line 13 is a hex dump of the BIOS ROM area at F000:0. Line 14 is a hex dump of the Disk Emulator ROM at CA00:0.
SECTION TWO - FRONT PANEL OPERATION F4 (Path) Main-Util-Info-Path F4 (Path) displays the following screen, which shows the path file. In the standard order, these are the directories for ROM, RAM, Parts, Display, and Floppy. Below the Parts directory is shown the available parts space in bytes. For the ROM, Parts, and Display directories, the DOS volume ID for that drive is shown to the right. Note: The path file is reloaded when the above information is displayed.
SECTION TWO - FRONT PANEL OPERATION F5 (Time) Main-Util-Info-Time F5 (Time) displays the times and distances calculated when verifying a program. Timing information is for 100% on the feedrate override for tool changes, spindle up to speed, block stops, etc. Times are in hrs, min., sec. Distance is in inches or mm. Tool changes add 10 seconds to the feed time. This above screen shows timing information for the last program verified. The times displayed assume the feedrate override is 100%.
SECTION TWO - FRONT PANEL OPERATION F7 (Diag) Main-Util-Info-Diag F7 (Diag) displays the following screen, which shows the diagnostics of the machine just prior to the machine e-stopping. F7 is used mainly for diagnostic purposes to determine the source of the e-stop. The user is capable of viewing the states of the inputs and outputs for each axis. F9 (Blank) Main-Util-Blank F9 (Blank) will blank the screen. Using this function will reduce images being burned into the CRT.
SECTION THREE - CONVERSATIONAL INPUT SCREENS 113
SECTION THREE - CONVERSATIONAL INPUT SCREENS Each conversational program has a text program associated with it. The conversation program file starts with letter P followed by four digits such as P1234. The text file starts with the letter O followed by four digits such as O1234. The text program is created, or posted, from the conversational program. Changes in the conversational program create a new text program from the modified conversational program.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F1 (Pos) Main-Prog-Conv-Pos The position screen will normally be used to do rapid positioning; however, feed moves may be made by toggling the feedrate field and entering a feedrate. The conversational screen for Cartesian rapid positioning appears as follows. Note: See page 194, Section 4 for further information on positioning. The conversational screen for polar feed position appears as follows.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F1 (Start) Mill-Start The F1 (Start) screen is used to begin a continuous single or multi-depth milling cycle. Milling will start at the first Z depth specified and continue stepping down by the Z increment until the final Z depth has been reached. The conversational screen for tool pierce start mill cycle appears as follows. The start mill cycle is normally followed by geometry and ended with an “end mill cycle” event.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F2 (Geom) Mill-Geom The F2 (Geom) selection brings up the following soft keys. F1 (Line) Mill-Geom-Line The F1 (Line) key displays the following conversational screen for Cartesian linear interpolation, which is used to execute linear interpolation in feed mode. Note: See page 194, Section 4 for further information on positioning.
SECTION THREE - CONVERSATIONAL INPUT SCREENS In conversational programming, for any feedrate or spindle speed input fields, the F12 key will be active. Pressing the F12 key will offer the operator help in calculating the appropriate spindle speed and feedrate for the appropriate inputs. The only exception is the feedrate on the position screen because this feedrate is intended to be a rapid move. After pressing the F12 key, the following screen will appear.
SECTION THREE - CONVERSATIONAL INPUT SCREENS The conversational screens for polar linear interpolation appear as below. Note: See page 196, Section 4 for further information on polar definition of a line. When Extend Back [ON] is selected, the following screen appears. Note: See page 212, Section 4 for further information on back line. The conversational screen for line with round corner appears as follows. Note: See page 210, Section 4 for further information on corner rounding.
SECTION THREE - CONVERSATIONAL INPUT SCREENS The conversational screen for line with chamfer appears as follows. See page 211, Section 4 for further information on angle chamfering. F2 (Arc) Mill-Geom-Arc The F2 (Arc) screen is used to execute circular interpolation in feed mode. Arc Sample 1 The XY plane, incremental center, CW circular interpolation conversational screen appears as follows. Note: See page 197, Section 4 for further information on circular interpolation.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Arc Sample 2 The ZX plane, absolute center, CCW circular interpolation conversational screen appears as follows. Note: See page 197, Section 4 for further information on circular interpolation. Arc Sample 3 The XY plane, polar, CCW helical interpolation, with round corner appears as follows. Note: See page 196, Section 4 for further information on describing an arc using polar definitions.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Arc Sample 4 The XY plane, radius only, CCW circular interpolation conversational screen appears as follows. Note: See page 199, Section 4 for further information on describing an arc using a radius.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F3 (Tangs) Mill-Geom-Tangs The F3 (Tangs) screen is used to compute the intersection points necessary for a tangent arc or tangent line between two arcs. When this function is used the first arc and the tangent line or arc will be entered into the program. The second arc information will only be used for calculation purposes. This feature was developed to enable a series of tangent lines or arcs to be programmed consecutively.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Tangent Line The conversational screen for tangent line appears as below. Note: See page 330, Section 6 for further information on tangent line. Tangent Arc The conversational screen for tangent arc appears as follows. Note: See page 330, Section 6 for further information on tangent arc.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F4 (CGen) Mill-Geom-CGen To use F4 (CGen), which is the circle generator function, fill in any three points on an arc. These three points will be used to compute the center and radius of the specified arc. The conversational screen for circle generator appears as follows. Note: The circle generator screen does not move to the first point on the arc before cutting the arc. In most cases, the circle generator screen is preceded by a line move to this position.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F8 (E-Isl) Mill-Geom-E-Isl The end island screen is used to end the geometry in an island. Following is a sample program using a mill cycle with pocket clear and islands.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Event 1 of 16 Tool Pierce - Start Mill Cycle Z Pierce Feedrate [25 ] Return Point [Clearance] Clearance [.1 ] Final Z Depth [-1 ] 1st Z Depth [-.3 ] Z Increment [.3 ] X Pierce Point X[0 ] Y Pierce Point Y[0 ] Compensation [Left] [Polar] Angle AB[90 ] Options [Pocket Clear 1] XYFeedrate[50 ] Cut Width [.2 ] Finish Stock[.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Event 4 of 16 Mill Geometry - Arc Plane [XY] Feedrate F[ ] Direction [CCW] Center [Abs Center] Arc Radius R[1.5 ] Arc Center XC[1.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Event 7 of 16 Start Island Island Number #[1 ] X Pierce Point X[1 Y Pierce Point Y[1 ] ] Compensation [Left] [Polar] Angle AB[0 ] --------------------------------------------------Event 8 of 16 Mill Geometry - Line Feedrate F[50 ] Coordinates [Cartesian] X-axis X[2 Y-axis Y[2 Z-axis Z[ ] ] ] End [---] Extend Back [Off ] --------------------------------------------------Event 9 of 16 Mill Geometry - Line Feedrate F[ ] Coordinates [Cartesian] X-axis X[2 Y-axis
SECTION THREE - CONVERSATIONAL INPUT SCREENS Event 10 of 16 Mill Geometry - Line Feedrate F[ ] Coordinates [Cartesian] X-axis X[1 Y-axis Y[1 Z-axis Z[ ] ] ] End [---] Extend Back [Off ] --------------------------------------------------Event 11 of 16 End Island Point on part after tool retract [Polar] Angle AB[45 ] --------------------------------------------------Event 12 of 16 Start Island Island Number #[2 ] X Pierce Point X[.75 ] Y Pierce Point Y[2.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Event 13 of 16 Mill Geometry - Arc Plane [XY] Feedrate F[50 ] Direction [CW] Center [Abs Center] Arc Radius R[.5 ] Arc Center XC[1.25 ] YC[2.75 ] End Point [Absolute] X[1.75 ] Y[2.75 ] Z[ ] End Option [---] --------------------------------------------------Event 14 of 16 Mill Geometry - Arc Plane [XY] Feedrate F[ ] Direction [CW] Center [Abs Center] Arc Radius R[.5 ] Arc Center XC[1.25 ] YC[2.75 ] End Point [Absolute] X[.75 ] Y[2.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Event 16 of 16 End of Program Spindle off [Yes] Coolant off [Yes] Z to Toolchange [Yes] X Position (home relative)[ ] Y Position (home relative)[ ] --------------------------------------------------The previous program will generate the following graphic. Note: See page 316, Section 5 for more information on pocket clear. F3 (Misc) Mill-Misc See page 177, Section 3 for explanation of miscellaneous.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Start Mill Cycle and NO Tool Retract End Mill Cycle = ERROR # 602 Missing WEND Statement This may be caused by a start mill cycle without an end mill cycle. Tool Retract End Mill Cycle and NO Start Mill Cycle = ERROR # 601 Missing WHILE Statement This may be caused by an end mill cycle without a start mill cycle. The conversational screen for tool retract end mill cycle appears as follows.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Event 1 of 7 Tool Pierce - Start Mill Cycle Z Pierce Feedrate [20 ] Return Point [Clearance] Clearance [.1 ] Final Z Depth [-1 ] 1st Z Depth [-.2 ] Z Increment [.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Event 4 of 7 Mill Geometry - Line Feedrate F[ ] Coordinates [Cartesian] X-axis X[0 Y-axis Y[ Z-axis Z[ ] ] ] End [---] Extend Back [Off ] --------------------------------------------------Event 5 of 7 Mill Geometry - Arc Plane [XY] Feedrate F[ ] Direction [CCW] Center [Polar] Arc Radius R[1 ] Start Angle AA[90 ] End Point [Polar] End Angle AB[-90 ] Z[ ] End Option [---] --------------------------------------------------Event 6 of 7 Tool Retract End Mill Cycle
SECTION THREE - CONVERSATIONAL INPUT SCREENS Event 7 of 7 End of Program Spindle off [Yes] Coolant off [Yes] Z to Toolchange [Yes] X Position (home relative)[ ] Y Position (home relative)[ ] --------------------------------------------------The following graphic is the isometric view of the mill program.
SECTION THREE - CONVERSATIONAL INPUT SCREENS The conversational screen for pocket clear option using tool pierce start mill cycle appears as follows. The following graphic is the top view of the sample mill program using the pocket clear 1 option on the tool pierce start mill cycle. Note: See page 316, section 4 for further information on pocket clear 1.
SECTION THREE - CONVERSATIONAL INPUT SCREENS The conversational screen for pocket clear option using tool pierce start mill cycle appears as follows. The following graphic is the top view of the sample mill program using the pocket clear 2 option on the tool pierce start mill cycle. Note: See page 316, section 5 for further information on pocket clear 2. Note: This option can be used to clear away from a framed mill cycle as well.
SECTION THREE - CONVERSATIONAL INPUT SCREENS The conversational screen for tool pierce start mill cycle with tapered walls option appears as follows. The following graphic illustrates the sample mill program using the tapered walls option on the tool pierce start mill cycle. 0° is a vertical wall; 90° is impossible. The tapered wall also has an option for an end mill. Cutter comp must be on to use the tapered walls option. The first Z depth should be the top of the wall.
SECTION THREE - CONVERSATIONAL INPUT SCREENS The conversational screen for tool pierce start mill cycle with rounded walls option appears as follows.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Event 1 of 4 Tool Pierce - Start Mill Cycle Z Pierce Feedrate [20 ] Return Point [Clearance] Clearance [.1 ] Final Z Depth [-2 ] 1st Z Depth [0 ] Z Increment [.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Event 4 of 4 End of Program Spindle off [Yes] Coolant off [Yes] Z to Toolchange [Yes] X Position (home relative)[ ] Y Position (home relative)[ ] --------------------------------------------------The following graphic illustrates the sample mill program using the round walls option on the start mill cycle. 0° is a vertical wall; 90° is impossible. The round wall also has an option to use an end mill tool. Cutter comp must be on to use the tapered walls option.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Mill START and END are not to be used with pocket routines. Note: All milling auto routines must be activated with the tool at the center of the routine. The conversational screen for pocket mill setup appears as follows. Note: See pages 218, 225 in Section 4 and 316 in Section 5 for further information on pocket routines. F2 (Circ) Mill-Pockt-Circ The F2 (Circ) selection brings up the following soft key selections.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F2 (Fin) Mill-Pockt-Circ-Fin The conversational screen for inside CW circular pocket finish appears as follows. Note: See page 219, Section 4 for more information on circular finish inside. F3 (Rect) Mill-Pockt-Rect The F3 (Rect) rectangular pocket selection brings up the following soft keys. F1 (Clear) Mill-Pockt-Rect-Clear The conversational screen for CW rectangular pocket clear appears as follows.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F2 (Fin) Mill-Pockt-Rect-Fin The conversational screen for inside CW rectangular pocket finish appears as follows. Note: See page 226, Section 4 for further information on rectangular finish inside. F3 (Face) Mill-Pockt-Rect-Face The conversational screen for facing cycle appears as follows.
SECTION THREE - CONVERSATIONAL INPUT SCREENS To add manual points in conversational select F2 (Mill) - F5( Pockt) - F4 (Manul). The manual mode pocket clear screen looks like the following: The fields on the screen are similar to a start mill cycle. The tool number is used to graphically show a tool (from the tool diameter in the tool table). After entering the fields on the screen and pressing F1 (Store). The part being programmed will be verified (part and tool paths).
SECTION THREE - CONVERSATIONAL INPUT SCREENS F5 (Polyg) Mill-Pockt-Polyg The conversational screen for the polygon cycle appears below. Note: see page 231 , Section 4 for further information on the polygon cycle. F6 (Frame) Mill-Frame The F6 (Frame) frame mill selection brings up the following soft keys. F1 (Setup) Mill-Frame-Setup The F1 (Setup) screen is used to set parameters necessary for circular and rectangular frame mill routines. Setting parameters must be done prior to any frame milling routines.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F2 (Circ) Mill-Frame-Circ The conversational screen for outside CCW circular frame mill appears as follows. Note: See page 221, Section 4 for further information on circular finish outside. F3 (Rect) Mill-Frame-Rect The conversational screen for rectangular finish outside appears as follows: Note: See page 229, Section 4 for further information on rectangular finish outside.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F7 (3dPkt) Mill-3dPkt The F7 (3dPkt) selection brings up the following soft keys. F1 (Start) Mill-3dPkt-Start The F1 (Start) key brings up the conversational screen for start 3D sweep cycle, which appears below. Notes on 3D Sweep Cycle Note 1: If sweep start angle = sweep end angle, then no arc is made. Note 2: Negative start angles specify a female part, positive start angles specify a male part.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F4 (End) Mill-3dPkt-End The F4 (End) key must be selected to terminate the 3D pocket cycle or an error will occur. The conversational screen for disable 3D sweep cycle appears as follows.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Event 1 of 6 Start 3D sweep cycle Clearance [.1 ] Z Pierce Feedrate [15 ] Arc Feedrate [20 ] Start point X [2 ] Y [1 ] Z [0 ] Sweep start radius R [1 ] Sweep start angle AA [-.0001 ] Sweep end angle AB [180 ] Pass width [.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Event 4 of 6 3D Geometry - Arc Plane Feedrate Direction Center Arc Radius Arc Center [XY] F [ ] [CW] [Abs Center] R [1 ] XC [3 ] YC [5 ] End Point [Absolute] X [2 ] Y [5 ] Z [ ] --------------------------------------------------Event 5 of 6 Disable 3d Sweep Cycle --------------------------------------------------Event 6 of 6 End of Program Spindle off [No] Coolant off [No] Z to Toolchange [No] X Position (home relative) [ ] Y Position (home relative) [ ] -------
SECTION THREE - CONVERSATIONAL INPUT SCREENS F5 (3dArc) Mill-3dPkt-3dArc The F5 (3dArc) brings up the conversational screen for the 3d Arc subroutine call, which appears below.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Event 1 of 2 3d Arc Subroutine Call Rotate the path in the given subroutine including arcs out of the given plane. Does not support cutter comp or trighelp All Arcs must have absolute centers.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Event 1 of 5 Mill Geometry - Line Feedrate F[ ] Coordinates [Cartesian] X-axis X[2 Y-axis Y[1 Z-axis Z[ ] ] ] End [---] Extend Back [Off ] --------------------------------------------------Event 2 of 5 Mill Geometry - Line Feedrate F[ ] Coordinates [Cartesian] X-axis X[3 Y-axis Y[3 Z-axis Z[ ] ] ] End [---] Extend Back [Off ] --------------------------------------------------Event 3 of 5 Mill Geometry - Line Feedrate F[ ] Coordinates [Cartesian] X-axis X[ Y-a
SECTION THREE - CONVERSATIONAL INPUT SCREENS Event 4 of 5 Mill Geometry - Arc Plane [XY] Feedrate F[ ] Direction [CW] Center [Abs Center] Arc Radius R[1 ] Arc Center XC[3 ] YC[5 ] End Point [Absolute] X[2 ] Y[5 ] Z[ ] End Option [---] --------------------------------------------------Event 5 of 5 End of Program Spindle off [Yes] Coolant off [Yes] Z to Toolchange [No] X Position (home relative)[ ] Y Position (home relative)[ ] --------------------------------------------------The following graphic illustrate
SECTION THREE - CONVERSATIONAL INPUT SCREENS F9 (Thred) Mill-Thred The F9 (Thred) key brings up the thread milling input screen. Two examples are shown below. Note: See page 234, Section 4 for the correct combination of cutter comp, cut direction. F3 (Drill) Drill The F3 (Drill) selection brings up the following menu. All drill cycles must be started prior to execution and ended after the last hole. This is done with the F1 (Start) and F5 (End) selections.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Conversational Screens F3 (Drill) start drill cycle screen has a toggle field to select which type of drilling is to be executed. The start drill cycle is normally followed by the positions for the holes and ended with an end drill cycle event. The optional drill cycles are shown below. Drill The conversational screen for drill appears as follows. Note: See page 281, Section 4 for further information on the drill cycle.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Drill/Peck The conversational screen for peck drilling cycle appears as follows. Note: See page 282, Section 4 for more information on peck drilling cycle. Chip Breaker Drill The conversational screen for chip breaker drill cycle appears as follows. Note: See page 275, Section 4 for further information on chip breaker drilling cycle. Bore The conversational screen for bore cycle appears as follows.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Bore/Dwell The conversational screen for bore/dwell appears as follows. Note: See page 289, Section 4 for more information on the bore/dwell cycle. Bore 2 The conversational screens for bore 2 appears as follows. Fast bore Note: See page 285, Section 4 for further information on fast bore cycle. Fine bore Note: See page 277, Section 4 for further information on fine bore cycle.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Back bore Note: See page 286, Section 4 for more information on the back bore cycle. Manual bore Note: See page 280, Section 4 for more information on the manual bore cycle. Counter bore Note: See page 284, Section 4 for more information on the counter bore cycle.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Tap (Drill-Start-Tap) The conversational screens for tap drill cycle appear as follows. Soft right tap Note: See page 283, Section 4 for more information on the soft right tap cycle. Soft left tap Note: See page 276, Section 4 for more information on the soft left tap cycle. Hard right tap Note: See page 288, Section 4 for more information on the hard tap cycle.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Hard left tap Note: See page 288, Section 4 for more information on the hard tap cycle. Hard peck right tap Note: See page 288, Section 4 for more information on the hard tap cycle. Hard peck leftt tap Note: See page 288, Section 4 for more information on the hard tap cycle. F2 (Pos) Drill-Pos, F3 (Misc) Drill-Misc, F4 (Call) Drill-Call The F2 (Pos) key brings up the position screens. They are used to enter the drill positions.
SECTION THREE - CONVERSATIONAL INPUT SCREENS The screen pictured above is the single position hole drill screen. One hole will be drilled or tapped at (1,2). If a dimension is entered in the Z field on this screen it will drill the new depth at (1,2) and subsequent holes. If the only dimension entered appears in the Z field, the Z axis will move to that position; no hole will be drilled, and the Z depth will remain unchanged. This can be useful for clearing clamps or fixtures.
SECTION THREE - CONVERSATIONAL INPUT SCREENS The screen pictured below is the position drill screen using the spaced holes option. It will drill or tap six holes, including the hole at (1,2). If the X spacing field is 0, the line of holes would be drilled in a vertical line. If the Y spacing is 0, the holes would be drilled in a horizontal line. The above screen would create the hole pattern shown below.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F3 (Misc) brings up the miscellaneous function screen and allows those functions to be programmed during drill cycles. The F4 (Call) screen allows subprograms to be called during a drill cycle. These subprograms would normally contain the drilling positions for different drilling operations. Note: See page 177, Section 3 for more information on miscellaneous. See page 178, Section 3 for more information on call.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Dimensions [Absolute] Units [English] Work Coordinate [---] Setup Notes: [ ] [ ] [ ] [ ] [ ] [ ] --------------------------------------------------Event 1 of 17 Tool Change Tool Tool Change Position [Change] X[ ] Y[ ] Tool Number T[1 ] Tool Description [DRILL Next Tool Number [] ] Spindle Speed S[2000] Spindle Restart [CW] Stop For Speed Change [No] Coolant [Flood] --------------------------------------------------Event 2 of 17 Enable Drill Cycle [Drill Cycle
SECTION THREE - CONVERSATIONAL INPUT SCREENS Z axis Z[ ] Grid of Holes [---] Spaced Holes [---] --------------------------------------------------Event 4 of 17 Position Drill Feedrate Coordinates [Rapid] [Cartesian] X axis Y axis Z axis X[2 ] Y[ ] (Z to –2") Z[ ] Grid of Holes [---] Spaced Holes [---] --------------------------------------------------Event 5 of 17 Position Drill Feedrate Coordinates [Rapid] [Cartesian] X axis Y axis Z axis X[ ] Y[ ] Z[3 ] (Z to 3" to get over a clamp) Grid of Hole
SECTION THREE - CONVERSATIONAL INPUT SCREENS Event 7 of 17 Position Drill Feedrate Coordinates [Rapid] [Cartesian] X axis X[5 ] Y axis Y[ ] (Z to –1") Z axis Z[ ] Grid of Holes [---] Spaced Holes [---] --------------------------------------------------Event 8 of 17 Disable Drill Cycle --------------------------------------------------Event 9 of 17 Tool Change Tool Tool Change Position [Change] X[ ] Y[ ] Tool Number T[2 ] Tool Description [BORE ] Next Tool Number [] Spindle Speed S[2000] Spindle Restart
SECTION THREE - CONVERSATIONAL INPUT SCREENS X axis Y axis Z axis X[1 ] Y[1 ] Z[ ] (Z to –2") Grid of Holes [---] Spaced Holes [---] --------------------------------------------------Event 12 of 17 Position Drill Feedrate Coordinates [Rapid] [Cartesian] X axis Y axis Z axis X[2 ] Y[ ] (Z to –2") Z[ ] Grid of Holes [---] Spaced Holes [---] --------------------------------------------------Event 13 of 17 Position Drill Feedrate Coordinates [Rapid] [Cartesian] X axis Y axis Z axis X[ ] Y[ ] Z[3 ] (Z
SECTION THREE - CONVERSATIONAL INPUT SCREENS Spaced Holes [---] --------------------------------------------------Event 15 of 17 Position Drill Feedrate Coordinates [Rapid] [Cartesian] X axis Y axis Z axis X[5 ] Y[ ] (Z to –1") Z[ ] Grid of Holes [---] Spaced Holes [---] --------------------------------------------------Event 16 of 17 Disable Drill Cycle --------------------------------------------------Event 17 of 17 End of Program Spindle off Coolant off Z to Tool change [Yes] [Yes] [Yes] X Position
SECTION THREE - CONVERSATIONAL INPUT SCREENS F4 (Bolt) The following conversational bolt hole drill screens are displayed upon selecting the bolt hole drill cycles. The first part of the screen contains information used to set up the appropriate drill cycle, whereas the last part contains information used to set up the bolt hole cycle.
SECTION THREE - CONVERSATIONAL INPUT SCREENS 173
SECTION THREE - CONVERSATIONAL INPUT SCREENS Sample Bolt Hole Program Event 0 of 3 Program Setup Program name Dimensions Units Work Coordinate [Sample Bolt hole Program] [Absolute] [English] [---] Setup Notes: [ ] [ ] [ ] [ ] [ ] [ ] --------------------------------------------------Event 1 of 3 Tool Change Tool [Change] Tool Change Position X[ Y[ Tool Number T[1 ] Tool Description Next Tool Number Spindle Speed Spindle Restart Stop For Speed Change Coolant ] ] [DRILL [] S[2000] [CW] [No] [Flood] ]
SECTION THREE - CONVERSATIONAL INPUT SCREENS Bolt hole Radius Angle Of 1st Hole # Of Holes To Be Made # of Holes in 360 Deg [-3 ](-R for CCW) [90 ] [8 ] [14 ] --------------------------------------------------Event 3 of 3 End of Program Spindle off [Yes] Coolant off [Yes] Z to Toolchange [Yes] X Position (home relative) [ ] Y Position (home relative) [ ] Notes: See page 272, Section 4 for further information on bolt hole routine.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F5 (TChng) Tool Change When a new tool needs to be put in the machine tool, the tool change screen should be used. The two tool change screens are tool call and tool change. The tool call is used to initiate a new set of tool offsets without physically changing the tool. The tool change puts the machine in a tool change mode and calls for a new tool.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F6 (Misc) As a program is being created it may be necessary to add certain miscellaneous functions such as coolant and stop commands. This is done through the F6 (Misc) screen. Conversational screens for miscellaneous appear below. The miscellaneous line is used to type in any M code that is not part of the standard list.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F7 (Call) The program call screen is used to transfer program execution to another program for a specified number of loops. The conversational screen for program call appears below. If the number of loops is left blank, the subprogram is called once. Note: See page 317, Section 5 for further information on subprogram call.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Subprogram calls can be used to create a number of identical parts in a row or a grid. The screen below can be used to call a subprogram that cuts a slot. F8 (Spec) These are screens for setting or adjusting various parameters in the Centurion 6 control. The parameters control various functions, such as tool offsets, scale factors, rotation angles, mirror image, floating zeroes, and the parameters listed in Appendix A. The keys are as follows.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F1 (Parms) Spec-Parms The conversational screen for adjust parameter appears below. Loading a parameter will set the parameter to the specified value. Adjusting a parameter will add the specified value to the current setting. F2 (Tools) Spec-Tools The conversational screen for set tool offset appears below. Note: See page 253, Section 4 for further information on tool length offset.
SECTION THREE - CONVERSATIONAL INPUT SCREENS The conversational screen for adjust tool offset appears below. F4 (Scale) Spec-Scale The conversational screen for turn scale factor on appears below. The conversational screen for turn scale factor off appears below. Note: See page 254, Section 4 for further information on set and cancel scaling.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F5 (Rot) Spec-Rot The conversational screen for turn rotation on appears as follows. Note: See page 260, Section 4 for further information on coordinate system rotation. The conversational screen for set 3D rotation angle appears below. 3D rotation is used to tilt parts out of the plane.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F6 (Mirr) Spec-Mirr The conversational screen for set mirror image on appears below. The conversational screen for set mirror image off appears below. Note: See page 265, Section 4 for further information on mirror image set and cancel. F7 (Flz) Spec-Flz The conversational screen for set floating zero appears below. Note: See page 294, Section 4 for further information on floating zeros.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F8 (Text) Spec-Text The conversational screen for text appears below. The conversational screen for text on an arc: F9 (Subs) These screens are used to define and call subroutines.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F1 (Gosub) Subs-Gosub Gosub is used to call a subroutine. The screen below calls subroutine 1 fifteen times. If the number of loops is left blank, the subroutine is called 1 time. Another option on the gosub screen is used to call the subroutine and repeat it in a rectangular pattern. Note: The other option is to call the subroutine using XY spacing between each. The grid and the spaced are similar to holes in the drill cycles on page 162, Section 3.
SECTION THREE - CONVERSATIONAL INPUT SCREENS F2 (Start) Subs-Start The start subroutine screen defines the start of a subroutine. F3 (End) Subs-End The end subroutine screen defines the end of the subroutine.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Sample Program Using Subroutines Conversational Program C:\CNC\PARTS\P0523 Event 0 of 12 Program Setup Program name [ ] Dimensions Units Work Coordinate [Absolute] [English] [---] Setup Notes: [ ] [ ] [ ] [ ] [ ] [ ] --------------------------------------------------Event 1 of 12 Tool Change Tool Tool Change Position [Change] X[ ] Y[ ] Tool Number Tool Description Next Tool Number Spindle Speed Spindle Restart T[1 ] [ ] [] S[600 ] [CW] Coolant [Flood] --
SECTION THREE - CONVERSATIONAL INPUT SCREENS --------------------------------------------------Event 3 of 12 Tool Change Tool Tool Change Position [Change] X[ ] Y[ ] Tool Number Tool Description Next Tool Number Spindle Speed Spindle Restart T[2 ] [ ] [] S[1200 ] [CW] Coolant [Mist] --------------------------------------------------Event 4 of 12 Goto Subroutine Subroutine Number [2 ] Options [Grid] 1st Position X[0 ] Y[0 # of Rows[4 ] # of Cols[3 ] X Spacing[3 ] Y Spacing[2.
SECTION THREE - CONVERSATIONAL INPUT SCREENS Event 6 of 12 Pocket Mill Setup X Pocket Center Y Pocket Center [0 ] [0 ] XY Feedrate [10 ] Z Pierce Feedrate [5 ] Return Point [Clearance] Clearance [.1 ] Final Z Depth [-.4 ] First Z Depth [-.1 ] Z Increment [.
SECTION THREE - CONVERSATIONAL INPUT SCREENS --------------------------------------------------Event 11 of 12 End Subroutine --------------------------------------------------Event 12 of 12 End of Program Spindle off Coolant off Z to Toolchange [No] [No] [No] X Position (home relative)[ ] Y Position (home relative)[ ] --------------------------------------------------The above program makes the following: End of Program The conversational screen for end of program appears below.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) These codes are used if the operator is programming the Centurion 6 in the text mode or MDI mode. They are also generated from conversational programs. It should be noted that most programmers, particularly new programmers, use the conversational programming mode. If you are planning to use text mode of programming, pay close attention to this section for it explains these codes.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Active On Power-up Modal One Shot 25 Circular finish inside X 26 28-30 Circular finish outside Reference point return X X Z to clearance Z to tool change Facing cycle Rectangular pocket clear Rectangular finish inside Rectangular finish outside Threading mill cycle Cutter compensation cancel Cutter compensation left X X X X X X X 31 32 33 34 35 36 39 40 41 42 43 44 45 46 47 49 50 51 52 53 54 55-59 60 61 63 64 65 68 69 70 71 X Cutter compensation ri
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Active On Power-up Modal 72 Bolt hole routine X 73 74 Woodpecker Left hand tapping X X 75 76 77 78 79 80 81 82 83 Counter bore Fine bore Custom drill cycle Manual bore Custom drill cycle Cancel canned cycle Drill Drill/dwell Peck/drill X X X X X X X X X 84 85 86 87 88 89 90 91 92 93 94 95 98 99 271 666 990 991 995 996 997 998 Right-hand tapping Bore Fast bore Back bore Hard tap Bore/dwell Absolute dimension Incremental dimension Work coordinate chg.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Note: Unrecognized G codes will cause an error 549 to occur. Interpolation functions There are four modes of interpolation: G0 Rapid linear G1 Feed linear G2 Clockwise arcs G3 Counterclockwise arcs Positioning (G00) rapid traverse (modal) Example: G0 X3 Y2 G00 specifies positioning in rapid traverse mode. There is no need to program rapid traverse rates because the rates are preset by parameters.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Note: The rapid traverse rate in the G00 command is set for each axis independently by the machine tool builder. Accordingly, the rapid traverse rate cannot be specified in the address F. In the positioning mode actuated by G00, the tool is accelerated to a predetermined speed at the start of a block and is decelerated at the end of a block. Execution proceeds to the next block after confirming the in-position.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Feedrate Override: The per minute feed can be overridden using the feedrate override button on the machine operator's panel by 0 to 140% (per every 10%). Feedrate override cannot be applied to functions in which override is inhibited (e.g. tapping cycle). Polar definition of a line A polar line is specified by a polar radius/length (R), an angle (AB), and a polar center (AA or I, J, K, or XC, YC, ZC). Polar definitions are valid in any plane.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Circular interpolation (G02, G03) The general command format to move along a circular arc is as follows. G17 G18 G19 G02 X Y I J or or XZIK G03 Y Z J K or AB R *(1) *(2) *(3 or 6) XC YC R or or XC ZC R or YC ZC R *(4 or 5) R or or or R R AA R F or AA R F or AA R F *(7) *These numbers are referenced in the chart that follows.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Circular Interpolation DATA TO BE GIVEN 1 2 3 4 COMMAND Plane selection G17 Specify arc on XY plane G18 Specify arc on ZX plane G19 Specify arc on YZ plane G02 Clockwise (CW) G03 Counterclockwise (CCW) G90 mode One, Two, or Three of X, Y, and Z End point position in work coordinate system G91 mode One, Two, or Three of X, Y, and Z Distance from start point to end point Two of I, J, and K The signed distance from start point to center R=√
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Clockwise and Counterclockwise Directions The view above is from the positive direction of the Z, Y, or X axis to the negative direction on XY, XZ, YZ, or ZX plane in a right-hand Cartesian coordinate system. Method I Describing an Arc Using Incremental Center The end point of an arc is specified by address X, Y, or Z and is expressed as an absolute or incremental value depending on G90 or G91.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Arc End Points The radius is always specified as its true value. The end points are incremental or absolute depending on G90 and G91. If a radius is used without a center point, there are two types of arcs that can be generated. One is less than 180°, and the other is greater than 180°, as shown in the figure that follows. When the arc exceeds 180° the radius must be specified as a negative value.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Trig Help will allow the programmer to estimate both the start and end points of any arc. The control will calculate the true start and end points based on the moves preceding and trailing the arc. Where there are two possible correct answers, the control will choose the point closest to the estimated point. If the slope of the line entering or leaving the arc is such that no intersection occurs, the line will be made tangent to the arc.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Program 2 Programmed path G1 X0 Y0 X2 Y1 (estimated start point) G2 R1.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Program 3 Programmed path G1 X0 Y0 X7 Y6 (estimated start point) G2 R1.5 XC4 YC2 X5 Y.2 (estimated end point) G1 X5 Y0 Path generated by Program 3 In general, when dealing with lines and arcs, if the line is programmed short of the arc it will be extended to the arc. If the line is programmed past the arc it will be shortened to the arc, and if the line does not intersect the arc it will be made tangent.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Program 4 Programmed path G1 X0 Y0 X2.5 Y2 (estimated start point) G2 R1 XC5 YC4 X5 Y5 (estimated end point) R2 XC7.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Program 5 Programmed path G1 X0 Y0 X2.5 Y2 (estimated point) G2 R1 XC5 YC4 X5 Y3 (estimated end point) G3 R2 XC7.5 YC5 X9 Y5 (estimated end point) G1 Y0 Path generated by Program 5 In general, when estimating arc-to-arc intersections, the easiest end points to pick are one of the quadrant points (0°, 90°, 180°, or 270°).
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Things To Remember When Estimating Points • Estimating can be used with line to circle, circle to circle, and circle to line paths. • The center and radius of arcs cannot be estimated. • For line-to-circle and circle-to-line, the start and end point estimates should lie on the line; i.e. the slopes of the lines entering or leaving the arc must be correct.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) The block X2 Y6 is pulled in tangent to the arc. The cutter compensation has already taken into consideration the previous two lines, and it has calculated the compensated point based on the original line rather than the tangent line. The compensated path for this program will not cut the correct part. To avoid this problem, you must verify the program with cutter compensation off (or 0 tool radius). Note the actual tangent point (X4.8276, Y5.0690).
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) The polar format for arcs can be mixed with the Cartesian formats. The following are legal formats. G17 G2 X_____ Y_____ AA_____ R_____ end point start angle G17 G2 AB_____ XC_____ YC_____ R_____ end angle center point G17 G2 I_____ J_____ AB_____ center point The above formats are written for the XY plane but are valid in any plane or direction. Trig Help is only valid in polar when using an arc with valid center point and radius.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) 2. Absolute coordinates (Polar Trig Help) G90 G1 X0 Y0 R1 AB45 G3 R3 XC3 YC7 AB0 G2 R4 XC5 YC3 X8 Y.5 G1 Y0 X0 Note: When using Trig Help, you must have a valid arc center and radius. That is why the G2 and G3 lines have a fixed format. 3. Absolute coordinates (Cartesian No Trig Help) G90 G1 X0 Y0 X4.2929 Y4.2929 G3 R3 XC3 YC7 X5.9973 Y6.8737 or G3 I-1.2929 J2.7071 X5.9973 Y6.8737 or G3 R3 X5.9973 Y6.8737 G2 R4 XC5 YC3 X8 Y.3542 or G2 R4 X8 Y.3542 G1 Y0 X0 4.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) 5. Incremental coordinates G91 G1 X0 Y0 X4.2929 Y4.2929 G3 I-1.2929 J2.7071 X-1.7044 Y2.5058 or G3 R3 XC3 Yc7 X-1.7044 Y2.5808 or G2 I-.9973 J-3.8737 X2.0027 Y-6.5195 G2 X2.0027 Y-6.5195 I-.9973 J-3.8737 or G2 R4 X2.0021 Y-6.5195 or G2 R4 XC5 YC3 X2.0027 Y-6.5195 G1 Y-.3542 X-8 Note: In Incremental, Trig Help cannot be used as each point is related to the current position. Trig Help can be shut off by setting bit 2 of the miscellaneous special flags parameter.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Angle chamfering (,C) By adding ,C___ to the end of blocks commanding linear interpolation, angle chamfering is automatically inserted. G91 G01 X0 Y0 X1,C.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Back line The back line function can be used on any line command. This function reverses the direction of a programmed line. It would normally be used when you know the end point of the line and not its start point. The end point would be programmed and the line would be extended backwards to the start point. All Trig Help functions are still valid when using this function.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) W135 This line does not intersect with the arc; therefore, the line will be rotated until it is tangent. X0 Y0 X3 Y1 X4 Y0 X0 Y0 BACK C0 or C2 W165 This example used a back line between two lines to program an unknown point.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Notes on Circular and Linear Milling The feedrate in circular and linear is equal to the feedrate specified by the F address. This feedrate is the tangential feedrate along the arc and the vector feed on the linear moves. Note 1: I0, J0, and K0 can be omitted. Note 2: If X, Y, and Z are all omitted – or if the end point is located at the same position as the start point and the center is commanded by I, J and K – an arc of 360° (a complete circle) is assumed.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) The above formats for helical milling illustrate the general concept. Any of the previous arc formats can be used to do helical cutting by simply adding the third axis end point to the arc command. An F address specifies a feedrate along a circular arc. Therefore, the feedrate of the linear axis is as follows.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Set data on/off (G10, G11) This function allows all the CNC's configuration, setup, axis, and offset table parameters to be loaded via a program rather than through the front panel. (This function is the only way to change parameters 700 and higher from a program.) The format for loading the parameters is as follows.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Metric dimensioning mode (modal) (G21) This function will cause the system to go into the metric mode. In this mode the system will accept dimensions in millimeters (mm). In metric the actual machine position may not exactly agree with the program position because of the conversion. Feedrate in the metric mode is in millimeters per minute (mmpm). Note: The CNC does a conversion - -from metric to inch and inch to metric - on all tool offsets.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Circular pocket clear (G24) The G24 autoroutine is used to clear a circular pocket by starting in the center and spiraling out to the programmed diameter. Circular Pocket Clear Program N1 N2 N3 N4 N5 N6 N7 N8 N9 G20 G90 (Inch/Absolute) G00 X0 Y0 (rapids to center of pocket) S1000 M3 D1 G43 H1 (spindle CW-1000 RPM, calls tool #1's offsets) F25 (X-Y feedrate) P150=1 (pocket radius) P153=.015 (X-Y finish stock) P154=.005 (Z finish stock) P155=.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) CW Circular Pocket Clearing Block # N9 Block 9 CCW Circular Pocket Clearing Block Entry Info G2 G42 Selects CW circle, and turns ON right cutter compensation Block # N9 Block 9 Block Entry Info G3 G41 Selects CCW circle and turns ON left cutter compensation Circular finish inside (G25) If a tool radius is specified, cutter compensation can be used in all autoroutines.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) The figure below “Inside CW Finish Circle” shows the tool path of the following program. The figure below “Inside CCW Finish Circle” shows the same program with the change indicated in line N9.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Note: Parameter P150 is the pocket radius. If no finish stock is desired, parameters P153 and P154 should be set to zero. The F20 programmed in N5 is the XY feedrate and the F5 in N9 affects only the Z axis feed. Once parameters are set to a value they do not change and can be utilized further in the program. When an autoroutine is called, any parameters that are not re-initialized will default to the previous value of the parameter.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) *5 *6 *7 *8 *9 Plunge Final Z depth First Z depth Z increment Z feedrate Outside CW Finish Circle N7 Outside CCW Finish Circle G2, G42 selects CW direction and left cutter compensation N7 G3, G42 selects CCW direction and right cutter compensation Reference point return (G28, G29, G30) These commands allow the machine to be commanded to a fixed point (reference point) by first passing through an intermediate point on the way to the reference point.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Example 1: G28 (No axis movement) Example 2: G91 G28 Example 3: X1 Y0 Z-2 G28 X3 X3 then X-10 (Relative to machine zero.) X-3 Y2 Z-8 G28 Z-7 G29 Z -7 then Z-0.1 (Relative to machine zero.) Z to -7 Example 4: Z0 (Z to -0.1 Relative to machine zero) The G29 command is the converse of a G28. G29 will return the machine to the programmed point via the last intermediate point stored by a G28 command. The command format is as follows.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Example of G28 and G29: X1 Y1 G28 X3 Y2 G29 X6 Y1.5 Point A Point B then Point R Point B then Point C G30 2nd, 3rd, 4th Reference Point Return This function works in an identical manner to the G28 reference point return except that a 2nd, 3rd, and 4th reference point can be called. The command format is as follows.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Z to clearance (G31) The G31 function will retract Z to the clearance position. This position defaults to the last clearance position but may be changed by editing parameter 140 or set in canned cycles with the "R" parameter. Z to tool change (G32) The G32 function will retract Z to the tool change position. This position is set by the machine tool builder but may be changed by editing the tool change coordinate parameter.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Rectangular Pocket Clear Program N1 N2 N3 N4 N5 N6 N7 N8 N9 N10 N11 G20 G90 (Inch/Absolute) S1000 M3 D1 G43 H1 (spindle CW-1000 RPM, calls tool #1's offsets) G00 X0 Y0 (rapids to pocket center) F20 (X-Y feedrate) P150=.75 (corner radius) P151=4 (X pocket dimension) P152=2 (Y pocket dimension) P153=.015 (X-Y finish stock) P154=.005 (Z finish stock) P155=.5 (cut width) G34 G99 G42 G2 R.1 P199=1 Z-.5 V-.3 Q.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Rectangular Finish Inside Program N1 N2 N3 N4 N5 N6 N7 N8 N9 N10 G20 G90 (Inch/Absolute) S1000 M3 D1 G43 H1 (spindle CW-1000 RPM, calls tool #1's offsets) G00 X0 Y0 (rapids to center of rectangle) F20 (X-Y feedrate) P150=.25 (corner radius) P153=0 (X-Y finish stock) P154=0 (Z finish stock) P151=4 (X pocket dimension) P152=2 (Y pocket dimension) G35 G99 G42 G2 R.1 P199=1 Z-.5 V-.3 Q.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Block # N10 Line Entry Info G2 G42 selects CW direction and right cutter comp Block # N10 Inside CW Finish Rectangular X < Y P151 < P152 Block # N10 Line Entry Info G3 G41 selects CCW direction and left cutter comp Line Entry Info G2 G42 selects CW direction and right cutter comp Inside CW Finish Rectangular X>Y P151>P152 Block # N10 Inside CCW Finish Rectangular Corners and X < Y P151 < P152 Line Entry Info G3 G41 selects CCW direction and left cutter
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Rectangular finish outside (G36) The G36 autoroutine is used to remove finish stock around the outside of a rectangular boss. The G36 autoroutine works in an identical manner to the G34 autoroutine. It starts in the center, makes a rapid move to the outside of the part, then feeds the tool down. The circle to the edge is always on the bottom side of the boss.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Block # Line Entry Info N11 G3 G42 selects CCW direction and right cutter comp N11 Outside CCW Finish Block # Line Entry Info G2 G41 selects CW direction and left cutter comp Outside CW Finish Threading (G39) The G39 autoroutine is used for cutting threads. It is possible to program either internal or external threads. G39 works on the same principles as the G25 circular finish inside and the G26 circular finish outside.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) For internal threads, the start point is the center of the thread for cutter compensation both on and off. If external threads are programmed, it starts at the center and rapids to the feed down point using the following formula for cutter compensation off. X = thread radius + [2 X tool radius] + 0.1 Cutter compensation on the control uses the following formula to calculate the feed down point. X = thread radius + [3 X tool radius] + 0.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Inside polygon program G0 X2 Y3 (Center) F20 (XY Feedrate) P126=2 (Radius to the corner) P127=0 (Angle to the 1st corner) P125=6 (Number of sides) P128=.3 (Corner radius) P132=0 (Inside/outside) G666 G99 G3 G41 R.2 P199=1 Z-1 V-.1 Q.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Outside Polygon Program G0 Z2 G65 X2 Y3 (Center) F20 (XY Feedrate) P126=3 (Radius to the corner) P127=60 (Angle to the 1st corner) P125=3 (Number of sides) P128=.1 (Corner radius) P132=1 (Inside/outside) G666 G98 G2 G41 R.1 P199=0 Z-1 V-.2 Q.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) N1 N3 N4 N5 N6 N7 N8 N9 N10 N11 N12 *1 *2 *3 *4 *5 *6 G20 G90 (Inch, Absolute) N2 G0 X0 Y0 (Rapid position to X center, Y center for internal)(use a G65 for external) F100 (Feedrate) P121 = 0 (Angle of taper specified by the half angle or angle with the centerline, 0 for a straight thread) P122 = 10 (Threads per unit) P123 = 1 (1 for internal threads, 2 for external threads) P125 = .
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) directly off the print, then by entering the actual tool radius into the system and activating cutter compensation, the operator can make the control calculate the displaced path. Throughout the program the control keeps a record of the previous programmed point, the current programmed point, and the next programmed point along the tool path.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Explanation of How Displaced Tool Paths Cannot Have an Intersection (a) Path of a cutter with (b) 0" tool diameter Path of a cutter with non-zero tool diameter The solution of the above part is to introduce a 00.0001" chamfer or round corner at Point 5 between the non-intersecting surfaces. Explanation of How a 00.0001" Chamfer Should Be Introduced to Solve a Non-intersection Problem Note: The “,C” used to chamfer can only be used between two lines.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Outside "V" Cutter Compensation Note: Compensation point (4') is displaced more than the tool radius away from (4). The figure below shows how a 00.0001" chamfer or round corner added at point (4) has saved an unnecessary departure. Outside "V" Cutter Compensation Solution The figure below shows how the compensated point for an inside "V" will stay away from the programmed point by more than the tool radius.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Inside "V" Cutter Compensation Note: The tool stays away from the programmed point (2) by a distance more than the tool radius. If the compensated point (2') was any closer to (2), the tool would gouge the sides of the part. Sample part exercise As the system requires three points to generate a compensated point, care should be taken when the cutter compensation is turned on or off.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Determining How the Compensated Path Will Look Step 1. Sketch actual part and label points in sequence. Step 2. Sketch lines displaced by tool radius away from part surface from point 1 to point 11.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Step 3. Check to verify all paths in the sequence intersect. If yes, then (except for the start and end points) connect the displaced path and label points of intersection. If even one intersection cannot be found, the part will not run unless the error is corrected. Step 4. Since points 1 and 11 do not have two points on either side, they will be the uncompensated points.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Step 5. The above displaced path is what the system will trace if the part is run. However, a problem has become apparent from the rough sketch. Note that the lower left-hand corner will be left uncut because the tool going from (1) to (2) will leave a small notch of uncut material. A similar case is obvious in the tool path from (10) to (11). There again the corner will be left uncut.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Step 6. Note how points 1, 2, 10, and 11 have been moved slightly. The result will be as follows. Note: It is now seen that when the tool moved from (2) to (3), and (9) to (10), the corner will be properly cut. In Step 6, the cutter compensation was turned on by using the G41 command for turning on left cutter compensation at point (2) and turned off by using the G40 command at point (11).
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Note 5: Cutter compensation is shut off at the start of each program. How To Compensate for a Cavity If the part is a cavity, then the start and end points will have to change. Simply changing the G41 to G42 (right cut) will not help. This is because the tool will still come down on the part. The reason for that is as explained earlier: the system uses the previous, current, and the next programmed points to calculate its compensation.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Programming with Cutter Compensation When programming with cutter radius compensation, the first and last move the cutter makes should be done off the part per the figure below. The movement made prior to cutting should be at least the distance of the cutter diameter being used. Block # Block Entry Info N1001 N1002 N1003 N1004 N1005 N1006 N1007 N1008 N1009 N1010 G0 X-1 Y-1 G41 X0 D1 (D offset = tool radius) G1 Y3 F10 X3.5 G3 R.5 XC4 YC3 X4.5 Y3 G1 X6.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) G65 will allow the programmer to turn cutter compensation on and get the tool to drop or retract at a specific point without doing any extra moves. Generally the no-move point would be chosen to be a point on the part that directly precedes the tool down point. On a tool retract, the no-move point would be a point on the part directly after the tool up point. The no-move point does not have to lie on the part, but points on the part generally work the best.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Starting and Ending Cutter Compensation G41 Tool Left D1 = Tool Radius (Previously Set in D1) PIERCE 1=point on part before pierce point 2=pierce point 3=first cut move RETRACT 1=last position before retract 2=tool retract position 3=point after retract 246
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) G42 Tool Right D1 = Tool Radius (Previously Set in D1) PIERCE 1=point on part before pierce point 2=pierce point 3=first cut move RETRACT 1=last position before retract 2=tool retract position 3=point after retract 247
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Sample Program for Enter-Exit Cutter Compensation G0 X-5 Y1 G41 D1 F10 G65 X0 Y1 X0 Y0 G1 Z-1 X1 Y1 X0 Y0 G65 X1 Y0 G40 G0 Z0 part load/unload point cutter comp. on offset #1 no move compensation point tool down cutter comp. off no move exit point tool up Note that the tool enters and exits the part tangent to both walls because of the G65 lines.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Note 5: All autoroutines use the present axis position as their center. For this reason it should be made sure that the cutter compensation is turned off in a program using these routines so that the axis can position to the programmed center. If a compensation center is used, the entire pocket will be shifted. Note 6: If the programmed point rather than the compensated point is desired, a G40 command should be added to the block containing that point.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) In the above cases, the tool will back up as it tries to place itself tangent to the walls of the slots or v. This case will give a “compensated line/arc do not intersect” error.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Sample Programs Cutter comp on using a G41 X-1 Y1 G41 X0 Y0 X1 Y.2 X0 Y1.5 Cutter comp on using a G45 X-1 Y1 G45 X0 Y0 X1 Y.2 X1.1 Y1 X0 Y1.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Cutter comp off using a G40 X-1 Y1 G41 X0 Y0 X1 Y.2 G40 X1.1 Y1 X0 Y1.5 Cutter comp off using a G47 X-1 Y1 G41 X0 Y0 X1 Y.2 G47 X1.1 Y1 X0 Y1.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Tool length offset (G43, G44, G49) A tool length offset is activated using a G43 or G44 command. Command format: G43 G44 or G43 G44 or G43 Z ____ H____; (Z moves to dimension selected referenced to tool length offset selected by H) H____; H10; 1st offset H14; 2nd offset H13; 3rd offset H15; 4th offset The direction of the offset is controlled by G43 and G44; the magnitude of the offset is set by the offset value in the H table.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) H offsets from the tool table H01 = 1.5 H02 = -.5 H03 = -1.25 H04 = 5 Various program lines and results G17 G43 H1 G90 Z0 Z1 H3 G44 H3 Z0 H4 Z0 G19 G43 H2 X0 H0 X0 G49 X0 Z0 Z moves to 1.5 (from home) Z moves to -.25 (from home) Z moves to 1.25 (from home) Z moves to -5 (from home) X moves to -.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) P1 - P4 P1'- P4' P0 original program no scaling scaled program scaling center Notes on Scaling Note 1: Once set, scaling remains in effect until canceled by a G50. Note 2: If arcs are being scaled, the primary axis scale factor is used. Note 3: G27, G28, G29, G30, and G92 are not affected by the scale factors. Note 4: To scale all axes to the same scale factor use G51 P. Note 5: G50 sets scale factors to 1 and scaling centers to zero.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Coordinate systems Machine zero is a fixed point on the machine. The machine tool builder normally decides the machine zero point. A limit switch and encoder marker pulse on each axis sets it. The machine zero point is established when the F1(Home) command is first executed. Once the machine zero point is established, it is not changed by reset, coordinate system call (G54-G59), coordinate system shift (G92), or local coordinate system setting (G52).
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) A coordinate system used to align the work part dimensions to the machine's programs is called a work coordinate system. The work coordinate system is set by either of the following methods. 1. using a G92 command 2. using a G53 command 3. using G54 -G59 commands 4. using A G52 command Work coordinate systems (G54 - G59)(G5#0…G5#9) The dimensions of the work coordinates are always relative to the G92 Floating Zero Point.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Note 3: G52 offsets are not affected by the position of the machine. G92 offsets are affected by the position of the machine. Note 4: G52 offsets are zeroed on power-up, after homing, after setting work offset in handwheel or jog, and after any G92 command. Note 5: G52 offsets are restored to there initial values after the program ends. G55 X2 Y2 G52 X1 Y1 X1 Y1 X2 Y2 moves to P3 sets zero at P2 dim. rel.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Single direction or one shot rapid positioning (G60) For accurate positioning without backlash, positioning from one direction is available. G60 X___ Y___ G60 is a one-shot G code and is used in place of G00. Notes on Single Direction Positioning Note 1: The amount of overrun is pre-set by the machine tool builder. Note 2: Overrun direction is not affected by mirror imaging.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Example: *G65 P1402 A500 (calls program #1402 and sets parameter #1 to 500, parameter #16 to 1402, and parameter #7 to 65) * Parameters not specified are set to -999. The addresses refer to the parameters as follows. Address Parameter # A B C . . X Y Z 1 2 3 . . 24 25 26 Notes on Calling a Program with G65 Note 1: If the program specified by address P does not exist, an error will occur. Note 2: The program called is the rounded value of address P.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) G69 zeros the rotation angle and rotation center. Care needs to be taken when using rotation in conjunction with other functions. Functions such as mirror image, scaling, and cutter compensation need to be carefully considered when used together with rotations. Some of the basic rules are as follows. 1. Cutter compensation should be off (G40) when rotation is called. (Cutter compensation can be turned on after rotation is called.) 2.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) 7. R can be used instead of AA for rotation angle. 3D Rotation (G0, G1, G2, G3, G68 AND G69) G0, G1, G2, and G3 respond to 3D rotation when a G68 ABm has been entered. G68 ABm The ABm signifies 3D rotation. The angle m in degrees is the rotation of the primary axis into the tertiary. For example, G17 G68 AB30 causes a 30 degree rotation of X coordinates into Z coordinates.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Note: Any AA in plane rotation is ignored. Cutter compensation and trig help are not fully supported in 3D rotation. G69 Cancels all rotation, including 3D. Part Scaled then Rotated G51 I4 J1.5 X.7 Y.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Part Rotated then Scaled G68 I3 J1 AA45.00 G51 I4 J1.5 X.9 Y.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Cancel mirror image (G70) Set mirror image (G71) The mirror image commands allow mirroring about any centerline. The mirror image centerline is not affected by either scaling or rotation being on or off. Mirror image is shut off at the start of each program. The command is as follows. G71 X____ Y____ Z____ X,Y, and Z specify the axes to mirror. Their values specify the distance from the current coordinate zero to create the mirror centerline.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) G70 cancels mirror image. Mirroring in one axis will reverse climb cutting and conventional cutting. Mirroring an axis is similar to scaling by –1. Canned cycles A canned cycle simplifies a program by using a single block with a G code to specify the machining operations usually specified by several blocks.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Canned Cycles Drilling -Z Operation at Hole Bottom Retraction +Z G73 Intermittent feed - Rapid traverse High-speed peck drilling cycle G74 Feed Dwell → spindle CW Feed Left hand Tapping cycle G75 Feed - Rapid Counter bore Feed Dwell →orient spindle → move in X Y G code G76 Rapid → moves in XY G77 Application Fine Boring cycle Custom Drill Cycle G78 Feed Dwell → stop spindle → handwheel → Rapid Manual Boring cycle G80 - - - C
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Operation 1: Operation 2: Operation 3: Operation 4: Operation 5: Operation 6: Positioning of axes X and Y (or 4th and 5th if enabled) Rapid traverse to point R Hole machining Operation at the bottom of a hole Retraction to point R Rapid traverse up to the initial point Canned Cycle Operation Positioning is normally performed on the XY plane, and hole machining is performed with the Z axis.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) . G89 Note: The initial level means the value of the Z axis when the canned cycle is first turned on. The figure below shows how to specify data in G90 or G91 mode. Absolute and Incremental Programming If the tool is to be returned to point R or to the initial level, it is specified by G98 or G99. (See figure below.) Use G99 for the first hole, and use G98 for the last hole.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Initial Level and Point R Level The drilling data is specified following G73,G74,G76,G77,G78, G81 to G89. Data is stored in the control as modal values and is retained for future use in other cycles. The machining data in a canned cycle is specified as shown below. G __ __ Drilling Mode X__ Y__ Hole Position Data Drilling mode . . . Hole position data Drilling data Z__ R__ V__ Q__ P__ F__ Drilling Data G__ __See canned cycle table.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) For drilling cycles you may use: P140 P141 P142 P143 P144 P145 P146 P147 P148 P149 for for for for for for for for for for Clearance plane Final Z depth Z initial level Z increment 1st Z depth Z feedrate Peck up increment Peck clearance Dwell before spindle reverses in tap cycles Dwell The drilling mode (G__ __) remains unchanged until another drilling mode is specified or the canned cycle is canceled with a G80.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Bolt hole routine (G72) The bolt circle autoroutine can be used with any of the drilling cycles. Drilling cycles, when used with this autoroutine, differ in that hole positions are not specified. The G72 line indirectly specifies all the hole positions based on specific input: number of holes in 360°, number of holes to be drilled, the radius of the bolt circle, the starting angle of the first hole, and the center of the bolt circle.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Program to Drill a 5 Hole 1" Radius Bolt Circle N1 N2 N3 G20 G90 (Inch/Absolute) S1000 M3 G43 H1 (spindle CW 1000 RPM, activates tool #1's length offsets) G81 G99 Z-1 R.1 F10 G81 G99 Z-1 R.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Note 4: The G65 cannot be on the G72 block because there is also a P on the block that will cause a program call to program #5. You may also use: G81 G99 Z-1 2.1 F10 P156=1 (Bolt hole radius) P157=45 (Bolt hole start angle) P158=5 (# of holes in 360°) P159=5 (# of holes to be made) G72 G65 X0 Y0 (Bolt hole center) Note 5: The initial Z level corresponds to where Z is when the drilling code (G73 through G78,G81 to G89) is executed.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) High speed peck drilling cycle (G73) G73 G98/G99 Z___ R___ V___ Q___ U___ D___ F___ The G73 command specifies the high speed peck cycle. This cycle will do the following. 1. 2. 3. 4. 5. 6. 7. Rapids to point R Feeds down to point V Rapids up U value Rapids down to D value Feeds down by Q value or Z point (whichever is less) Repeat steps 3-5 until point Z is reached Rapids to initial point/point R as determined by G98/G99 Note: The V command is optional.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Left hand soft tapping cycle (G74) G74 G98/G99 Z___ R___ B___ P___ F___ The G74 command specifies the left hand soft tapping cycle. At each axis position, this cycle will do the following. 1. 2. 3. 4. 5. 6. 7. 8.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Example: 1/4-20 tap, spindle rpm 400 1/20 = .05 (lead) 400 x .05 = 20 (feedrate) Feedrate may need adjustment for proper operation of tap holder. If tap is pulled too far in the holder, feedrate should be increased. If tap is pushed into the holder, feedrate should be decreased. Counter Bore (G75) The counter bore is identical to the circular finish inside cycle (G25). It always does a climb cut (counter clockwise).
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) 2. 3. 4. 5. 6. Feeds down to point V. Counter bores the hole (to radius P150). Feeds down by Q value or Z point (whichever is less). Repeats steps 3-4 until point Z is reached. Rapids to initial point / point R as determined by G98/G99. Note 1: The V command is optional. If left out, the 1st depth would equal R__ - Q__ Note 2: It is possible to do a conventional cut (clockwise) by using mirror image.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) G76 F____ P____ R____ Z____ G98/G99 The G76 command specifies the fine bore drilling cycle. At each axis position, this cycle will execute the following.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Drilling cycle, manual bore (G78) G78 F____ P____ R____ Z____ G98/G99 The G78 command specifies the manual bore drilling cycle. At each following axis position, this cycle will do the following. 1. 2. 3. 4. 5. 6. 7. Rapids to point R Feeds down to point Z Dwells P seconds Stops the spindle Enters the handwheel mode (user can handwheel the axes, turn spindle on/off, remove tool, etc.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Drilling cycle (G81) G81 G98/G99 Z___ R___ F___ The G81 command specifies the drilling cycle. This cycle will do the following. 1. 2. 3.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) The G82 command is similar to the G81 command; however, a dwell (specified by the P command) is performed at the bottom of the hole. This cycle will do the following. 1. 2. 3. 4. Rapids to point R Feeds down to point Z Dwells by P___ seconds Rapids to initial point/point R as determined by G98/G99 Peck drilling cycle (G83) G83 G98/G99 Z___ R___ V___ Q___ D___ F___ The G83 command specifies the peck drill cycle. This cycle will do the following. 1. 2. 3. 4.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Right-hand soft tapping cycle (G84) G84 G98/G99 Z___ R___ B___ P___ F___ The G84 command specifies the right-hand tapping cycle. At each axis position this cycle will do the following. 1. 2. 3. 4. 5. 6. 7. 8.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Feedrate may need adjustment for proper operation of the tap holder. If the tap is pulled too far in the holder, feedrate should be increased. If the tap is pushed into the holder, feedrate should be decreased. Boring cycle (G85) G85 G98/G99 Z___ R____ F___ The G85 command specifies the boring cycle. At each axis position this cycle will do the following. 1. 2. 3. 4.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Fast bore cycle (G86) G86 G98/G99 Z___ R___ F___ The G86 command specifies the fast bore cycle. At each axis position this cycle will do the following. 1. 2. 3. 4. 5. 6. 7.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Back Boring cycle (G87) G87, G98 F____ R____ Z____ The distance and angle is specified by control parameters "Bore Relief Angle" and "Bore Relief Distance". The G87 command specifies the back bore drilling cycle. At each axis position, this cycle will execute the following. 1. 2. 3. 4. 5. 6. 7. 8. 9.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) 10. 11.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Hard tap cycle (G88) G88 G98/G99 Z____ R____ F____ P____ (Q____ V____) The G88 command specifies the hard tapping cycle. P(dwell) can be used if the distance between holes is small to give the spindle time to reverse to its proper direction. This cycle will do the following. 1. 2. 3. 4. 5. 6. 7.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Bore/Dwell cycle (G89) G89 G98/G99 Z___ P___ F___ The G89 command specifies the bore with dwell cycle. At each following axis position this cycle will do the following. 1. 2. 3. 4. 5. Rapid to point R Feed to point Z Dwell at bottom (specified by P code) Feed to point R Rapid to initial point, if specified by the G98 code Sample program to drill holes in the YZ plane. G19 G81 R.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Notes on Canned Cycle Specifications Note 1: The spindle must be turned on by M code, M3 or M4, before the canned cycle is specified. M3 Spindle CW . . . G __ __ ......Correct M5 Spindle Stop . . . G __ __ ......Incorrect (M3 or M4 must be specified before this block.) Note 2: If the block contains an X and/or Y move, drilling is performed in canned cycle mode. If the block does not contain an X and/or Y move, drilling is not performed.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Note 4: Specify drilling data in the block where drilling is performed. Entries (V, Q, B, Z, R, F, or P) are stored as modal data. Drill Example: G90 G81 G0 R.1 Z-2 F10 (drill clearance .1, depth -2, Z feed 10) X1 (drill hole -2 deep at X1) X2.5 F5 (drill hole -2 deep at X2.5, Z feed 5) X3.5 Z-1 (drill hole at X3.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) G00 M___ G86 X___ Y___ Z___ R___ F___ G04 P___ (Dwell is performed, but drilling is not.) X__ Y___ G04 P___ (Dwell is performed, but drilling is not.) X__ Y___ G04 P___ (Dwell is performed, but drilling is not.) . . . . . . This may not have to be considered if spindle up-to-speed is available on the machine tool.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Absolute Positioning G90 X0 Y0 X1 Y1.5 X2 Y2 P1 P2 P3 Incremental mode (modal) (G91) This function causes the control to go into the incremental mode. In this mode all dimensions are entered relative to the machine position in the previous block. In the case of MDI, the dimensions are relative to the current machine position. Dimensions in G91 can be either positive or negative. Care should be taken when using G91.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Incremental Positioning G90 X0 Y0 G91 X1 Y1.5 X1 Y.5 P1 P2 P3 Floating zero (G92) This command establishes the work coordinate system. The position of the tool becomes the programmed position in the current work coordinate system. When using this G92 command, think of it as “call this position” X_ Y_ Z_. If the machine is positioned at P2, which is a command of X1 Y1, and then a G92 X0 Y0 is commanded, the next time X.5 Y.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) machine is positioned at P1 and G92 X-1 Y-1 is commanded, the next time X.5 Y.5 is commanded the machine will position to P3. When using G92's for calling subprograms, the G92 is saved prior to calling the subprogram and restored when returning from the subprogram.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) moves that will slow down if any axis in the move goes faster than the maximum feed parameter for that particular axis. While in inverse time mode, the feedrate must be specified in every move block, or an error 611 will be reported. Example: G93 X-10Y-2.4A-3F.25 (Assuming feedrate units of 1/sec, the move will take 1/.25 = 4 seconds regardless of where the machine is moving from.) X-5 (This line generates an error 611 because no feedrate is specified.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) 21.6 seconds, where 5000 is the maximum feedrate for rotary axis A. Feed Per Revolution (G95) This G code is a modal G code that instructs the control to interpret feed commands as mm or inches per revolution of the spindle. G1 F.005 would cause the axis to advance .005" for every revolution of the spindle. Note: The machine must have the hard tapping option to use this G code.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) G65 X1 Y0 G40 N1235 (The ‘Q’ specifies the end of the pocket) This program will clear a pocket that looks like this. The Cut Width is the distance between 1 pass and the next. The Finish stock is not removed with a final pass. To remove the stock another mill cycle needs to be programmed. The Finish Stock is not an option if the cutter comp is off. Note 1 : The ‘I’ value requires that cutter comp is on.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) The cycle can be used to clear around islands. Sample program with islands: P145=10 (Z Feedrate) F321 (XY Feed-rate to clear the pocket) G271 P1234 Q1235 R.1 Z-1 D.1 I.05 ('R' is the R plane, 'Z' is the Z-depth, 'D' is the Cut Width and 'I' is the Finish Stock) N1234 (The 'P' specifies the start of the pocket) G41 G65 X0 Y1 G0 X0 Y0 G1 X2 Y1 G3 R1 AA-90 AB90 G1 Y4 X0 Y0 G65 X1 Y0 G40 P516 = 1 (Specifiles and Island) G45 G0 X1 Y1 G2 R.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) This program will clear a pocket that looks like: A discussion follows on several specialized and non-standard G codes. Store Restore parameters (G990/G991) Pp Ll Qq G990 (store parameters) Pp Ll Qq G991 (restore parameters) G990/991 allow parameters to be saved and restored using file names C:/RAM/Q0000-Q9999. Parameters are: Pp (base parameter number, default 0), Ll (number of parameters, default 10), Qq (file identification, default 0).
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Read byte parameter (G995) P1=b G995 (sets P0 to value of byte b) Example: P1=79 G995 (sets P0 to value of byte 79, G18 plane select, XZ=0, ZX=1) valid P1 values are 0 to 639 Valid P1 values are 0 to 639 Valid P0 values are 0 to 255 Note: The G995 is identical to P0=PB##. Write byte parameter (G996) P1=b P0=V sets byte parameter b to value v.
SECTION FOUR - PREPARATORY FUNCTIONS (G CODES) Force Error (G997) Forces an error code to be displayed. Error code generated is round (parameter #1). Example: P1=408 G997 (Forces a 408 Y axis excess error to be displayed. Y axis does not cause an excess error, it only displays the error). Note: P1=0 will not produce an error. All valid error codes on the control are between 1 and 999. Beep (G998) G998 will cause the speaker to beep if a speaker is installed.
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) These codes are used if the operator is programming the Centurion 6 in the text mode or MDI mode. They are also generated from conversation programs. It should be noted that most programmers – particularly new programmers – use the conversational programming mode. If you are planning to use text mode programming, pay close attention to this section explaining these codes.
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) M codes M codes Function Executed Before Move Executed After Move X X X X M00 M01 M02 M30 Program Stop Optional Stop End of Program End of Program/ Spindle Off M03 M04 M05 Spindle on CW Spindle On CCW Spindle Off M06 Tool Change M07 M08 M09 Mist Coolant On Flood Coolant On Coolant Off X* X* M10 M11 M19 Clamps Brake Unclamps Brake Orient Spindle (ATC Option) X* X* X* M31 E-Stop X* M32 Test Wait Channel X* M90 Graphics Off X* M91 Graph
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) Caution: The control will accept more than one M code on a line; however, it is recommended that only one M code per line be programmed. When more than one M code per line exists, the order of execution is somewhat undefined and the program may not run as expected. In general the M codes will execute in numerical order "M00 first M99 last" unless they have been defined to execute after the move statements. (See Post M codes Table on page 55, Section 4.
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) comment is on the M6 block, it will be displayed to prompt the operator. The control shuts off the spindle and coolant, and then it waits until it receives a tool-change-complete signal. The spindle cannot be turned on until the tool change is completed. After the tool-change-complete signal, the program will resume running.
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) Channel (M32) This code causes the control to wait for the wait channel, X input 7, then continues the program. Miscellaneous M codes (M65/75, M67/77, M68/78, M69/79, M50/60) The standard M code is controlled by M65 (on) and M66 (off). These optional M codes control the four spare functions. Spare function one is controlled by M67 (on) and M77 (off). Spare function two is controlled by M68 (on) and M78 (off).
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) The starting point is stored in the following parameter. 121 for X axis 122 for Y axis 123 for Z axis To create a female part the starting angle must be between greater than 180° and less than 360°. For female parts that start at 0° use -.0001° or 359.9999°. For female parts that start at 180° use 180.00001° or -179.9999°. Z can change in the geometry as well. Example: P120=9 P127=1 P128=-.0001 P129=180 P130=.1 P145=10 F15 P121=0 P122=0 P123=0 P140=.
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) Example 1: Offset Island Taper Offset round/tapered walls parameter = yes First cut is offset to avoid over cutting vertical wall. Example 2: No Offset Island Taper Offset round/tapered walls parameter = no Offset is not needed to cut this part.
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) Example 3: Offset Cavity Taper Offset round/tapered walls parameter = yes First cut is offset to avoid cutting vertical wall. Example 4: Offset Cavity Taper Offset round/tapered walls parameter = no There is no need to offset tool on this part. Note: The first cut at first Z depth is always offset by the entire tool radius. First Z depth should be at the top of the surface to cut.
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) Wall angles are described as follows, regardless of pockets or islands. If you are using a ball-nosed tool with the tapered walls, use an M95 EO (or M95). If you are using an end mill, use M95 E1. Example Program: This program makes a 2" x 3" cavity with 30° walls. P140=.1 P141=-1 P143=.
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) Rounded Walls (M96) M96 can be used for rounding walls in pockets or on islands. This command takes a start angle, wall radius, first and final Z depths, and the Z increment as parameters. The M96 must be within a while-wend loop. The tool radius, parameter #160 (the current Z depth) and cutter compensation must be on to use the round walls feature. The M96 sets parameter #162 to 2 when the cycle is completed. The M96 assumes that a ball-nosed tool is used.
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) Example 3: Offset Cavity Rounded Wall Offset round/tapered walls parameter = yes First cut is offset to avoid cutting vertical wall. Example 4: No Offset Cavity Rounded Wall Offset round/tapered walls = no No need to offset tool on this part.
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) This program makes a 2" x 3" island with rounded walls. The wall has a 2" radius and starts at a slope of 30°. P140=.1 P141=-1 P143=.
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) Notes on Rounded Walls Note 1: The first cut at the first Z depth is always offset the entire tool radius. Note 2: The first Z depth should be at the top of the surface to cut. Note 3: If the wall radius and start angle will not span the first Z depth and final Z depth, an error will occur. Start angles are defined and illustrated in the following drawings. Negative start angles are allowed.
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) Pocket Clear (M97) M97 can be used for clearing pockets as well as clearing away material from islands. It can also be used for finish passes on irregular pockets or islands. This command takes two parameters: the number of passes to make and the cut width of each pass. The command must be within a while-wend loop. The cut width is added or subtracted to the cutter radius and moves toward or away from the part.
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) The previous program makes this for a .1" radius tool: To clear away from an island with the same shape, change the G41 to G42. To make a finish pass, load the tool table with a tool radius bigger than the actual tool in use. P163=2 P164=-.01 Make 2 passes Correction to actual tool size/finish stock to clean up Note: Pocket clearing is used to remove stock from a part. If too many passes are programmed, the surface may be violated.
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) When the main program calls a subprogram, it is regarded as a one loop nest. A two loop nesting can be executed as shown below. When used with an L___ command, an M98 command can call a subprogram repeatedly. An L___ command can specify up to 999 repetitions of a subprogram. Nesting with up to 50 loops is allowed. M2 can be used instead of M99. If a subprogram ends without an M2 or M99 it will return to the calling program as if an M2 or M99 was encountered.
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) Subprogram execution A subprogram is executed when called by the main program or another subprogram. A subprogram call has the following format. M98 PXXXX LXXX Where And PXXXX LXXX Example: = = subprogram number number of times the subprogram is to be repeated M98 P0002 L5 M98 P2 L5 Call 2 L5 This command reads, call subprogram number 2 five times. When the loop number is omitted, the subprogram is run once.
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) Notes on Subprograms Note 1: If the subprogram number specified cannot be found, a 603 error “program O#### does not exist” message is displayed. Note 2: A subprogram call M98___ cannot be executed from MDI. In this case write a short program to call the subprogram. 0XXXX M98PXXX M02 Note 3: Then execute it in the run mode.
SECTION FIVE - MISCELLANEOUS FUNCTIONS (M CODES) The text program can reside in the RAM directory or in the parts directory. The program in the RAM directory holds precedence over the program in the parts directory. If you call any custom M or G code from within a custom code, it will execute its normal function. If a syntax error exists in a custom code, a message will be given on power-up. Example 1: Set F3 (Power) parameter custom M code O9025 to 014 and enter a program into C:/RAM/O9025.
SECTION SIX - PARAMETRIC PROGRAMMING Parametric programming is similar to macro programming in that equations can be used to specify axis position rather than decimal numbers. The Centurion 6 does not restrict the use of parametrics to subroutines or macros. They may be used anywhere throughout a program. Parametric expressions may be used to specify M, G, F, and S functions. When a parametric expression is used for an axis position, it will first be evaluated and then cutter compensation will be applied.
SECTION SIX - PARAMETRIC PROGRAMMING Arithmetic operators The following list shows the available arithmetic operators. Operator + * ** / DIV MOD Operation addition subtraction multiplication exponent division integer division remainder Note: The value of A DIV B is the mathematical quotient of A/B with any fractional portion or remainder dropped. Examples: 3/2 = 1.5 24/5 = 4.8 72/8 = 9.0 5.46/2.1 = 2.6 3 DIV 2 = 1 24 DIV 5 = 4 72 DIV 8 = 9 5.46 DIV 2.
SECTION SIX - PARAMETRIC PROGRAMMING Function operators A function call is specified by the function name (e.g. SIN, ATAN, . . .) followed by the function argument in brackets. When a function is used for a coordinate position it must be contained in brackets. Examples: X [SIN [45]] Y [ATAN[1/2]] Z [SQRT[9]] A function returns a value and can be used interchangeably anywhere a decimal value is accepted. The functions supported are as follows. Sine (SIN) returns the sine of the argument.
SECTION SIX - PARAMETRIC PROGRAMMING Rounds (ROUND) rounds a decimal value to an integer value. Values halfway in-between are rounded up. ROUND [2.3] = 2 ROUND [7.88] = 8 ROUND [1.5] = 2 ROUND [-1.5] = -2 Values exactly halfway between are rounded to the nearest even number. ROUND [2.5] = 2 ROUND [3.5] = 4 Mathematic expressions Any combination of the previously described expressions are made up of arithmetic functions. Examples: X[SIN[P123]*COS[P124]] Y[2.
SECTION SIX - PARAMETRIC PROGRAMMING The above two statements accomplish the same thing. If the statement is true, N15 is executed; if it is false, N21 is executed. Examples: IF P1*P3/COS[P90] GE TAN[P6] THEN X1 IF P4/P3 LT P6 GOTO 25 IF P1 = P2 THEN P4 = P5 - P6 Multiple IF statements can be used to check for multiple conditions. Example: IF P36<5 THEN IF P1<>0 THEN M5 Defined, this means if P36 is less than 5 and P1 does not equal 0, shut the spindle off. Note: The word THEN is optional in all cases.
SECTION SIX - PARAMETRIC PROGRAMMING GOTO statement The statement N### defines a label. GOTO’s/GOSUB’s can branch or transfer control to blocks containing these labels. A GOTO statement transfers progam execution to the block prefixed by the block label referenced in the GOTO statement. GOTO 30 (The next block executed is block N30.) Note: If there is more than one N30 program, it will transfer to the first N30. CALL statement A CALL statement transfers control to any program residing in the CNC's memory.
SECTION SIX - PARAMETRIC PROGRAMMING The GOSUB format is as follows. GOSUB XXXX Line # LXXX Loop Count (optional) If the L is omitted the GOSUB routine will be executed once. N1 N2 N3 N4 GOSUB 100 N5 . . . N90 M30 N100 N101 . Main Program . . N200 N201 RETURN N202 Subroutine When the GOSUB is executed in N4 the program will jump to N100 and start executing until N201 is reached. At N201 control will transfer to N5 and lines N5 thru N90 will be executed.
SECTION SIX - PARAMETRIC PROGRAMMING Computational functions 1. Tangent Arc TANA 2. Tangent Line TANL 3. 3 Point Circle Generate CGEN The above three functions can be used anywhere throughout a program to solve various intersection problems. These functions receive input data in parameters P90 thru P96, and they return the answer in parameters P80 through P85. The answers can then be used in line and circle commands to produce the desired results. The format for these three functions follows.
SECTION SIX - PARAMETRIC PROGRAMMING TANA Cases 1st C0 = Right C1 = Left C2 = Right C3 = Left C4 = Left C5 = Right C6 = Left C7 = Right 2nd Center Right Right Left Left Left Left Right Right Left Left Left Left Right Right Right Right TANL Cases C0 = C1 = C2 = C3 = 1st 2nd Right Left Right Left Right Right Left Left 331
SECTION SIX - PARAMETRIC PROGRAMMING Sample Program Using TANA or TANL N1 N2 N3 N4 N5 N6 N7 N8 N9 P90=0 P91=0 P92=1.5 P93=5 P94=4 P95=2 P96=5 XC of arc 1 YC of arc 1 radius of arc 1 XC of arc 2 YC of arc 2 radius of arc 2 radius of tangent arc (not used for tangent line) TANA C3 or TANL C3 G2 R1.
SECTION SIX - PARAMETRIC PROGRAMMING The circle generate function will calculate the center and radius of an arc through any three nonco-linear points. The general format for the CGen function is as follows.
SECTION SIX - PARAMETRIC PROGRAMMING N1 N2 N3 N4 N5 N6 N7 N8 P140=.1 P141=-.2 P145=5 G1 F10 S1000 M3 X-4 Y.5 Text [MILLTRONICS MFG] M30 Clearance of .1 Depth of cut .2 inches Plunge feedrate of 5 ipm XY feedrate of 10 ipm Spindle on CW Position of first letter Desired text End program This program will write "MILLTRONICS MFG" at a depth of -.2" in 1" by 1" block letters starting at a position of X-4 Y.5. The text cycle can also be used to engrave parameter values, times and dates. Example: P28 = -6.
SECTION SIX - PARAMETRIC PROGRAMMING Miscellaneous Commands Spaces Spaces can be used anywhere within the program. For example, Z1.234 can be written as Z 1 . 23 4 if desired. Blocks Blocks without any information are allowed. Comments Comments are any text enclosed in parentheses and they are ignored by the control. Comments can be anywhere in a program or in a block.
SECTION SIX - PARAMETRIC PROGRAMMING #n[LT] #n[LT] displays parameter n with L leading digits and T trailing digits. Example: P100=1.235 P101=2.87656 PRINT [P100=#100[04] P101=#101[33]] shows “P100=1.2350 P101=002.877” If the leading and trailing fields are left blank, the default leading and trailing format for the machine setup parameters is used. When LT=0, exceptions apply. If LT=0, the ASCII value of the parameter is shown.
SECTION SIX - PARAMETRIC PROGRAMMING DPRNT DPRNT outputs text to a file or RS-232 port which is specified by the POPEN command. Example: DPRNT [PLEASE CLEAR THE WORK AREA] #n writes the value of a parameter Example: DPRNT [X#208 Y#209 Z#210] outputs the current X, Y,and Z positions to a file or an RS-232 port. #n[LT] will output parameter n with L leading and T trailing digits. Example: P100=1.235 P101=2.87656 DPRNT [P100=#100[04] P101=#101[33]] outputs “P100=1.2350 P101=002.
SECTION SIX - PARAMETRIC PROGRAMMING INPUT The INPUT statement is used for data input from the front panel. Example: INPUT (X START POSITION) P1 The operator will be prompted to input data. The operator can use the data displayed by pressing the ENTER key. If ESC is pressed during an input statement, the program will be terminated. The HDW command can be used to enter the handwheel mode during a program. A comment may be added to prompt the operator during the HDW command.
SECTION SIX - PARAMETRIC PROGRAMMING PULSE0 Pulses an output pin. Example 1: PULSE0 Z10 (clears Z output #10, delays for the number of milliseconds specified by the MISC parameter PULSEx pulse delay(ms) then sets output Z10) Example 2: PULSE0 X2 P3.5 (clears X output #2 and delays for 3.
SECTION SIX - PARAMETRIC PROGRAMMING out7 out8 out9 out10 out11 out12 1018 1019 1020 1021 1022 1023 2018 2019 2020 2021 2022 2023 3018 3019 3020 3021 3022 3023 4018 4019 4020 4021 4022 4023 5018 5019 5020 5021 5022 5023 Note: PIN statements can be used in conditional statements such as IF-THEN and WHILEWEND. Examples: IF PIN[2017] EQ 1 THEN PB50=1 WHILE PIN[1005] NE 0 M62 M63 WEND P5=P3 + PIN[2011] IPIN IPIN refers to an input pin. The argument is the input number. IPIN [32] is the 32nd input.
SECTION SIX - PARAMETRIC PROGRAMMING Back line The back line function may be used on any line command. This function reverses the direction of the programmed line. Back line is normally used when you know the end point of the line and not its starting point. The end point is programmed and the line is extended backward to the start point. When using this function all Trig Help functions are still valid. Example 1: X6 Y2 X5 X4 Y1.5 G2 R1 XC3 YC1.
SECTION SIX - PARAMETRIC PROGRAMMING MOD MOD is used to shift an axis position. It is generally used for rotary axis to obtain a positive position between 0 and 360 degrees. It can be useful after a rotary axis has made several revolutions in the same direction. Examples: G0 A750 MOD A360 (A axis position is now 30°) G0 A-100 MOD A360 (A axis position is now 240°) G0 A-500 MOD A360 (A axis position is now 220°) G0 A437 MOD A20 (A axis position is now 17°) G0 A33.285 MOD A2.1 (A axis position is now 1.
SECTION SIX - PARAMETRIC PROGRAMMING The following illustrates the parametric program for cutting five 45° segments of a fan blade. P2=0 N2 P1=.5 P140=.1 G31 N1 G0 X[P1] Y0 G1 Z0 G3 R[P1] AA0 AB45 Z[[.5-P1]/5] G31 P1=P1+.1 IF P1 LE 2 GOTO 1 P2=P2+72 G68 AA[P2] I0 J0 IF P2 LT 360 GOTO 2 In the above example, the tool makes sixteen passes for each blade starting at X.5 to X2 in .1" steps. Z is 0 on the entire front edge of the blade and drops to 0 on the first pass and to -.3" on the last pass.
SECTION SIX - PARAMETRIC PROGRAMMING Sample Program Using Some Special Statements (Outside digitizing program. Assumes the center is 0,0.) INPUT (Diameter) P1 INPUT (Z depth) P2 INPUT (Angle increment) P3 TI M6 (Probe) H43 H1 D1 G0 X [P1/2+.5] Y0 (Move past the diameter +.5) Z[P2] (To the Z depth) P81=7 (Set byte parameter special flags to shut off trig help and cutter compensation) POPEN P0 (Open file for output. Set report file to c:/parts/O0100.
SECTION SIX - PARAMETRIC PROGRAMMING . . . X1.0149Y-0.3694 X1.0301Y-0.3028 X1.0242Y-0.1806 X1.0560Y-0.0924 X1.13000Y-0.
SECTION SEVEN - SAMPLE PROGRAMS The following sample programs illustrate a variety of programming problems and show possible solutions to these problems using the Centurion 6 control. The program given for each sample part is by no means the only solution for that sample part. Each sample part discussion begins with a drawing of the part, and then it gives the standard EIA (G and M codes), followed by an EIA program explanation, and finally a conversational program of the sample part.
SECTION SEVEN - SAMPLE PROGRAMS EIA Program Sample 1 N1 N2 N3 N4 N5 N6 N7 N8 N9 N10 N11 N12 N13 N14 N15 N16 G0 G17 G20 G32 G40 G50 G69 G80 G90 T1 M6 X-1 Y-1 S3000 M03 G43 H1 Z.1 M08 G01 Z-.375 F5 G41 D1 X0 F25 Y3.5 X1.5 G3 R1 AA180 AB-45 G1 R.S AB45 G2 R1 XC5.9142 YC4.0858 AB0 G1 Y0 X-1 G40 Y-1 G0 Z.1 M9 M5 Explanation of EIA Program Sample 1 N1 Selects rapid, XY plane, inch, and Z to tool change position; cancels cutter compensation, scaling, rotation, and canned cycles; selects absolute dimensioning.
SECTION SEVEN - SAMPLE PROGRAMS N12 Line move to Y0 N13 Line move to X-1 Y0 N14 Turn off cutter compensation during move to X-1 Y-1 N15 Rapids Z to .
SECTION SEVEN - SAMPLE PROGRAMS Event 2 of 11 Tool Pierce - Start Mill Cycle Z Pierce Feedrate Return Point Clearance Final Z Depth 1st Z Depth Z Increment X Pierce Point Y Pierce Point Compensation [5 ] [Clearance] [.1 ] [-.375 ] [-.375 ] [1 ] X[0 ] Y[0 ] [Auto Left] Options [---] --------------------------------------------------Event 3 of 11 Mill Geometry - Line Feedrate Coordinates F[ ] [Cartesian] X axis Y axis Z axis X[ ] Y[3.
SECTION SEVEN - SAMPLE PROGRAMS Event 5 of 11 Mill Geometry - Arc Plane Feedrate Direction Center Arc Radius Start Angle End Point End Angle [XY] F[ ] [CCW] [Polar] R[1 ] AA[180 ] [Polar] AB[-45 ] Z[ ] End Option [---] --------------------------------------------------Event 6 of 11 Mill Geometry - Line Feedrate Coordinates Plane Type F[ ] [Polar] [XY] [Current] Length End Angle Z axis R[.
SECTION SEVEN - SAMPLE PROGRAMS Event 7 of 11 Mill Geometry - Arc Plane [XY] Feedrate Direction Center Arc Radius Arc Center F[ ] [CW] [Abs Center] R[1 ] XC[5.9142 ] YC[4.
SECTION SEVEN - SAMPLE PROGRAMS Event 10 of 11 Tool Retract End Mill Cycle Point on part after tool retract [Auto] --------------------------------------------------Event 11 of 11 End of Program Spindle off Coolant off Z to Toolchange [Yes] [Yes] [No] X Position (home relative) [ ] Y Position (home relative) [ ] --------------------------------------------------Sample 2A 353
SECTION SEVEN - SAMPLE PROGRAMS EIA Program Sample 2A N1 N2 N3 N4 N5 N6 N7 N8 N9 N10 N11 N12 N13 N14 T1 M6 G0 X-1 Y1 S3000 M3 G43 H1 Z.1 M8 G1 Z-.375 F5 G42 D1 X0 F25 Y-1.5 G3 XC1 YC-1.5 AB-45 R1 G2XC2.7071 YC-3.2071 AB-45 R1.4142 G3 XC4.4142 YC-1.5 AB0 R1 G1 Y0 X-1 G40 Y1 G0 Z.1 M9 M05 Explanation of EIA Program Sample 2A N1 Tool change #1 N2 Rapid position to X-1 Y1; turns spindle on CW (3000 rpm) N3 Calls tool #1's “H” offset and positions Z to .1; turns on coolant N4 Feeds Z-.
SECTION SEVEN - SAMPLE PROGRAMS N13 Rapid Z axis to .
SECTION SEVEN - SAMPLE PROGRAMS Event 2 of 10 Tool Pierce - Start Mill Cycle Z Pierce Feedrate Return Point Clearance Final Z Depth 1st Z Depth Z Increment [5 ] [Clearance] [.1 ] [-.375 ] [-.375 ] [1 ] X Pierce Point Y Pierce Point Compensation X[0 ] Y[0 ] [Auto Right] Options [---] --------------------------------------------------Event 3 of 10 Mill Geometry - Line Feedrate Coordinates F[ ] [Cartesian] X axis Y axis Z axis X[ ] Y[-1.
SECTION SEVEN - SAMPLE PROGRAMS Event 5 of 10 Mill Geometry - Arc Plane Feedrate Direction Center Arc Radius Arc Center End Point End Angle [XY] F[ ] [CW] [Abs Center] R[1.4142 ] XC[2.7071 ] YC[-3.197 ] [Polar] AB[-45 ] Z[ ] End Option [---] --------------------------------------------------Event 6 of 10 Mill Geometry - Arc Plane [XY] Feedrate F[ ] Direction [CCW] Center [Abs Center] Arc Radius R[1 ] Arc Center XC[4.4142 ] YC[-1.
SECTION SEVEN - SAMPLE PROGRAMS Event 8 of 10 Mill Geometry - Line Feedrate Coordinates F[ ] [Cartesian] X axis Y axis Z axis X[0 ] Y[ ] Z[ ] End [---] Extend Back [Off ] --------------------------------------------------Event 9 of 10 Tool Retract End Mill Cycle Point on part after tool retract [Auto] --------------------------------------------------Event 10 of 10 End of Program Spindle off Coolant off Z to Toolchange [Yes] [Yes] [No] X Position (home relative) [ ] Y Position (home relative) [ ] 3
SECTION SEVEN - SAMPLE PROGRAMS Sample 2B Same part as sample 2A but programmed using tangent arc function. EIA Program Sample 2B N1 N2 N3 N4 N5 N6 N7 N8 N9 N10 N11 N12 N13 N14 N15 N16 N17 N18 N19 N20 N21 N22 T1 M6 G0 X-1 Y1 S3000 M3 G43 H1 Z.1 M8 G1 Z-.375 F5 G42 D1 X0 F25 Y-1.5 P90 = 1 P91 = -1.5 P92 = 1 P93 = 4.4142 P94 = -1.5 P95 = 1 P96 = 1.4142 TANA C7 G3 XC1 YC-1.5 AB-45 R1 G2 XC[P84] YC[P85] R[P96] X[P82] Y[P83] G3 R1 XC4.4142 YC-1.5 AB0 G1 Y0 X-1 G40 Y1 G0 Z.
SECTION SEVEN - SAMPLE PROGRAMS Explanation of EIA Program Sample 2A N1 Tool change #1 N2 Rapid position to X-1 Y1; turns spindle on CW (3000 rpm) N3 Calls tool #1's "H" offset and positions Z to .1; turns on coolant N4 Feeds Z-.375 at 5 ipm N5 Selects right cutter compensation, calls tool #1's "D" offset, and moves to X0 at 25 ipm. Note: Cutter compensation will ramp on during this move. N6 Line move to X0 Y-1.
SECTION SEVEN - SAMPLE PROGRAMS Conversational Program Sample 2B Event 0 of 9 Program Setup Program name [SAMPLE 2B Dimensions Units Work Coordinate [Absolute] [English] [---] Setup Notes: [ ] [ ] [ ] [ ] [ ] [ ] --------------------------------------------------Event 1 of 9 Tool Change Tool Tool Change Position [Change] X[ ] Y[ ] Tool Number T[1 ] Tool Description [ ] Next Tool Number [] Spindle Speed S[3000] Spindle Restart [CW] Coolant [Flood] --------------------------------------------------- 36
SECTION SEVEN - SAMPLE PROGRAMS Event 2 of 9 Tool Pierce - Start Mill Cycle Z Pierce Feedrate Return Point Clearance Final Z Depth 1st Z Depth Z Increment X Pierce Point Y Pierce Point Compensation [5 ] [Clearance] [.1 ] [-.375 ] [-.375 ] [1 ] X[0 ] Y[0 ] [Auto Right] Options [---] --------------------------------------------------Event 3 of 9 Mill Geometry - Line Feedrate Coordinates F[25] [Cartesian] X axis Y axis Z axis X[ ] Y[-1.
SECTION SEVEN - SAMPLE PROGRAMS Event 4 of 9 Connect two arcs with tangent line or arc in the Plane [XY] Mill First arc in direction R1 XC1 YC1 [CCW] [1 ] [1 ] [-1.5 ] Second Arc for computation is: R2 [1 ] XC2 [4.4142 ] YC2 [-1.5 ] Exit 1st arc [Right] Enter 2nd arc Right] Connect with [an Arc] Center to the [Right] Radius [1.
SECTION SEVEN - SAMPLE PROGRAMS Event 6 of 9 Mill Geometry - Line Feedrate Coordinates F[ ] [Cartesian] X axis Y axis Z axis X[ ] Y[0 ] Z[ ] End [---] Extend Back [Off ] --------------------------------------------------Event 7 of 9 Mill Geometry - Line Feedrate Coordinates F[ ] [Cartesian] X axis Y axis Z axis X[0 ] Y[ ] Z[ ] End [---] Extend Back [Off ] --------------------------------------------------Event 8 of 9 Tool Retract End Mill Cycle Point on part after tool retract [Auto] -----------
SECTION SEVEN - SAMPLE PROGRAMS Sample 3A EIA Program Sample 3A N1 N2 N3 N4 N5 N6 N7 N8 N9 N10 N11 N12 N13 N14 N15 N16 N17 N18 T1 M6 G41 D1 S3000 M03 G65 X0 Y99 G0 Y0 G43 H1 Z.1 M8 G1 Z-.375 F5 X1 F25 G2 XC2 YC0 AB135 R1 G1 AB45 R.5 G2 XC4 YC2 X5 Y2 R1 G3 XC7 YC2 X9 R2 G1 Y5 X0 Y0 G65 X99 G40 G0 Z.
SECTION SEVEN - SAMPLE PROGRAMS N3 Sets a "point before pierce" of X0 Y99 Note: Machine does not move to this position. N4 Sets a "pierce point" of X0 Y0; moves to its compensated point as established by the previous block N5 Calls tool #1's "H" offset, positions Z to .1, and turns on coolant N6 Feeds Z-.375 at 5 ipm N7 Line move to X1 Y0 at 25 ipm N8 CW arc 1" radius using an XC2 YC0 and an end angle of AB135 N9 Line move using an estimated end point and described polarly, angle 45 radius .
SECTION SEVEN - SAMPLE PROGRAMS Conversational Program Sample 3A Event 0 of 12 Program Setup Program name Dimensions Units Work Coordinate [SAMPLE 3A [Absolute] [English] [---] Setup Notes: [ ] [ ] [ ] [ ] [ ] [ ] --------------------------------------------------Event 1 of 12 Tool Change Tool Tool Change Position [Change] X[ ] Y[ ] Tool Number T[1 ] Tool Description [ ] Next Tool Number [] Spindle Speed S[3000] Spindle Restart [CW] Coolant [Flood] --------------------------------------------------- 36
SECTION SEVEN - SAMPLE PROGRAMS Event 2 of 12 Tool Pierce - Start Mill Cycle Z Pierce Feedrate Return Point Clearance Final Z Depth 1st Z Depth Z Increment [5 ] [Clearance] [.1 ] [-.375 ] [-.
SECTION SEVEN - SAMPLE PROGRAMS Event 4 of 12 Mill Geometry - Arc Plane Feedrate Direction Center Arc Radius Start Angle End Point End Angle [XY] F[ ] [CW] [Polar] R[1 ] AA[180 ] [Polar] AB[135 ] Z[ ] End Option [---] --------------------------------------------------Event 5 of 12 Mill Geometry - Line Feedrate Coordinates Plane Type F[ ] [Polar] [XY] [Current] Length End Angle Z axis R[.
SECTION SEVEN - SAMPLE PROGRAMS Event 6 of 12 Mill Geometry - Arc Plane Feedrate Direction Center Arc Radius Arc Center [XY] F[ ] [CW] [Abs Center] R[1 ] XC[4 ] YC[2 ] [Absolute] X[5 ] Y[2 ] Z[ ] End Point End Option [---] --------------------------------------------------Event 7 of 12 Mill Geometry - Arc Plane [XY] Feedrate F[ ] Direction [CCW] Center [Abs Center] Arc Radius R[2 ] Arc Center XC[7 ] YC[2 ] End Point [Absolute] X[9 ] Y[ ] Z[ ] End Option [---] ---------------------------------------------
SECTION SEVEN - SAMPLE PROGRAMS Event 8 of 12 Mill Geometry - Line Feedrate Coordinates F[ ] [Cartesian] X axis Y axis Z axis X[ ] Y[5 ] Z[ ] End [---] Extend Back [Off ] --------------------------------------------------Event 9 of 12 Mill Geometry - Line Feedrate Coordinates X axis Y axis Z axis F[ ] [Cartesian] X[0 ] Y[ ] Z[ ] End [---] Extend Back [Off ] --------------------------------------------------Event 10 of 12 Mill Geometry - Line Feedrate Coordinates F[ ] [Cartesian] X axis Y axis Z
SECTION SEVEN - SAMPLE PROGRAMS Event 11 of 12 Tool Retract End Mill Cycle Point on part after tool retract [Cartesian] X[99 ] Y[0 ] --------------------------------------------------Event 12 of 12 End of Program Spindle off Coolant off Z to Toolchange [Yes] [Yes] [No] X Position (home relative) [ ] Y Position (home relative) [ ] 372
SECTION SEVEN - SAMPLE PROGRAMS Sample 3B Same part as sample 3A but programmed using tangent line function. EIA Program Sample 3B N1 N2 N3 N4 N5 N6 N7 N8 N9 N10 N11 N12 N13 N14 N15 N16 N17 N18 N19 N20 N21 N22 N23 N24 T1 M6 G41 D1 S3000 M3 G65 X0 Y99 G0 Y0 G43 H1 Z.1 M8 G1 Z-.375 F5 X1 F25 P90=2 P91=0 P92=1 P93=4 P94=2 P95=1 TANL C3 (See TANL explanation for values of C.) G2 XC[P90] YC[P91] R[P92] X[P80] Y[P81] G1 X[P82] Y[P83] G2 XC4 YC2 X5 Y2 R1 G3 XC7 YC2 X9 Y2 R2 G1 Y5 X0 Y0 G65 X99 G40 G0 Z.
SECTION SEVEN - SAMPLE PROGRAMS N25 M5 Note: Lines N8 thru N13 could be written as follows: N9 P90=2 P91=0 P92=1 P93=4 P94=2 P95=1 Explanation of EIA Program 3B N1 Tool change #1 N2 Selects left cutter compensation, activates tool #1's "D" offset, and turns on spindle CW (3000 rpm) N3 Sets a "point before pierce" of X0 Y99 Note: Machine does not move to this position.
SECTION SEVEN - SAMPLE PROGRAMS N21 Line move to X0 Y0 N22 Establishes a "point after pierce" of X99 Y0 Note: Machine does not move to this position. N23 Turns off cutter compensation N24 Rapids Z to .
SECTION SEVEN - SAMPLE PROGRAMS Event 2 of 11 Tool Pierce - Start Mill Cycle Z Pierce Feedrate Return Point Clearance Final Z Depth 1st Z Depth Z Increment [5 ] [Clearance] [.1 ] [-.375 ] [-.
SECTION SEVEN - SAMPLE PROGRAMS Event 4 of 11 Connect two arcs with tangent line or arc in the Plane [XY] Mill First arc in direction R1 XC1 YC1 [CW] [1 ] [2 ] [0 ] Second Arc for computation is: R2 [2 ] XC2 [4 ] YC2 [2 ] Exit 1st arc [Left] enter 2nd arc [Left] Connect with [a Line] --------------------------------------------------Event 5 of 11 Mill Geometry - Arc Plane [XY] Feedrate F[ ] Direction [CW] Center [Abs Center] Arc Radius R[1 ] Arc Center XC[4 ] YC[2 ] End Point [Absolute] X[5 ] Y[2 ] Z[ ]
SECTION SEVEN - SAMPLE PROGRAMS Event 6 of 11 Mill Geometry - Arc Plane Feedrate Direction Center Arc Radius Arc Center End Point [XY] F[ ] [CCW] [Abs Center] R[2 ] XC[7 ] YC[2 ] [Absolute] X[9 ] Y[ ] Z[ ] End Option [---] --------------------------------------------------Event 7 of 11 Mill Geometry - Line Feedrate Coordinates F[ ] [Cartesian] X axis Y axis Z axis X[ ] Y[5 ] Z[ ] End [---] Extend Back [Off ] --------------------------------------------------Event 8 of 11 Mill Geometry - Line Feedrat
SECTION SEVEN - SAMPLE PROGRAMS Event 9 of 11 Mill Geometry - Line Feedrate Coordinates F[ ] [Cartesian] X axis Y axis Z axis X[ ] Y[0 ] Z[ ] End [---] Extend Back [Off ] --------------------------------------------------Event 10 of 11 Tool Retract End Mill Cycle Point on part after tool retract [Cartesian] X[99 ] Y[0 ] --------------------------------------------------Event 11 of 11 End of Program Spindle off Coolant off Z to Toolchange [Yes] [Yes] [No] X Position (home relative) [ ] Y Position (ho
SECTION SEVEN - SAMPLE PROGRAMS Sample 4A N1 N2 N3 N4 N5 N6 N7 N8 N9 N10 N11 N12 N13 N14 N15 N16 EIA Program Sample 4A T1 M6 G41 D01 S3000 M3 G65 X99 Y0 G0 X0 G43 H1 Z.1 M8 G1 Z-.375 F5 Y-2 F25 G2 XC0 YC-3 AB-45 R1 G3 XC2.1213 YC-2.2929 AB-45 R2 G2 XC4.2426 YC-3 AB90 R1 G1 Y0 X0 G65 Y-99 G40 G0 Z.
SECTION SEVEN - SAMPLE PROGRAMS Explanation of EIA Program Sample 4A N1 Tool change #1 N2 Selects left cutter compensation, activates tool #1's "D" offset, and turns on spindle CW (3000 rpm) N3 Establishes a "point before pierce" of X99 Y0 Note: Machine does not move to this position. N4 Sets a "pierce point" of X0 Y0; moves to its compensated point as established by the previous block N5 Calls tool #1's "H" offset, positions Z to .1, and turns on coolant N6 Feeds Z-.
SECTION SEVEN - SAMPLE PROGRAMS Conversational Program Sample 4A Event 0 of 10 Program Setup Program name [SAMPLE 4A Dimensions Units Work Coordinate [Absolute] [English] [---] Setup Notes: [ ] [ ] [ ] [ ] [ ] [ ] --------------------------------------------------Event 1 of 10 Tool Change Tool Tool Change Position [Change] X[ ] Y[ ] Tool Number T[1 ] Tool Description [ ] Next Tool Number [] Spindle Speed S[3000] Spindle Restart [CW] Coolant [Flood] ---------------------------------------------------
SECTION SEVEN - SAMPLE PROGRAMS Event 2 of 10 Tool Pierce - Start Mill Cycle Z Pierce Feedrate Return Point Clearance Final Z Depth 1st Z Depth Z Increment [5 ] [Clearance] [.1 ] [-.375 ] [-.
SECTION SEVEN - SAMPLE PROGRAMS Event 4 of 10 Mill Geometry - Arc Plane Feedrate Direction Center Arc Radius Arc Center End Point End Angle [XY] F[ ] [CW] [Abs Center] R[1 ] XC[0 ] YC[-3 ] [Polar] AB[-45 ] Z[ ] End Option [---] --------------------------------------------------Event 5 of 10 Mill Geometry - Arc Plane [XY] Feedrate F[ ] Direction [CCW] Center [Abs Center] Arc Radius R[2 ] Arc Center XC[2.1213 ] YC[-2.
SECTION SEVEN - SAMPLE PROGRAMS Event 7 of 10 Mill Geometry - Line Feedrate Coordinates F[ ] [Cartesian] X axis Y axis Z axis X[ ] Y[0 ] Z[ ] End [---] Extend Back [Off ] --------------------------------------------------Event 8 of 10 Mill Geometry - Line Feedrate Coordinates F[ ] [Cartesian] X axis Y axis Z axis X[0 ] Y[ ] Z[ ] End [---] Extend Back [Off ] --------------------------------------------------Event 9 of 10 Tool Retract End Mill Cycle Point on part after tool retract [Cartesian] X[0
SECTION SEVEN - SAMPLE PROGRAMS Sample 4B Programming arc using 3 point circle generate. Points X1, X2, X3 are the points used to program each arc. EIA Program Sample 4B N1 N2 N3 N4 N5 N6 N7 N8 N9 N10 N11 N12 N13 N14 N15 N16 N17 N18 T1 M6 G41 D1 S3000 M03 G65 X99 Y0 X0 G43 H1 Z.1 M8 G1 Z-.375 F5 Y-2 F25 P90=0 P91=-2 P92=1 P93=-3 P94=0 P95=-4 CGEN G2 XC[P80] YC[P81] R[P82] AB300 P90=.1213 P91=-2.2929 P92=2.
SECTION SEVEN - SAMPLE PROGRAMS N19 N20 N21 N22 N23 N24 N25 N26 N27 N28 N29 N30 N31 N32 N33 N34 N35 N36 N37 P93=-4.2929 P94=4.1213 P95=-2.2929 CGEN G3 XC[P80] YC[P81] R[P82] AB300 P90=4.2426 P91=-4 P92=3.2426 P93=-3 P94=4.2426 P95=-2 CGEN G2 XC[P80] YC[P81] R[P82] X[P94] Y[P95] G1 Y0 X0 G65 Y-99 G40 G0 Z.
SECTION SEVEN - SAMPLE PROGRAMS N16- Are the coordinates of 3 points on the second circle N21 N22 Calculates second circle based on the 3 points N23 Arc command which moves to the calculated points N24- Are the coordinates of 3 points on the third circle N29 N30 Calculates third circle based on the 3 points N31 Arc command which moves to the calculated points N32 Line move to X4.
SECTION SEVEN - SAMPLE PROGRAMS Event 1 of 10 Tool Change Tool [Change] Tool Change Position X[ ] Y[ ] Tool Number T[1 ] Tool Description [ ] Next Tool Number [] Spindle Speed S[3000] Spindle Restart [CW] Coolant [Flood] --------------------------------------------------Event 2 of 10 Tool Pierce - Start Mill Cycle Z Pierce Feedrate Return Point Clearance Final Z Depth 1st Z Depth Z Increment [5 ] [Clearance] [.1 ] [-.375 ] [-.
SECTION SEVEN - SAMPLE PROGRAMS Event 3 of 10 Mill Geometry - Line Feedrate Coordinates F[25 ] [Cartesian] X axis Y axis Z axis X[ ] Y[-2 ] Z[ ] End [---] Extend Back [Off ] --------------------------------------------------Event 4 of 10 Three Point Circle Generator Plane [XY] Direction [CW] X1 [0 ] Y1 [-2 ] X2 [1 ] Y2 [-3 ] X3 [0 ] Y3 [-4 ] Use X3,Y3 as End Point [No] End Angle [300 ] --------------------------------------------------Event 5 of 10 Three Point Circle Generator Plane [XY] Direction [CC
SECTION SEVEN - SAMPLE PROGRAMS Event 7 of 10 Mill Geometry - Line Feedrate Coordinates F[ ] [Cartesian] X axis Y axis Z axis X[ ] Y[0 ] Z[ ] End [---] Extend Back [Off ] --------------------------------------------------Event 8 of 10 Mill Geometry - Line Feedrate Coordinates F[ ] [Cartesian] X axis Y axis Z axis X[0 ] Y[ ] Z[ ] End [---] Extend Back [Off ] --------------------------------------------------Event 9 of 10 Tool Retract End Mill Cycle Point on part after tool retract [Cartesian] X[0
SECTION SEVEN - SAMPLE PROGRAMS Sample 5 EIA Program Sample 5 N1 N2 N3 N4 N5 N6 N7 N8 N9 N10 N11 N12 N13 N14 N15 T1 M6 G42 D1 S3000 M03 G65 X99 Y0 G0 X0 G43 H1 Z.1 M8 G1 Z-.375 F5 Y2 F25 G2 XC2 YC2 AB45 R2,R.0001 X5 YC2 AB0 R2 G1 Y0 X0 G65 Y99 G40 G0 Z.1 M9 M5 Explanation of EIA Program 5 N1 Tool change #1 N2 Selects right cutter compensation, calls tool #1's "D" offset, and turns on spindle CW (3000 rpm) N3 Establishes a "point before pierce" of X99 Y0 Note: Machine does not move to this position.
SECTION SEVEN - SAMPLE PROGRAMS N4 Sets a "pierce point" of X0 Y0; moves to its compensated point as established by the previous block N5 Calls tool #1's "H" offset, positions Z to .1, and turns on coolant N6 Feeds Z-.375 at 5 ipm N7 Line move to X0 Y2 at 25 ipm N8 CW arc 2" radius using an XC2 YC2, an estimated end angle of 45° degrees, and an end option (round corner) of .0001" radius Note: The end option of a .0001 radius forces an intersection between the arcs.
SECTION SEVEN - SAMPLE PROGRAMS Event 1 of 9 Tool Change Tool Tool Change Position [Change] X[ ] Y[ ] Tool Number T[1 ] Tool Description [ ] Next Tool Number [] Spindle Speed S[3000] Spindle Restart [CW] Coolant [Flood] --------------------------------------------------Event 2 of 9 Tool Pierce - Start Mill Cycle Z Pierce Feedrate Return Point Clearance Final Z Depth 1st Z Depth Z Increment [5 ] [Clearance] [.1 ] [-.375 ] [-.
SECTION SEVEN - SAMPLE PROGRAMS Event 3 of 9 Mill Geometry - Line Feedrate Coordinates F[25 ] [Cartesian] X axis Y axis Z axis X[ ] Y[2 ] Z[ ] End [---] Extend Back [Off ] --------------------------------------------------Event 4 of 9 Mill Geometry - Arc Plane [XY] Feedrate F[ ] Direction [CW] Center [Abs Center] Arc Radius R[2 ] Arc Center XC[2 ] YC[2 ] End Point [Polar] End Angle AB[45 ] Z[ ] End Option [Round Corner] Radius [.
SECTION SEVEN - SAMPLE PROGRAMS Event 6 of 9 Mill Geometry - Line Feedrate Coordinates F[ ] [Cartesian] X axis Y axis Z axis X[ ] Y[0 ] Z[ ] End [---] Extend Back [Off ] --------------------------------------------------Event 7 of 9 Mill Geometry - Line Feedrate Coordinates F[ ] [Cartesian] X axis Y axis Z axis X[0 ] Y[ ] Z[ ] End [---] Extend Back [Off ] --------------------------------------------------Event 8 of 9 Tool Retract End Mill Cycle Point on part after tool retract [Cartesian] X[0 ]
SECTION SEVEN - SAMPLE PROGRAMS Sample 6 EIA Program Sample 6 N1 N2 N3 N4 N5 N6 N7 N8 N9 N10 N11 N12 N13 N14 N15 N16 N17 N18 T1 M6 G42 D1 S3000 M3 G65 X0 Y0 X.5 Y1.5 G43 H1 Z.1 M8 G1 Z-.375 F5 X1 Y3 F25 X0 G3 XC-1.2689 YC2.2 X-3 R1.5 G1 X-4 X-6.1 Y.5 Y0 X0 X.5 Y1.5 G65 X1 Y3 G40 G0 Z.
SECTION SEVEN - SAMPLE PROGRAMS N3 Establishes a "point before pierce" of X0 Y0 Note: Machine does not move to this position. N4 Establishes a "pierce point" of X.5 Y1.5; moves to its compensated point as established by the previous block N5 Calls tool #1's "H" offset, positions Z to .1, and turns coolant on N6 Feeds Z-.375 at 5 ipm N7 Line move to X1 Y3 at 25 ipm N8 Line move to an estimated end point of X0 N9 CCW arc 1.5" radius using an XC-1.2689 YC2.
SECTION SEVEN - SAMPLE PROGRAMS Conversational Program Sample 6 Event 0 of 11 Program Setup Program name [SAMPLE 6 Dimensions Units Work Coordinate [Absolute] [English] [---] Setup Notes: [ ] [ ] [ ] [ ] [ ] [ ] --------------------------------------------------Event 1 of 12 Tool Change Tool Tool Change Position [Change] X[ ] Y[ ] Tool Number T[1 ] Tool Description [ ] Next Tool Number [] Spindle Speed S[3000] Spindle Restart [CW] Coolant [Flood] --------------------------------------------------- 39
SECTION SEVEN - SAMPLE PROGRAMS Event 2 of 12 Tool Pierce - Start Mill Cycle Z Pierce Feedrate Return Point Clearance Final Z Depth 1st Z Depth Z Increment [5 ] [Clearance] [.1 ] [-.375 ] [-.375 ] [1 ] X Pierce Point Y Pierce Point Compensation X[.5 ] Y[1.
SECTION SEVEN - SAMPLE PROGRAMS Event 5 of 12 Mill Geometry - Arc Plane Feedrate Direction Center Arc Radius Arc Center End Point [XY] F[ ] [CCW] [Abs Center] R[1.5 ] XC[-1.2689 ] YC[2.
SECTION SEVEN - SAMPLE PROGRAMS Event 8 of 12 Mill Geometry - Line Feedrate Coordinates F[ ] [Cartesian] X axis Y axis Z axis X[ ] Y[0 ] Z[ ] End [---] Extend Back [Off ] --------------------------------------------------Event 9 of 12 Mill Geometry - Line Feedrate Coordinates F[ ] [Cartesian] X axis Y axis Z axis X[.5 ] Y[1.
SECTION SEVEN - SAMPLE PROGRAMS --------------------------------------------------Event 11 of 12 Tool Retract End Mill Cycle Point on part after tool retract [Auto] --------------------------------------------------Event 12 of 12 End of Program Spindle off Coolant off Z to Toolchange [Yes] [Yes] [No] X Position (home relative) [ ] Y Position (home relative) [ ] 403
SECTION SEVEN - SAMPLE PROGRAMS Sample 7 This sample program uses the rotary axis. The "A" axis is programmed in decimal degrees in XXX.XXX format and performs linear interpolation with the X, Y, and Z axes. The feedrate for the rotary axis is specified in degrees per minute divided by 10. Example: G1 A90 F18.0 In the above example, A will feed to 90° at a rate of 180 DPM (degrees per minute). Example of Rotary Axis Programming Sample 7 03119 G20 G90 N1 G0 Z.1 N2 X0 Y0 A0 N3 G1 F20 Z-.
APPENDIX Error Messages 001 Invalid function number Note what just occurred and call for technical support. A call was made to a nonexistent DOS function. 002 File not found File name specified as OLD does not exist. Try MENU. 003 Path not found The drive or subdirectory specified does not exist. 004 Too many open files Check Config.sys for FILES=20. 005 File access denied The file may be read only or is on a write-protected disk.
APPENDIX 100 Disk read error An attempt was made to edit a file that has been corrupted in some way, perhaps loss of power while editing, or an error 101 occurred while editing. Try a different file to see if the problem is specific to one particular file. If this is the case, the program must be recreated. Note: This error occurs when trying to edit conversational files that were created with SLS software.
APPENDIX 150 Disk is write-protected Check the write protect tab on the floppy disk that is being used. 151 Unknown unit 152 Drive not ready Check to see that there is a disk in the floppy drive. 153 Unknown command 154 CRC error in data The disk being read is corrupted. 155 Bad drive request structure length 156 Disk seek error Check the cabling from the control to the floppy drive.
APPENDIX Steps to take to avoid ERROR 203 (Heap overflow: Insufficient RAM memory) If text cycles or canned cycles are being loaded and not being used, turn them off. See PARMS-SETUP-MISC. 1) (F7) PARMS 2) (F9) CTRL 3) Move cursor to Load Text Cycles 4) Toggle to "No" 5) (ESC) 6) (ESC) to the main menu. 7) Power the machine OFF, then ON, again. If you are running a large program, try running it through the RS-232 RUN mode.
APPENDIX This error may occur anytime a menu is being created for file selection when there are no files. There may be an unformatted disk in the floppy drive. Parts memory may be empty. 303 Problem saving program(s) to disk There is no floppy disk in the disk drive. The floppy disk may not have room to store additional files. There may be an unformatted disk in the drive. 304 Problem loading program(s) from disk Disk was removed from floppy drive after setting files.
APPENDIX the floppy disk and the floppy path changed to save files to the sub-directory. This allows full use of the disk space. 316 Not enough storage to create a new file There is not enough parts space to create a new conversational program. Erase unnecessary programs to free up parts space. 317 Simulator allows only 15 events 319 Send file aborted 320 Invalid PLC program. One of the ACRO.HEX (or NCB.HEX) files in the RAM directory is corrupt. 321 Error in program O.
APPENDIX 407 408 409 410 411 412 X axis excess error condition Y axis excess error condition Z axis excess error condition A axis excess error condition B axis excess error condition C axis excess error condition These errors are caused by the axis not being able to keep up with the programmed move at the programmed speed. Does the error occur during rapid moves only? Y__ N__ If so, check bus voltage and rapid feed parameters.
APPENDIX 453 Tool pot not up during turret movement Check to see if the POT UP switch is functioning as it should be. 454 Not at tool change position Try commanding a G32 before the M6 command. 455 ATC arm is not out, axis movement not allowed 456 Can't process auto tool change after switching to manual 457 Move length too great for control (split into smaller moves) 458 X axis is in the manual mode. Push reset to enable it 459 Y axis is in the manual mode.
APPENDIX 517 Parameter out of range Parameter number is less than zero. For parameter numbers greater than 699 you must use data mode (G10, G11). 518 Illegal program statement Command in program statement is not considered valid. 519 Feedrate out of range The programmed feedrate is beyond the "maximum feedrate" parameter value in the machine setup parameters. The program feedrate may be negative.
APPENDIX 533 Colinear arc to arc in round corner 535 Chamfer length is < 0 Chamfer length must be a positive number. 536 Can't chamfer and round the same corner Choose either chamfer or round corner. 537 Can't chamfer to or from arcs 538 Loop counter out of range The maximum number of loops for a call is 999. 539 Dwell time out of range Probably a negative number was specified. The maximum dwell time is 999999999 seconds. 540 Illegal dwell time "#" encountered Try G4 F##.
APPENDIX 550 Bad numeric format Expecting a numeric value, or a parameter value enclosed within [ ], after an address X, Y, Z, R, etc. 551 Multiple decimal points Multiple decimal points were detected within one numeric value. 552 Missing "]" Always use square brackets in pairs. 553 Missing "[" Always use square brackets in pairs. 554 Tangent function overflow Trying to find the tangent of a number close to 90Ε 555 Missing "/" Arctan "ATAN" syntax is P## = ATAN[#/#].
APPENDIX 573 Round wall is not in a Start/End mill cycle -WHILE WEND loopUse START at the beginning of the mill cycle and END at the end of the mill cycle. 574 Round wall radius will not span 1st Z depth and final Z depth 575 Tapered wall is not in a Start/End mill cycle -WHILE WEND loopUse START at the beginning of the mill cycle and END at the end of the mill cycle.
APPENDIX 605 Can't modify dry run status while program is running Program must be halted before changing dry run status. Try HALT-DRY-RESUME. 606 Program N#### is empty Text program being run or verified is empty. Try editing and reposting the conversational file. 607 Can't exit DNC run mode while program is running The DNC mode must be halted before exiting.
APPENDIX 805 Invalid probe setup Input file does not start with a comment containing three asterisks. Also, the following three blocks should be X, Y, Z, or Y, X, Z depending on scan plane. 806 Scan origin expected Multiple pick segment started without defining the start of the scans within that segment. 807 Probe file not found Could not find the selected input file. 808 Setup not selected Tried to probe without selecting both the input file and the output mode from the probe setup screen.
APPENDIX 953 Obsolete bit access for ncb controller. 954 Control not detected. 955 Interface not detected.
APPENDIX 072 073 075 076 077 078 079 080 081 082 083 085 086 087 088 089 090 091 092 093 094 096 097 099 100-109 110-119 120-129 130-145 146 160-175 190 192 193 194 195 196 197 198 199 200 201 202 203 204 206 209 Spindle on in Dry Run Tool Table Diameters\Radius Load Engraving Cycles Load Canned Cycles Check Spindle up to Speed Check Spindle Zero Speed G18 is ZX or XZ plane Cad Type DXF or CDL Special Flags Offset Round and Tapered Walls Full Dos File Names Primary Serial Port COM1 Baud Rate; COM1 Data/Sto
APPENDIX 212 213 214 215 218 219 220 221 222 223 227 228 229 230 231 232 233 234 275-291 294 295 296 298 320-335 338-353 354-369 370 371 374 375 376-391 392 396 397 398 399 400 404 530 532 533 534 535 536 537 541 Second Hand-Wheel Axis Probe Axis Probe Input Cranking Factor (for hand-wheeling thru a program) Serial Key board European Code Door Open Axis Door Open Input Door Over-Ride Axis Door Over-Ride Input End of Cycle Axis = 227; End of Cycle Output = 228; Yaskawa Axis Drives Third Hand-Wheel Axis Inve
APPENDIX 542 543 544 Yaskawa M5 drive Machine State 0=Nothing 1=Verifying 2=Program Running Check Spindle in Gear Real Parameters Great care must be taken when writing to any parameters other than the User Parameters P00-P99.
APPENDIX P211 P212 P213 P214 P215 P216 P217 P218 P219 P220 P221 P222 P223 P224 P225 P226 P227 P228 P229 P230 P231 P232 P233 P234 P235 P236 P237 P238 P239 P240 P241 P242 P243 P244 P245 P246 P247 P248 P149 P250 P251 P252 P253 P254 P255 P256 Current position (A) Current position (B) Current pos. opt. axis Current pos. opt. axis Current pos. opt. axis Previous machine (X) Previous machine (Y) Previous machine (Z) Previous machine (A) Previous mach. opt. axis Previous mach. opt. axis Previous mach. opt.
APPENDIX P316 P317 P318 P319 P320 P321 P322 P323 P324 P325 P326 P327 P328 P329 P330 Scale Rotate Mirror Work system Primary Secondary Tertiary Return plane Tapping Custom code Custom M-code Custom G-code Feed per Rev (wait for marker) Feedrate override Lock Spindle override Lock P331P334 Unassigned P335 Hard Tap Fudge Factor P336P343 Unassigned P344 P345 P346 P347 Inverse Time Feedrate Bore Type G76 Orient Bore Angle G76 Orient Bore Distance P348P349 Unassigned P350P361 Used in tool setting sof
APPENDIX P440 P441 P442 P443 P444 P445 P446 P447 P448 P449 P450 P451 P452 P453 P454 P455 P456 P457 P458 P459 P460 P461 P462 P463 P464 P465 P466 Work coordinate 5 (B) Work coord. 5 opt. axis Work coordinate 6 (X) Work coordinate 6 (Y) Work coordinate 6 (Z) Work coordinate 6 (A) Work coordinate 6 (B) Work coord. 6 opt. axis Tool change offset (X) Tool change offset (Y) Tool change offset (Z) Tool change offset (A) Tool change offset (B) Tool chg. offset opt.
APPENDIX P850 P851 P852 P853 P854 P855 ADC Sample ADC Scale ADC Value ADC Trigger Tapping Ramp High Gear Spindle Encoder PPU2 P856P892 Unassigned P893 P894 P895 P896 P897 P898 P899 Soft Start Delay Clamped Feedrate Cranking Max ipm Handwheel Encoder PPU Cranking Minutes Per Turn Screen Blank Time Digitizing Enable P900P962 Unassigned P963 P964 P965 Max Corner Deviation Unassigned SpindleScale (fraction of full spindle dac) Minimum Block Time (seconds, min time when not in fast DNC) Unassigned Minim
APPENDIX P1043 P1044 P1045 P1046 G30 reference point 2 (X) G30 reference point 3 (X) G30 reference point 4 (X) Max Handwheel Error (X) P1556- Tool Slots for swing arm style tool P1595 changers P1596- Unassigned P1598 P1047- Unassigned (X) P1048 P1599 P1049 P1050 P1051 P1052 P1053 P1054 P1055 P1056 Feed Back (X) Invert Handwheel (X) (non-zero = invert handwheel direction) Gain Proportional (X) Gain Velocty (X) Gain Acceleration (X) Gain Handwheel (X) Feed S-Curve Acc\Dec (X) Rapid S-Curve Acc\Dec (X) P
