User’s Manual MANUALplus 4110 NC Software 526 488-xx English (en) 9/2007
MANUALplus 4110, Software and Functions This manual describes functions that are available in MANUALplus 4110 controls with NC software numbers 507 807-xx and 526 488-xx. The machine manufacturer adapts the features offered by the control to the capabilities of the specific machine tool by setting machine parameters. Therefore, some of the functions described in this manual may not be among the features provided by the MANUALplus on your machine tool.
Contents 1 2 3 4 5 6 7 8 9 10 Introduction and Fundamentals Basics of Operation Machine Mode of Operation Cycle Programming ICP Programming DIN Programming Tool Management Mode Organization Mode of Operation Examples Tables and Overviews HEIDENHAIN MANUALplus 4110 3
1 Introduction and Fundamentals 19 1.1 The MANUALplus ..... 20 The C axis ..... 20 1.2 Features ..... 21 1.3 MANUALplus Design ..... 22 Lathe design ..... 22 Machine operating panel ..... 24 1.4 Axis Designations and Coordinate System ..... 25 Axis designations ..... 25 Coordinate system ..... 25 Absolute coordinates ..... 26 Incremental coordinates ..... 26 Polar coordinates ..... 26 1.5 Machine Reference Points ..... 27 Machine zero point ..... 27 Workpiece zero point ..... 27 Reference points ..... 27 1.
2 Basics of Operation 31 2.1 The MANUALplus Screen ..... 32 2.2 Operation and Data Input ..... 33 Modes of operation ..... 33 Menu selection ..... 33 Soft keys ..... 33 Data input ..... 34 List operations ..... 34 Alphanumeric keyboard ..... 35 2.3 Error Messages ..... 36 Direct error messages ..... 36 Error display ..... 36 Clearing an error message ..... 37 System error, internal error ..... 37 PLC error, PLC status display ..... 37 Warnings during simulation ..... 38 2.4 Explanation of Terms .....
3 Machine Mode of Operation 41 3.1 Machine Mode of Operation ..... 42 3.2 Switch-On / Switch-Off ..... 43 Switch-on ..... 43 Traversing the reference marks ..... 43 Monitoring EnDat encoders ..... 44 Switch-off ..... 45 3.3 Machine Data ..... 46 Input and display of machine data ..... 46 Tool call ..... 47 Tools in different quadrants ..... 48 Feed rate ..... 48 Spindle ..... 49 3.4 Machine Setup ..... 50 Defining the workpiece zero point ..... 50 Setting the protection zone .....
3.9 Graphic Simulation ..... 68 Views ..... 70 Graphic elements ..... 71 Warnings ..... 72 Magnify / Reduce ..... 73 3.10 Time Calculation ..... 74 3.11 Program Management ..... 75 Program information ..... 75 Functions for program management ..... 76 3.12 Conversion into DIN Format ..... 77 3.13 Inch Mode ..... 78 4 Cycle Programming 79 4.1 Working with Cycles ..... 80 Starting point of cycles ..... 80 Cycle transitions ..... 80 DIN macros ..... 81 Graphical test run (simulation) ..... 81 Cycle keys .....
4.4 Roughing Cycles ..... 98 Roughing, longitudinal/transverse ..... 101 Roughing, longitudinal/transverse—Expanded ..... 103 Finishing cut, longitudinal/transverse ..... 105 Finishing cut, longitudinal/transverse—Expanded ..... 107 Plunge longitudinal/transverse ..... 109 Plunge, longitudinal/transverse—Expanded ..... 111 Finishing plunge, longitudinal/transverse ..... 113 Finishing plunge, longitudinal/transverse—Expanded ..... 115 ICP contour-parallel, longitudinal/transverse .....
4.6 Thread and Undercut Cycles ..... 162 Thread cycle (longitudinal) ..... 165 Thread cycle (longitudinal)—Expanded ..... 166 Tapered thread ..... 168 API thread ..... 170 Recut (longitudinal) thread ..... 172 Recut (longitudinal) thread—Expanded ..... 174 Recut tapered thread ..... 176 Recut API thread ..... 178 Undercut DIN 76 ..... 180 Undercut DIN 509 E ..... 182 Undercut DIN 509 F ..... 184 Examples of thread and undercut cycles ..... 186 4.7 Drilling Cycles ..... 190 Drilling, axial/radial .....
5 ICP Programming 241 5.1 ICP Contours ..... 242 5.2 Editing ICP Contours ..... 243 Programming and adding to ICP contours ..... 244 Absolute or incremental dimensions ..... 244 Transitions between contour elements ..... 245 Contour graphics ..... 246 Changing the ICP contour graphics ..... 247 Selection of solutions ..... 248 Contour direction ..... 249 5.3 Importing of DXF Contours ..... 250 Fundamentals ..... 250 DXF import ..... 251 Configuring the DXF import ..... 252 5.
6 DIN Programming 277 6.1 DIN Programming ..... 278 Program and block structure ..... 279 6.2 Editing DIN Programs ..... 281 Block functions ..... 281 Word functions ..... 283 Address parameters ..... 283 Comments ..... 284 Block functions ..... 285 Menu structure ..... 286 Programming G functions ..... 287 6.3 Definition of Workpiece Blank ..... 288 Chuck part, cylinder/tube G20 ..... 288 Workpiece blank contour G21 ..... 289 6.4 Tool Positioning without Machining ..... 290 Rapid traverse G0 .....
6.10 Oversizes ..... 308 Axis-parallel oversize G57 ..... 308 Contour-parallel oversize (equidistant) G58 ..... 309 6.11 Contour-Based Turning Cycles ..... 310 Contour definition ..... 310 End of cycle G80 ..... 310 Longitudinal contour roughing G817/G818 ..... 311 Longitudinal contour roughing with recessing G819 ..... 313 Transverse contour roughing G827/G828 ..... 314 Transverse contour roughing with recessing G829 ..... 316 Contour-parallel roughing G836 ..... 317 Contour finishing G89 ..... 318 6.
6.16 Undercut Cycles ..... 344 Undercut contour G25 ..... 344 Undercut cycle G85 ..... 345 Undercut according to DIN 509 E with cylinder machining G851 ..... 347 Undercut according to DIN 509 F with cylinder machining G852 ..... 348 Undercut according to DIN 76 with cylinder machining G853 ..... 349 Undercut type U G856 ..... 350 Undercut type H G857 ..... 351 Undercut type K G858 ..... 352 6.17 Parting Cycle ..... 353 Parting cycle G859 ..... 353 6.18 Drilling Cycles ..... 354 Drilling cycle G71 .....
6.22 Pattern Machining ..... 383 Linear pattern, face G743 ..... 383 Circular pattern, face G745 ..... 385 Linear pattern, lateral surface G744 ..... 387 Circular pattern, lateral surface G746 ..... 389 6.23 Other G Functions ..... 391 Period of dwell G4 ..... 391 Precision stop G9 ..... 391 Deactivate protection zone G60 ..... 391 Wait for moment G204 ..... 391 6.24 Set T, S, F ..... 392 Tool number, spindle speed /cutting speed and feed rate ..... 392 6.25 Data Input and Data Output ..... 393 INPUT .....
7 Tool Management Mode 411 7.1 Tool Management Mode of Operation ..... 412 Tool types ..... 412 Tool life management ..... 413 7.2 Tool Organization ..... 414 7.3 Tool Texts ..... 416 7.4 Tool Data ..... 418 Tool orientation ..... 418 Reference point ..... 418 Editing tool data ..... 418 Lathe tools ..... 419 Recessing and recess-turning tools ..... 421 Thread-cutting tools ..... 422 Drilling tools ..... 423 Tapping tools ..... 424 Milling tools ..... 425 7.5 Tool Data—Supplementary Parameters .....
8 Organization Mode of Operation 429 8.1 Organization Mode of Operation ..... 430 8.2 Parameters ..... 431 Current parameters ..... 432 Configuration parameters ..... 435 8.3 Transfer ..... 441 Data backup ..... 441 Data exchange with DataPilot 4110 ..... 441 Printer ..... 441 Interfaces ..... 442 Basics of data transfer ..... 442 Configuring for data transfer ..... 444 Transferring programs (files) ..... 446 8.4 Service and Diagnosis ..... 453 Access authorization ..... 453 System service .....
Introduction and Fundamentals
1.1 The MANUALplus 1.1 The MANUALplus The MANUALplus control combines modern control and drive technology with the functional features of a hand-operated machine tool. You can run simple machining operations, such as turning or facing, on MANUALplus just like on any conventional lathe. The axes are moved as usual by handwheel or joystick. For machining difficult contours, such as tapers, radii, chamfers, undercuts or threads, MANUALplus offers fixed cycles.
1.2 Features 1.2 Features The functions of the MANUALplus are grouped into operating modes: Machine mode of operation This operating mode includes all functions for machine setup, workpiece machining, and cycle and DIN program definition. The cycle programming functions are available in both manual and automatic modes. You can program cycles for roughing, recessing, thread-cutting and drilling operations.
1.3 MANUALplus Design 1.3 MANUALplus Design The dialog between machinist and control takes place via: Screen Soft keys Data input keypad Machine operating panel The entered data can be displayed and checked on the screen. With the function keys directly below the screen, you can select functions, capture position values, confirm entries, and a lot more. With the information key (also found beneath the screen), you can call error and PLC information and activate the PLC diagnostic function.
Symbol Data input keypad Menu Call the main menu. ENTER Confirm the entered value. Process Select a new mode of operation. Store Conclude data input and transfer values. Backspace Delete the character to the left of the cursor. Arrow keys Switching key Switch between help graphics for internal/external machining. Clear Delete error messages. Numbers (0 to 9) For entering values and selecting soft keys. Symbol Move the cursor in the indicated direction by one position (character, field, line, etc.
1.3 MANUALplus Design Machine operating panel The machine operating panel is interfaced to the lathe by the machine tool builder. The controls on your machine may deviate slightly from those shown in the illustration. Your machine documentation provides more detailed information. 8 Controls and displays 10 1 2 3 4 5 6 7 24 Handwheel resolution Set the handwheel resolution to 1/10 mm, 1/100 mm or 1/ 1000 mm per graduation mark—or to other resolutions defined by the machine tool builder.
1.4 Axis Designations and Coordinate System 1.4 Axis Designations and Coordinate System Axis designations The cross slide is referred to as the X axis and the saddle as the Z axis (see figure at top right). All X-axis values that are displayed or entered are regarded as diameters. When programming paths of traverse, remember to: Program a positive value to depart the workpiece. Program a negative value to approach the workpiece.
1.4 Axis Designations and Coordinate System Absolute coordinates If the coordinates of a position are referenced to the workpiece zero point, they are referred to as absolute coordinates. Each position on a workpiece is clearly defined by its absolute coordinates (see figure at upper right). Incremental coordinates Incremental coordinates are always referenced to the last programmed position. They specify the distance from the last active position and the subsequent position.
1.5 Machine Reference Points 1.5 Machine Reference Points Machine zero point The point of intersection of the X and Z axes is called the "machine zero point." On a lathe, the machine zero point is usually the point of intersection of the spindle axis and the spindle surface. The machine zero point is designated with the letter "M" (see figure at upper right). Workpiece zero point For machining a workpiece, it is easier to reference all input data to a zero point located on the workpiece.
1.6 Tool Dimensions 1.6 Tool Dimensions MANUALplus requires data on the specific tools for a variety of tasks, such as positioning the axes, calculating cutting radius compensation or proportioning of cuts. Tool length All position values that are programmed and displayed are referenced to the distance between the tool tip and workpiece zero point.
1.6 Tool Dimensions Milling cutter radius compensation (MCRC) In milling operations, the outside diameter of the milling cutter determines the contour. When the MCRC function is not active, the system defines the center of the cutter as reference point. The MCRC function compensates for this error by calculating a new path of traverse, the equidistant line.
Basics of Operation
2.1 The MANUALplus Screen 2.1 The MANUALplus Screen MANUALplus shows the data to be displayed in windows. Some windows only appear when they are needed, for example, for typing in entries. In addition, MANUALplus shows the type of operation and the soft-key display on the screen. Each function that appears in a field of the soft-key row is activated by pressing the soft key directly below it. Screen windows displayed Machine window Position display, display of machine data, machine status, etc.
2.2 Operation and Data Input 2.2 Operation and Data Input Modes of operation The active mode of operation is highlighted. MANUALplus differentiates between the following operating modes: Machine—with the submodes: Manual mode (display: "Machine") Teach-in Program run Tool administration (tool management) Organization You can switch between the different operating modes using the Process key. Press the Process key once to activate the operatingmode bar.
2.2 Operation and Data Input Data input Input windows comprise several input fields. You can move the cursor to the desired input field with the vertical arrow keys. The function of the selected field is shown in the bottom line of the window. Place the highlight on the desired input field and enter the data. Existing data are overwritten. With the horizontal arrow keys, you can move the cursor within the input field and place it on the position where you want to delete, copy or add characters.
2.2 Operation and Data Input Alphanumeric keyboard Program descriptions, tool descriptions, comments, etc. are entered with the on-screen alphanumeric keyboard. You select the desired character with the arrow keys and confirm the character with ENTER. You can switch between upper and lower case letters with the SHIFT button. To edit existing texts, place the cursor on the desired position: Press the Up arrow key repeatedly until the cursor reaches the input line.
2.3 Error Messages 2.3 Error Messages The appearance and effect of a MANUALplus error message depend on the current operation. Direct error messages The MANUALplus uses direct error messages whenever immediate error correction is possible and advisable, for example if the input value of a cycle parameter exceeds the valid input range. Confirm the message with ENTER and correct the error (see figure to the upper right).
2.3 Error Messages Clearing an error message You can cancel the error message on which the cursor is located with the "Backspace" key, or cancel all of the error messages with the "Clear" key. The error symbol remains set in the top line until all of the errors have been canceled. You can exit the error window without clearing any error messages by pressing Back. Information in the error message: The error description explains the error that has occurred.
2.3 Error Messages Warnings during simulation If during simulation of a cycle, an entire cycle program or a DIN program MANUALplus detects problems, it displays a warning in the soft key to the extreme left (see figure to the lower right). Press the soft key to call these messages.
2.4 Explanation of Terms 2.4 Explanation of Terms Cursor: In lists, or during data input, a list item, an input field or a character is highlighted. This "highlight" is called a cursor. Entries and operations, like copying, deleting, inserting a new item, etc., refer to the current cursor position. Arrow keys: The cursor is moved with the horizontal and vertical arrow keys and with the PgUp/PgDn keys. Page keys: The PgUp/PgDn keys are also called "Page keys.
Machine Mode of Operation 41 3 Machine Mode of Operation
3.1 Machine Mode of Operation 3.1 Machine Mode of Operation The Machine mode of operation includes all functions for machine setup, workpiece machining, and cycle and DIN program definition. Machine setup For preparations like setting axis values (defining workpiece zero point), measuring tools or setting the protection zone. Manual operation Machine a workpiece manually or semi-automatically. Teach-in "Teach-in" a new cycle program, change an existing program, or graphically simulate cycles.
3.2 Switch-On / Switch-Off 3.2 Switch-On / Switch-Off Switch-on In the screen headline, MANUALplus displays the individual steps that are performed during system start. When the system has completed all tests and initializations, it switches to the Machine mode of operation. The tool display shows the tool that was last used. Whether a reference run is necessary depends on the encoders used. If errors are encountered during system start, MANUALplus displays the error symbol on the screen.
3.2 Switch-On / Switch-Off Standard encoder: The axes move to known, machine-based points. As soon as a reference mark is traversed, a signal is transmitted to the control. The control knows the distance between the reference mark and the machine zero point and can now establish the precise position of the axis. In case you traverse the reference marks separately for the X and Z axes, you only traverse in either the X or the Z axis.
3.2 Switch-On / Switch-Off Switch-off Proper switch-off is recorded in the error log file. Switch-off Go to the main level of the Machine mode of operation. Press the Switch off soft key. MANUALplus displays a confirmation request. Press ENTER to terminate the control. Wait until MANUALplus requests you to switch off the machine.
3.3 Machine Data 3.3 Machine Data Input and display of machine data In Manual mode, the machine data for tool, spindle speed and feed rate are entered in "Set T, S, F ." In cycle programs the machine data are included in the cycle parameters, and in DIN programs they are part of the NC program. In "Set T, S, F" you also define the "maximum speed" and the "stopping angle.
3.
3.3 Machine Data If a driven tool is active, the spindle speed and speed limitation refer to the tool. Your machine documentation provides information on whether the driven tool can be operated with feed per revolution. Tools with more than one cutting edge If you use special tools with more than one cutting edge, different tool parameters apply (set-up dimensions, cutting radius, etc.). Enter more than one tool definition to define these tools.
"S" is the identification letter for spindle data. Depending on which mode of the Constant speed soft key is active, data is entered in: Revolutions per minute (constant speed) Meters per minute (constant cutting speed). Spindle symbols (S display) Direction of spindle rotation M3 The input range is limited by the maximum spindle speed. You define the speed limitation in "Set T, S, F", in machine parameters 805/855, or in DIN programming with the G26 command.
3.4 Machine Setup 3.4 Machine Setup The machine always requires a few preparations, regardless of whether you are machining a workpiece manually or automatically. In Manual mode the following functions are subitems of the "Setup" menu item: Setting the axis values (defining workpiece zero point) Setting the protection zone Defining the tool change position Setting C-axis values Defining the workpiece zero point Select "Setup." „Select "Set axis values." Touch the workpiece zero point (end face).
3.4 Machine Setup Setting the protection zone Whenever the tool is moved, MANUALplus checks whether the "protection zone" is violated (in the negative Z direction). If it detects such a violation, it stops the axis movement and generates an error message. The graphic support window shows the current setting for the protection zone: Distance between machine zero point and protection zone. "-99999.000" means: Protection zone (in the negative Z direction) is not monitored.
3.4 Machine Setup Defining the tool change position With the cycle "Move to tool change position" or the DIN command G14, the slide moves to the tool change point. Always program the tool change point as far from the workpiece as possible to avoid damage to the workpiece during tool change. Defining the tool change position Select "Setup." Press "Tool change point." Approach the tool change position. Move to the tool change point using the jog keys or the handwheel.
3.4 Machine Setup Setting C-axis values The zero point for the C axis can be defined as follows: Defining the zero point of the C axis Select "Setup." Press "Set C-axis values." Position the C axis. Define the position as the zero point of the C axis. Enter the zero point shift of the C axis. Confirm entry for MANUALplus to calculate the zero point of the C axis. Delete zero point shift of the C axis.
3.5 Setting up Tools 3.5 Setting up Tools MANUALplus offers functions for measuring tools by touching the workpiece with the tool or by using a touch probe or an optical gauge. Set the measuring method in machine parameter 6. If the tool dimensions are already known, you can enter the setup dimensions directly in the "Tool management" mode of operation. Finding the tool dimensions by touch-off with the tool In the tool table, enter the tool you want to measure (see “Tool Data” on page 418).
3.5 Setting up Tools There are several ways to determine tool dimensions. The following method describes how the dimensions are determined by comparing a tool with an already measured tool. The graphic support window shows the details of the tool measurement process, taking the selected tool type and tool orientation into account.
3.5 Setting up Tools Finding the tool dimensions by using a touch probe In the tool table, enter the tool you want to measure (see “Tool Data” on page 418). Insert the tool and enter the T number in "Set T, S, F." Activate Measure tool. Pre-position the tool for the first direction of measurement. Press the soft key for this direction (e.g. Z direction). Press Cycle START. The tool moves in the direction of measurement.
3.5 Setting up Tools Finding the tool dimensions by using an optical gauge In the tool table, enter the tool you want to measure (see “Tool Data” on page 418). Insert the tool and enter the T number in "Set T, S, F." Activate Measure tool. Position the tool at the cross hairs of the optical gauge by using the jog keys or the handwheel. Save the tool dimension in Z (the compensation value is deleted). Save the tool dimension in X (the compensation value is deleted). Enter the cutting radius.
3.5 Setting up Tools Tool compensation The tool compensation in X and Z as well as the special compensation for recessing tools compensate for wear of the cutting edge. A compensation value must not exceed 99 mm. Defining tool compensation Select "Set T, S, F" (only available in Manual mode). Press Tool correct. Select X offset for tool. The compensation values that you determine per handwheel are now shown in the "Distance-to-go" display. Transfer the compensation value to the tool table.
3.5 Setting up Tools Tool life monitoring If desired, you can have MANUALplus monitor tool life or the number of parts that are produced with a specific tool. The tool life monitoring function adds the times a tool is traversed at the machine feed rate and counts the number of finished parts. The count is compared with the entry in the tool data.
3.6 Manual Mode 3.6 Manual Mode With manual workpiece machining, you move the axes with the handwheels or jog controls. You can also use cycles for machining complex contours (semi-automatic mode). The paths of traverse and the cycles, however, are not stored. After switch-on and traversing the reference marks, MANUALplus is always in Manual mode. This mode remains active until you select Teach-in or Program run. You can return to Manual mode with the "Menu" key.
3.6 Manual Mode Cycles in Manual mode Set the spindle speed. Set the feed rate Insert tool, define T number and check tool data (T0 is not permitted). Approach cycle start point. Select the cycle and enter cycle parameters. Graphic control of cycle run. Run the cycle.
3.7 Teach-In Mode 3.7 Teach-In Mode In Teach-in mode (cycle mode), you machine a workpiece step by step with the help of cycles. MANUALplus "memorizes" how the workpiece was machined and stores the necessary working steps in a cycle program, which you can call up again at any time. The Teach-in mode can be switched on by soft key and is displayed in the header. Each cycle program is given a number and a short description.
3.8 Program Run Mode 3.8 Program Run Mode In Program run mode, you use cycle programs and DIN programs for parts production. You cannot change the programs in this mode. The "graphic simulation" feature, however, allows you to check the programs before you run them. MANUALplus also offers the "Single block" mode with which you can machine a workpiece, for example, the first of a whole batch, step by step.
3.8 Program Run Mode Start block search and program execution Preconditions for defining a start block: The MANUALplus must be prepared by the machine tool builder for the start block function. The start block function must be activated (Organization mode of operation: "Current parameters—NC switches—Settings“ or control parameter 1) MANUALplus starts program run from the cursor position. The starting position is not changed by a previous graphic simulation.
3.8 Program Run Mode Entering compensation values during program execution Compensation values can be entered during program execution. Entered values are added to the existing compensation values and are effective immediately. Entering tool compensation values Activate the tool compensation. Enter the tool number. Press Save for the valid compensation data to be displayed in the input window. Enter the compensation values. Transfer the compensation values (see “Setting up Tools” on page 54).
3.8 Program Run Mode MANUALplus manages 16 additive compensation values as "parameters." You can edit the additive compensation values in the "Organization mode of operation—Current parameters." Additive compensation values need to be activated with "G149" in a DIN program or a DIN macro. Setting compensation values with the handwheel The “Compensation values via handwheel” function is only available if bit 13 of the configuration code (MP 18 – control configuration) is set.
3.8 Program Run Mode Program execution in “dry run” mode The dry run mode is used for fast program execution up to a point at which machining is to resume. The prerequisites for a dry run are: The MANUALplus must be prepared by the machine tool builder for dry run (The function is activated with a keylock switch or a key.) The Program Run mode must be activated In dry run, all feed paths (except thread cuts) are traversed at the rapid rate.
3.9 Graphic Simulation 3.9 Graphic Simulation The graphic simulation feature enables you to check the machining sequence, the proportioning of cuts and the finished contour before actual machining. In the Manual and Teach-in modes, this function simulates the execution of a single cycle—in Program run mode it simulates a complete cycle or DIN program. A programmed workpiece blank is displayed in the simulation graphics.
3.9 Graphic Simulation The motion simulation depicts the workpiece blank material as a "filled surface" and "machines" it during simulation by "erasing" the material (erasing graphics). The tools move at the programmed feed rate (program-run graphics). If during running simulation you switch to the motion simulation, it will not become effective until the simulation function is restarted. You can interrupt the motion simulation at any time, even during simulation of an NC block.
3.9 Graphic Simulation Views Machining operations with traversable spindle or a C axis can be controlled in the face view or surface view (under "Extra functions"). The "Lathe, Face or Surface view" can be displayed as an alternative. Lathe view Representation in the X/Z plane. Face view Representation in the XK/YK plane. The coordinate system is based on Cartesian coordinates. The origin is located in the turning center, with the angle C=0° positioned on the positive XK axis (see figure at top right).
3.9 Graphic Simulation Graphic elements During simulation, MANUALplus shows the following elements and tool movements in the graphics window: Origin of the coordinate system The workpiece zero point serves as the origin of the coordinate system. Contour At the beginning of a cycle simulation, the programmed contour of that cycle is depicted in cyan. In the Teach-in mode, you can display the preceding contour elements of the cycle program (function "Display contour elements).
3.9 Graphic Simulation Displays beneath the graphics window: Field "N" Block number of the simulated block. Fields "X" and "Z" Target coordinates of the simulated rapid traverse or feed path. Field "C" Spindle angle for positioned spindle (M19) or C axis. Field "T" Simulated tool (programmed T number). Input box For cycle programs, the cycle designation and the parameters are displayed. Soft keys Call the "Time calculation" (see “Time Calculation” on page 74).
3.9 Graphic Simulation Magnify / Reduce With cycle programs, the simulation feature selects the area to be simulated in such a way that all paths of traverse can be illustrated. With DIN programs and DIN macros, the area to be simulated is taken from "Current parameters—Graphic parameters—Standard window size / Standard blank." This is also the case for the face and lateral-surface views.
3.10 Time Calculation 3.10 Time Calculation During simulation, the machining and idle-machine times are calculated. MANUALplus shows the machining times under the menu item "Extra functions—Process times (machining times)." The machining times, idle times and total times are shown in the table "Time calculation" (green: machining times; yellow: idle times). If you are working with cycle programs, each cycle is shown in a separate line.
3.11 Program Management 3.11 Program Management MANUALplus differentiates between the following program groups: Cycle programs ICP contours DIN programs DIN macros Program information Program number The program number (1 to 8 characters) serves to identify the program within a program group. Completing zeros are part of the program number. Program description You can describe a program by a short text of up to 35 alphanumeric characters. This text is displayed in the program list.
3.11 Program Management Functions for program management First select the desired program and then press the corresponding function key. The selected program is displayed in the "Program number" field. Sort program list The programs of a program group can be listed in alphabetical order or by date. Select program You can select the desired program from the list or enter the program number. Activate program When you press Select program, the control returns to the previous operating environment.
3.12 Conversion into DIN Format 3.12 Conversion into DIN Format The "Convert to DIN" function enables you to convert a cycle program to a DIN program with the same functionality. You can then optimize, expand such a DIN program, etc. Conversion into DIN format Press Cyc.prog. --> DIN. Select the program to be converted. Press Create DIN prog. The generated DIN program has the same program number as the cycle program.
3.13 Inch Mode 3.13 Inch Mode You can operate MANUALplus in the metric or inch system (for inch mode, see illustration to the right). Units in inch mode: Coordinates, lengths, path data in inches Feed rate in inch/revolution or inch/min Cutting speed in ft/min (feet/min) The inch/metric setting is also evaluated for the displays and entries in tool management and parameters. For accuracies for displays and entries, see the table at right.
Cycle Programming HEIDENHAIN MANUALplus 4110 79
4.1 Working with Cycles 4.1 Working with Cycles Before you can use the cycles, you must set the workpiece zero point and ensure that the tools you are going to use are described. The machine data (tool, feed rate, spindle speed) are entered with the other cycle parameters in Teach-in mode. In Manual mode, you must program these machine data before calling a cycle.
4.1 Working with Cycles Help graphics The functionalities and parameters of the cycles are illustrated in the graphic support window. These graphics usually show an external machining operation. The Circle key allows you to switch to the help graphics for internal machining, and to switch between the help graphics for internal and external machining.
4.1 Working with Cycles Switching functions (M functions) Whether switching functions are triggered automatically or must be commanded manually depends on your specific machine. MANUALplus generates all switching functions that are necessary for running a cycle. The direction of spindle rotation must be defined in the tool parameters. Using the tool parameters, the cycles generate spindle trigger functions (M3 or M4).
4.1 Working with Cycles Cycle menu The main menu shows the cycle groups. Once a cycle group has been selected, the soft keys for the individual cycles appear. You can use ICP cycles for complex contours, and DIN macros for technologically sophisticated machining operations (see “ICP Contours” on page 242 and “DIN Programming” on page 278). In cycle programs, the numbers of the ICP contours or DIN macros are at the end of the line of the cycle. Some cycles offer optional parameters.
4.1 Working with Cycles Soft keys in cycle programming Depending on the type of cycle, you define the functions for the cycle by soft key. The table to the right lists the soft keys used in cycle programming. Soft keys in cycle programming Call the ICP editor. Approach the tool change position. Activate spindle positioning (M19). On: Tool returns to the cycle start point. Off: Tool remains at cycle end position. Linear hole pattern on face or lateral surface.
4.2 Workpiece Blank Cycles 4.2 Workpiece Blank Cycles The workpiece blank cycles describe the workpiece blank and the setup used. The workpiece blank cycles do not influence the machining process. This information is evaluated during the simulation of the machining process. Workpiece blank Symbol Blank—bar/tube Define the standard blank. ICP workpc. blank contour Define workpiece blank contours with ICP.
4.2 Workpiece Blank Cycles Blank—bar/tube Select the function for defining a workpiece blank. Select "Blank—bar/tube." The cycle describes the workpiece blank and the setup used. This information is evaluated during the simulation.
4.2 Workpiece Blank Cycles ICP workpc. blank contour Select the function for defining a workpiece blank. Select "ICP workpiece blank contour." The cycle integrates the workpiece blank defined with ICP and describes the setup used. This information is evaluated during the simulation.
4.3 Single Cut Cycles 4.3 Single Cut Cycles In the single cut cycles you position the tool in rapid traverse, perform linear or circular cuts, machine chamfers or rounding arcs, and enter M functions. Single cuts Symbol Rapid traverse positioning Approach the tool change position Linear machining, longitudinal/transverse Single longitudinal/transverse cut. Linear machining at angle Single oblique cut. Circular machining Single circular cut (for cutting direction, see menu key). Machine a chamfer.
4.3 Single Cut Cycles Rapid traverse positioning Call the single-cut menu. Select the "Rapid traverse positioning" cycle. The tool moves at rapid traverse from the starting point to the target point.
4.3 Single Cut Cycles Approach the tool change position Call the single-cut menu. Select the "Rapid traverse positioning" cycle. Activate the T-Change approach function The tool moves at rapid traverse from the current position to the tool change position (see “Defining the tool change position” on page 52).
4.3 Single Cut Cycles Linear machining, longitudinal Call the single-cut menu. Select the "Longitudinal linear machining" cycle. With return soft key: Off: When the cycle is completed, the tool remains at the cycle end position. On: Tool returns to the starting point. Longitudinal linear machining The tool moves from the starting point to the contour end point at the programmed feed rate and remains at the cycle end position.
4.3 Single Cut Cycles Linear machining, transverse Call the single-cut menu. Select the "Transverse linear machining" cycle. With return soft key: Off: When the cycle is completed, the tool remains at the cycle end position. On: Tool returns to the starting point. Transverse linear machining The tool moves from the starting point to the contour end point at the programmed feed rate and remains at the cycle end position.
4.3 Single Cut Cycles Linear machining at angle Call the single-cut menu. Select the "Linear machining at angle" cycle. With return soft key: Off: When the cycle is completed, the tool remains at the cycle end position. On: Tool returns to the starting point. Linear machining at angle MANUALplus calculates the target position and moves the tool on a straight line from the starting point to the target position at the programmed feed rate.
4.3 Single Cut Cycles Circular machining Call the single-cut menu. Select the "Circular machining cycle" (clockwise). Select the "Circular machining cycle" (counterclockwise). With return soft key: Off: When the cycle is completed, the tool remains at the cycle end position. On: Tool returns to the starting point. Circular machining The tool moves in circular arc from the starting point to the contour end point at the programmed feed rate and remains at the cycle end position.
4.3 Single Cut Cycles Chamfer Call the single-cut menu. Select the "Chamfer" cycle. With return soft key: Off: When the cycle is completed, the tool remains at the cycle end position. On: Tool returns to the starting point. Chamfer The cycle produces a chamfer that is dimensioned relative to the corner of the workpiece contour. When the cycle is completed, the tool remains at the cycle end position.
4.3 Single Cut Cycles Rounding Call the single-cut menu. Select the "Rounding" cycle. With return soft key: Off: When the cycle is completed, the tool remains at the cycle end position. On: Tool returns to the starting point. Rounding The cycle produces a rounding that is dimensioned relative to the corner of the workpiece contour. When the cycle is completed, the tool remains at the cycle end position.
4.3 Single Cut Cycles M functions Machine commands (M functions) are not executed until Cycle START has been pressed. For the meaning of the M functions, refer to your machine manual (see “M Functions” on page 408). M function Call the single-cut menu. Select "M function." Enter the number of the M function. Conclude entry. Press Cycle START. Spindle stop M19 (spindle positioning) Call the single-cut menu. Select "M function." Switch M19 on. Enter the stopping angle. Conclude entry.
4.4 Roughing Cycles 4.4 Roughing Cycles Roughing cycles rough and finish simple contours in "basic mode" and complex contours in "expanded mode." With ICP cutting cycles, you can machine contours defined with ICP (see “Editing ICP Contours” on page 243). Proportioning of cuts: MANUALplus calculates an infeed that is <= infeed depth P. An "abrasive cut" is avoided. Oversizes: In "expanded" mode. Cutter radius compensation: Active.
4.4 Roughing Cycles Tool position It is important that you observe the tool positions (starting point X, Z) before executing any of the roughing cycles in expanded mode. However, they also apply for all cutting and infeed directions as well as for roughing and finishing (see examples of linear cycles in figures at right). The starting point must not be located in the shaded area. The area to be machined starts at the starting point X, Z if the tool is positioned before the contour area.
4.
4.4 Roughing Cycles Roughing, longitudinal/transverse Call the "Roughing, longitudinal/transverse" cycles. Select "Cut longitudinal" (see figures at right). Select "Cut transverse" (see figures on the following page). The "Cut longitudinal" cycle machines the rectangular area defined by X, Z and X1, Z2. The "Cut transverse" cycle machines the rectangular area defined by X, Z and X2, Z1.
4.4 Roughing Cycles Cycle run 1 2 3 4 Calculate the proportioning of cuts (infeed). Approach workpiece for first pass from X, Z. Move to end point Z2 at programmed feed rate. Depending on algebraic sign of infeed depth P: P>0: Machine contour outline. P<0: Retract at angle of 45°. 5 6 7 Retract and approach for next pass. Repeat steps 3 to 5 until X1 or Z1 is reached. Return to starting point on diagonal path.
4.4 Roughing Cycles Roughing, longitudinal/transverse—Expanded Call the "Roughing, longitudinal/transverse" cycles. Select "Cut longitudinal" (see figures at right). Select "Cut transverse" (see figures on the following page). Press the Expanded soft key. The "Cut longitudinal" cycle machines the area defined by X, Z and X1, Z2, taking the oversizes into account. The "Cut transverse" cycle machines the area defined by X, Z and Z1, X2, taking the oversizes into account.
4.4 Roughing Cycles Cycle run 1 2 3 4 5 6 7 Calculate the proportioning of cuts (infeed). Approach workpiece for first pass from X, Z. Move to contour end point Z2 or contour end point X2, or if defined, to one of the optional contour elements at programmed feed rate. Depending on algebraic sign of P: P>0: Machine contour outline. P<0: Retract at angle of 45°. Retract and approach for next pass. Repeat steps 3 to 5 until X1 or Z1 is reached. Return to starting point on paraxial path.
4.4 Roughing Cycles Finishing cut, longitudinal/transverse Call the "Roughing, longitudinal/transverse" cycles. Select "Cut longitudinal" (see figures at right). Select "Cut transverse" (see figures on the following page). Press the Finishing run soft key. The cycle "Finishing cut, longitudinal" finishes the contour area from X1 to Z2. The cycle "Finishing cut, transverse" finishes the contour area from Z1 to X2. At the end of cycle, the tool returns to the starting point.
4.4 Roughing Cycles Execution of "Finishing cut, transverse" cycle 1 2 3 Move in transverse direction from X, Z to contour starting point Z1. Finish first in transverse direction, then in longitudinal direction. Return in transverse direction to starting point.
4.4 Roughing Cycles Finishing cut, longitudinal/transverse— Expanded Call the "Roughing, longitudinal/transverse" cycles. Select "Cut longitudinal" (see figures at right). Select "Cut transverse" (see figures on the following page). Press the Expanded soft key. Press the Finishing run soft key. The cycle finishes the contour area from X1, Z1 to X2, Z2. When the cycle is completed, the tool remains at the cycle end position.
4.4 Roughing Cycles Cycle run 1 2 Move in transverse direction from X, Z to X1, Z1. Finish contour area from X1, Z1 to X2, Z2, taking optional contour elements into account.
4.4 Roughing Cycles Plunge longitudinal/transverse Call the "Roughing, longitudinal/transverse" cycles. Select "Plunge longitudinal" (see figures at right). Select "Plunge transverse" (see figures on the following page). This cycle machines the area defined by X1/Z1, X2/Z2 and plunging angle A. The steeper the tool plunges into the material, the greater the feed rate decrease (max. 50%). Pay attention to the dimensions of facing tools (see “Facing tools” on page 419).
4.4 Roughing Cycles Cycle run 1 2 3 4 5 6 7 8 Calculate the proportioning of cuts (infeed). Approach workpiece on paraxial path for first pass from X, Z. Plunge-cut at plunging angle A with reduced feed. Move to contour end point Z2 or X2 or, if programmed, to oblique contour element defined by W at programmed feed rate. Depending on algebraic sign of P: P>0: Machine contour outline. P<0: Retract at angle of 45°. Return and approach again for next pass. Repeat steps 3 to 5 until X2 or Z2 is reached.
4.4 Roughing Cycles Plunge, longitudinal/transverse—Expanded Call the "Roughing, longitudinal/transverse" cycles. Select "Plunge longitudinal" (see figures at right). Select "Plunge transverse" (see figures on the following page). Press the Expanded soft key. This cycle machines the area defined by X1/Z1, X2/Z2 and plunging angle A, taking the oversizes into account. The steeper the tool plunges into the material, the greater the feed rate decrease (max. 50%).
4.4 Roughing Cycles S spindle speed / cutting speed F feed per revolution I, K oversize X, Z By setting the following optional parameters, you can define additional contour elements: W: R: B1: B2: Oblique cut at contour end Rounding (in both corners of the contour valley) Chamfer/Rounding at contour start Chamfer/Rounding at contour end Cycle run 1 2 3 4 5 6 7 8 Calculate the proportioning of cuts (infeed). Approach workpiece on paraxial path for first pass from X, Z.
4.4 Roughing Cycles Finishing plunge, longitudinal/transverse Call the "Roughing, longitudinal/transverse" cycles. Select "Plunge longitudinal" (see figures at right). Select "Plunge transverse" (see figures on the following page). Press the Finishing run soft key. The cycle finishes the contour area from X1, Z1 to X2, Z2. At the end of cycle, the tool returns to starting point X, Z. The steeper the tool plunges into the material, the greater the feed rate decrease (max. 50%).
4.4 Roughing Cycles Cycle run 1 2 3 Move in transverse direction from X, Z to contour starting point X1, Z1. Finish defined contour area. Return to starting point on paraxial path.
4.4 Roughing Cycles Finishing plunge, longitudinal/transverse—Expanded Call the "Roughing, longitudinal/transverse" cycles. Select "Plunge longitudinal" (see figures at right). Select "Plunge transverse" (see figures on the following page). Press the Expanded soft key. Press the Finishing run soft key. The cycle finishes the contour area from X1, Z1 to X2, Z2. When the cycle is completed, the tool remains at the cycle end position.
4.4 Roughing Cycles By setting the following optional parameters, you can define additional contour elements: W: R: B1: B2: Oblique cut at contour end Rounding (in both corners of the contour valley) Chamfer/Rounding at contour start Chamfer/Rounding at contour end Cycle run 1 2 Move on paraxial path from X, Z to contour starting point X1, Z1. Finish defined contour area, taking optional contour elements into account.
4.4 Roughing Cycles ICP contour-parallel, longitudinal/transverse Call the "Roughing, longitudinal/transverse" cycles. Select "ICP contour-parallel, longitudinal" (see figures at right). Select "ICP contour-parallel, transverse" (see figures on the following page). The cycle machines parallel to the contour, depending on the J parameter: J=0: The area defined by X, Z and the ICP contour, taking the oversizes into account.
4.4 Roughing Cycles Cycle run 1 Calculate the proportioning of cuts (infeed), taking the parameter J into account. J=0: The cutting geometry is taken into account. This may result in the use of different infeeds for the longitudinal and transverse directions. J>0: The same infeed is used for both the longitudinal and the transverse direction. 2 3 Approach workpiece on paraxial path for first pass from X, Z. Machine the workpiece according to the calculated proportioning of cuts.
4.4 Roughing Cycles ICP contour-parallel finishing, longitudinal/ transverse Call the "Roughing, longitudinal/transverse" cycles. Select "ICP contour-parallel, longitudinal" (see figures at right). Select "ICP contour-parallel, transverse" (see figures on the following page). Press the Finishing run soft key. The cycle finishes the contour area defined by the ICP contour. When the cycle is completed, the tool remains at the cycle end position.
4.4 Roughing Cycles Cycle run 1 2 Move on paraxial path from X, Z to contour starting point. Finish defined contour area.
4.4 Roughing Cycles ICP roughing, longitudinal/transverse Call the "Roughing, longitudinal/transverse" cycles. Select "ICP cut, longitudinal" (see figures at right). Select "ICP cut, transverse" (see figures on the following page). The cycle machines the area defined by X, Z and the ICP contour, taking the oversizes into account. Danger of collision! If the tool angle and the tool point angle have not been defined, the tool plunge-cuts at the plunging angle.
4.4 Roughing Cycles Cycle run 1 2 3 4 5 6 7 8 Calculate the proportioning of cuts (infeed). Approach workpiece on paraxial path for first pass from X, Z. For sloping contours, plunge into the material at reduced feed rate. Machine the workpiece according to the calculated proportioning of cuts. Depending on algebraic sign of P: P>0: Machine contour outline. P<0: Retract by the safety clearance at 45°. Return and approach for next pass. Repeat 3 to 6 until the defined area has been machined.
4.4 Roughing Cycles ICP finishing, longitudinal or transverse Call the "Roughing, longitudinal/transverse" cycles. Select "ICP cut, longitudinal" (see figures at upper and center right). Select "ICP cut, transverse" (see figures on the following page). Press the Finishing run soft key. The cycle finishes the contour area defined by the ICP contour. When the cycle is completed, the tool remains at the cycle end position.
4.4 Roughing Cycles Cycle run 1 2 Move on paraxial path from X, Z to contour starting point. Finish defined contour area.
4.4 Roughing Cycles Examples of roughing cycles Roughing and finishing an outside contour The shaded area from "AP" (starting point of contour) to "EP" (contour end point) is first rough-machined with the cycle "Cut longitudinal—Expanded," taking oversizes into account (see figure at upper right). This contour area is to be finished subsequently with the cycle "Finishing cut longitudinal—Expanded" (see figure at lower right).
4.4 Roughing Cycles Roughing and finishing an inside contour The shaded area from "AP" (starting point of contour) to "EP" (contour end point) is first rough-machined with the cycle "Cut longitudinal—Expanded," taking oversizes into account (see figure at upper right). This contour area is to be finished subsequently with the cycle "Finishing cut longitudinal—Expanded" (see figure at lower right). The rounding and the chamfer at the contour end are also machined in "expanded mode.
4.4 Roughing Cycles Roughing (recess clearance) with plunge cycle The tool to be used cannot plunge at the required angle of 15°. The roughing process for the area therefore requires two steps. First step: The shaded area from "AP" (starting point of contour) to "EP" (contour end point) is rough-machined with the cycle "Plunge longitudinal—Expanded," taking oversizes into account. The "starting angle A" is defined with 15°, as specified in the workpiece drawing.
4.4 Roughing Cycles Second step: The area that was left out in the first step (shaded area in top left figure) is machined with the cycle "Plunge, longitudinal—Expanded." Before executing this step, you must change tools. The rounding arcs in the contour valley are also machined in "expanded mode." The parameters for contour starting point X1, Z1 and contour end point X2, Z2 determine the cutting and infeed directions—in this example, external machining and infeed in negative X-axis direction.
4.5 Recessing cycles 4.5 Recessing cycles The recessing cycle group comprises recessing, recess turning, undercut and parting cycles. Simple contours are machined in "basic mode," complex contours in "expanded mode." With ICP recessing cycles, you can machine any type of contour defined with ICP (see “ICP Contours” on page 242). Proportioning of cuts: MANUALplus calculates an infeed that is <= infeed depth P. Oversizes: In "expanded" mode.
4.
4.5 Recessing cycles Recessing, radial/axial Call the recessing menu. Select the "Recessing, radial" cycle (see figures at right). Select "Recessing axial" (see figures on the following page). The cycle machines the number of recesses defined in Q. The parameters X/Z to X2/Z2 define the first recess (position, recess depth and recess width). Cycle parameters X, Z starting point X2, Z2 contour end point P recessing width: Infeeds <= P No input: P = 0.
4.5 Recessing cycles Cycle run 1 2 3 4 5 6 7 8 Calculate the recess positions and the proportioning of cuts. Approach workpiece for next recess from starting point or from last recess on paraxial path. Move to end point X2 or end point Z2 at programmed feed rate. Remain at this position for dwell time "E." Retract and approach for next pass. Repeat 3 to 5 until the complete recess has been machined. Repeat 2 to 6 until all recesses have been machined. Return to starting point on paraxial path.
4.5 Recessing cycles Recessing, radial/axial—Expanded Call the recessing menu. Select the "Recessing, radial" cycle (see figures at right). Select "Recessing axial" (see figures on the following page). Press the Expanded soft key. The cycle machines the number of recesses defined in Q. The parameters X1/Z1 to X2/Z2 define the first recess (position, recess depth and recess width).
4.5 Recessing cycles Cycle run 1 2 3 4 5 6 7 8 Calculate the recess positions and the proportioning of cuts. Approach workpiece for next recess from starting point or from last recess on paraxial path. Move to contour end point X2 or contour end point Z2, or if defined, to one of the optional contour elements at programmed feed rate. Remain at this position for a dwell time of two revolutions. Retract and approach for next pass. Repeat 3 to 5 until the complete recess has been machined.
4.5 Recessing cycles Recessing radial/axial, finishing Call the recessing menu. Select the "Recessing, radial" cycle (see figures at right). Select "Recessing axial" (see figures on the following page). Press the Finishing run soft key. The cycle finishes the number of recesses defined in Q. The parameters X/Z to X2/Z2 define the first recess (position, recess depth and recess width).
4.5 Recessing cycles Cycle run 1 2 3 4 5 6 7 Calculate the recess positions. Approach workpiece for next recess from starting point or from last recess on paraxial path. Finish first side and the contour valley up to position just before recess end point. Approach workpiece for finishing the second side on paraxial path. Finish the second side and the remainder of the contour valley. Repeat 2 to 5 until all recesses have been machined. Return to starting point on paraxial path.
4.5 Recessing cycles Recessing radial/axial, finishing—Expanded Call the recessing menu. Select the "Recessing, radial" cycle (see figures at right). Select "Recessing axial" (see figures on the following page). Press the Expanded soft key. Press the Finishing run soft key. The cycle machines the number of recesses defined in Q. The parameters X/Z to X2/Z2 define the first recess (position, recess depth and recess width).
4.5 Recessing cycles Cycle run 1 2 3 4 5 6 7 Calculate the recess positions. Approach workpiece for next recess from starting point or from last recess on paraxial path. Finish first side, taking optional contour elements into account; then finish contour valley up to position just before recess end point. Approach workpiece for finishing the second side on paraxial path. Finish second side, taking optional contour elements into account; then finish remainder of contour valley.
4.5 Recessing cycles ICP recessing cycles Call the recessing menu. Select the "ICP recessing, radial" cycle (see figures at right). Select "ICP recessing axial" (see figures on the following page). The cycle machines the number of recesses defined in Q with the ICP recessing contour. The parameters "X, Z" define the position of the first recess. Cycle parameters X, Z starting point P recessing width: Infeeds <= P No input: P = 0.
4.5 Recessing cycles Cycle run 1 2 3 4 5 6 7 Calculate the recess positions and the proportioning of cuts. Approach workpiece for next recess from starting point or from last recess on paraxial path. Machine along the defined contour. Return and approach for next pass. Repeat 3 to 4 until the complete recess has been machined. Repeat 2 to 5 until all recesses have been machined. Return to starting point on paraxial path.
4.5 Recessing cycles ICP recessing radial/axial, finishing Call the recessing menu. Select the "ICP recessing, radial" cycle (see figures at right). Select "ICP recessing axial" (see figures on the following page). Press the Finishing run soft key. The cycle finish-machines the number of recesses defined in Q with the ICP recessing contour. The parameters "X, Z" define the position of the first recess. At the end of cycle, the tool returns to the starting point.
4.5 Recessing cycles Cycle run 1 2 3 4 5 Calculate the recess positions. Approach workpiece for next recess from starting point or from last recess on paraxial path. Finish the recess. Repeat 2 to 3 until all recesses have been machined. Return to starting point on paraxial path.
4.5 Recessing cycles Recess turning The workpiece is machined by alternate recessing and roughing movements. The machining process requires a minimum of retraction and infeed movements. To influence recess-turning operations, use the following parameters: Recessing feed rate O: Feed rate for recessing movement. Turning operation, unidirectional/bidirectional U: You can perform a unidirectional or bidirectional turning operation.
4.5 Recessing cycles Recess turning, radial/axial Call the recessing menu. Select the "Recess turning" cycle. Select the "Recess turning, radial" cycle (see figures at right). Select "Recess turning, axial" (see figures on the following page). The cycle machines the rectangular area defined by X, Z and X2, Z2 (see also “Recess turning” on page 143).
4.5 Recessing cycles Cycle run 1 2 3 4 5 6 Calculate the proportioning of cuts. Approach workpiece for first pass from X, Z. Execute the first cut (recessing). Machine perpendicularly to recessing direction (turning). Repeat 3 to 4 until contour end point Z2/X2 is reached. Return to starting point on paraxial path.
4.5 Recessing cycles Recess turning, radial/axial—Expanded Call the recessing menu. Select the "Recess turning" cycle. Select the "Recess turning, radial" cycle (see figures at right). Select "Recess turning, axial" (see figures on the following page). Press the Expanded soft key. The cycle machines the area defined by X/Z1 and X2, Z2, taking the oversizes into account (see also “Recess turning” on page 143).
4.5 Recessing cycles By setting the following optional parameters, you can define additional contour elements: A: W: R: B1: B2: Oblique cut at contour start Oblique cut at contour end Rounding (in both corners of the contour valley) Chamfer/Rounding at contour start Chamfer/Rounding at contour end Cycle run 1 2 3 4 5 6 7 Calculate the proportioning of cuts. Approach workpiece for first pass from X, Z. Execute the first cut (recessing). Machine perpendicularly to recessing direction (turning).
4.5 Recessing cycles Recess turning radial/axial, finishing Call the recessing menu. Select the "Recess turning" cycle. Select the "Recess turning, radial" cycle (see figures at right). Select "Recess turning, axial" (see figures on the following page). Press the Finishing run soft key. The cycle finishes the contour area from X, Z to X2, Z2 (see also “Recess turning” on page 143). With "oversizes I, K" for the workpiece blank, you define the material to be machined during the finishing cycle.
4.5 Recessing cycles Cycle run 1 2 3 4 5 Approach contour area from X, Z. Finish first side, then finish contour valley up to position just before contour end point Z2/X2. Move on paraxial path: radially to X/Z2. axially to Z/X2. Finish second side, then finish remainder of contour valley. Return to starting point on paraxial path.
4.5 Recessing cycles Recess turning radial/axial, finishing—Expanded Call the recessing menu. Select the "Recess turning" cycle. Select the "Recess turning, radial" cycle (see figures at right). Select "Recess turning, axial" (see figures on the following page). Press the Expanded soft key. Press the Finishing run soft key. The cycle finishes the contour area from X1, Z1 to X2, Z2 (see also “Recess turning” on page 143).
4.5 Recessing cycles By setting the following optional parameters, you can define additional contour elements: A: W: R: B1: B2: Oblique cut at contour start Oblique cut at contour end Rounding (in both corners of the contour valley) Chamfer/Rounding at contour start Chamfer/Rounding at contour end With "oversizes I, K" for the workpiece blank, you define the material to be machined during the finishing cycle.
4.5 Recessing cycles ICP recess turning, radial/axial Call the recessing menu. Select the "Recess turning" cycle. Select the "ICP recess turning, radial" cycle (see figures at right). Select "ICP recess turning axial" (see figures on the following page). The cycle proceeds as follows, taking oversizes into account: For descending contours, the area defined by X, Z and the ICP contour is machined. For ascending contours, the area defined by X1, Z1 and the ICP contour is machined.
4.5 Recessing cycles Cycle run 1 2 3 4 5 6 Calculate the proportioning of cuts. Approach workpiece for first pass from X, Z. Execute the first cut (recessing). Machine perpendicularly to recessing direction (turning). Repeat 3 to 4 until the defined area has been machined. Return to starting point on paraxial path.
4.5 Recessing cycles ICP recess turning radial/axial, finishing Call the recessing menu. Select the "Recess turning" cycle. Select "ICP recess turning radial " (see figures at upper and center right). Select "ICP recess turning axial" (see figures on the following page). Press the Finishing run soft key. The cycle finishes the contour area defined by the ICP contour (see also “Recess turning” on page 143). At the end of cycle, the tool returns to the starting point.
4.5 Recessing cycles Cycle run 1 2 3 4 5 Approach contour area from X, Z on paraxial path. Finish first side and contour area up to position just before end point X2/Z2. Approach workpiece for finishing the second side on paraxial path. Finish second side, then finish remainder of contour valley. Return to starting point on paraxial path.
4.5 Recessing cycles Undercut type H Call the recessing menu. Select the "Undercut H" cycle. The contour depends on the parameters defined. If you do not define an "undercut radius R," the oblique cut will be executed up to "contour corner Z1" (tool radius = undercut radius). If you do not define "plunging angle W," it is calculated from "undercut length K" and "undercut radius R." The final point of the undercut is then located at the "contour corner.
4.5 Recessing cycles Undercut type K Call the recessing menu. Select the "Undercut K" cycle. This cycle performs only one cut at an angle of 45°. The resulting contour geometry therefore depends on the tool that is used. Cycle parameters X, Z starting point X1, Z1 contour corner I undercut depth T tool number S spindle speed / cutting speed F feed per revolution Cycle run 1 2 3 Pre-position at an angle of 45° to safety clearance above contour corner point X1, Z1 in rapid traverse.
4.5 Recessing cycles Undercut type U Call the recessing menu. Select the "Undercut U" cycle. This cycle machines an "Undercut type U" and, if programmed, finishes the adjoining plane surface. The undercut is executed in several passes if the undercut width is greater than the cutting width of the tool. If the cutting width of the tool is not defined, the control assumes that the tool's cutting width equals K. A chamfer or rounding (optional) is machined.
4.5 Recessing cycles Parting Call the recessing menu. Select the "Cut-off" cycle. The cycle parts the workpiece. If programmed, a chamfer or rounding arc is machined on the outside diameter.
4.5 Recessing cycles Examples of recessing cycles Recess outside The machining operation is to be executed with the "Recessing, radial—Expanded" cycle, taking oversizes into account (see figure at upper right). This contour area is to be finished subsequently with the "Recessing radial, finishing—Expanded" cycle (see figure at lower right). The rounding arcs in the corners of the contour valley and the oblique surfaces at the contour start and end are also machined in "expanded mode.
4.5 Recessing cycles Recess inside The machining operation is to be executed with the "Recessing, radial—Expanded" cycle, taking oversizes into account (see figure at upper right). This contour area is to be finished subsequently with the "Recessing radial, finishing—Expanded" cycle (see figure at lower right). As the "plunge width P" is not input, the MANUALplus plunge-cuts with 80% of the plunge-width of the tool. In expanded mode, the chamfers are machined at the start/end of the contour.
4.6 Thread and Undercut Cycles 4.6 Thread and Undercut Cycles These cycles machine single or multistart longitudinal and tapered threads, as well as thread undercuts. In Manual mode you can: Repeat the last cut to compensate for tool inaccuracies. Use the function Recut to rework damaged threads. Threads are cut with constant speed. "Cycle STOP" becomes effective at the end of a thread cut. The feed rate and spindle speed overrides are not effective during cycle execution.
4.6 Thread and Undercut Cycles Angle of infeed (thread angle) With some thread cycles, you can indicate the angle of infeed. The figures to the right show the operating sequence of the MANUALplus at an angle of infeed of –30° (figure at upper right) and an angle of infeed of 0° (figure at center right). Thread depth, proportioning of cuts The thread depth is programmed for all thread cycles. MANUALplus reduces the cutting depth with each cut (see figure at center right).
4.6 Thread and Undercut Cycles Last cut After the cycle is finished, the MANUALplus presents the Last cut option. You can use this function to repeat the last thread cut with an updated tool compensation. Sequence for the “last cut” function: Initial situation: The thread cut cycle has been performed, and the thread depth is not correct.
4.6 Thread and Undercut Cycles Thread cycle (longitudinal) Call the thread-cutting menu. Select the "Thread cycle." Inner thread soft key On: Internal thread Off: External thread This cycle cuts a single external or internal thread with a thread angle of 30°. Tool infeed is performed in the X axis only. Cycle parameters X, Z starting point of thread Z2 end point of thread F1 thread pitch (= feed rate) U thread depth No input: Depth is calculated External thread: U=0.
4.6 Thread and Undercut Cycles Thread cycle (longitudinal)—Expanded Call the thread-cutting menu. Select the "Thread cycle." Press the Expanded soft key. Inner thread soft key On: Internal thread Off: External thread This cycle cuts a single or multi-start external or internal thread. The thread starts at starting point X and ends at end point Z2 (without a thread run-in or run-out).
4.6 Thread and Undercut Cycles Cycle run 1 2 3 4 5 6 7 Calculate the proportioning of cuts. Start first pass for first thread groove at Z. Move to end point Z2 at programmed feed rate. Return on paraxial path and approach for next thread groove. Repeat 3 and 4 for all thread grooves. Approach for next pass, taking the reduced cutting depth and the "feed angle A" into account. Repeat 3 to 6 until "no. threads D" and "depth U" are reached.
4.6 Thread and Undercut Cycles Tapered thread Call the thread-cutting menu. Select "Tapered thread." Inner thread soft key On: Internal thread Off: External thread This cycle cuts a single or multi-start tapered external or internal thread. Cycle parameters X, Z starting point X1, Z1 starting point of thread (without run-in) X2, Z2 end point of thread (without run-out) F1 thread pitch (= feed rate) U thread depth No input: Depth is calculated External thread: U=0.
4.6 Thread and Undercut Cycles Parameter combinations for taper angle: X1/Z1, X2/Z2 X1/Z1, Z2, W Z1, X2/Z2, W Cycle run 1 2 3 4 5 6 7 Calculate the proportioning of cuts. Move to starting point X1, Z1. Move to end point Z2 at programmed feed rate. Return on paraxial path and approach for next thread groove. Repeat 3 and 4 for all thread grooves. Approach for next pass, taking the reduced cutting depth and the "feed angle A" into account. Repeat 3 to 6 until "no. threads D" and "depth U" are reached.
4.6 Thread and Undercut Cycles API thread Call the thread-cutting menu. Select "API thread." Inner thread soft key On: Internal thread Off: External thread This cycle cuts a single or multi-start API external or internal thread. The depth of thread decreases at the overrun at the end of thread.
4.6 Thread and Undercut Cycles Cycle run 1 2 3 4 5 6 7 Calculate the proportioning of cuts. Move to thread starting point X1, Z1. Move to end point Z2 at programmed feed rate, taking the "run-out angle WE" into account. Return on paraxial path and approach for next thread groove. Repeat 3 and 4 for all thread grooves. Approach for next pass, taking the reduced cutting depth and the "feed angle A" into account. Repeat 3 to 6 until "no. threads D" and "depth U" are reached.
4.6 Thread and Undercut Cycles Recut (longitudinal) thread Call the thread-cutting menu. Select the "Thread cycle." Press the Recut soft key. Inner thread soft key On: Internal thread Off: External thread The cycle reworks a single-start thread. Since you have already unclamped the workpiece, MANUALplus needs to know the exact position of the thread.
4.6 Thread and Undercut Cycles Cycle run 1 2 3 4 5 Pre-position threading tool to center of thread groove. Transfer the tool position ZC and the spindle angle C with Take over position. Move the tool manually out of the thread groove. Position the tool to starting point X, Z. Start cycle with "Input finished", then press "Cycle START.
4.6 Thread and Undercut Cycles Recut (longitudinal) thread—Expanded Call the thread-cutting menu. Select the "Thread cycle." Press the Expanded soft key. Press the Recut soft key. Inner thread soft key On: Internal thread Off: External thread This cycle recuts a single or multi-start external or internal thread. Since you have already unclamped the workpiece, MANUALplus needs to know the exact position of the thread.
4.6 Thread and Undercut Cycles Cycle run 1 2 3 4 5 Pre-position threading tool to center of thread groove. Transfer the tool position ZC and the spindle angle C with Take over position. Move the tool manually out of the thread groove. Position the tool to starting point X, Z. Start cycle with "Input finished", then press "Cycle START.
4.6 Thread and Undercut Cycles Recut tapered thread Call the thread-cutting menu. Select "Tapered thread." Press the Recut soft key. Inner thread soft key On: Internal thread Off: External thread The cycle recuts a single or multi-start tapered external or internal thread. Since you have already unclamped the workpiece, MANUALplus needs to know the exact position of the thread.
4.6 Thread and Undercut Cycles Cycle run 1 2 3 4 5 Pre-position threading tool to center of thread groove. Transfer the tool position ZC and the spindle angle C with Take over position. Move the tool manually out of the thread groove. Position the tool in front of the workpiece. Start cycle with "Input finished", then press "Cycle START.
4.6 Thread and Undercut Cycles Recut API thread Call the thread-cutting menu. Select "API thread." Press the Recut soft key. Inner thread soft key On: Internal thread Off: External thread The cycle recuts a single or multi-start API external or internal thread. Since you have already unclamped the workpiece, MANUALplus needs to know the exact position of the thread.
4.6 Thread and Undercut Cycles Cycle run 1 2 3 4 5 Pre-position threading tool to center of thread groove. Transfer the tool position ZC and the spindle angle C with Take over position. Move the tool manually out of the thread groove. Position the tool in front of the workpiece. Start cycle with "Input finished", then press "Cycle START.
4.6 Thread and Undercut Cycles Undercut DIN 76 Call the thread-cutting menu. Select the "Undercut DIN 76" cycle. With return soft key: Off: When the cycle is completed, the tool remains at the cycle end position (see figures at right). On: Tool returns to the starting point (see figures on next page). The cycle machines a thread undercut according to DIN76, a thread chamfer, then the cylinder, and finishes with the plane surface.
4.6 Thread and Undercut Cycles All parameters that you enter will be accounted for—even if the standard table prescribes other values. Undercut parameters that are not defined are automatically calculated from the standard table (see “DIN 76—undercut parameters” on page 525"): "Thread pitch FP" is calculated from the diameter X1. The parameters I, K, W, and R are calculated from FP. Cycle run 1 Approach workpiece from X, Z to starting point X1, or for the thread chamfer.
4.6 Thread and Undercut Cycles Undercut DIN 509 E Call the thread-cutting menu. Select the "Undercut DIN 509 E" cycle. With return soft key: Off: When the cycle is completed, the tool remains at the cycle end position (see figures at right). On: Tool returns to the starting point (see figures on next page). The cycle machines a thread undercut according to DIN 509 type E, a cylinder start chamfer, then the adjoining cylinder, and finishes with the plane surface.
4.6 Thread and Undercut Cycles Cycle run 1 Approach workpiece from X, Z to cylinder starting point X1, or for the thread chamfer. 2 3 4 5 6 Machine thread chamfer, if defined. Finish cylinder up to beginning of undercut. Machine undercut. Finish to end point X2 on plane surface. Without return: Tool remains at the end point X2. With return: Return to starting point on diagonal path.
4.6 Thread and Undercut Cycles Undercut DIN 509 F Call the thread-cutting menu. Select the "Undercut DIN 509 F" cycle. With return soft key: Off: When the cycle is completed, the tool remains at the cycle end position (see figures at right). On: Tool returns to the starting point (see figures on next page). The cycle machines a thread undercut according to DIN 509 type F, a cylinder start chamfer, then the adjoining cylinder, and finishes with the plane surface.
4.6 Thread and Undercut Cycles Cycle run 1 Approach workpiece from X, Z to cylinder starting point X1, or for the thread chamfer. 2 3 4 5 6 Machine thread chamfer, if defined. Finish cylinder up to beginning of undercut. Machine undercut. Finish to end point X2 on plane surface. Without return: Tool remains at the end point X2. With return: Return to starting point on diagonal path.
4.6 Thread and Undercut Cycles Examples of thread and undercut cycles External thread and thread undercut The machining operation is to be performed in two steps. Thread undercut DIN 76 produces the undercut and thread chamfer. In the second step, the thread cycle cuts the thread. First step The parameters for the undercut and thread chamfer are programmed in two superimposed input windows (see figure at right).
4.6 Thread and Undercut Cycles Second step The "Thread cycle (longitudinal)—Expanded" cuts the thread. The cycle parameters define the thread depth and the proportioning of cuts (see figure at top right).
4.6 Thread and Undercut Cycles Internal thread and thread undercut The machining operation is to be performed in two steps. Thread undercut DIN 76 produces the undercut and thread chamfer. In the second step, the thread cycle cuts the thread. First step The parameters for the undercut and thread chamfer are programmed in two superimposed input windows (see figure at bottom right and figure on next page at top right). MANUALplus determines the undercut parameters from the standard table.
4.6 Thread and Undercut Cycles Second step The "Thread cycle (longitudinal)" cuts the thread. The thread pitch is defined. MANUALplus automatically determines all other values from the standard table (see figure at right). You must pay attention to the setting of the Inner thread soft key.
4.7 Drilling Cycles 4.7 Drilling Cycles The drilling cycles allow you to machine axial and radial holes. For pattern machining, see “Drilling/ Milling Patterns” on page 227. The "constant cutting speed" may only be programmed with driven tools on machines with spindle control.
4.7 Drilling Cycles Drilling, axial/radial Call the drilling menu. Select the "Drilling, axial" cycle. Select the "Drilling, radial" cycle. This cycle drills a hole on the face / lateral surface of the workpiece.
4.7 Drilling Cycles Cycle run 1 2 3 4 Position spindle to "spindle angle C" (in Manual mode, machining starts from the current spindle angle). If defined, move at rapid traverse to Z1 (axial). X1 (radial). Start drilling at reduced feed rate, if defined. Depending on "V": Drill at programmed feed rate to End point Z2 (axial). End point X2 (radial). Remain at end of hole for dwell time "E," if defined. or Drill at programmed feed rate to position Z2 – AB (axial). X2 – AB (radial).
4.7 Drilling Cycles Deep-hole drilling, axial/radial Call the drilling menu. Select the "Deep-hole drilling, axial" cycle. Select the "Deep-hole drilling, radial" cycle. The cycle produces a bore hole on the face / lateral surface in several passes. After each pass, the drill retracts and, after a dwell time, advances again to the first pecking depth, minus the safety clearance. You define the first pass with "1st hole depth P.
4.7 Drilling Cycles Drilling radial: X1 starting point of hole—default: Drilling starts from position X X2 end point of hole If "AB" and "V" are programmed, the feed rate is reduced by 50% during both pre-drilling and through-boring. MANUALplus uses the tool parameter "driven tool" to determine whether the programmed spindle speed and feed rate apply to the spindle or the driven tool.
4.7 Drilling Cycles Tapping, axial/radial Call the drilling menu. Select the "Tapping, axial" cycle. Select the "Tapping, radial" cycle. With this cycle, you can tap a thread on the face / lateral surface of a workpiece. Meaning of "retraction length L": Use this parameter for floating tap holders. The cycle calculates a new nominal pitch on the basis of the thread depth, the programmed pitch, and the "retract length." The nominal pitch is somewhat smaller than the pitch of the tap.
4.7 Drilling Cycles Cycle run 1 2 Position spindle to "spindle angle C" (in Manual mode, machining starts from the current spindle angle). If defined, move at rapid traverse to Z1 (axial). X1 (radial). 3 Tap thread to End point Z2 (axial). End point X2 (radial). 4 If X1/Z1 has been defined, retract at return speed SR to Starting point of hole Z1 (axial). Starting point of hole X1 (radial). If X1/Z1 has not not been defined, retract to Starting point Z (axial).
4.7 Drilling Cycles Thread milling, axial Call the drilling menu. Select the "Thread milling, axial" cycle. The cycle mills a thread in existing holes. Use threading tools for this cycle. Danger of collision! Be sure to consider the hole diameter and the diameter of the milling cutter when programming "approaching radius R.
4.7 Drilling Cycles Cycle run 1 2 3 4 5 Position spindle to "spindle angle C" (in Manual mode, machining starts from the current spindle angle). Position the tool to "milling floor Z2" inside the hole. Approach on "approach arc R." Mill the thread in a rotation of 360°, while advancing by "thread pitch F1." Retract the tool and return it to the starting point.
4.7 Drilling Cycles Examples of drilling cycles Centric drilling and tapping The machining operation is to be performed in two steps. In the first step, the "Drilling, axial" cycle drills the hole. In the second, the "Tapping, axial" cycle taps the thread. The drill is positioned at the safety clearance to the workpiece surface (starting point X, Z). The hole starting point Z1 is therefore not programmed. In the parameters "AB" and "V," you program a feed reduction (see figure at upper right).
4.7 Drilling Cycles Deep-hole drilling A hole is to be bored through the workpiece outside the turning center with the cycle "Deep-hole drilling, axial." This machining operation requires a traversable spindle and driven tools. The parameters “1st hole depth P” and “hole depth reduction value IB” define the individual passes and the “minimum hole depth JB” limits the hole reduction value.
4.8 Milling Cycles 4.8 Milling Cycles Milling cycles for axial and radial slots, contours, pockets, surfaces and polygons. For pattern machining, see “Drilling/ Milling Patterns” on page 227. In Teach-in mode these cycles include the activation/ deactivation of the C axis and the positioning of the spindle. In Manual mode you can activate the C axis with "Rapid traverse positioning" and position the spindle before the actual milling cycle. The milling cycles then automatically deactivate the C axis.
4.8 Milling Cycles Rapid traverse positioning Call the milling menu. Select the "Rapid traverse positioning" cycle. The cycle activates the C axis and positions the spindle (C axis) and the tool. "Rapid traverse positioning" is only required in Manual mode. The C axis is deactivated by a subsequent manual milling cycle. Cycle parameters X2, Z2 target point C2 end angle (C-axis position)—default: Current spindle angle Cycle run 1 2 3 Activate C axis. Position to end angle C2 at rapid traverse.
4.8 Milling Cycles Slot, axial Call the milling menu. Select the "Slot, axial" cycle. This cycle mills a slot on the face of the workpiece. The slot width equals the diameter of the milling cutter.
4.8 Milling Cycles Figure, axial Call the milling menu. Select the "Figure, axial" cycle. Depending on the parameters, the cycle mills one of the following contours or roughs/finishes a pocket on the face: Rectangle (Q=4, L<>B) Square (Q=4, L=B) Circle (Q=0, RE>0, L and B: No input) Triangle or polygon (Q=3 or Q>4, L>0) Notes on parameters/functions: Machining of contour or pocket: defined in "U.
4.
4.
4.8 Milling Cycles Cycle run 1 2 Activate the C axis and position to spindle angle C at rapid traverse (only in Teach-in mode). Calculate the proportioning of cuts (infeeds to the milling planes, infeeds in the milling planes). Contour milling: 3 4 5 6 7 Depending on "R," approach the workpiece and plunge to the first milling plane. Mill the first plane. Plunge to the next milling plane. Repeat 5 to 6 until the milling depth is reached. Position to starting point Z and deactivate C axis.
4.8 Milling Cycles ICP contour, axial Call the milling menu. Select "ICP contour, axial." Depending on the parameters, the cycle mills a contour or roughs/ finishes a pocket on the face. Notes on parameters/functions: Machining of contour or pocket: defined in "U." Milling direction: depends on definition in "H" and the direction of tool rotation (see “Cutting direction for contour milling and pocket milling” on page 224).
4.
4.8 Milling Cycles Cycle run 1 2 Activate the C axis and position to spindle angle C at rapid traverse (only in Teach-in mode). Calculate the proportioning of cuts (infeeds to the milling planes, infeeds in the milling planes). Contour milling: 3 4 5 6 7 Depending on "R," approach the workpiece and plunge to the first milling plane. Mill the first plane. Plunge to the next milling plane. Repeat 5 to 6 until the milling depth is reached. Position to starting point Z and deactivate C axis.
4.8 Milling Cycles Face milling Call the milling menu. Select the "Face milling" cycle. Depending on the parameters, the cycle mills the following contours on the face.
4.
4.
4.8 Milling Cycles Cycle run 1 2 3 Activate the C axis and position to spindle angle C at rapid traverse (only in Teach-in mode). Calculate the proportioning of cuts (infeeds to the milling planes, infeeds in the milling planes). Move to the safety clearance and plunge to the first milling plane. Roughing 4 5 6 7 Machine the milling plane, taking "J" (unidirectional or bidirectional) into account. Plunge to the next milling plane. Repeat 4 to 5 until the milling depth is reached.
4.8 Milling Cycles Slot, radial Call the milling menu. Select the "Slot, radial" cycle. This cycle mills a slot on the lateral surface. The slot width equals the diameter of the milling cutter.
4.8 Milling Cycles Figure, radial Call the milling menu. Select the "Figure, radial" cycle. Depending on the parameters, the cycle mills one of the following contours or roughs/finishes a pocket on the lateral surface: Rectangle (Q=4, L<>B) Square (Q=4, L=B) Circle (Q=0, RE>0, L and B: No input) Triangle or polygon (Q=3 or Q>4, L>0) Notes on parameters/functions: Machining of contour or pocket: defined in "U.
4.
4.
4.8 Milling Cycles Cycle run 1 2 Activate the C axis and position to spindle angle C at rapid traverse (only in Teach-in mode). Calculate the proportioning of cuts (infeeds to the milling planes, infeeds in the milling planes). Contour milling: 3 4 5 6 7 Depending on "Approaching radius R," approach the workpiece and plunge to the first milling plane. Mill the first plane. Plunge to the next milling plane. Repeat 5 to 6 until the milling depth is reached.
4.8 Milling Cycles ICP contour, radial Call the milling menu. Select "ICP contour, radial." Depending on the parameters, the cycle mills a contour or roughs/ finishes a pocket on the lateral surface. Notes on parameters/functions: Machining of contour or pocket: defined in "U." Milling direction: depends on definition in "H" and the direction of tool rotation (see “Cutting direction for contour milling and pocket milling” on page 224).
4.
4.8 Milling Cycles Cycle run 1 2 Activate the C axis and position to spindle angle C at rapid traverse (only in Teach-in mode). Calculate the proportioning of cuts (infeeds to the milling planes, infeeds in the milling planes). Contour milling: 3 4 5 6 7 Depending on "R," approach the workpiece and plunge to the first milling plane. Mill the first plane. Plunge to the next milling plane. Repeat 5 to 6 until the milling depth is reached. Position to starting point Z and deactivate C axis.
4.8 Milling Cycles Helical-slot milling, radial Call the milling menu. Select the "Helical-slot milling, radial" cycle. The cycle mills a helical slot from Z1 to Z2. Starting angle C1 defines the starting position for the slot. The slot width equals the diameter of the milling cutter.
4.
Direction of tool rotation TRC Left (J=3) Climb milling (H=1) Mx03 Left Right (J=3) Climb milling (H=1) Mx04 Right Milling direction for pocket milling Machining Cutting direction operation Machining direction Direction of tool rotation Roughing Up-cut milling (H=0) From inside towards outside (J=0) Mx03 Finishing Up-cut milling (H=0) — Mx03 Roughing Up-cut milling (H=0) From inside towards outside (J=0) Mx04 Finishing Up-cut milling (H=0) — Mx04 Roughing Climb milling (H=0) F
4.8 Milling Cycles Examples of milling cycles Milling on the face In this example, a pocket is milled. The milling example in "9.8 ICP Example, Milling Cycle" illustrates the complete machining process on the face, including contour definition. The machining process is performed with the cycle "ICP contour, axial." To describe a contour, define the basic contour first. Then superimpose the rounding arcs.
4.9 Drilling/Milling Patterns 4.9 Drilling/Milling Patterns Note on using drilling/milling patterns: Drilling patterns: MANUALplus generates the machine commands M12, M13 (apply/release block brake) under the following conditions: the drill/tap must be entered as driven tool (parameter "Driven tool H") and the "direction of rotation MD" must be defined.
4.9 Drilling/Milling Patterns Drilling/milling pattern linear, axial Drilling pattern linear, axial Call the drilling menu. Select "Drilling axial " (see figure at upper right). Select "Deep-hole drilling, axial " (see figure at center right). Select "Tapping, axial " (see figure at lower right). Press the Pattern linear soft key. Milling pattern linear, axial Call the milling menu. Select "Slot axial " (see figure at top of next page). Select "ICP contour, axial" (see middle figure on next page).
4.
4.9 Drilling/Milling Patterns Drilling/milling pattern circular, axial Drilling pattern circular, axial Call the drilling menu. Select "Drilling axial " (see figure at upper right). Select "Deep-hole drilling, axial " (see figure at center right). Select "Tapping, axial " (see figure at lower right). Press the Pattern circular soft key. Milling pattern circular, axial Call the milling menu. Select "Slot axial " (see figure at top of next page).
4.9 Drilling/Milling Patterns Cycle parameters X, Z starting point C spindle angle (C-axis position)—default: Current spindle angle XM, CM pattern center: Position, angle (polar coordinates) XK, YK pattern center (Cartesian coordinates) K/KD pattern diameter—default: Starting point X is the pattern diameter A angle of 1st hole/slot—default: 0° Wi angle increment (pattern spacing)—default: Holes, slots, etc.
4.9 Drilling/Milling Patterns Drilling/milling pattern linear, radial Drilling pattern linear, radial Call the drilling menu. Select "Drilling, radial " (see figure at upper right). Select "Deep-hole drilling, radial " (see figure at center right). Select "Tapping, radial " (see figure at lower right). Press the Pattern linear soft key. Milling pattern linear, radial Call the milling menu. Select "Slot radial" (see figure at top of next page).
4.9 Drilling/Milling Patterns Cycle parameters X, Z starting point C spindle angle (C-axis position)—default: Current spindle angle Z1 starting point of pattern: Position of 1st hole/slot (polar coordinates) C1 angle of 1st hole/slot: Starting angle (polar coordinates) ZE end point of pattern—default: Z1 Wi angle increment (pattern spacing)—default: Holes, slots, etc. are arranged at a regular spacing on the circumference.
4.9 Drilling/Milling Patterns Drilling/milling pattern circular, radial Drilling pattern circular, radial Call the drilling menu. Select "Drilling, radial " (see figure at upper right). Select "Deep-hole drilling, radial " (see figure at center right). Select "Tapping, radial " (see figure at lower right). Press the Pattern circular soft key. Milling pattern circular, radial Call the milling menu. Select "Slot radial" (see figure at top of next page).
4.9 Drilling/Milling Patterns Cycle parameters X, Z starting point C spindle angle (C-axis position)—default: Current spindle angle ZM, CM pattern center: Position, angle (polar coordinates) K/KD pattern diameter—default: Starting point X is the pattern diameter A angle of 1st hole/slot—default: 0° Wi angle increment (pattern spacing)—default: Holes, slots, etc.
4.9 Drilling/Milling Patterns Examples of pattern machining Linear hole pattern on face A linear hole pattern is to be machined on the face of the workpiece with the "Drilling, axial" cycle. This machining operation requires a traversable spindle and driven tools. The pattern is programmed by entering the coordinates of the first and last hole, and the number of holes (see figure at upper right). Only the depth is indicated for the drilling cycle (see figure at lower right).
4.9 Drilling/Milling Patterns Circular hole pattern on face A circular hole pattern is to be machined on the face of the workpiece with the "Drilling, axial" cycle. This machining operation requires a traversable spindle and driven tools. The pattern center point is entered in Cartesian coordinates (see figure at top right).
4.9 Drilling/Milling Patterns Linear hole pattern on lateral surface A linear hole pattern is to be machined on the lateral surface of the workpiece with the "Drilling, axial" cycle. This machining operation requires a traversable spindle and driven tools. The drilling pattern is defined by the coordinates of the first hole, the number of holes, and the spacing between the holes (see figure to the upper right). Only the depth is indicated for the drilling cycle (see figure at lower right).
4.10 DIN Cycles 4.10 DIN Cycles „Select "DIN cycle." This function allows you to select a DIN cycle (DIN macro) and integrate it in a MANUALplus cycle program. The machine data that are programmed in the DIN cycle (in Manual mode, the currently active machine data) become effective as soon as you start the DIN macro. You can change the machine data (T, S, F) at any time by editing the DIN macro.
ICP Programming
5.1 ICP Contours 5.1 ICP Contours The Interactive Contour Programming (ICP) feature provides graphic support when you are defining the workpiece contours for ICP cycles. (ICP is the abbreviation of "Interactive Contour Programming".) The contours are defined using linear and circular contour elements as well as form elements like chamfers, roundings, and undercuts. For lathes used in the machining of ICP contours, you need to define the tool angle and point angle.
5.2 Editing ICP Contours 5.2 Editing ICP Contours An ICP contour consists of definitions of the individual contour elements it is made up of. Each ICP contour is clearly identified by its number and a short description. ICP contours are integrated in ICP cycles. You program an ICP contour by entering the individual contour elements one after the other in the correct sequence. The starting point is defined when you describe the first contour element.
5.2 Editing ICP Contours Programming and adding to ICP contours After selecting a contour element, you enter the known parameters. MANUALplus automatically calculates parameters that have not been defined from the adjoining contour elements. You can usually program the contour elements with the dimensions given in the production drawing. You can toggle between the lines and arcs menus by soft key. Form elements (chamfers, roundings, and undercuts) are selected with the menu key.
A transition between two contour elements is called "tangential" when one contour element makes a smooth and continuous transition to the next. There is no visible kink or corner at the intersection. With geometrically complex contours, tangential transitions are useful for reducing the input of dimensional data to a minimum and eliminating the possibility of mathematically contradictory entries.
5.2 Editing ICP Contours Contour graphics As soon as you have entered a contour element, MANUALplus checks whether the element is "solved" or "unsolved." A "solved" element is a contour element that is fully and unambiguously defined. It is drawn immediately. "Unsolved" contour element: has not yet been fully defined. MANUALplus shows a symbol below the graphics window, which reflects the element type and the line direction / direction of rotation.
5.2 Editing ICP Contours Changing the ICP contour graphics MANUALplus selects the area to be represented such that all entered contour elements are displayed. You can magnify/reduce the displayed graphics with the PgUp/PgDn keys, and pan the detail with the arrow keys. These functions are available when the contour is displayed but is not being edited.
5.2 Editing ICP Contours Selection of solutions If the entered data permit several possible solutions, you can inspect the mathematically possible solutions with Next solution / Continue solution and confirm the correct solution with Select solution (see figures at right). If the contour still contains unsolved contour elements when you exit the editing mode, MANUALplus will ask you whether to cancel these elements.
5.2 Editing ICP Contours Contour direction The cutting direction depends on the direction of the contour. If the contour is described in the negative Z-axis direction, the control uses a longitudinal cycle (see figure to the upper right). If the contour is described in the negative X-axis direction, the control uses a transverse cycle (see figure at center right). ICP cut, longitudinal/transverse (roughing) MANUALplus machines the workpiece in the contour direction.
5.3 Importing of DXF Contours 5.3 Importing of DXF Contours Fundamentals Contours available in DXF format can be imported into the ICP editor. DXF contours describe contour trains for ICP cycles (recessing, cutting and milling cycles). For contour trains for recessing and cutting cycles, DXF layers should contain only one contour. For contours for milling cycles multiple DXF contours can be contained and imported. DXF import is available as of software versions 507 807-11 and 526 488-03.
5.3 Importing of DXF Contours DXF import The ICP editor offers the DXF import during the contour entry phase. DXF import Press Edit ICP. Press Insert element. Press DXF Import. Select the file with the DXF contour(s). Press Next contour or Previous contour to select the DXF layer. Press Assume contour. The ICP editor loads the selected DXF contour and converts it to ICP format.
5.3 Importing of DXF Contours Configuring the DXF import After you have selected a file with DXF contours, you can adapt the parameters for configuring the DXF import. Adapting the DXF parameters Press DXF parameters. The MANUALplus opens the “DXF parameters” dialog box. Enter the DXF parameters (see the meanings below). Press Save. The MANUALplus assumes the parameters. Setting the DXF parameters to standard values Call the DXF parameters dialog box. Press Reset.
5.3 Importing of DXF Contours Maximum distance: The DXF import sets the starting point to one of the two contour points farthest apart from each other. The program automatically determines which of these points is the starting point. It is not possible to influence this decision. Marked point: If one of the contour points in the DXF drawing is marked with a complete circle, then this point is specified as the starting point. The contour point must be at the center of the complete circle.
5.4 Programming Changes to ICP Contours 5.4 Programming Changes to ICP Contours You can edit existing contours by: Editing contour elements Deleting contour elements Extending the contour (adding to the contour) Editing individual contour sections Superimposing form elements (refining the contour) Editing a contour element Editing a contour element Press Change element—a contour element is marked "selected" (highlighted in color). Select the contour element to be edited.
5.4 Programming Changes to ICP Contours Editing an unsolved contour element If a contour contains "unsolved" contour elements, the "solved" elements cannot be changed. You can, however, set or delete the "tangential transition" for the contour element located directly before the unsolved contour area. If the element to be edited is an unsolved element, the associated symbol is marked "selected." The element type and the direction of rotation of a circular arc cannot be changed.
5.4 Programming Changes to ICP Contours Shifting a contour You can shift a contour if it is not at the desired position. Select a suitable contour element (reference element). For shifting you enter the new position of the starting point of the reference element. The entire contour is shifted when function is completed. Shifting a contour Press Change element—a contour element is marked "selected" (highlighted in color). Select the reference element Press Shift contour.
5.4 Programming Changes to ICP Contours Adding a contour element Adding a contour element Press Insert element. "Append" additional contour elements to the existing contour. Deleting a contour element Deleting a contour element Press Delete element—a contour element is marked "selected" (highlighted in color). Select the contour element to be deleted. Delete the contour element. You can delete several successive contour elements.
5.4 Programming Changes to ICP Contours "Splitting" a contour If you delete a contour element which is located between preceding and subsequent elements, the contour is split into a basic contour and a remaining contour (see figure at upper right). The remaining contour cannot be edited—you can, however, change the basic contour and "link" it to the remaining contour. This is usually done by inserting new contour elements.
5.4 Programming Changes to ICP Contours Superimposing form elements When superimposing form elements, select the corner to be superimposed and then insert the desired form element. Superimposing form elements Press Superimpose form elements. Select the corner to be changed. Select the desired form element. Define the form element. Superimposing on contours with "unsolved" contour areas You can superimpose form elements even if the contour still contains unsolved contour areas.
5.5 ICP Contour Elements, Turning Contour 5.5 ICP Contour Elements, Turning Contour Entering lines, turning contour Use the menu symbol to select the direction of the contour element and assign it a dimension. When defining horizontal and vertical linear elements, it is not necessary to enter the X and Z coordinates, respectively. MANUALplus inhibits the corresponding input field if no unsolved elements exist. Vertical/horizontal lines Select the line direction.
5.5 ICP Contour Elements, Turning Contour Line at angle Select the line direction. You enter absolute or polar dimensions for the line and then define the transition to the next contour element. The direction of the angle is shown in the graphic support window.
5.5 ICP Contour Elements, Turning Contour Entering circular arcs, turning contour Select direction of rotation and type of dimensioning Arc with center and radius Arc with radius Arc with center You enter the dimensions of the arc and then define the transition to the next contour element. Parameters (for "Arc with radius," the center is not requested. For "Arc with center point," the radius is not requested.
5.5 ICP Contour Elements, Turning Contour Entering form elements Chamfer/rounding Chamfers/roundings are defined on contour corners. A "contour corner" is the point of intersection between the approaching and departing contour elements. MANUALplus cannot calculate a chamfer or rounding until the departing contour element is known. During the parameter input for the chamfer/rounding, the coordinates of the corner are shown in "starting point XS, ZS.
5.5 ICP Contour Elements, Turning Contour Chamfer/rounding, turning contour Chamfer Select form elements or chamfer/rounding. Choose chamfer. Choose rounding. The corner is predefined by the starting point. You need only enter the "chamfer width B" or "rounding radius B.
5.5 ICP Contour Elements, Turning Contour Undercuts, turning contour Thread undercut DIN 76 Select form elements. Select thread undercut DIN 76. For thread undercut DIN 76, the diameter of the longitudinal element represents the thread diameter (or, with internal threads, the core diameter).
5.5 ICP Contour Elements, Turning Contour Undercut DIN 509 E Select form elements. Select undercut DIN 509 E.
5.5 ICP Contour Elements, Turning Contour Undercut DIN 509 F Select form elements. Select undercut DIN 509 F.
5.6 ICP Contour Elements on the Face 5.6 ICP Contour Elements on the Face Enter the dimensions of the contour elements on face and lateral surface in Cartesian or polar values. You must pay attention to the setting of the Polar soft key. MANUALplus distinguishes Cartesian coordinates from polar coordinates by different address letters.
5.6 ICP Contour Elements on the Face Entering lines on the face Vertical/horizontal lines Select the line direction. You enter the dimensions of the line and then define the transition to the next contour element. Parameters XS, YS starting point (Cartesian coordinates) XD, CS starting point (polar coordinates) XK, YK target point (Cartesian coordinates) X, C target point (polar coordinates) L length of line F special feed Line at angle Select the line direction.
5.6 ICP Contour Elements on the Face Entering circular arcs on the face Entering an arc Arc with center and radius Arc with radius Arc with center You enter the dimensions of the arc and then define the transition to the next contour element. Parameters (for "Arc with radius," the center is not requested. For "Arc with center point," the radius is not requested.
5.6 ICP Contour Elements on the Face Entering chamfers/roundings on the face Entering a chamfer/rounding Select chamfer/rounding. Choose chamfer. Choose rounding. The corner is predefined by the starting point. You need only enter the "chamfer width B" or "rounding radius B.
5.7 ICP Contour Elements on the Lateral Surface 5.7 ICP Contour Elements on the Lateral Surface You can use the linear dimension as an alternative to the angular dimension. The setting of the Polar soft key determines which type of dimensioning is active. MANUALplus distinguishes angular dimensions from linear dimensions by different address letters.
5.7 ICP Contour Elements on the Lateral Surface Entering lines on the lateral surface Vertical/horizontal lines Select the line direction. You enter the dimensions of the line and then define the transition to the next contour element.
5.7 ICP Contour Elements on the Lateral Surface Entering circular arcs on the lateral surface Entering an arc Arc with center and radius Arc with radius Arc with center You enter the dimensions of the arc and then define the transition to the next contour element. Parameters (for "Arc with radius," the center is not requested. For "Arc with center point," the radius is not requested.
5.7 ICP Contour Elements on the Lateral Surface Entering chamfers/roundings on the lateral surface Entering chamfers/roundings Select chamfer/rounding. Choose chamfer. Choose rounding. The corner is predefined by the starting point. You need only enter the "chamfer width B" or "rounding radius B.
DIN Programming HEIDENHAIN MANUALplus 4110 277
6.1 DIN Programming 6.1 DIN Programming The structure of programs and program blocks follows the standard DIN 66025 (ISO 6983) and is therefore called "DIN programming." MANUALplus supports DIN programs and DIN macros. DIN programs are independent NC programs. In other words, they contain all traversing and switching commands that are necessary for producing the desired workpiece. DIN macros are integrated into cycle programs.
6.1 DIN Programming Program and block structure Program structure Program number, starting with the character "%" followed by up to eight characters and the extension "nc" for main programs or "ncs" for subprograms. Program designation (definition in the second program line). NC blocks or comment blocks. The term "END" with main programs or "RETURN" with macros and subprograms. The first and last lines of an NC program cannot be edited. The program designation can be edited, but not deleted.
6.1 DIN Programming Overview of DIN commands Traversing commands For moving the slide on a linear or circular path. Cycles For roughing, recessing, finishing, threading, and drilling. Switching commands For machine components. Zero point shifts For adjusting the dimensional system. Commands for program organization Program branches, program repeats and subprograms. Comments For explaining the program.
6.2 Editing DIN Programs 6.2 Editing DIN Programs Loading the desired DIN program Call the DIN editor. Call the program list. Select DIN programs. Select DIN macros. Select a DIN program / DIN macro or define a new program number. Call the DIN program / DIN macro. Block functions With the arrow keys and paging keys, you move the cursor within the DIN program to the position you wish to delete, change or add to. Place the cursor at the beginning of a block, NC word, or parameter.
6.2 Editing DIN Programs Changing block numbers Position the cursor on the NC block. Press Change block no. Enter the new block number. Transfer the new block number. Renumbering blocks Position the cursor on any NC block. Press Change block no. Press Renumber. Define the block number increment. Press Renumber again. The block number increment you defined is also effective for automatic block numbering.
The functions ("Delete word," "Change word," etc.) refer to the "word" at which the cursor is located. What is actually deleted or changed depends on the meaning of the "word." Examples: The cursor is located on a G command. Change word: First the command and then the associated parameters can be edited. Delete word: The command and the associated parameters are deleted. The cursor is located on an address letter of a parameter. Change word: All parameters of the function can be edited.
6.2 Editing DIN Programs Comments If you enter a comment in an empty block, the block number is deleted and only the comment is stored in this block. (An "empty block" is a block that consists of the block number only.) If the NC block already contains NC commands, the comment is appended to the end of the block. To change comments, place the cursor at the beginning of the comment and press Change word. MANUALplus then displays the "alphanumeric keyboard" and the current text of the comment.
6.2 Editing DIN Programs Block functions Mark several successive NC blocks (block sequence) to be able to cut, copy or delete them. If you cut or copy the block sequence, it is taken into the clipboard. You can then insert this block sequence at a different position in the program, or call a different DIN program and insert the block sequence there. The block sequence remains stored in the clipboard until it is overwritten or MANUALplus is switched off.
6.2 Editing DIN Programs Menu structure Select the function group by menu key. G and M functions: The function number and further parameters that vary depending on the function are entered subsequently. Comment, subprogram and T, S, F: The required parameters are entered subsequently. Variable functions: MANUALplus switches to other menus for entering further data. DIN functions Menu key G function Traversing commands, cycles, and other G commands.
6.2 Editing DIN Programs Programming G functions Direct programming of a G function Select "G function." Enter the G number. Call the G function. Enter the parameters. Transfer the G function. If you do not know the number of the G function, you can select it from the list of G functions. Selecting a G function Select "G function." Call the "G function list." Select the G function. Transfer the G function. Call the G functions. Enter the parameters. Transfer the G function.
6.3 Definition of Workpiece Blank 6.3 Definition of Workpiece Blank Chuck part, cylinder/tube G20 G20 describes the workpiece blank and the setup used. This information is evaluated during the simulation. Parameters X diameter Z length (including transverse allowance and clamping range) K right edge (transverse allowance) I inside diameter for workpiece blank "tube" B clamping range J type of clamping 0: Not clamped 1: Externally clamped 2: Internally clamped Example: G20 %20.
6.3 Definition of Workpiece Blank Workpiece blank contour G21 G21 describes the setup used. The workpiece blank is described with G1, G2, G3, G12 and G13 commands that follow immediately after G21. G80 concludes the contour description. This information is evaluated during the simulation. Parameters X diameter Z length B clamping range J type of clamping 0: Not clamped 1: Externally clamped 2: Internally clamped Example: G21 %21.
6.4 Tool Positioning without Machining 6.4 Tool Positioning without Machining Rapid traverse G0 Geometry command: G0 defines the starting point of contour definition. Machining command: The tool moves at rapid traverse along the shortest path to the target point X, Z. Rapid traverse paths can be executed when the spindle is stationary. Parameters X target point (diameter value) Z target point Example: G0 %0.nc [G0] N1 T3 G95 F0.25 G96 S200 M3 N2 G0 X120 Z2 N3 G819 P5 I1 K0.
6.4 Tool Positioning without Machining Tool change point G14 The slide moves at rapid traverse to the tool change position. In setup mode, define permanent coordinates for the tool change point (see “Defining the tool change position” on page 52). Parameters Q sequence (default: 0): Determines the sequence of traverse.
6.5 Simple Linear and Circular Movements 6.5 Simple Linear and Circular Movements Linear path G1 Geometry command: G1 defines a linear segment in a contour. Machining command: The tool moves on a linear path at feed rate to the end point X, Z. Parameters X end point (diameter value) Z end point A angle—for angle direction, see graphic support window. B chamfer/rounding: At the end of the linear path you can program a chamfer/rounding or a tangential transition to the next contour element.
6.5 Simple Linear and Circular Movements Circular path G2, G3—incremental center coordinates Geometry command: G2/G3 defines a circular arc in a contour. Machining command: The tool moves on a circular arc at feed rate to the end point. The direction of rotation is shown in the graphic support window.
6.5 Simple Linear and Circular Movements Parameters G2, G3 Example: G2, G3 X end point (diameter value) Z end point R radius I center point incremental—(distance from starting point to center point; diameter value) K center point incremental—(distance from starting point to center point) Q point of intersection (default: Q=0): Specifies the end point if two solutions are possible (see graphic support window).
6.5 Simple Linear and Circular Movements Circular path G12, G13—absolute center coordinates Geometry command: G12/G13 defines a circular arc in a contour. Machining command: The tool moves on a circular arc at feed rate to the end point. The direction of rotation is shown in the graphic support window.
6.5 Simple Linear and Circular Movements Parameters G12, G13 X end point (diameter value) Z end point R radius I center point absolute—(diameter value) K center point absolute Q point of intersection (default: Q=0): Specifies the end point if two solutions are possible (see graphic support window). B chamfer/rounding: At the end of the circular arc you can program a chamfer/rounding or a tangential transition to the next contour element.
6.6 Feed Rate and Spindle Speed 6.6 Feed Rate and Spindle Speed Speed limitation G26/G126 Example: G26, G126 G26: Speed limitation for spindle G126: Speed limitation for spindle 1 (driven tool) %26.nc [G26, G126] The speed limit remains in effect until a new value is programmed for G26/G126. N1 G14 Q0 Parameters N2 T3 G95 F0.25 G96 S200 M3 N3 G0 X0 Z2 S speed: Maximum speed The speed limitation remains in effect even after concluding the DIN program and exiting "Program run" mode.
6.6 Feed Rate and Spindle Speed Feed per tooth G193 G193 defines the feed rate with respect to the number of teeth of the cutter. Parameters F feed per tooth in mm/tooth or inch/tooth The actual value display shows the feed rate in mm/rev. Example: G193 %193.nc [G193] N1 M5 N2 T71 G197 S1010 G193 F0.08 M104 N3 M14 N4 G152 C30 N5 G110 C0 N6 G0 X122 Z-50 N7 G744 X122 Z-50 ZE-50 C0 Wi90 Q4 N8 G792 K30 A0 X100 J11 P5 F0.
6.6 Feed Rate and Spindle Speed Constant cutting speed G96/G196 G96/G196 defines a constant cutting speed. Example: G96, G196 G96: The speed of the spindle depends on the X position of the tool tip. %96.nc G196: The spindle speed depends on the diameter of the tool. N1 T3 G195 F0.25 G196 S200 M3 [G96, G196] N2 G0 X0 Z2 Parameters S cutting speed in m/min or ft/min N3 G42 N4 G1 Z0 N5 G1 X20 B-0.5 N6 G1 Z-12 N7 G1 Z-24 A20 N8 G1 X48 B6 N9 G1 Z-52 B8 N10 G1 X80 B4 E0.
6.7 Tool-Tip / Milling-Cutter Radius Compensation 6.7 Tool-Tip / Milling-Cutter Radius Compensation Fundamentals Tool-tip radius compensation (TRC) If TRC is not used, the theoretical tool tip is the reference point for the paths of traverse. This might lead to inaccuracies when the tool moves along non-paraxial paths of traverse. The TRC function corrects programmed paths of traverse (see “Tool-tip radius compensation (TRC)” on page 28).
6.7 Tool-Tip / Milling-Cutter Radius Compensation G40: Switch off TRC/MCRC The TRC/MCRC remains in effect until a block with G40 is reached. The block containing G40, or the block after G40 only permits a linear path of traverse (G14 is not permissible). G41/G42: Switch on TRC/MCRC A straight line segment (G0/G1) must be programmed in the block containing G41/G42 or after the block containing G41/G42. The TRC/MCRC is taken into account from the next path of traverse.
6.8 Compensation Values 6.8 Compensation Values (Changing the) cutter compensation G148 MANUALplus manages three wear compensation values for recessing tools (DX, DZ, and DS). The parameter "O" allows you to define which wear compensation values are to be taken into account. DX, DZ become effective after program start and after a T command (G148 O0). The compensation values defined with G148 remain in effect until the next T command or the end of the program.
6.8 Compensation Values Additive compensation G149 MANUALplus manages 16 tool-independent compensation values, which are assigned the designations D901 to D916. These compensation values are added to the active wear compensation values of the tools.
6.8 Compensation Values Compensation of right-hand tool nose G150 Compensation of left-hand tool nose G151 With recessing tools, the "tool orientation" function defines whether the tool reference point is set at the left or the right side of the tool tip (see “Recessing and recess-turning tools” on page 421). G150/G151 switches the reference point. Example: G150, G151 %148.nc [G148] G150: Reference point on right tip N1 T31 G95 F0.
6.9 Zero Point Shifts 6.9 Zero Point Shifts Zero point shift G51 G51 shifts the workpiece zero point by "Z" (or "X"). The shift is referenced to the workpiece zero point defined in setup mode (see “Defining the workpiece zero point” on page 50). Even if you shift the zero point several times with G51, it is still always referenced to the workpiece zero point defined in setup mode.
6.9 Zero Point Shifts Additive zero point shift G56 G56 shifts the workpiece zero point by "Z" (or "X"). The shift is referenced to the currently active workpiece zero point. If you shift the workpiece zero point more than once with G56, the shift is always added to the currently active zero point. Parameters X shift (diameter value) Z shift G51 or G59 cancel additive zero point shifts. Danger of collision! Cycle programming: With DIN macros, the zero point shift is reset at the end of the cycle.
6.9 Zero Point Shifts Absolute zero point shift G59 G59 sets the workpiece zero point to the position "X, Z." The new zero point remains in effect to the end of the program. Parameters X zero point shift (diameter value) Z zero point shift G59 cancels all previous zero point shifts (with G51, G56 or G59). Danger of collision! Cycle programming: With DIN macros, the zero point shift is reset at the end of the cycle. Therefore, do not use any DIN macros with zero point shifts in cycle programming.
6.10 Oversizes 6.10 Oversizes Axis-parallel oversize G57 G57 defines different oversizes for X and Z. G57 is programmed before the recessing or roughing cycle. Parameters X oversize X (diameter value) Z oversize Z The following cycles take the oversizes into account: Roughing cycles: G81, G817, G818, G819, G82, G827, G828, G829, G83 Recessing cycles: G86x Recess turning cycles: G81x, G82x The cycles G81, G82 and G83 do not cancel the oversizes after execution of the cycle.
6.10 Oversizes Contour-parallel oversize (equidistant) G58 G58 defines a contour-parallel oversize. G58 is programmed before recessing or roughing cycles. Parameters P oversize A negative oversize is permitted with the cycle G89. The following cycles take the oversizes into account: Roughing cycles: G817, G818, G819, G827, G828, G829, G83 Recessing cycles: G86x Recess turning cycles: G81x, G82x The cycle G83 does not cancel the oversizes after execution of the cycle.
6.11 Contour-Based Turning Cycles 6.11 Contour-Based Turning Cycles Contour definition For contour-based cycles (turning / recessing / recess turning cycles), the cycle call is followed by the contour definition: G0 defines the starting point of the contour section. The contour section is described with G1, G2, G3, G12 and G13 commands. G80 concludes the contour definition. End of cycle G80 G80 concludes the contour definition after roughing, recessing and undercut cycles.
6.11 Contour-Based Turning Cycles Longitudinal contour roughing G817/G818 The cycles machine the contour area described by the current tool position and the data defined in the subsequent blocks in longitudinal direction without recessing (see “Contour definition” on page 310). Parameters G817, G818 X cutting limit (diameter value): The control machines up to the cutting limit.
6.11 Contour-Based Turning Cycles Note on the execution of the cycle: MANUALplus automatically determines the cutting and infeed directions from the current tool position relative to the starting point / end point of the contour area. Tool position at the end of the cycle: G817: Cycle starting point Z; last retraction diameter X G818: Cycle starting point Descending contour elements are not machined. The tool must be located outside the defined contour area.
6.11 Contour-Based Turning Cycles Longitudinal contour roughing with recessing G819 The cycle machines the contour area described by the current tool position and the data defined in the subsequent blocks in a longitudinal direction with recessing (see “Contour definition” on page 310). Parameters X cutting limit (diameter value): The control machines up to the cutting limit.
6.11 Contour-Based Turning Cycles Transverse contour roughing G827/G828 The cycle machines the contour area described by the current tool position and the data defined in the subsequent blocks in transverse direction without recessing (see “Contour definition” on page 310). Parameters Z cutting limit: The control machines up to the cutting limit. P maximum infeed: The proportioning of cuts is calculated so that an "abrasive cut" is avoided and the infeed distance is <= P.
MANUALplus automatically determines the cutting and infeed directions from the current tool position relative to the starting point / end point of the contour area. Tool position at the end of the cycle: G827: Cycle starting point X; last retraction diameter in Z G828: Cycle starting point Descending contour elements are not machined. The tool must be located outside the defined contour area. Cutting radius compensation: Active.
6.11 Contour-Based Turning Cycles Transverse contour roughing with recessing G829 The cycle machines the contour area described by the current tool position and the data defined in the subsequent blocks in transverse direction with recessing (see “Contour definition” on page 310). Parameters Z cutting limit: The control machines up to the cutting limit. P maximum infeed: The proportioning of cuts is calculated so that an "abrasive cut" is avoided and the infeed distance is <= P.
6.11 Contour-Based Turning Cycles Contour-parallel roughing G836 G836 machines the workpiece sections parallel to the contour. The starting point of the contour is defined either in the cycle with X,Z or in the G0 block after the cycle call. The blocks following G836 describe the contour area. G80 concludes the contour description. Parameters X starting point (diameter value) Z starting point P maximum infeed: The infeed depth is determined taking J into account.
6.11 Contour-Based Turning Cycles Contour finishing G89 G89 finishes the contour area defined in the subsequent blocks (see “Contour definition” on page 310). In the NC block after G89, the tool-tip radius compensation (TRC) is called with G41/G42 (without parameters) and allows you to define the position of the tool (reference: contour direction): G41: Tool moves to the right of the contour. G42: Tool moves to the left of the contour. MANUALplus switches off the TRC at the end of the cycle.
6.12 Simple Turning Cycles 6.12 Simple Turning Cycles Roughing longitudinal G81 G81 machines the contour area defined by the current tool position and "X, Z" in longitudinal direction. Parameters X starting point of contour section (diameter value) Z end point of contour section I maximum infeed in X: The proportioning of cuts is calculated so that an "abrasive cut" is avoided and the calculated infeed distance is <= I.
6.12 Simple Turning Cycles Roughing transverse G82 G82 machines the contour area defined by the current tool position and "Z, X" in transverse direction. Parameters X end point of contour section (diameter value) Z starting point of contour section I offset: Infeed in Z (default: 0) K maximum infeed in X: The proportioning of cuts is calculated so that an "abrasive cut" is avoided and the calculated infeed distance is <= K.
6.12 Simple Turning Cycles Simple contour repeat cycle G83 G83 repeatedly executes the machining cycle programmed in the subsequent blocks. The machining cycle may contain simple traverse paths or cycles (without contour definition). G80 ends the machining cycle. "X, Z" define the starting point of the contour. G83 starts the cycle execution from the current tool position. Before each pass, the tool advances by the infeed distance defined in "I, K.
6.12 Simple Turning Cycles Line with radius G87 G87 machines transition radii at orthogonal, paraxial inside and outside corners. A preceding longitudinal or transverse element is machined if the tool is located at the X or Z coordinate of the corner before the cycle is executed. The radii are machined in one pass. MANUALplus determines the direction of the radius from the "tool orientation" (see “Lathe tools” on page 419).
6.12 Simple Turning Cycles Line with chamfer G88 G88 machines chamfers at orthogonal, paraxial outside corners. A preceding longitudinal or transverse element is machined if the tool is located at the X or Z coordinate of the corner before the cycle is executed. The chamfers are machined in one pass. MANUALplus determines the direction of the chamfer from the "tool orientation" (see “Lathe tools” on page 419).
6.13 Recessing Cycles 6.13 Recessing Cycles Contour recessing axial G861 / radial G862 The cycles machine an axial/radial recess in the contour area described by the current tool position and the data defined in the subsequent blocks (see “Contour definition” on page 310). Parameters P recessing width P is not defined: Infeeds <= 0.
MANUALplus determines the cutting direction from the current tool position relative to the starting point / end point of the contour area. Tool position at the end of the cycle: Cycle starting point Example: G861 6.13 Recessing Cycles Note on the execution of the cycle: %861.nc [G861] N1 T38 G95 F0.15 G96 S200 M3 Cutting radius compensation: Active. G57/G58 oversizes are taken into account if I/K is not programmed. After the cycle has been executed, the oversizes are canceled.
6.13 Recessing Cycles Contour recessing cycle, finishing, axial G863 / radial G864 The cycles axially/radially finish the contour area defined in the subsequent blocks (see “Contour definition” on page 310).
Tool position at the end of the cycle: Cycle starting point Cutting radius compensation: Active. Example: G863 6.13 Recessing Cycles Note on the execution of the cycle: %863.nc [G863] N1 T38 G95 F0.15 G96 S200 M3 N2 G0 X110 Z2 N3 G863 E0.08 N4 G0 X100 Z2 N5 G1 Z-6 B3 N6 G1 X88 B2 N7 G1 Z-13 A-20 B2 N8 G1 X60 B3 N9 G1 Z0 B-1 N10 G1 X55 N11 G80 END Example: G864 %864.nc [G864] N1 T30 G95 F0.15 G96 S200 M3 N2 G0 X87 Z-35 N3 G864 E0.11 N4 G0 X85 Z-29.
6.13 Recessing Cycles Simple recessing cycle, axial G865 / radial G866 The cycles axially/radially machine the rectangle described by the tool position and "X, Z." Parameters X base corner X (diameter value) Z base corner Z P recessing width P is not defined: Infeeds <= 0.
6.13 Recessing Cycles Recessing finishing, axial G867 / radial G868 The cycles axially/radially finish the contour area described by the tool position and "X, Z." Tool position at the end of the cycle: Cycle starting point Parameters X base corner X (diameter value) Z base corner Z E finishing feed (default: Active feed rate) Note on the execution of the cycle: Tool position at the end of the cycle: Cycle starting point Cutting radius compensation: Active. Example: G867 %867.
6.13 Recessing Cycles Simple recessing cycle G86 G86 machines simple radial/axial inside and outside recesses with chamfers. From the "tool orientation," the control determines the type of recess (radial/axial; inside/outside, see “Lathe tools” on page 419). Parameters X base corner X (diameter value) Z base corner Z I oversize Radial recess: Oversize for precutting Axial recess: Recess width—no input: A single cut is machined (recess width = tool width).
6.14 Recess-Turning Cycles 6.14 Recess-Turning Cycles Function of recess turning cycles The defined contour area is machined by alternate recessing and roughing movements. The machining process requires a minimum of retraction and infeed movements. The contour to be machined may contain various valleys. If required, the area to be machined is divided into several sections.
6.14 Recess-Turning Cycles Simple recess-turning cycle, longitudinal G811 / transverse G821 The cycles machine the rectangle described by the tool position and "X, Z." Parameters X base corner X (diameter value) Z base corner Z P maximum infeed: The proportioning of cuts is calculated so that an "abrasive cut" is avoided and the infeed distance is <= P.
6.14 Recess-Turning Cycles Recess-turning cycle, longitudinal G815 / transverse G825 The cycles machine the contour area described by current tool position and the data defined in the subsequent blocks (see “Contour definition” on page 310). Parameters X cutting limit (diameter value) Z cutting limit P maximum infeed: The proportioning of cuts is calculated so that an "abrasive cut" is avoided and the infeed distance is <= P.
6.14 Recess-Turning Cycles Note on the execution of the cycle: Tool position at the end of the cycle: Cycle starting point It is absolutely necessary to define the oversizes I, K for recess turning—finishing (Q=2), since they define the material to be machined during the finishing cycle. Cutting radius compensation: Active. G57/G58 oversizes are taken into account if I/K is not programmed. After the cycle has been executed, the oversizes are canceled. Example: G815 %815.nc [G815] N1 T38 G95 F0.
6.15 Thread Cycles 6.15 Thread Cycles Universal thread cycle G31 G31 cuts threads in any desired direction and position (longitudinal, tapered or transverse threads; internal or external threads). You can also machine successions of threads.
6.15 Thread Cycles G31 with contour definition: "X, Z" is not programmed. G31 is followed by NC blocks defining up to 6 contour elements on which the thread is to be machined. Contour definition is completed with G80. Transverse threads or successive threads are programmed "with contour definition." Internal or external threads: See algebraic sign of "U." The infeeds are calculated on the basis of "V:" V=0: Constant cross section for all cuts. "I" defines the first (maximum) infeed.
6.15 Thread Cycles Single thread G32 G32 cuts a simple thread in any desired direction and position (longitudinal, tapered or transverse thread; internal or external thread). The thread starts at the current tool position and ends at the "end point X, Z.
6.15 Thread Cycles Thread single path G33 G33 cuts threads in any desired direction and position with variable pitch (longitudinal, tapered or transverse threads; internal or external threads). The thread starts at the current tool position and ends at the "end point X, Z.
6.15 Thread Cycles Metric ISO thread G35 G35 cuts a longitudinal thread (internal or external thread). The thread starts at the current tool position and ends at the "end point X, Z." From the tool position relative to the end point of the thread, MANUALplus automatically determines whether an internal or external thread is to be cut.
6.15 Thread Cycles Simple longitudinal single-start thread G350 G350 cuts a longitudinal thread (internal or external thread). The thread starts at the current tool position and ends at the "end point X, Z." Parameters Z end point of thread F thread pitch U thread depth U>0: Internal thread U<=0: External thread (lateral surface or front face) U= +999 or –999: Thread depth is calculated I maximum infeed—no input: I is calculated from the thread pitch and the thread depth.
6.15 Thread Cycles Extended longitudinal multi-start thread G351 G351 machines a single or multi-start longitudinal thread (internal or external thread) with variable pitch. The thread starts at the current tool position and ends at the "end point X, Z.
6.15 Thread Cycles Tapered API thread G352 This cycle cuts a tapered single or multi-start API thread. The depth of thread decreases at the overrun at the end of thread.
6.15 Thread Cycles Tapered thread G353 G353 cuts a tapered single or multi-start thread with variable pitch.
6.16 Undercut Cycles 6.16 Undercut Cycles Undercut contour G25 G25 generates an undercut form element (DIN 509 E, DIN 509 F, DIN 76) that can then be integrated in roughing or finishing cycles. The table in the graphic support window describes the parameters for undercuts.
6.16 Undercut Cycles Undercut cycle G85 With the function G85, you can machine undercuts according to DIN 509 E, DIN 509 F and DIN 76 (thread undercut). The adjoining cylinder is machined if you position the tool at the cylinder diameter "in front of" the cylinder. If the tool is not positioned at the cylinder diameter, it approaches the workpiece on a diagonal path to machine the undercut.
6.
6.16 Undercut Cycles Undercut according to DIN 509 E with cylinder machining G851 The cycle machines the adjoining cylinder, the undercut, and finishes with the plane surface. It also machines a cylinder start chamfer when you enter at least one of the parameters "B" or "RB.
6.16 Undercut Cycles Undercut according to DIN 509 F with cylinder machining G852 The cycle machines the adjoining cylinder, the undercut, and finishes with the plane surface. It also machines a cylinder start chamfer when you enter at least one of the parameters "B" or "RB.
6.16 Undercut Cycles Undercut according to DIN 76 with cylinder machining G853 The cycle machines the adjoining cylinder, the undercut, and finishes with the plane surface. It also machines a cylinder start chamfer when you enter at least one of the parameters "B" or "RB.
6.16 Undercut Cycles Undercut type U G856 Cycle G856 machines an undercut and finishes the adjoining plane surface. A chamfer or rounding (optional) can be machined. Parameters I undercut diameter (diameter value) K undercut length B chamfer/rounding B>0: Radius of rounding B<0: Width of chamfer Note on the execution of the cycle: At the end of cycle, the tool returns to the starting point.
6.16 Undercut Cycles Undercut type H G857 The cycle G857 machines an undercut. The end point is determined from the plunging angle in accordance with "Undercut type H." At the end of cycle, the tool returns to the starting point. Parameters X contour corner (diameter value) Z contour corner K undercut length R radius—no input: No circular element (tool radius = undercut radius) W plunge angle—no input: W is determined from "K" and "R.
6.16 Undercut Cycles Undercut type K G858 The cycle G858 machines an undercut. This cycle performs only one cut at an angle of 45°. The resulting contour geometry therefore depends on the tool that is used. At the end of cycle, the tool returns to the starting point. Parameters X contour corner (diameter value) Z contour corner I undercut depth Undercuts can only be executed in orthogonal, paraxial contour corners along the longitudinal axis. Cutting radius compensation: Active.
6.17 Parting Cycle 6.17 Parting Cycle Parting cycle G859 The cycle G859 parts the workpiece. If programmed, a chamfer or rounding arc is machined on the outside diameter. At the end of cycle, the tool retracts and returns to the starting point. You can define a feed rate reduction after position "I." Parameters X parting diameter Z parting position I diameter for feed reduction I is defined: The control switches to feed rate "E" after this position.
6.18 Drilling Cycles 6.18 Drilling Cycles Drilling cycle G71 You can use cycle G71 with stationary tools for drilling axial holes in the turning center and with driven tools for drilling axial and radial holes.
6.18 Drilling Cycles Deep-hole drilling cycle G74 You can use cycle G74 with stationary tools for drilling axial holes in the turning center and with driven tools for drilling axial and radial holes. The hole is drilled in several passes. After each pass, the drill retracts and advances again to the first drilling depth, minus the "safety clearance." The drilling depth is reduced with each subsequent pass.
6.18 Drilling Cycles Notes: The control starts execution of the cycle at the current tool and spindle position. The starting point is approached at rapid traverse. Axial hole: Do not program "X." Define "Z." Radial hole: Define "X." Do not program "Z." X and Z are programmed: The control uses the "tool orientation" to decide whether a radial or an axial hole is machined (see “Drilling tools” on page 423).
6.18 Drilling Cycles Tapping G36 You can use cycle G36 with stationary tools for cutting axial threads in the turning center and with driven tools for cutting axial and radial threads. Meaning of "retraction length J": Use this parameter for floating tap holders. The cycle calculates a new nominal pitch on the basis of the thread depth, the programmed pitch, and the "retract length." The nominal pitch is somewhat smaller than the pitch of the tap.
6.18 Drilling Cycles Thread milling, axial G799 The cycle mills a thread in existing holes. Place the tool on the center of the hole before calling G799. The cycle positions the tool on the end point of the thread within the hole. The tool then approaches on "approaching radius R," mills the thread in a rotation of 360°, while advancing by "F." Following that, the cycle retracts the tool and returns it to the starting point.
6.19 C-Axis Commands 6.19 C-Axis Commands Zero point shift, C axis G152 G152 defines an absolute zero point for the C axis (reference: machine parameter 1005, "Reference point, C axis"). The zero point is valid until the end of the program. Parameters C angle: Spindle position of "new" C-axis zero point Example: G152 %152.nc [G152] N1 M5 N2 T71 G197 S1010 G193 F0.08 M104 N3 M14 N4 G152 C30 N5 G110 C0 N6 G0 X122 Z-50 N7 G744 X122 Z-50 ZE-50 C0 Wi90 Q4 N8 G792 K30 A0 X100 J11 P5 F0.
6.20 Face Machining 6.20 Face Machining Starting point of contour / rapid traverse G100 Geometry command: G100 defines the starting point of a contour on the face. Machining command: The tool moves at rapid traverse along the shortest path to the end point.
6.20 Face Machining Linear segment, face G101 Geometry command: G101 defines a linear segment in a contour on the face. Machining command: The tool moves on a linear path at feed rate to the end point.
6.20 Face Machining Circular arc, face G102/G103 Geometry command: G102/G103 defines a circular arc in a contour on the face. Machining command: The tool moves on a circular arc at feed rate to the end point. The direction of rotation is shown in the graphic support window.
6.20 Face Machining Linear slot, face G791 G791 mills a slot from the current tool position to the end point. The slot width equals the diameter of the milling cutter. Oversizes are not taken into account.
6.20 Face Machining Contour and figure milling cycle, face G793 G793 mills figures or (open or closed) "independent" contours on the face.
Q cycle type (default: 0): Depending on "U," the following applies: Contour milling (U=0): – Q=0: Milling center on the contour – Q=1—closed contour: Inside milling – Q=1—open contour: Left in machining direction – Q=2—closed contour: Outside milling – Q=2—open contour: Right in machining direction – Q=3—open contour: Milling location depends on "H" and the direction of tool rotation—see graphic support window Pocket milling (U>0): – Q=0: From the inside toward the outside – Q=1: From the outside toward
6.20 Face Machining Area milling, face G797 Depending on "Q," G797 mills surfaces, polygons or the figure defined in the command following G797. Parameters X limiting diameter Z milling top edge ZE milling floor B width across flats (omit for Q=0): B defines the remaining material. For an even number of surfaces, you can program "B" as an alternative to "V.
O roughing/finishing (default: 0) O=0: Roughing O=1: Finishing J milling direction: For polygons without chamfers/roundings, J defines whether a unidirectional or bidirectional milling operation is to be executed. J=0: Unidirectional J=1: Bidirectional 6.20 Face Machining Notes: With "Q=0," one of the following figures is programmed in the subsequent command. A G80 is programmed after the command.
6.20 Face Machining Figure definition: Full circle, face G304 G304 defines a full circle on the face. Program this figure in conjunction with G793 or G797. Parameters XK center YK center R radius of circle Example: G304 %304.nc [G304] N1 T70 G197 S1200 G195 F0.2 M104 N2 M14 N3 G110 C0 N4 G0 X100 Z2 N5 G793 Z2 ZE-5 P2 U0.5 R0 I0.5 F0.
6.20 Face Machining Figure definition: Rectangle, face G305 G305 defines a rectangle on the face. Program this figure in conjunction with G793 or G797. Parameters XK center YK center A angle—reference: see graphic support window K length of rectangle B height of rectangle R chamfer/rounding R<0: Chamfer length R>0: Rounding arc Example: G305 %305.nc [G305] N1 T70 G197 S1200 G195 F0.2 M104 N2 M14 N3 G110 C0 N4 G0 X100 Z2 N5 G793 Z2 ZE-5 P2 U0.5 R0 I0.5 F0.
6.20 Face Machining Figure definition: Eccentric polygon, face G307 G307 defines a polygon on the face. Program this figure in conjunction with G793 or G797. Parameters XK center YK center Q number of edges: Range: 3 <= Q <= 127 A angle—reference: see graphic support window K width across flats (SW) / length K<0: Width across flats (inside diameter) K>0: Edge length R chamfer/rounding R<0: Chamfer length R>0: Rounding arc Example: G307 %307.nc [G307] N1 T70 G197 S1200 G195 F0.
6.21 Lateral Surface Machining 6.21 Lateral Surface Machining Reference diameter G120 G120 determines the reference diameter of the unrolled lateral surface. Program G120 if you use "CY" for G110 to G113. G120 is a modal function. Parameters X diameter Example: G120 %111.nc [G111, G120] N1 T71 G197 S1200 G195 F0.2 M104 N2 M14 N3 G120 X100 N4 G110 C0 N5 G0 X110 Z5 N6 G41 Q2 H0 N7 G110 Z-20 CY0 N8 G111 Z-40 N9 G113 CY39.2699 K-40 J19.635 N10 G111 Z-20 N11 G113 CY0 K-20 J19.
6.21 Lateral Surface Machining Starting point of contour / rapid traverse G110 Geometry command: G110 defines the starting point of contour definition on the lateral surface. Machining command: The tool moves at rapid traverse along the shortest path to the end point. Parameters Z end point C end angle CY end point as linear value (reference: G120 reference diameter) X end point (diameter value)—(default: Current X position) Define the contour starting point or end point either with "C" or "CY.
6.21 Lateral Surface Machining Linear segment, lateral surface G111 Geometry command: G111 defines a linear segment in a contour on the lateral surface. Machining command: The tool moves on a linear path at feed rate to the end point.
6.21 Lateral Surface Machining Circular arc, lateral surface G112/G113 Geometry command: G112/G113 defines a circular arc in a contour on the lateral surface. Machining command: The tool moves on a circular arc at feed rate to the end point. The direction of rotation is shown in the graphic support window.
Define the center or end point either with "C/W" or "CY/J." Program either center or radius. If you do not program the center, MANUALplus automatically calculates the possible solutions for the center and chooses that point as the center which results in the shortest arc. Permitted as geometry command only for G112/G113: Parameters Q, B Permitted as machining command only for G112/G113: Parameter X %110.nc [G110, G111, G113, G794] N1 T71 G197 S1200 G195 F0.
6.21 Lateral Surface Machining Linear slot, lateral surface G792 G792 mills a slot from the current tool position to the end point. The slot width equals the diameter of the milling cutter. Oversizes are not taken into account.
6.21 Lateral Surface Machining Contour and figure milling cycle, lateral surface G794 G794 mills figures or (open or closed) "independent" contours on the lateral surface.
6.
6.21 Lateral Surface Machining Helical-slot milling G798 G798 mills a helical slot from the current tool position to end point X, Z. The slot width equals the diameter of the milling cutter. For the first infeed, "I" is effective—MANUALplus then calculates all further infeed movements as follows: Current infeed = I * (1 – (n–1) * E) n: nth infeed The infeed movement is reduced down to >= 0.5 mm. Following that, each infeed movement will amount to 0.5 mm.
6.21 Lateral Surface Machining Figure definition: Full circle, lateral surface G314 G314 defines a full circle on the lateral surface. Program this figure in conjunction with G794. Parameters Z center point CY center point as linear value (reference: G120 reference diameter) C center point Angle to center—for angle direction, see graphic support window R radius of circle Example: G314 %314.nc [G314] N1 T71 G197 S1200 G195 F0.2 M104 N2 M14 N3 G110 C0 N4 G0 X110 Z5 N5 G794 X100 XE97 P2 U0.5 R0 K0.
6.21 Lateral Surface Machining Figure definition: Rectangle, lateral surface G315 G315 defines a rectangle on the lateral surface. Program this figure in conjunction with G794.
6.21 Lateral Surface Machining Figure definition: Eccentric polygon, lateral surface G317 G317 defines a polygon on the lateral surface. Program this figure in conjunction with G794.
6.22 Pattern Machining 6.22 Pattern Machining Linear pattern, face G743 With cycle G743, you can machine linear hole patterns or figure patterns in which the individual features are arranged at a regular spacing on the face. If "ZE" has not been defined, the drilling/milling cycle of the next NC block is used as a reference.
6.22 Pattern Machining Examples for command sequences: [ Simple drilling pattern ] N.. G743 XK.. YK.. Z.. ZE.. I.. J.. Q.. ... [ Drilling pattern with deep-hole drilling ] N.. G743 XK.. YK.. Z.. I.. J.. Q.. N.. G74 Z.. P.. I.. ... [ Milling pattern with linear slot ] N.. G743 XK.. YK.. Z.. I.. J.. Q.. N.. G791 K.. A.. Z.. ... [ Milling pattern with "independent contour" ] N.. G743 XK.. YK.. Z.. I.. J.. Q.. N.. G793 ZE.. U.. Q.. N.. G100 XK.. YK.. N.. . . . N.. G80 ...
6.22 Pattern Machining Circular pattern, face G745 With cycle G745, you can machine hole patterns or figure patterns in which the individual features are arranged at a regular spacing in a circle or circular arc on the face. If "ZE" has not been defined, the drilling/milling cycle of the next NC block is used as a reference.
6.22 Pattern Machining Examples for command sequences: [ Simple drilling pattern ] N.. G745 XK.. YK.. Z.. ZE.. A.. W.. Q.. ... [ Drilling pattern with deep-hole drilling ] N.. G745 XK.. YK.. Z.. ZE.. A.. W.. Q.. N.. G74 Z.. P.. I.. ... [ Milling pattern with linear slot ] N.. G745 XK.. YK.. Z.. ZE.. A.. W.. Q.. N.. G791 K.. A.. Z.. ... [ Milling pattern with "independent contour" ] N.. G745 XK.. YK.. Z.. ZE.. A.. W.. Q. N.. G793 ZE.. U.. Q.. N.. G100 XK.. YK.. N.. . . . N.. G80 ...
6.22 Pattern Machining Linear pattern, lateral surface G744 With cycle G744, you can machine linear hole patterns or figure patterns in which the individual features are arranged at a regular spacing on the lateral surface. Parameter combinations for defining the starting point and the pattern positions: Starting point of pattern: Z and C Pattern positions: W and Q Wi and Q If XE has not been defined, the drilling/milling cycle or the figure definition of the next NC block is used as a reference.
6.22 Pattern Machining Examples for command sequences: [ Simple drilling pattern ] N.. G744 Z.. C.. X.. XE.. ZE.. W.. Q.. ... [ Drilling pattern with deep-hole drilling ] N.. G744 Z.. C.. X.. XE.. ZE.. W.. Q.. N.. G74 Z.. P.. I.. ... [ Milling pattern with linear slot ] N.. G744 Z.. C.. X.. XE.. ZE.. W.. Q.. N.. G792 K.. A.. X.. ... [ Milling pattern with "independent contour" ] N.. G744 Z.. C.. X.. XE.. ZE.. W.. Q.. N.. G794 XE.. U.. Q.. N.. G110 Z.. C.. N.. . . . N.. G80 ...
6.22 Pattern Machining Circular pattern, lateral surface G746 With cycle G746, you can machine hole patterns or figure patterns in which the individual features are arranged at a regular spacing in a circle or circular arc on the lateral surface.
6.22 Pattern Machining Examples for command sequences: [ Simple drilling pattern ] N.. G746 Z.. C.. X.. XE.. K.. A.. W.. Q.. ... [ Drilling pattern with deep-hole drilling ] N.. G746 Z.. C.. X.. XE.. K.. A.. W.. Q.. N.. G74 Z.. P.. I.. ... [ Milling pattern with linear slot ] N.. G746 Z.. C.. X.. XE.. K.. A.. W.. Q.. N.. G792 K.. A.. X.. ... [ Milling pattern with "independent contour" ] N.. G746 Z.. C.. X.. XE.. K.. A.. W.. Q.. N.. G794 XE.. U.. Q.. N.. G110 Z.. C.. N.. . . . N.. G80 ...
6.23 Other G Functions 6.23 Other G Functions Period of dwell G4 The system interrupts the program run for the programmed length of time before executing the next command. If G4 is programmed together with a path of traverse in the same block, the dwell time only becomes effective after the path of traverse has been executed.
6.24 Set T, S, F 6.24 Set T, S, F Tool number, spindle speed /cutting speed and feed rate The values for feed rate and spindle speed that are programmed with "Set T, S, F" always refer to the spindle. MANUALplus then transfers the parameters to the DIN program together with the identification letters or G functions. T: "T.." S: G96/G97 S.. F: G94/G95 F.. Entering T, S, F Select "Set T, S, F." Select the soft keys, enter the parameters.
6.25 Data Input and Data Output 6.25 Data Input and Data Output INPUT INPUT (assigning values to variables) Press "Program variable function." Select "Input function" (see top right figure on next page). Define the "input text." Enter the "Variable number for request" (see figure at top right). When programming the "INPUT command," you define the "input text" and number of the "variable for request." The "input text" explains the input.
6.25 Data Input and Data Output WINDOW WINDOW (defining the output window) Press "Program variable function." Select "WINDOW" (see figure to the top right). Select the size of the output window with "lines for output." Close the output window with "lines for output = 0." With the "WINDOW" command, you can define a specific size for the "output" window that is to be used for output of information to the machinist.
6.25 Data Input and Data Output PRINT PRINT (output of information) Press "Program variable function." Select "PRINT" (see figure to the top right). Define the "output texts" and the "variable numbers" (see figure to the right). During execution of this command, MANUALplus displays the "output text" and the value (contents) of the defined "program variable for output" in the "output window." The PRINT command can be used for defining more than one text and variable.
6.26 Programming Variables 6.26 Programming Variables Fundamentals The MANUALplus interprets NC programs before the program run. The system therefore differentiates between two types of variables: Syntax Mathematical functions # variables are evaluated during NC program interpretation. V variables (or events) are evaluated during NC program run.
MANUALplus uses value ranges to define the scope of variables: #0 .. #45 global variables Global variables are retained after the program has been completed and can be processed by the following NC program. #46 .. #50 variables only for expert programs Do not use these variables in your NC program. #256 .. #285 local variables These variables are effective only within a subprogram. Example: "# variables" . . . N.. #1=PARA(1,7,2) [reads "machine dimension 1 Z“ in variable #1 ] N.. . . . N.. #1=#1+1 N.
6.26 Programming Variables Precondition for tool information: A tool call must be programmed for the variables to become effective. The assignment of variables #519..#521 varies depending on the type of tool.
6.26 Programming Variables V variables The MANUALplus uses value ranges to define the following scope of variables: Real: V1 .. V199 Integer: V200 .. V299 Reserved: V300 .. V900 Requests and assignments: Read/write machine dimensions (machine parameter 7) Syntax: V{Mx[y]} x = dimension 1..9 y = coordinate: X, Y, Z, U, V, W, A, B or C Example: "V variable" . . . N.. V{M1[Z]=300} [ sets "machine dimension 1 Z" to "300" ] . . .
6.26 Programming Variables Information contained in variables V901, V902 and V919 are used for the G functions G901, G902 and G903 (see table). X values are saved as radius values. Note: Functions G901, G902 and G903 overwrite the variable! This also applies to variables that have not yet been evaluated. Variable assignment Slide 1 (X, Z) V901 C axis V919 V902 Note on interpreter stop (G909) The MANUALplus pre-interprets approx. 15 to 20 NC blocks.
6.27 Program Branches, Program Repeats 6.27 Program Branches, Program Repeats IF (...) (conditional program branch) Press "Program variable function." Select "Conditional program branch." Enter the "variable condition" (see figure to the top right). You can use both "Mathematical functions" and "Calculating operations" in the same mathematical expression. The mathematical functions are arranged on two menu levels. To switch to the next menu level, press ">>.
6.27 Program Branches, Program Repeats WHILE (program repeat) Press "Program variable function." Select "Program repeat." Enter the "variable condition" (see figure to the top right). A "program repeat" consists of the elements: "WHILE"—followed by a condition (comparison). "ENDWHILE"—concludes the conditional program branch. The NC blocks that are programmed between WHILE and ENDWHILE are executed repeatedly for as long as the "condition" is fulfilled.
6.28 Variables as Address Parameters 6.28 Variables as Address Parameters Variables as address parameters Select the input parameters (see figure to the top right) Press Variable. Press # program variable. Select "Program variable." Enter the variable number. Transfer the variable number. Enter a mathematical expression, if required: Mathematical function or Select the Calculating operation (see figure to the lower right). Transfer the variable/variable calculation as address parameter.
6.
6.28 Variables as Address Parameters You can program NC blocks that contain only variable calculations (see figure at right). Calculating variables Press "Program variable function." Select "Assignment (#)." Enter the variable number. Transfer the variable number. Enter the mathematical expression: Mathematical function or Select the Calculating operation (see figure to the lower right). Transfer the variable/variable calculation as address parameter.
6.29 Subprograms 6.29 Subprograms Calling a subprogram Select the "Subprogram call." Select the DIN macro list. Call the subprogram. Select Assume DIN macro. Enter transfer parameters Entering subprogram names directly Select the "Subprogram call." Enter the program name (see figure at top right). Enter transfer parameters General information on subprograms: Subprograms are defined in a separate file. They can be called from any main program or other subprogram. (DIN macros are subprograms.
Dialog texts You can define the parameter descriptions that precede/follow the input fields in an external subprogram. MANUALplus automatically sets the unit of measure for parameter values to the metric system or inches. A maximum of 19 descriptions can be entered. The parameter descriptions can be positioned within the subprogram as desired. 6.29 Subprograms You can add up to 20 "transfer values" to a subprogram. These are: LA to LF, LH, I, J, K, O, P, R, S, U, W, X, Y, Z.
6.30 M Functions 6.30 M Functions With M functions, you can control the program run and program switching functions for the machine (machine commands). Entering M functions Select "M function." Enter the number of the M function. Define the parameters, if applicable. M commands for program-run control M00 Program stop interrupts execution of a DIN program. Program run is continued after Cycle START has been pressed.
Please refer to your machine manual for detailed information on which of the M commands listed are supported by your machine and which additional M commands are available. HEIDENHAIN MANUALplus 4110 6.30 M Functions Machine commands The effect of machine commands depends on the configuration of your machine. The table lists the M commands used on most machines.
Tool Management Mode 411 7 Tool Management Mode
7.1 Tool Management Mode of Operation 7.1 Tool Management Mode of Operation You usually program the coordinates for the contour by taking the dimensions from the drawing. To enable MANUALplus to calculate the slide path, compensate the cutting radius and determine the proportioning of cuts, you need to enter the tool length, cutting radius, tool angle, etc. MANUALplus can save tool data for up to 99 tools, whereby each tool is identified with a number (1...99).
7.1 Tool Management Mode of Operation Drilling tools—this group comprises: Centering tools NC center drills Twist drills Indexable-insert drills Countersinks/counterbores Reamers Taps: All kind of tapping tools Milling tools—this group comprises: Twist drill cutter End milling cutter Thread cutter You will certainly use more than these tool types. Special care has been taken to clearly structure the tool types available on the MANUALplus.
7.2 Tool Organization 7.2 Tool Organization The entries in the tool list are designated T1...T99. The tool tip in the graphic display shows the tool type and the tool orientation. In the tool list, the MANUALplus displays important parameters and the tool description. The input window shows additional data on the tool that is highlighted in the tool list. You can navigate within the tool list with the arrow keys and "PgUp/PgDn" to check the entries.
7.2 Tool Organization Find entries Press Search. Select the tool type with the menu key. MANUALplus scrolls through the list and stops at the next entry of this type. Press the tool type menu key again: MANUALplus scrolls through the list and stops at the next entry of this type. When MANUALplus has reached the last entry in the list for the selected tool type, it displays the first entry for this type again. Available functions: – Change: MANUALplus opens the input window.
7.3 Tool Texts 7.3 Tool Texts A description or designation makes it easier to find a specific tool whenever you need it again. You can describe each tool by an identification number or a general designation, depending on your method of organization. Connections: The descriptions are managed in the tool text list. Each entry is preceded by a "Q number." The parameter "Tool text Q" contains the reference number for the "tool text" list. The text is then displayed in the tool list.
7.3 Tool Texts Transfer text number Position the cursor on the text entry. Press Take over text no. MANUALplus transfers the "Q number" of the text entry as "tool text Q" and switches back to the tool data editing mode. If you switch back to the tool data editing mode with Back, the parameter "tool text Q" remains unchanged.
7.4 Tool Data 7.4 Tool Data Tool orientation From the tool orientation, MANUALplus determines the position of the tool tip and, depending on the selected tool type, additional information such as the setting-angle direction, reference-point position, etc. This information is necessary, for example, for calculating the cutting radius compensation, plunging angle, etc. Reference point The "setting dimensions X, Z" refer to the tool reference point.
7.4 Tool Data Lathe tools Select lathe tools. The graphic support window illustrates how goose-necked roughing and finishing tools for longitudinal machining are dimensioned (WO 1, 3, 5 and 7). On the next page you will find information on the dimensions of facing tools, neutral tools and button tools.
7.4 Tool Data Neutral tools The tool orientation values WO=2, 4, 6, 8 are used for "neutral" tools. Neutral means the cutting edge is perpendicular to the X or Z axis (see figure at right). Button tools The following aspects are important when dimensioning button tools: Nose angle B=0: identifies the tool as button tool. Tool angle: is used for plunge cycles to check or calculate the plunging angle. MANUALplus needs the tool angle during simulation for calculating the tool position.
7.4 Tool Data Recessing and recess-turning tools Select recessing tools.
7.4 Tool Data Thread-cutting tools Select thread-cutting tools.
7.4 Tool Data Drilling tools Select drilling tools.
7.4 Tool Data Tapping tools Select tapping tools.
7.4 Tool Data Milling tools Select milling tools.
7.5 Tool Data— Supplementary Parameters 7.5 Tool Data— Supplementary Parameters The second input window contains information on direction of rotation, cutting data, data on tool life monitoring, etc. You can switch between the input windows using PgUp/PgDn. Driven tool The "Tool driven" parameter allows you to define for drilling and tapping tools whether switching commands are generated for the spindle or the driven tool. Milling tools are always considered "driven tools.
7.5 Tool Data— Supplementary Parameters Tool life management MANUALplus can "count" either the machining time of a tool (i.e. the time a tool is traversed at the programmed feed rate) or the number of parts that were produced with that tool. These two options are used for tool life management. As soon as the tool life expires or the programmed quantity is reached, the system interrupts machining and asks you to replace the tool or cutting edge.
Organization Mode of Operation
8.1 Organization Mode of Operation 8.1 Organization Mode of Operation This mode of operation offers various functions for communication with other systems, data security, setting of parameters, and diagnosis. The following functions are available: Parameter settings Parameters enable you to adapt MANUALplus to your specific requirements. The "Parameter" menu provides functions to display and edit parameters. Transfer Input and output of programs, parameters, and tool data.
8.2 Parameters 8.2 Parameters Parameters that are preset for the usual "daily operations" are grouped under the menu item Cur.(rent) para(meters) [1]. Selecting this menu item calls the following: Setup (menu) [1] Machine parameters [2] NC switches [3] PLC parameters [4] Graphics parameters [5] Machining [6] A small arrow to the right of the menu line indicates that a menu item has a submenu (see figure to the top right). After you have selected a parameter, the input window is opened.
8.2 Parameters Current parameters Current parameters "Setup (menu) [1]" menu item Workpiece zero point [1]—Main spindle [1] Distance between "Machine zero point and workpiece zero point" (usually determined with "Set axis values"). Zero point coordinate X [mm] Zero point coordinate Z [mm] Tool change point [2] Distance between "Machine zero point and tool change point" (usually determined with "Set tool change point").
Speeds [2] For spindle 1 (main spindle) and spindle 2 (driven tool): Zero point shift (M19) [°] The parameter determines the offset in position between the spindle reference point and the reference point of the angle encoder (rotary encoder). After receiving the reference pulse from the rotary encoder, the current actual position is overwritten by the parameter value. Number of revolutions for chip breaking Number of additional spindle revolutions for disengaging the tool during spindle stop.
8.2 Parameters Current parameters Settings [3] Set the system to "metric mode" or "inch mode" and define the behavior for searching the start block. Changes do not take effect until the control is restarted. Output to printer—non-functional Metric/Inch 0: Metric 1: Inch Start block search 0: Off 1: On (Note: The system must be prepared for the start block function.) "PLC parameters [4]" menu item The PLC parameters are described in your machine manual.
8.2 Parameters Configuration parameters You can call the Config(uration parameters) [2] menu item only with "system manager" authorization (see “Access authorization” on page 453). The configuration parameters are divided into three groups: Machine parameters Control parameters PLC parameters (see machine manual) The parameters are identified with numbers. You can either call a parameter directly if you already know its number, or display the parameter list.
8.2 Parameters Machine parameters (MP) Display setting [MP 17] The data is displayed in the "Actual value display" fields (machine window).
Tool mount n [MP 601, ..] If you use tool holders in different quadrants, the additional tool holder is defined as "mirrored“ (see “Tools in different quadrants” on page 48). The distance between the additional tool holder and the principal tool holder is usually defined in "compensation X, Z.
8.2 Parameters Control parameters (SP) Settings [SP 1] Set the system to "metric mode" or "inch mode" and define the behavior for searching the start block. Output to printer—non-functional Metric/Inch 0: Metric 1: Inch Start block search 0: Off 1: On (Note: The system must be prepared for the start block function.) Time calculation for simulation, general [SP 20] The times set in this parameter are taken into account for calculating the idle machine times.
Simulation: Settings [SP 27] The machining simulation is delayed by the “path delay” time after the path has been simulated graphically. The simulation speed can thus be influenced. Path delay Allocation to interfaces [SP 40] Interface 1 [SP 41] Interface 2 [SP 42] MANUALplus stores the "settings" of the serial interface in these parameters. The parameters are usually defined in "Transfer— Settings" (see “Settings in the "Serial" and "Printer" modes” on page 445).
8.
8.3 Transfer 8.3 Transfer The Transfer mode is used for data backup and data exchange with PCs. When we speak of "files" in the following, we mean programs, parameters and tool data. The following file types can be transferred: Programs (cycle programs, DIN programs, DIN macros, and ICP contour descriptions) Parameters Tool data Data backup HEIDENHAIN recommends backing up the tool data and programs created on MANUALplus on a PC at regular intervals. You should also back up the parameters.
8.3 Transfer Interfaces Data transfer is carried out over the Ethernet or the serial interface. We recommend using transfer modes via Ethernet interface, since the transmission rate and transmission security are higher than with serial interfaces. WINDOWS networks (via Ethernet): With a WINDOWS network you can integrate your lathe in a LAN network. MANUALplus supports the networks provided by WINDOWS. MANUALplus allows you to send/receive files.
8.3 Transfer Access control for networks Passwords for read/write access to directories can be assigned by the remote system (WINDOWS: "Access control to shared levels"). In this case, the "Enter network password" dialog box appears when you try to access directories of the remote system. In Diagnosis mode, the MANUALplus files can be assigned passwords for read access or write access (see “Diagnosis” on page 455).
8.3 Transfer Configuring for data transfer Press Settings. Press Network and define the directory of the remote station ("Device name" input field)—see figure to the upper right. Press Serial and define the interface parameters—see figure to the lower right. Press Printer and define the interface parameters. Transfer the settings. Press Back. Access authorization as “system manager” is necessary to access the settings (see “Access authorization” on page 453).
8.3 Transfer Settings in the "Serial" and "Printer" modes Baud rate: In bits per second Word length: 7 or 8 bits per character Parity: Select even/odd parity or "no parity." The setting "word length = 8 bits" is required whenever you want to use "even/odd parity." Stop bits: 1, 1 1/2 and 2 stop bits Protocol Hardware (hardware handshake) The receiver informs the sender through "RTS/CTS signals" that it is temporarily not able to receive data.
8.3 Transfer Transferring programs (files) When selecting a program, place the highlight on the desired program and press Mark. You can also select all programs with Mark all. „A marked program is indicated with a diamond. To unmark a program, simply press Mark once again. If you want to transfer a single program, place the highlight on the program and press Transmit file or Receive file. Below the window, MANUALplus displays the file size of the highlighted program and the time it was last changed.
8.3 Transfer Selecting the program group Press Program. Press Program selection. DIN programs or DIN macros, or Cycle programs, or ICP contours, or DXF Import. Press Back. When DIN programs, or cycle programs, or ICP contours have been selected, only the file name is displayed. MANUALplus uses the extensions (see table at right) to differentiate between the individual program groups.
8.3 Transfer Program transfer (Network mode) "Network" shows its own directory in the left window and the directory of the remote station in the right window (see figure to the right). To switch back and forth between the two windows, press the horizontal arrow keys (or ENTER). Transmitting files Press Program. Place the highlight in the left window. Highlight the program, or Select and Mark programs, or Press Mark all. Press Transmit file. Receiving files Press Program.
8.3 Transfer Program transfer (Serial mode) MANUALplus displays its own directory (see figure at right). Transmitting files Highlight the program, or Select and Mark programs, or Press Mark all. Press Transmit file. Receiving files Press Receive file. If you have selected "Receive file," MANUALplus waits for the transmission of data from the serial interface. The "progress display" shows that data transfer is active. If you want to cancel the receiving status, press Back.
8.3 Transfer Printing DIN programs/macros Press Program. Press Program selection. Press DIN programs or DIN macros. Press Back. Highlight the program, or Select and Mark programs, or Press Mark all. Press Transmit file. The information displayed during transfer is described in “Transferring programs (files)” on page 446. You can only print out DIN programs and DIN macros.
8.3 Transfer Transferring parameters Press Parameter. Press Transmit parameter. Press Receive parameter. The transmitted parameter files receive the file name that was entered for "Backup name" in the "Settings" menu. MANUALplus appends the following extension to the file name: *.BEA *.MAS *.PRO *.PLC *.
8.3 Transfer Transferring tool data Press Tool. Press Transmit tool. Press Receive tool. The transmitted tool files receive the file name that was entered for "Backup name" in the "Settings" menu. MANUALplus appends the following extension to the file name: *.TXT *.WKZ (tool texts) (tool parameters) The information displayed during transfer is described in “Transferring programs (files)” on page 446. Receipt of tool files: "Network" mode: The file name is checked.
8.4 Service and Diagnosis 8.4 Service and Diagnosis When you select Service [3], MANUALplus offers the following functions or function groups: Logon [1] Logoff [2] Usr. Srv. [3] (user service) Sys.Srv. [4] (system service) Diag.(nosis) [6] Some service and diagnostic functions are not accessible (reserved for service and commissioning personnel). Access authorization The functions logon, logoff, and user service are provided for managing access authorization.
8.4 Service and Diagnosis MANUALplus differentiates between the following user groups: Without protection class NC programmers System managers Service personnel (of the machine tool builder) MANUALplus is delivered with a preset authorization for the user "password 1234". The password is 1234. After you have logged on as the user "Password 1234", you can program the users that operate the machine (with system manager authorization). You should then delete the user "Password 1234".
8.4 Service and Diagnosis System service "System service" provides the following functions: Date/Time [1] Enter the date and/or time. Error messages are recorded together with the date and time they occurred. You should therefore always ensure that the date and time are correctly set. Language switchover [3] After calling this function, you can select the desired language with the >> soft key. Then confirm your selection with OK.
Examples
9.1 Working with MANUALplus 9.1 Working with MANUALplus The following example illustrates how to set up the machine and how to machine a workpiece using the cycle programming feature. The machining operation is to be performed in Teach-in mode. This has the advantage that, once you have machined the first workpiece, you have a cycle program that can be repeated any time. Required tools Roughing tool: Position T1 WO = 1 Tool orientation A = 93° Setting angle B = 55° Nose angle R = 0.
9.1 Working with MANUALplus Setting up the machine Prerequisite: Tools T1, T2, and T3 are entered. Setting up the machine Clamp the workpiece blank Insert the reference tool and specify the machine data in "Set T, S, F." Prepare for setting the workpiece zero point and measuring the tools (in Manual mode with handwheels / jog controls): Machine an end face. Prepare the diameter. Set the workpiece zero point Select "Setup." Press "Set axis values.
9.1 Working with MANUALplus Selecting a cycle program A new cycle program with the number "999" is created. Creating a cycle program Switch to Teach-in mode. Press Program list. Enter "999" as program number. Activate program "999". Press Change text. Enter the program designation (here: "Example workpiece"). Transfer the program designation. Start programming the cycle.
9.1 Working with MANUALplus Creating a cycle program The individual cycles for machining workpieces are described below. The current working step is displayed in the workpiece graphic; the cycles and the cycle parameters are displayed in the graphics to the right. The machine data display indicates the status after execution of the cycle. Sequence of working steps for each cycle: Select the cycle. Program the cycle. Check the cycle by running a graphical simulation. Run the cycle.
9.1 Working with MANUALplus Roughing cycle 2 The "starting point X, Z" is defined such that it is located shortly before the area to be machined. It is approached at rapid traverse. The cycle machines the area marked in the drawing. The expanded mode is selected for programming the allowances, the rounding and the chamfer. Roughing cycle 3 The cycle machines the area marked in the drawing. The expanded mode is selected for programming the allowances and the oblique cut.
9.1 Working with MANUALplus Roughing cycle 4 The cycle machines the area marked in the drawing. The expanded mode is selected for programming the allowances. Positioning the tool for tool change Before you can replace the roughing tool by the finishing tool, you must move it to a "safe position.
9.1 Working with MANUALplus Machining a thread chamfer and undercut The thread chamfer / undercut and the following finishing cycles are programmed in such a way that the contour area is machined in a single uninterrupted cut. MANUALplus approaches the "starting point X, Z" in rapid traverse. No further positioning movements therefore need to be programmed. The thread chamfer and undercut are machined with the "Undercut DIN 76" cycle. "With return" is switched off.
9.1 Working with MANUALplus Finishing cycle 1 The three following finishing cycles finish the contour area shown in the graphic. The expanded mode is used for all finishing cycles so that contour elements such as oblique cuts, roundings, or chamfers can be machined. In expanded mode, the tool stops at the end of the cycle. This is necessary to be able to finish the contour area "in a single cut.
9.1 Working with MANUALplus Finishing cycle 3 Positioning the tool for tool change Before you can replace the finishing tool by the threading tool, you must move it to a "safe position.
9.1 Working with MANUALplus Thread cycle This cycle produces a single-start thread with a thread pitch of 1.5 mm. The depth of thread and the proportioning of cuts is calculated automatically by MANUALplus. Tool positioning The workpiece is completely machined. To remove the finished workpiece, you must move the tool to a "safe position.
9.1 Working with MANUALplus Program list The figure to the right shows the resulting cycle program. Simulation in program run The program is simulated in the "Program run" mode. Press the "Menu" key to return to the main menu and select Program run. MANUALplus loads the program that was last machined. In this case, the cycle program "999" is loaded. In the figure to the right, the complete machining operation for producing the workpiece was simulated in the Program run mode.
9.1 Working with MANUALplus Finished workpiece The figure to the right shows the resulting workpiece.
9.2 ICP Example "Threaded Stud" 9.2 ICP Example "Threaded Stud" This example illustrates how to machine a threaded stud using the ICP programming feature. The individual working steps for machining the ICP contour and integrating the contour into ICP cycles are based on the workpiece drawing. The machining operation is performed with the "ICP cutting longitudinal" cycle. In the process described below, you create an ICP contour description and a cycle program for parts production.
9.2 ICP Example "Threaded Stud" ICP cutting longitudinal The procedure presupposes that the machine has been set up and the control is in "Teach-in" mode. The infeed depth and the allowances for roughing are programmed in the ICP cutting cycle. In this example, the number ("888") of the ICP contour is entered before calling the ICP editor (see figure to the top right). You then switch to the ICP editor and press Insert element to enter the contour elements.
9.2 ICP Example "Threaded Stud" Contour element 1 The contour starts with a chamfer (thread chamfer). The starting point of the contour is defined in "XS, ZS" when programming the first contour element. The starting point, in this case, is the corner that is cut off by the chamfer. If you program a chamfer as the first contour element, you must specify the position of the chamfer with the parameter "element position J"—here: "J=1" (see figure to the upper right).
9.2 ICP Example "Threaded Stud" Contour element 2 The next connecting contour element is an undercut. The form element "undercut" describes the preceding cylinder, the actual undercut and the subsequent plane surface. The part of the contour you have entered up to now is unambiguously defined. MANUALplus draws the contour elements and clears the symbol for the "unsolved chamfer element." To define the undercut, the thread pitch is programmed in addition to the "target point.
9.2 ICP Example "Threaded Stud" Contour element 3 The next connecting contour element is an oblique cut. After you have entered the "target point X, Z," the line is unambiguously defined. MANUALplus draws the contour elements in the graphics window.
9.2 ICP Example "Threaded Stud" Contour element 4 The next connecting contour element is a horizontal line. After you have entered the "target point Z," the line is unambiguously defined. MANUALplus draws the contour elements in the graphics window.
9.2 ICP Example "Threaded Stud" Contour element 5 The next connecting contour element is a rounding. You only need to enter "rounding radius B." When the rounding is programmed, the control does not yet know the next connecting contour element. The rounding and the preceding linear element are therefore considered "unsolved elements." MANUALplus displays the symbols for these elements below the graphics window and depicts the preceding horizontal line in gray.
9.2 ICP Example "Threaded Stud" Contour element 6 The next connecting contour element is a vertical line. After you have entered the "target point X," the line and the preceding rounding are unambiguously defined. MANUALplus draws the contour elements and clears the symbols for the "unsolved elements.
9.2 ICP Example "Threaded Stud" Contour element 7 The next connecting contour element is a chamfer. The only parameter that needs to be defined is the "chamfer width B." When you program the chamfer, the control does not yet know the subsequent contour element which connects to the chamfer. The chamfer and the preceding linear element are therefore considered "unsolved elements.
9.2 ICP Example "Threaded Stud" Contour element 8 The next connecting contour element is a horizontal line. After you have entered the "target point Z," the line and the preceding chamfer are unambiguously defined. MANUALplus draws the contour elements and clears the symbols for the "unsolved elements.
9.2 ICP Example "Threaded Stud" Contour element 9 The next connecting contour element is a vertical line. After you have entered the "target point X," the line is unambiguously defined. MANUALplus draws the contour elements in the graphics window. The ICP contour has been completely defined. Back concludes ICP programming and Input finished concludes the ICP cycle.
9.2 ICP Example "Threaded Stud" Checking the ICP cutting cycle With the graphic simulation function, you can check the execution of the cycle (Graphics soft key). You can then transfer the cycle to the cycle program with the Save or Overwrite. ICP finishing The ICP contour "888" (threaded stud) is also used for the finishing cycle.
9.2 ICP Example "Threaded Stud" Checking the ICP finishing cycle With the graphic simulation function, you can check the execution of the ICP finishing cycle (Graphics soft key). You can then transfer the cycle to the cycle program with the Save or Overwrite. MANUALplus finishes the contour in the defined "contour direction" (see figure to the top right).
9.3 ICP Example "Matrix" 9.3 ICP Example "Matrix" This example illustrates how to machine a matrix using the ICP programming feature. The individual working steps for machining the ICP contour and integrating the contour into ICP cycles are based on the workpiece drawing. In the process described below, you create an ICP contour description and a cycle program for parts production. The machining operation is performed with the "ICP cutting transverse" cycle.
9.3 ICP Example "Matrix" ICP cutting transverse The procedure presupposes that the machine has been set up and the control is in "Teach-in" mode. The infeed depth and the allowances for roughing are programmed in the ICP cutting cycle. The number of the ICP contour is entered before calling the ICP editor (see figure to the top right). Switch to the ICP programming function with Edit ICP.
9.3 ICP Example "Matrix" Contour element 3 The next connecting contour element is an oblique cut. Only the angle of the linear element is known. MANUALplus displays the symbol for an "unsolved element" below the graphics window and depicts the unsolved line in gray (color for unsolved elements).
9.3 ICP Example "Matrix" Contour element 4 The next connecting contour element is a circular arc whose center and radius are known. MANUALplus displays the possible solutions for selection (see figure to the bottom right and, on the next page, to the top right).
9.3 ICP Example "Matrix" To transfer the correct solution, press Select solution. The preceding oblique cut is now unambiguously defined. The circular arc still permits several solutions. MANUALplus displays the symbol for an "unsolved element" below the graphics window and depicts the unsolved line in gray (color for unsolved elements).
9.3 ICP Example "Matrix" Contour element 5 The next connecting contour element is an oblique cut. After you have entered the "target point X, Z" and the "angle A," the line is unambiguously defined. MANUALplus displays the possible solutions for selection (see figure to the bottom right and, on the next page, to the top right).
9.3 ICP Example "Matrix" To transfer the correct solution, press Select solution. The preceding circular arc and the oblique cut are now unambiguously defined. MANUALplus draws the contour elements and clears the symbols for the "unsolved elements." The "rough contour" has been completely defined. You can now exit the input mode with Back.
9.3 ICP Example "Matrix" Rounding the corners The rounding arcs are "superimposed" on the existing contour. This is done by selecting the individual contour corners and defining the corresponding rounding radii. You call the function for superimposing elements with the superposition soft key (represented by a symbol—see figure at upper right). You can then select the position of the rounding with Previous corner / Next corner (see figure at lower right).
9.3 ICP Example "Matrix" Defining a rounding To define the rounding, enter "Rounding radius B." MANUALplus inserts the rounding in the existing ICP contour and draws the "perfected" contour. If the contour contains further corners, MANUALplus offers the next contour corner for selection (see figure to the bottom right).
9.3 ICP Example "Matrix" The ICP contour has been completely defined. Back concludes ICP programming and Input finished concludes the ICP cycle. Checking the ICP cutting cycle After the cutting operation has been completed, it is checked with the Simulation function. The simulation function is called with the Graphics soft key. You can then transfer the cycle to the cycle program with the Save or Overwrite.
9.3 ICP Example "Matrix" ICP finishing The ICP contour "777" ("Matrix") is also used for the finishing cycle. Checking the ICP finishing cycle With the graphic simulation function, you can check the execution of the ICP finishing cycle (Graphics soft key). You can then transfer the cycle to the cycle program with the Save or Overwrite. MANUALplus finishes the contour in the defined "contour direction" (see figure to the bottom right).
9.3 ICP Example "Matrix" Cycle program "ICP example Matrix" Besides the ICP cycles, the created cycle program also includes the positioning cycles for tool change (see figure to the right).
9.4 ICP Example "Recessing Cycle" 9.4 ICP Example "Recessing Cycle" This example illustrates the use of an ICP recessing cycle. The individual working steps for machining the ICP contour and integrating the contour into ICP cycles are based on the workpiece drawing. In the process described below, you create an ICP contour description and a cycle program for parts production. The machining operation is performed with the "ICP recessing radial" cycle.
9.4 ICP Example "Recessing Cycle" ICP recessing radial The procedure presupposes that the machine has been set up and the control is in "Teach-in" mode. The allowances for pre-cutting are programmed in the ICP recessing cycle. The cutting width is not entered. MANUALplus automatically calculates the proportioning of cuts such that the infeed per pass is < 80% of the cutting width defined in the tool data (see figure to the top right).
9.4 ICP Example "Recessing Cycle" Contour element 1 The contour starts with a horizontal line which is connected "tangentially" to the subsequent circular arc. The starting point of the ICP contour is defined in "XS, ZS" when programming the first contour element. After you have entered the "target point Z," the line is unambiguously defined. MANUALplus draws the contour element in the graphics window.
9.4 ICP Example "Recessing Cycle" Contour element 2 The next connecting contour element is a circular arc. Only its radius is known. The circular arc still permits several solutions. MANUALplus displays the corresponding symbol below the graphics window and depicts the arc in gray, which is the color used for identifying unsolved elements.
9.4 ICP Example "Recessing Cycle" Contour element 3 The next connecting contour element is an oblique cut whose target point and angle are known. MANUALplus displays the "selection of possible solutions." To transfer the correct solution, press Select solution (see figure to the lower right). The preceding circular arc and the oblique cut are now unambiguously defined.
9.4 ICP Example "Recessing Cycle" Contour element 4 The next connecting contour element is an oblique cut whose target point is known. After you have entered the "target point X, Z," the oblique cut is unambiguously defined. MANUALplus draws the contour elements in the graphics window.
9.4 ICP Example "Recessing Cycle" Contour element 5 The next connecting contour element is a horizontal line. After you have entered the "target point Z," the line is unambiguously defined. MANUALplus draws the contour elements in the graphics window.
9.4 ICP Example "Recessing Cycle" Contour element 6 The next connecting contour element is an oblique cut whose target point is known. After you have entered the "target point X, Z," the oblique cut is unambiguously defined. MANUALplus draws the contour elements in the graphics window.
9.4 ICP Example "Recessing Cycle" Contour element 7 The next connecting contour element is a horizontal line. After you have entered the "target point Z," the line is unambiguously defined. MANUALplus draws the contour elements in the graphics window. The "rough contour" has been completely defined. You can now exit the input mode with Back.
9.4 ICP Example "Recessing Cycle" Rounding the corners The rounding arcs are "superimposed" on the existing contour. Then select the corner (Next corner/ Previous corner). Following that, define the "rounding radius B." MANUALplus inserts the rounding in the existing ICP contour and draws the "perfected" contour. MANUALplus offers the next contour corner for selection. In this example, all existing corners need to be rounded. The ICP contour is completely programmed (see figure at lower right).
9.4 ICP Example "Recessing Cycle" Checking the "ICP recessing radial" cycle With the graphic simulation function, you can check the execution of the ICP recessing cycle (Graphics soft key). Activating the Single block function allows you to check the paths of traverse more carefully one block at a time. In the figure to the upper right, the recessing operation has not been completed yet. You can then transfer the cycle to the cycle program with Save or Overwrite.
9.4 ICP Example "Recessing Cycle" Checking the "ICP recessing radial, finishing" cycle With the graphic simulation function, you can check the execution of the ICP recessing, finishing cycle (Graphics soft key). In the figure to the upper right, the finishing operation has not been completed yet. You can then transfer the cycle to the cycle program with Save or Overwrite.
9.5 ICP Example "Milling Cycle" 9.5 ICP Example "Milling Cycle" The milling example illustrates the use of an ICP contour for machining a pattern. The individual working steps for machining the ICP contour and integrating the contour into ICP cycles are based on the workpiece drawing. In the process described below, you create an ICP contour description and a cycle program for parts production. The cycle used is "ICP contour, pattern circular, axial.
9.5 ICP Example "Milling Cycle" Milling cycle—roughing The roughing cycle used is "ICP contour, pattern circular, axial." After defining the cycle parameters, press Edit ICP to call the ICP programming function. The pattern diameter is "K=0", since the exact position of the "first milling contour" is defined and the ICP contours are symmetrically arranged around the face center.
9.5 ICP Example "Milling Cycle" Contour element 1 First you enter the "rough contour." Then you use the "superimposition" function to define the roundings. The contour starts with a horizontal line. The starting point of the ICP contour is defined in "XS, YS" when programming the first contour element. The element is defined unambiguously after the "length of line" has been entered. MANUALplus draws the contour element in the graphics window.
9.5 ICP Example "Milling Cycle" Contour element 2 The next connecting contour element is a circular arc. The target point and the radius must be defined. Since there are two solutions, MANUALplus asks which solution is to be used.
9.5 ICP Example "Milling Cycle" Contour element 3 A vertical line follows. The element is defined unambiguously after the "length of line" has been entered.
9.5 ICP Example "Milling Cycle" Contour element 4 A circular arc follows. The target point and the radius must be defined. Now the milling contour is closed. This is the precondition for milling pockets. Since there are two solutions, MANUALplus asks which solution is to be used.
9.5 ICP Example "Milling Cycle" Rounding the corners The rounding arcs are "superimposed" on the existing contour. Then select the corner (Next corner/ Previous corner). Following that, define the "rounding radius B." MANUALplus inserts the rounding in the existing ICP contour and draws the "perfected" contour. MANUALplus offers the next contour corner for selection. In this example, all existing corners need to be rounded. The ICP contour is completely programmed (see figure at lower right).
9.5 ICP Example "Milling Cycle" Milling cycle—finishing The workpiece is machined with "ICP contour, pattern circular, axial" and the generated ICP contour. "O=1" defines the finishing cycle—with "J=0," the pocket floor is finished from the inside towards the outside. The same cutter that was used for the roughing cycle is used for the finishing cycle.
9.5 ICP Example "Milling Cycle" Checking the ICP milling cycle (finishing) With the graphic simulation function, you can check the execution of the ICP milling (finishing) cycle (Graphics soft key). You can then transfer the cycle to the cycle program with Save or Overwrite. Cycle program "ICP milling example" Besides the ICP cycles, the created cycle program also includes the positioning cycles for tool change (see figure to the right). Functions of the cycles: N2: Pocket milling—Roughing.
9.6 DIN Programming Example "Threaded Stud" 9.6 DIN Programming Example "Threaded Stud" This example illustrates how to machine a threaded stud using the DIN programming feature. The individual working steps that are defined in the DIN program are based on the workpiece drawing. Required tools Roughing tool: Position T1 WO = 1 Tool orientation A = 93° Setting angle B = 55° Nose angle R = 0.
9.6 DIN Programming Example "Threaded Stud" DIN program "threaded stud" %888.nc Program number of the DIN program DIN example "threaded stud" Program description N1 G14 Q1 Approach the tool change position, insert the roughing tool N2 G96 S150 G95 F0.4 T1 Call roughing tool, program spindle speed and feed rate N3 G0 X62 Z2 Approach the workpiece N4 G819 P4 H0 I0.3 K0.
9.6 DIN Programming Example "Threaded Stud" N36 G14 Q1 Retract the tool (approach the tool change position) N37 M30 End of program END Checking the DIN program After you have written the DIN program "Threaded stud," switch to the "Program run" mode to test the program (see figure at upper right). The simulation shows the contour of the threaded stud and each individual tool movement (see figure at lower right).
9.7 DIN Programming Example "Milling Cycle" 9.7 DIN Programming Example "Milling Cycle" This example illustrates how to machine the face using the DIN programming feature. Required tool Milling tool (roughing and finishing): Position T40 WO = 8 Tool orientation I = 8 Cutter diameter K = 4 Number of teeth TF = 0.025 Feed per tooth Preconditions: The turning operation is completed. The tool dimensions have been determined.
9.7 DIN Programming Example "Milling Cycle" DIN program "face milling" %2005.nc Program number of the DIN program [Example of face milling] Program description N1 M5 Spindle STOP N2 G197 S3183 G195 F0.12 M103 Program the speed, feed rate N3 T40 Call the milling tool N4 M14 Activate the C axis N5 G110 C0 Position the C axis N6 G0 X80 Z2 Approach the workpiece N7 G793 Z0 ZE-6 P3 U0.5 I1 K0.15 F0.1 E0.
9.7 DIN Programming Example "Milling Cycle" Checking the DIN program After you have written the DIN program "face milling," switch to the "Program run" mode to test the program (see figure at upper right). To check the contours and each individual tool movement, switch the simulation to "Face view" (see figure to the bottom right).
Tables and Overviews HEIDENHAIN MANUALplus 4110 523
10.1 Thread Pitch 10.1 Thread Pitch If the thread pitch has not been defined, it is calculated from the diameter according to the following table. Diameter Thread pitch Diameter Thread pitch 1 0.25 12 1.75 1.1 0.25 14 2 1.2 0.25 16 2 1.4 0.3 18 2.5 1.6 0.35 20 2.5 1.8 0.35 22 2.5 2 0.4 24 3 2.2 0.45 27 3 2.5 0.45 30 3.5 3 0.5 33 3.5 3.5 0.6 36 4 4 0.7 39 4 4.5 0.75 42 4.5 5 0.8 45 4.5 6 1 48 5 7 1 52 5 8 1.25 56 5.5 9 1.25 60 5.
10.2 Undercut Parameters 10.2 Undercut Parameters DIN 76—undercut parameters MANUALplus determines the parameters from the thread pitch according to the following table. Designations: I = undercut diameter K = undercut length R = undercut radius W= undercut angle Thread undercut DIN 76—external thread Thread pitch I K R W Thread undercut DIN 76—internal thread Thread pitch I K R W 0.2 D –0.3 0.7 0.1 30° 0.2 D +0.1 1.2 0.1 30° 0.25 D –0.4 0.9 0.12 30° 0.25 D +0.1 1.4 0.
10.2 Undercut Parameters Thread undercut DIN 76—external thread Thread pitch I K R W Thread undercut DIN 76—internal thread Thread pitch I K R W 3 D –4.4 10.5 1.6 30° 3 D +0.5 15.2 1.6 30° 3.5 D –5 12 1.6 30° 3.5 D +0.5 17.7 1.6 30° 4 D –5.7 14 2 30° 4 D +0.5 20 2 30° 4.5 D –6.4 16 2 30° 4.5 D +0.5 23 2 30° 5 D –7 17.5 2.5 30° 5 D +0.5 26 2.5 30° 5.5 D –7.7 19 3.2 30° 5.5 D +0.5 28 3.2 30° 6 D –8.3 21 3.2 30° 6 D +0.5 30 3.
MANUALplus determines the parameters from the diameter according to the following table. Undercut 509 E Diameter I K R <= 1.6 0.1 0.5 > 1.6 – 3 0.1 > 3 – 10 Designations: I = undercut depth K = undercut length R = undercut radius W= undercut angle undercut depth A= transverse angle W Undercut 509 F Diameter I K R W P A 0.1 15° <= 1.6 0.1 0.5 0.1 15° 0.1 8° 1 0.2 15° > 1.6 – 3 0.1 1 0.2 15° 0.1 8° 0.2 2 0.2 15° > 3 – 10 0.2 2 0.4 15° 0.
10.3 Technical Information 10.3 Technical Information Specifications Control design Contouring control with integrated motor control 2 controlled axes X/Z, controlled spindle and 1 driven tool Display Integrated 10.4-inch TFT color flat-panel display Highlighted actual-value and status displays Load display for spindle Error messages in plain language Program memory Hard disk > 4.5 GB Input resolution and display step X axis: 0.5 µm, diameter: 1 µm Z axis: 1 µm C axis: 0.
Manual operation Manually controlled slide movement via intermediate switch or electronic handwheels Graphically supported entry and execution of cycles in conjunction with manual machine operation Thread repair function for reworking threads with unclamped and re-clamped workpieces Teach-in mode Sequential linking of machining cycles Graphic simulation of each machining cycle after completion of data input Immediate execution after input of cycle Storage of machining cycles with automatic
10.
Electronic handwheels For moving the axes as on a manual lathe; a maximum of two electronic handwheels can be connected. In addition, the portable handwheel HR410 can be connected. DataPilot Control software on PCs for: Programming and program test Program management Management of operating-resource data Data backup Training HEIDENHAIN MANUALplus 4110 531 10.
10.4 Peripheral Interface 10.4 Peripheral Interface Connector: 9-pin, D-sub pins Pin Signal RS-232 1 Do not assign 2 RxD Receive Data 3 TxD Transmit Data 4 DTR Data Terminal Ready 5 GND Signal Ground 6 DSR Data Set Ready 7 RTS Request to Send 8 CTS Clear to Send 9 Do not assign The interface is linked to the external PC by direct electrical connection. This may lead to interference in the interface, resulting from different power-supply reference levels.
A Absolute coordinates ... 26 Access authorization ... 453 Access control for networks ... 443 Additive compensation DIN cycle G149 ... 303 Input during program execution ... 65 Parameters ... 432 Address letters ... 279 Alphanumeric keyboard ... 35 Angle of infeed (thread cycle) ... 163 API thread Cycle programming ... 170 DIN cycle G352 ... 342 Arcs menu, calling (ICP) ... 244 Area milling, face G797 ... 366 Auto-logon ... 444 Axial holes ... 355 Axis designations ... 25 B Backup name ...
Index Contour roughing Contour-parallel G836 ... 317 Longitudinal G817/G818 ... 311 Longitudinal with recessing G819 ... 313 Transverse G827/G828 ... 314 Transverse with recessing G829 ... 316 Contour, splitting (ICP) ... 258 Contour-parallel roughing DIN cycle G836 ... 317 ICP contour-parallel (cycle programming) ... 117 Contours (ICP) Contour editing ... 254 Contour elements, face ... 268 Contour elements, lateral surface ... 272 Contour elements, turning contour ... 260 Contour graphics ...
F F display ... 47 Face (ICP contour elements) ... 268 Face milling (cycle programming) ... 211 Face view (simulation) ... 70 Facing ... 419 Facing tools ... 419 Feed per minute Cycle mode ... 48 DIN cycle G94 ... 298 Feed per revolution for manual control (parameter) ... 432 Feed per revolution, driven tools ... 47 Feed rate Cycle mode ... 48 DIN programming Constant feed rate G94 ... 298 Feed per revolution G95/G195 ... 298 Feed per tooth G193 ... 298 Feed rate, programming ...
Index I ICP contour elements Face ... 268 Lateral surface ... 272 Turning contour ... 260 ICP cycles Figure milling, axial ... 208 Figure milling, radial ... 220 Finishing contour-parallel ... 119 Finishing, longitudinal/transverse ... 123 Fundamentals ... 83 Recess turning radial/axial, finishing ... 154 Recess turning, radial/axial ... 152 Recessing radial/axial ... 139 Recessing radial/axial, finishing ... 141 Roughing, contour-parallel ... 117 Roughing, longitudinal/transverse ...
HEIDENHAIN MANUALplus 4110 G793 Contour and figure milling cycle, face ... 364 G794 Contour and figure milling cycle, lateral surface ... 377 G797 Area milling, face ... 366 G798 Helical-slot milling ... 379 G799 Thread milling, axial ... 358 G80 End of cycle ... 310 G81 Longitudinal roughing ... 319 G811 Simple recess-turning cycle, longitudinal ... 332 G815 Recess-turning cycle, longitudinal ... 333 G817 Longitudinal contour roughing ... 311 G818 Longitudinal contour roughing ...
Index M M functions DIN programming ... 408 Fundamentals of cycle programming ... 82 M cycle, entering … (cycle programming) ... 97 M19 (spindle positioning, cycle programming) ... 97 M00 Program STOP ... 408 Machine commands ... 409 Machine data Cycle programming ... 83 DIN programming ... 286 Display configuration ... 439 Input and display ... 46 Machine dimensions ... 435 Machine operating panel ... 24 Machine reference points ... 27 Machine setup ... 50 Machine variables ... 286 Machine zero point ...
HEIDENHAIN MANUALplus 4110 Protection zone Deactivate, DIN cycle G60 ... 391 Display of protection zone status ... 51 Protection zone, setting (setting up the machine) ... 51 Protocol (serial data transfer) ... 445 Q Quantity, monitoring for number of parts produced Fundamentals ... 59 Tool data ... 427 R Rapid traverse Contouring speed for manual control (parameter) ... 432 Cycle programming Rapid traverse positioning ... 89 Rapid-traverse positioning, C axis ... 202 DIN programming Rapid traverse G0 ..
Index Recessing cycles Cycle programming ICP recessing cycle ... 139 ICP recessing cycle, finishing ... 141 Recessing ... 131 Recessing finishing, expanded ... 137 Recessing finishing, simple ... 135 Recessing, expanded ... 133 DIN programming Contour recessing G861/G862 ... 324 Contour recessing, finishing G863/G864 ... 326 Recessing cycle, simple G865/G866 ... 328 Recessing, finishing G867/G868 ... 329 Recessing tools ... 412, 421 Recess-turning tools ... 412 Reference diameter G120 ...
T T display ... 47 Tangential transition ... 245 Tapered thread Cycle programming ... 168 DIN cycle G353 ... 343 Tapping tools ... 424 Teach-in ... 62 Terms used ... 39 Thread Cycle programming API thread ... 170 API thread, recutting ... 178 Tapered thread ... 168 Tapered thread, recutting ... 176 Tapping, axial/radial ... 195 Thread and undercut cycles ... 162 Thread chamfer ... 180 Thread cycle ... 165 Thread cycle, expanded ... 166 Thread depth ... 163 Thread milling, axial ... 197 Thread position ...
Index Transfer values for subprograms ... 407 Transferring parameters ... 451 Transferring tool data ... 452 Twist drill cutter ... 413 Twist drills ... 413 U Undercut ... 344, 345 Cycle programming Thread undercut DIN 76 ... 180 Undercut DIN 509 E ... 182 Undercut DIN 509 F ... 184 Undercut position ... 162 Undercut type H ... 156 Undercut type K ... 157 Undercut type U ... 158 DIN programming Undercut contour G25 ... 344 Undercut cycle G85 ... 345 Undercut DIN 509 E G851 ...
Definition of workpiece blank Page Tool compensation Page G20 Standard blank (bar, tube) 288 G148 Changing the cutter compensation 302 G21 Contour of workpiece blank 289 G149 Additive compensation 303 G150 Compensate right tool tip 304 G151 Compensate left tool tip 304 Tool positioning without machining Page G0 Positioning in rapid traverse 290 G14 Approach the tool change position 291 Zero point shifts Page G51 Zero point shift 305 G56 Additive zero point shift 306 G59
Overview of G functions Recessing cycles Page Undercut cycles, parting cycles Page G86 Simple recessing cycle 330 G25 344 G861 Axial contour recessing 324 Undercut contour (DIN509 E, DIN509 F, DIN76) G862 Radial contour recessing 324 G85 Undercut cycle (DIN509 E, DIN509 F, DIN76) 345 G863 Axial contour recessing, finishing 326 G851 Undercut with cylinder machining DIN 509 E 347 G864 Radial contour recessing, finishing 326 G852 Undercut with cylinder machining DIN 509 F 348 G865
Page Other functions Page G100 Rapid traverse, face 360 G4 Dwell time 391 G101 Linear path, face 361 G9 Block precision stop 391 G102 Circular arc, face 362 G60 Deactivate protection zone 391 G103 Circular arc, face 362 G204 Waiting for time 391 G304 Figure definition, full circle, face 368 G305 Figure definition, rectangle, face 369 G307 Figure definition, polygon, face 370 G743 Linear pattern, face 383 G745 Circular pattern, face 385 G791 Linear slot, face 363
Overview of Cycles Workpiece blank cycles Page Roughing cycles Page Overview 85 Overview Standard blank 86 Cut longitudinal Roughing and finishing cycle for simple contours 101 ICP blank 87 Cut transverse Roughing and finishing cycle for simple contours 101 109 88 Plunge, longitudinal Roughing and finishing cycle for simple contours 109 89 Plunge, transverse Roughing and finishing cycle for simple contours 117 90 ICP contour-parallel, longitudinal Roughing and finishing cycle for any
Recessing cycles Page Thread Cycles Page Overview 129 Overview 162 Recessing, radial Recessing and finishing cycles for simple contours 131 Thread cycle Longitudinal single or multi-start thread 165 Recessing, axial Recessing and finishing cycles for simple contours 131 Tapered thread Tapered single or multi-start thread 168 ICP recessing, radial 139 Recessing and finishing cycles for any type of contour API thread Single or multi-start API thread (API: American Petroleum Institute) 170 1
Drilling cycles Page Milling cycles Page Overview 190 Face milling For milling surfaces or polygons Axial drilling cycle For drilling single holes and patterns 191 Slot, radial 215 For milling single slots or slot patterns Radial drilling cycle For drilling single holes and patterns 191 Figure, radial For milling a single figure 216 Axial deep-hole drilling cycle For drilling single holes and patterns 193 Radial ICP contour For milling single ICP contours or contour patterns 220 Radial dee
DR. JOHANNES HEIDENHAIN GmbH Dr.-Johannes-Heidenhain-Straße 5 83301 Traunreut, Germany { +49 (86 69) 31-0 | +49 (86 69) 50 61 E-Mail: info@heidenhain.de Technical support | +49 (86 69) 32-10 00 Measuring systems { +49 (86 69) 31-31 04 E-Mail: service.ms-support@heidenhain.de TNC support { +49 (86 69) 31-31 01 E-Mail: service.nc-support@heidenhain.de NC programming { +49 (86 69) 31-31 03 E-Mail: service.nc-pgm@heidenhain.de PLC programming { +49 (86 69) 31-31 02 E-Mail: service.plc@heidenhain.
