TNC 640 User’s manual for cycle programming NC Software 340590-06 340591-06 340595-06 English (en) 9/2015
Fundamentals
Fundamentals About this Manual About this Manual The symbols used in this manual are described below. This symbol indicates that important information about the function described must be considered. WARNING This symbol indicates a possibly dangerous situation that may cause light injuries if not avoided.
TNC model, software and features TNC model, software and features This manual describes functions and features provided by TNCs as of the following NC software numbers. TNC model NC software number TNC 640 340590-06 TNC 640 E 340591-06 TNC 640 Programming Station 340595-06 The suffix E indicates the export version of the TNC.
Fundamentals TNC model, software and features Software options The TNC 640 features various software options that can be enabled by your machine tool builder.
TNC model, software and features DXF Converter (option 42) DXF converter Supported DXF format: AC1009 (AutoCAD R12) Adoption of contours and point patterns Simple and convenient specification of reference points Select graphical features of contour sections from conversational programs Adaptive Feed Control – AFC (option 45) Adaptive Feed Control Recording the actual spindle power by means of a teach-in cut Defining the limits of automatic feed rate control Fully automatic feed control during program ru
Fundamentals TNC model, software and features Visual Setup Control – VSC (option number 136) Camera-based monitoring of the setup situation Record the setup situation with a HEIDENHAIN camera system Visual comparison of planned and actual status in the workspace Cross Talk Compensation – CTC (option number 141) Compensation of axis couplings Determination of dynamically caused position deviation through axis acceleration Compensation of the TCP (Tool Center Point) Position Adaptive Control – PAC (optio
TNC model, software and features Feature Content Level (upgrade functions) Along with software options, significant further improvements of the TNC software are managed via the Feature Content Level upgrade functions. Functions subject to the FCL are not available simply by updating the software on your TNC. All upgrade functions are available to you without surcharge when you receive a new machine.
Fundamentals Optional parameters Optional parameters The comprehensive cycle package is continuously further developed by HEIDENHAIN. Every new software version thus may also introduce new Q parameters for cycles. These new Q parameters are optional parameters, some of which have not been available in previous software versions. Within a cycle, they are always provided at the end of the cycle definition.
New cycle functions of software New cycle functions of software 34059x-04 The character set of the fixed cycle 225 Engraving was expanded by more characters and the diameter sign see "ENGRAVING (Cycle 225, DIN/ISO: G225)", page 309 New machining cycle 275 Trochoidal milling see "TROCHOIDAL SLOT (Cycle 275, DIN ISO G275)", page 219 New machining cycle 233 Face milling see "FACE MILLING (Cycle 233, DIN/ISO: G233)", page 174 In Cycle 205 Universal Pecking you can now use parameter Q208 to define a feed rate f
Fundamentals New and changed cycle functions of software New and changed cycle functions of software 34059x-05 New Cycle 880 GEAR HOBBING (software option 50), see "GEAR HOBBING (Cycle 880, DIN/ISO: G880)", page 435 New Cycle 292 CONTOUR FINISHING TURNING INTERPOLATION (software option 96), see "CONTOUR TURNING INTERPOLATION (Cycle 292, DIN/ISO: G292, software option 96)", page 294 New Cycle 291 COUPLING TURNING INTERPOLATION (software option 96), see "COUPLING INTERPOLATION TURNING (cycle 291, DIN/ISO: G2
New and changed cycle functions of software New and changed cycle functions of software 34059x-06 New cycle 258 POLYGON STUD see "CIRCULAR STUD (cycle 258, DIN/ISO: G258)", page 169 New cycles 600 and 601 for Visual Setup Control (software option 136), see "Camera-based monitoring of the setup situation VSC (option number136)", page 596 Cycle 291 COUPLING TURNING INTERPOLATION (software option 96), was expanded by parameter Q561, see "COUPLING INTERPOLATION TURNING (cycle 291, DIN/ISO: G291, software optio
Fundamentals New and changed cycle functions of software 14 HEIDENHAIN | TNC 640 | User’s manual for cycle programming | 9/2015
Contents 1 Fundamentals / Overviews............................................................................................................51 2 Using Fixed Cycles......................................................................................................................... 55 3 Fixed Cycles: Drilling...................................................................................................................... 75 4 Fixed Cycles: Tapping / Thread Milling............................
Contents 16 HEIDENHAIN | TNC 640 | User’s manual for cycle programming | 9/2015
1 Fundamentals / Overviews............................................................................................................51 1.1 Introduction............................................................................................................................................52 1.2 Available Cycle Groups.........................................................................................................................53 Overview of fixed cycles......................................
Contents 2 Using Fixed Cycles......................................................................................................................... 55 2.1 Working with fixed cycles....................................................................................................................56 Machine-specific cycles...........................................................................................................................56 Defining a cycle using soft keys..........................
3 Fixed Cycles: Drilling...................................................................................................................... 75 3.1 Fundamentals........................................................................................................................................ 76 Overview................................................................................................................................................. 76 3.2 CENTERING (Cycle 240, DIN/ISO: G240).........
Contents 3.9 BORE MILLING (Cycle 208).................................................................................................................. 96 Cycle run................................................................................................................................................. 96 Please note while programming:............................................................................................................ 97 Cycle parameters.......................................
4 Fixed Cycles: Tapping / Thread Milling...................................................................................... 105 4.1 Fundamentals...................................................................................................................................... 106 Overview............................................................................................................................................... 106 4.2 TAPPING with a floating tap holder (Cycle 206, DIN/ISO: G206).
Contents 4.9 HELICAL THREAD DRILLING/MILLING (Cycle 265, DIN/ISO: G265)...............................................130 Cycle run............................................................................................................................................... 130 Please note while programming:.......................................................................................................... 131 Cycle parameters..........................................................................
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling........................................................141 5.1 Fundamentals...................................................................................................................................... 142 Overview............................................................................................................................................... 142 5.2 RECTANGULAR POCKET (Cycle 251, DIN/ISO: G251)............................
Contents 5.9 FACE MILLING (Cycle 233, DIN/ISO: G233)...................................................................................... 174 Cycle run............................................................................................................................................... 174 Please note while programming:.......................................................................................................... 178 Cycle parameters.....................................................
6 Fixed Cycles: Pattern Definitions................................................................................................ 185 6.1 Fundamentals...................................................................................................................................... 186 Overview............................................................................................................................................... 186 6.2 POLAR PATTERN (Cycle 220, DIN/ISO: G220).................
Contents 7 Fixed Cycles: Contour Pocket......................................................................................................195 7.1 SL Cycles.............................................................................................................................................. 196 Fundamentals........................................................................................................................................ 196 Overview...........................................
7.9 CONTOUR TRAIN (Cycle 25, DIN/ISO: G125)...................................................................................216 Cycle run............................................................................................................................................... 216 Please note while programming:.......................................................................................................... 216 Cycle parameters...................................................................
Contents 8 Fixed Cycles: Cylindrical Surface................................................................................................ 229 8.1 Fundamentals...................................................................................................................................... 230 Overview of cylindrical surface cycles..................................................................................................230 8.2 CYLINDER SURFACE (Cycle 27, DIN/ISO: G127, software option 1)..
9 Fixed Cycles: Contour Pocket with Contour Formula...............................................................247 9.1 SL cycles with complex contour formula.........................................................................................248 Fundamentals........................................................................................................................................ 248 Selecting a program with contour definitions............................................................
Contents 10 Cycles: Coordinate Transformations........................................................................................... 261 10.1 Fundamentals...................................................................................................................................... 262 Overview............................................................................................................................................... 262 Effect of coordinate transformations.....................
10.8 AXIS-SPECIFIC SCALING (Cycle 26)..................................................................................................275 Effect..................................................................................................................................................... 275 Please note while programming:.......................................................................................................... 275 Cycle parameters........................................................
Contents 11 Cycles: Special Functions............................................................................................................ 285 11.1 Fundamentals...................................................................................................................................... 286 Overview............................................................................................................................................... 286 11.2 DWELL TIME (Cycle 9, DIN/ISO: G04)..........
11.8 ENGRAVING (Cycle 225, DIN/ISO: G225)..........................................................................................309 Cycle run............................................................................................................................................... 309 Please note while programming:.......................................................................................................... 309 Cycle parameters...............................................................
Contents 12 Cycles: Turning.............................................................................................................................. 325 12.1 Turning Cycles (software option 50)..................................................................................................326 Overview............................................................................................................................................... 326 Working with turning cycles............................
12.8 TURN, LONGITUDINAL PLUNGE EXTENDED (Cycle 814, DIN/ISO: G814)....................................350 Application............................................................................................................................................. 350 Roughing cycle run................................................................................................................................350 Finishing cycle run................................................................................
Contents 12.13TURN, TRANSVERSE PLUNGE (Cycle 823, DIN/ISO: G823)........................................................... 369 Application............................................................................................................................................. 369 Roughing cycle run................................................................................................................................369 Finishing cycle run.........................................................
12.18RECESSING CONTOUR RADIAL (Cycle 840, DIN/ISO: G840)......................................................... 388 Application............................................................................................................................................. 388 Roughing cycle run................................................................................................................................388 Finishing cycle run....................................................................
Contents 12.23RADIAL RECESSING EXTENDED (Cycle 862, DIN/ISO: G862)........................................................ 407 Application............................................................................................................................................. 407 Roughing cycle run................................................................................................................................407 Finishing cycle run..........................................................
12.28THREAD LONGITUDINAL (Cycle 831, DIN/ISO: G831).................................................................... 424 Application............................................................................................................................................. 424 Cycle run............................................................................................................................................... 424 Please note while programming:............................................
Contents 13 Using Touch Probe Cycles........................................................................................................... 447 13.1 General information about touch probe cycles............................................................................... 448 Method of function............................................................................................................................... 448 Consideration of a basic rotation in the Manual Operation mode..................
14 Touch Probe Cycles: Automatic Measurement of Workpiece Misalignment.......................... 457 14.1 Fundamentals...................................................................................................................................... 458 Overview............................................................................................................................................... 458 Characteristics common to all touch probe cycles for measuring workpiece misalignment..............
Contents 15 Touch Probe Cycles: Automatic Datum Setting........................................................................ 479 15.1 Fundamentals...................................................................................................................................... 480 Overview............................................................................................................................................... 480 Characteristics common to all touch probe cycles for datum setting.
15.9 DATUM FROM INSIDE OF CORNER (Cycle 415, DIN/ISO: G415)....................................................512 Cycle run............................................................................................................................................... 512 Please note while programming:.......................................................................................................... 513 Cycle parameters...................................................................................
Contents 16 Touch Probe Cycles: Automatic Workpiece Inspection.............................................................533 16.1 Fundamentals...................................................................................................................................... 534 Overview............................................................................................................................................... 534 Recording the results of measurement....................................
16.8 MEASURE RECTANGLE OUTSIDE (Cycle 424, DIN/ISO: G424)...................................................... 558 Cycle run............................................................................................................................................... 558 Please note while programming:.......................................................................................................... 558 Cycle parameters..................................................................................
Contents 17 Touch Probe Cycles: Special Functions...................................................................................... 579 17.1 Fundamentals...................................................................................................................................... 580 Overview............................................................................................................................................... 580 17.2 MEASURE (Cycle 3).....................................
18 Visual Setup Control VSC (software option 136)..................................................................... 595 18.1 Camera-based monitoring of the setup situation VSC (option number136)................................ 596 Fundamentals........................................................................................................................................ 596 Produce live image...........................................................................................................
Contents 19 Touch Probe Cycles: Automatic Kinematics Measurement...................................................... 617 19.1 Kinematics Measurement with TS Touch Probes (KinematicsOpt option)................................... 618 Fundamentals........................................................................................................................................ 618 Overview....................................................................................................................
20 Touch Probe Cycles: Automatic Tool Measurement..................................................................649 20.1 Fundamentals...................................................................................................................................... 650 Overview............................................................................................................................................... 650 Differences between Cycles 31 to 33 and Cycles 481 to 483........................
Contents 21 Tables of Cycles............................................................................................................................ 665 21.1 Overview.............................................................................................................................................. 666 Fixed cycles...........................................................................................................................................666 Turning cycles.........................
1 Fundamentals / Overviews
1 Fundamentals / Overviews 1.1 1.1 Introduction Introduction Frequently recurring machining cycles that comprise several working steps are stored in the TNC memory as standard cycles. Coordinate transformations and several special functions are also available as cycles. Most cycles use Q parameters as transfer parameters. Danger of collision! Cycles sometimes execute extensive operations. For safety reasons, you should run a graphical program test before machining.
1 Available Cycle Groups 1.2 1.
1 Fundamentals / Overviews 1.
2 Using Fixed Cycles
2 Using Fixed Cycles 2.1 2.1 Working with fixed cycles Working with fixed cycles Machine-specific cycles In addition to the HEIDENHAIN cycles, many machine tool builders offer their own cycles in the TNC.
2 Working with fixed cycles 2.1 Defining a cycle using soft keys The soft-key row shows the available groups of cycles Press the soft key for the desired group of cycles, for example DRILLING for the drilling cycles Select the cycle, e.g. THREAD MILLING. The TNC initiates the programming dialog and asks for all required input values. At the same time a graphic of the input parameters is displayed in the right screen window. The parameter that is asked for in the dialog prompt is highlighted.
2 Using Fixed Cycles 2.1 Working with fixed cycles Calling a cycle Prerequisites The following data must always be programmed before a cycle call: BLK FORM for graphic display (needed only for test graphics) Tool call Direction of spindle rotation (M functions M3/M4) Cycle definition (CYCL DEF) For some cycles, additional prerequisites must be observed. They are detailed in the descriptions for each cycle.
2 Working with fixed cycles 2.1 Calling a cycle with CYCL CALL POS The CYCL CALL POS function calls the most recently defined fixed cycle once. The starting point of the cycle is the position that you defined in the CYCL CALL POS block. Using positioning logic the TNC moves to the position defined in the CYCL CALL POS block.
2 Using Fixed Cycles 2.2 Program defaults for cycles 2.2 Program defaults for cycles Overview All Cycles 20 to 25, as well as all of those with numbers 200 or higher, always use identical cycle parameters, such as the set-up clearance Q200, which you must enter for each cycle definition. The GLOBAL DEF function gives you the possibility of defining these cycle parameters at the beginning of the program, so that they are effective globally for all machining cycles used in the program.
2 Program defaults for cycles 2.2 Using GLOBAL DEF information If you have entered the corresponding GLOBAL DEF functions at the beginning of the program, then you can link to these globally valid values when defining any fixed cycle. Proceed as follows: Select the Programming and Editing operating mode Select fixed cycles Select the desired group of cycles, for example: drilling cycles Select the desired cycle, e.g.
2 Using Fixed Cycles 2.2 Program defaults for cycles Global data valid everywhere Set-up clearance: Distance between tool tip and workpiece surface for automated approach of the cycle start position in the tool axis 2nd set-up clearance: Position to which the TNC positions the tool at the end of a machining step.
2 Program defaults for cycles 2.
2 Using Fixed Cycles 2.3 PATTERN DEF pattern definition 2.3 PATTERN DEF pattern definition Application You use the PATTERN DEF function to easily define regular machining patterns, which you can call with the CYCL CALL PAT function. As with the cycle definitions, support graphics that illustrate the respective input parameter are also available for pattern definitions. PATTERN DEF is to be used only in connection with the tool axis Z.
2 PATTERN DEF pattern definition 2.3 Entering PATTERN DEF Select the Programming mode of operation Press the special functions key Select the functions for contour and point machining Open a PATTERN DEF block Select the desired machining pattern, e.g. a single row Enter the required definitions, and confirm each entry with the ENT key Using PATTERN DEF As soon as you have entered a pattern definition, you can call it with the CYCL CALL PAT function.
2 Using Fixed Cycles 2.3 PATTERN DEF pattern definition Defining individual machining positions NC blocks You can enter up to 9 machining positions. Confirm each entry with the ENT key. If you have defined a workpiece surface in Z not equal to 0, then this value is effective in addition to the workpiece surface Q203 that you defined in the machining cycle. 10 L Z+100 R0 FMAX 11 PATTERN DEF POS1 (X+25 Y+33.5 Z+0) POS2 (X+50 Y +75 Z+0) X coord.
2 PATTERN DEF pattern definition 2.3 Defining a single pattern If you have defined a workpiece surface in Z not equal to 0, then this value is effective in addition to the workpiece surface Q203 that you defined in the machining cycle. The Rotary pos. ref. ax. and Rotary pos. minor ax. parameters are added to a previously performed rotated position of the entire pattern. NC blocks 10 L Z+100 R0 FMAX 11 PATTERN DEF PAT1 (X+25 Y+33.
2 Using Fixed Cycles 2.3 PATTERN DEF pattern definition Defining individual frames If you have defined a workpiece surface in Z not equal to 0, then this value is effective in addition to the workpiece surface Q203 that you defined in the machining cycle. The Rotary pos. ref. ax. and Rotary pos. minor ax. parameters are added to a previously performed rotated position of the entire pattern. NC blocks 10 L Z+100 R0 FMAX 11 PATTERN DEF FRAME1 (X+25 Y+33.
2 PATTERN DEF pattern definition 2.3 Defining a full circle If you have defined a workpiece surface in Z not equal to 0, then this value is effective in addition to the workpiece surface Q203 that you defined in the machining cycle.
2 Using Fixed Cycles 2.3 PATTERN DEF pattern definition Defining a pitch circle If you have defined a workpiece surface in Z not equal to 0, then this value is effective in addition to the workpiece surface Q203 that you defined in the machining cycle.
2 Point tables 2.4 2.4 Point tables Application You should create a point table whenever you want to run a cycle, or several cycles in sequence, on an irregular point pattern. If you are using drilling cycles, the coordinates of the working plane in the point table represent the hole centers. If you are using milling cycles, the coordinates of the working plane in the point table represent the starting-point coordinates of the respective cycle (e.g. center-point coordinates of a circular pocket).
2 Using Fixed Cycles 2.4 Point tables Hiding single points from the machining process In the FADE column of the point table you can specify if the defined point is to be hidden during the machining process.
2 Point tables 2.4 Calling a cycle in connection with point tables With CYCL CALL PAT the TNC runs the point table that you last defined (even if you defined the point table in a program that was nested with CALL PGM).
3 Fixed Cycles: Drilling
3 Fixed Cycles: Drilling 3.1 Fundamentals 3.
3 CENTERING (Cycle 240) 3.2 3.2 CENTERING (Cycle 240, DIN/ISO: G240) Cycle run 1 The TNC positions the tool in the tool axis at rapid traverse FMAX to set-up clearance above the workpiece surface. 2 The tool is centered at the programmed feed rate F to the programmed centering diameter or centering depth. 3 If defined, the tool remains at the centering depth. 4 Finally, the tool path is retraced to setup clearance or—if programmed—to the 2nd setup clearance at rapid traverse FMAX.
3 Fixed Cycles: Drilling 3.2 CENTERING (Cycle 240) Cycle parameters Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Enter a positive value. Input range 0 to 99999.9999 Select depth/diameter (0/1) Q343: Select whether centering is based on the entered diameter or depth. If the TNC is to center based on the entered diameter, the point angle of the tool must be defined in the T ANGLE column of the tool table TOOL.T.
3 DRILLING (Cycle 200) 3.3 3.3 DRILLING (Cycle 200) Cycle run 1 The TNC positions the tool in the tool axis at rapid traverse FMAX to set-up clearance above the workpiece surface. 2 The tool drills to the first plunging depth at the programmed feed rate F. 3 The TNC returns the tool at FMAX to the set-up clearance, dwells there (if a dwell time was entered), and then moves at FMAX to the set-up clearance above the first plunging depth.
3 Fixed Cycles: Drilling 3.3 DRILLING (Cycle 200) Cycle parameters Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Enter a positive value. Input range 0 to 99999.9999 Depth Q201 (incremental): Distance between workpiece surface and bottom of hole. Input range -99999.9999 to 99999.9999 Feed rate for plunging Q206: Traversing speed of the tool in mm/min during drilling. Input range 0 to 99999.
3 REAMING (Cycle 201) 3.4 3.4 REAMING (Cycle 201, DIN/ISO: G201) Cycle run 1 The TNC positions the tool in the tool axis at rapid traverse FMAX to the entered set-up clearance above the workpiece surface. 2 The tool reams to the entered depth at the programmed feed rate F. 3 If programmed, the tool remains at the hole bottom for the entered dwell time. 4 The tool then retracts to set-up clearance at the feed rate F, and from there—if programmed—to the 2nd set-up clearance in FMAX.
3 Fixed Cycles: Drilling 3.4 REAMING (Cycle 201) Cycle parameters Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Input range 0 to 99999.9999 Depth Q201 (incremental): Distance between workpiece surface and bottom of hole. Input range -99999.9999 to 99999.9999 Feed rate for plunging Q206: Traversing speed of the tool during reaming in mm/min. Input range 0 to 99999.
3 BORING (Cycle 202) 3.5 3.5 BORING (Cycle 202, DIN/ISO: G202) Cycle run 1 The TNC positions the tool in the tool axis at rapid traverse FMAX to set-up clearance above the workpiece surface. 2 The tool drills to the programmed depth at the feed rate for plunging. 3 If programmed, the tool remains at the hole bottom for the entered dwell time with active spindle rotation for cutting free. 4 The TNC then orients the spindle to the position that is defined in parameter Q336.
3 Fixed Cycles: Drilling 3.5 BORING (Cycle 202) Please note while programming: Machine and TNC must be specially prepared by the machine tool builder for use of this cycle. This cycle is effective only for machines with servocontrolled spindle. Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0. The algebraic sign for the cycle parameter DEPTH determines the working direction. If you program DEPTH=0, the cycle will not be executed.
3 BORING (Cycle 202) 3.5 Cycle parameters Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Input range 0 to 99999.9999 Depth Q201 (incremental): Distance between workpiece surface and bottom of hole. Input range -99999.9999 to 99999.9999 Feed rate for plunging Q206: Traversing speed of the tool during boring at mm/min. Input range 0 to 99999.999; alternatively FAUTO, FU Dwell time at depth Q211: Time in seconds that the tool remains at the hole bottom.
3 Fixed Cycles: Drilling 3.6 3.6 UNIVERSAL DRILLING (Cycle 203) UNIVERSAL DRILLING (Cycle 203, DIN/ISO: G203) Cycle run 1 The TNC positions the tool in the tool axis at rapid traverse FMAX to the entered set-up clearance above the workpiece surface. 2 The tool drills to the first plunging depth at the entered feed rate F. 3 If you have programmed chip breaking, the tool then retracts by the entered retraction value.
3 UNIVERSAL DRILLING (Cycle 203) 3.6 Cycle parameters Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Input range 0 to 99999.9999 Depth Q201 (incremental): Distance between workpiece surface and bottom of hole. Input range -99999.9999 to 99999.9999 Feed rate for plunging Q206: Traversing speed of the tool during drilling in mm/min. Input range 0 to 99999.999; alternatively FAUTO, FU Plunging depth Q202 (incremental): Infeed per cut. Input range 0 to 99999.9999.
3 Fixed Cycles: Drilling 3.6 UNIVERSAL DRILLING (Cycle 203) Dwell time at depth Q211: Time in seconds that the tool remains at the hole bottom. Input range 0 to 3600.0000 Feed rate for retraction Q208: Traversing speed of the tool in mm/min when retracting from the hole. If you enter Q208 = 0, the TNC retracts the tool at the feed rate Q206. Input range 0 to 99999.
3 BACK BORING (Cycle 204) 3.7 3.7 BACK BORING (Cycle 204, DIN/ISO: G204) Cycle run This cycle allows holes to be bored from the underside of the workpiece. 1 The TNC positions the tool in the tool axis at rapid traverse FMAX to set-up clearance above the workpiece surface. 2 The TNC then orients the spindle to the 0° position with an oriented spindle stop and displaces the tool by the off-center distance.
3 Fixed Cycles: Drilling 3.7 BACK BORING (Cycle 204) Please note while programming: Machine and TNC must be specially prepared by the machine tool builder for use of this cycle. This cycle is effective only for machines with servocontrolled spindle. Special boring bars for upward cutting are required for this cycle. Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0.
3 BACK BORING (Cycle 204) 3.7 Cycle parameters Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Input range 0 to 99999.9999 Depth of counterbore Q249 (incremental): Distance between underside of workpiece and the top of the hole. A positive sign means the hole will be bored in the positive spindle axis direction. Input range -99999.9999 to 99999.9999 Material thickness Q250 (incremental): Thickness of the workpiece. Input range 0.0001 to 99999.
3 Fixed Cycles: Drilling 3.8 3.8 UNIVERSAL PECKING (Cycle 205) UNIVERSAL PECKING (Cycle 205, DIN/ISO: G205) Cycle run 1 The TNC positions the tool in the tool axis at rapid traverse FMAX to the entered set-up clearance above the workpiece surface. 2 If you enter a deepened starting point, the TNC move at the defined positioning feed rate to the set-up clearance above the deepened starting point. 3 The tool drills to the first plunging depth at the entered feed rate F.
3 UNIVERSAL PECKING (Cycle 205) 3.8 Please note while programming: Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0. The algebraic sign for the cycle parameter DEPTH determines the working direction. If you program DEPTH=0, the cycle will not be executed. If you enter different advance stop distances for Q258 and Q259, the TNC will change the advance stop distances between the first and last plunging depths at the same rate.
3 Fixed Cycles: Drilling 3.8 UNIVERSAL PECKING (Cycle 205) Cycle parameters Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Input range 0 to 99999.9999 Depth Q201 (incremental): Distance between workpiece surface and bottom of hole (tip of drill taper). Input range -99999.9999 to 99999.9999 Feed rate for plunging Q206: Traversing speed of the tool during drilling in mm/min. Input range 0 to 99999.
3 UNIVERSAL PECKING (Cycle 205) 3.8 Deepened starting point Q379 (incremental with respect to the workpiece surface): Starting position for actual drilling operation. The TNC moves at the feed rate for pre-positioning from the set-up clearance above the workpiece surface to the set-up clearance above the deepened starting point. Input range 0 to 99999.
3 Fixed Cycles: Drilling 3.9 3.9 BORE MILLING (Cycle 208) BORE MILLING (Cycle 208) Cycle run 1 The TNC positions the tool in the tool axis at rapid traverse FMAX to the programmed set-up clearance above the workpiece surface and then moves the tool to the bore hole circumference on a rounded arc (if enough space is available). 2 The tool mills in a helix from the current position to the first plunging depth at the programmed feed rate F.
3 BORE MILLING (Cycle 208) 3.9 Please note while programming: Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0. The algebraic sign for the cycle parameter DEPTH determines the working direction. If you program DEPTH=0, the cycle will not be executed. If you have entered the bore hole diameter to be the same as the tool diameter, the TNC will bore directly to the entered depth without any helical interpolation.
3 Fixed Cycles: Drilling 3.9 BORE MILLING (Cycle 208) Cycle parameters Set-up clearance Q200 (incremental): Distance between tool lower edge and workpiece surface. Input range 0 to 99999.9999 Depth Q201 (incremental): Distance between workpiece surface and bottom of hole. Input range -99999.9999 to 99999.9999 Feed rate for plunging Q206: Traversing speed of the tool in mm/min during helical drilling. Input range 0 to 99999.
3 SINGLE-LIP DEEP-HOLE DRILLING (Cycle 241) 3.10 3.10 SINGLE-LIP DEEP-HOLE DRILLING (Cycle 241, DIN/ISO: G241) Cycle run 1 The TNC positions the tool in the tool axis at rapid traverse FMAX to the entered set-up clearance above the workpiece surface. 2 Then the TNC moves the tool at the defined positioning feed rate to the set-up clearance above the deepened starting point and activates the drilling speed (M3) and the coolant.
3 Fixed Cycles: Drilling 3.10 SINGLE-LIP DEEP-HOLE DRILLING (Cycle 241) Cycle parameters Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Input range 0 to 99999.9999 Depth Q201 (incremental): Distance between workpiece surface and bottom of hole. Input range -99999.9999 to 99999.9999 Feed rate for plunging Q206: Traversing speed of the tool during drilling in mm/min. Input range 0 to 99999.
3 SINGLE-LIP DEEP-HOLE DRILLING (Cycle 241) 3.10 M function for coolant on? Q429: M function for switching on the coolant. The TNC switches the coolant on if the tool is in the hole at the deepened starting point. Input range 0 to 999 M function for coolant off? Q430: M function for switching off the coolant. The TNC switches the coolant off if the tool is at the hole depth. Input range 0 to 999 Dwell depth Q435 (incremental): Coordinate in the spindle axis at which the tool is to dwell.
3 Fixed Cycles: Drilling 3.11 Programming Examples 3.11 Programming Examples Example: Drilling cycles 0 BEGIN PGM C200 MM 1 BLK FORM 0.1 Z X+0 Y+0 Z-20 Definition of workpiece blank 2 BLK FORM 0.
3 Programming Examples 3.11 Example: Using drilling cycles in connection with PATTERN DEF The drill hole coordinates are stored in the pattern definition PATTERN DEF POS and are called by the TNC with CYCL CALL PAT. The tool radii are selected so that all work steps can be seen in the test graphics. Program sequence Centering (tool radius 4) Drilling (tool radius 2.4) Tapping (tool radius 3) 0 BEGIN PGM 1 MM 1 BLK FORM 0.1 Z X+0 Y+0 Z-20 Definition of workpiece blank 2 BLK FORM 0.
3 Fixed Cycles: Drilling 3.11 Programming Examples 11 CYCL DEF 200 DRILLING Q200=2 ;SET-UP CLEARANCE Q201=-25 ;DEPTH Q206=150 ;FEED RATE FOR PLNGNG Q202=5 ;PLUNGING DEPTH Q211=0 ;DWELL TIME AT TOP Q203=+0 ;SURFACE COORDINATE Q204=50 ;2ND SET-UP CLEARANCE Q211=0.
4 Fixed Cycles: Tapping / Thread Milling
4 Fixed Cycles: Tapping / Thread Milling 4.1 Fundamentals 4.
4 TAPPING with a floating tap holder (Cycle 206) 4.2 4.2 TAPPING with a floating tap holder (Cycle 206, DIN/ISO: G206) Cycle run 1 The TNC positions the tool in the tool axis at rapid traverse FMAX to the entered set-up clearance above the workpiece surface. 2 The tool drills to the total hole depth in one movement. 3 Once the tool has reached the total hole depth, the direction of spindle rotation is reversed and the tool is retracted to the setup clearance at the end of the dwell time.
4 Fixed Cycles: Tapping / Thread Milling 4.2 TAPPING with a floating tap holder (Cycle 206) Please note while programming: Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0. The algebraic sign for the cycle parameter DEPTH determines the working direction. If you program DEPTH=0, the cycle will not be executed. A floating tap holder is required for tapping.
4 TAPPING with a floating tap holder (Cycle 206) 4.2 Cycle parameters Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Input range 0 to 99999.9999 Guide value: 4x pitch. Thread depth Q201 (incremental): Distance between workpiece surface and root of thread. Input range -99999.9999 to 99999.9999 Feed rate F Q206: Traversing speed of the tool during tapping. Input range 0 to 99999.999 alternatively FAUTO Dwell time at bottom Q211: Enter a value between 0 and 0.
4 Fixed Cycles: Tapping / Thread Milling 4.3 4.3 RIGID TAPPING without a floating tap holder (Cycle 207) RIGID TAPPING without a floating tap holder (Cycle 207, DIN/ ISO: G207) Cycle run The TNC cuts the thread without a floating tap holder in one or more passes. 1 The TNC positions the tool in the tool axis at rapid traverse FMAX to the entered set-up clearance above the workpiece surface. 2 The tool drills to the total hole depth in one movement.
4 RIGID TAPPING without a floating tap holder (Cycle 207) 4.3 Please note while programming: Machine and TNC must be specially prepared by the machine tool builder for use of this cycle. This cycle is effective only for machines with servocontrolled spindle. Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0. The algebraic sign for the cycle parameter DEPTH determines the working direction.
4 Fixed Cycles: Tapping / Thread Milling 4.3 RIGID TAPPING without a floating tap holder (Cycle 207) Cycle parameters Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Input range 0 to 99999.9999 Thread depth Q201 (incremental): Distance between workpiece surface and root of thread. Input range -99999.9999 to 99999.9999 Thread pitch Q239: Pitch of the thread.
4 TAPPING WITH CHIP BREAKING (Cycle 209, DIN/ISO: G209) 4.4 4.4 TAPPING WITH CHIP BREAKING (Cycle 209, DIN/ISO: G209) Cycle run The TNC machines the thread in several passes until it reaches the programmed depth. You can define in a parameter whether the tool is to be retracted completely from the hole for chip breaking. 1 The TNC positions the tool in the tool axis at rapid traverse FMAX to the programmed set-up clearance above the workpiece surface. There it carries out an oriented spindle stop.
4 Fixed Cycles: Tapping / Thread Milling 4.4 TAPPING WITH CHIP BREAKING (Cycle 209, DIN/ISO: G209) Please note while programming: Machine and TNC must be specially prepared by the machine tool builder for use of this cycle. This cycle is effective only for machines with servocontrolled spindle. Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0. The algebraic sign for the cycle parameter "thread depth" determines the working direction.
4 TAPPING WITH CHIP BREAKING (Cycle 209, DIN/ISO: G209) 4.4 Cycle parameters Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Input range 0 to 99999.9999 Thread depth Q201 (incremental): Distance between workpiece surface and root of thread. Input range -99999.9999 to 99999.9999 Thread pitch Q239: Pitch of the thread. The algebraic sign differentiates between right-hand and left-hand threads: + = right-hand thread –= left-hand thread Input range -99.9999 to 99.
4 Fixed Cycles: Tapping / Thread Milling 4.4 TAPPING WITH CHIP BREAKING (Cycle 209, DIN/ISO: G209) Retracting after a program interruption Retracting in the Manual Operation mode You can interrupt the thread cutting process by pressing the NC Stop key. A soft key for retracting the tool from the thread is displayed in the soft-key row below the screen. When you press this soft key and the NC Start key, the tool retracts from the hole and returns to the starting point of machining.
4 Fundamentals of Thread Milling 4.5 4.5 Fundamentals of Thread Milling Prerequisites Your machine tool should feature internal spindle cooling (cooling lubricant at least 30 bars, compressed air supply at least 6 bars). Thread milling usually leads to distortions of the thread profile. To correct this effect, you need tool-specific compensation values which are given in the tool catalog or are available from the tool manufacturer.
4 Fixed Cycles: Tapping / Thread Milling 4.5 Fundamentals of Thread Milling Danger of collision! Always program the same algebraic sign for the infeeds: Cycles comprise several sequences of operation that are independent of each other. The order of precedence according to which the work direction is determined is described with the individual cycles. For example, if you only want to repeat the countersinking process of a cycle, enter 0 for the thread depth.
4 THREAD MILLING (Cycle 262, DIN/ISO: G262) 4.6 4.6 THREAD MILLING (Cycle 262, DIN/ISO: G262) Cycle run 1 The TNC positions the tool in the tool axis at rapid traverse FMAX to the entered set-up clearance above the workpiece surface. 2 The tool moves at the programmed feed rate for pre-positioning to the starting plane. The starting plane is derived from the algebraic sign of the thread pitch, the milling method (climb or up-cut milling) and the number of threads per step.
4 Fixed Cycles: Tapping / Thread Milling 4.6 THREAD MILLING (Cycle 262, DIN/ISO: G262) Please note while programming: Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0. The algebraic sign for the cycle parameter "thread depth" determines the working direction. If you program the thread DEPTH = 0, the cycle will not be executed. The nominal thread diameter is approached in a semicircle from the center.
4 THREAD MILLING (Cycle 262, DIN/ISO: G262) 4.6 Cycle parameters Nominal diameter Q335: Nominal thread diameter. Input range 0 to 99999.9999 Thread pitch Q239: Pitch of the thread. The algebraic sign differentiates between right-hand and left-hand threads: + = right-hand thread –= left-hand thread Input range -99.9999 to 99.9999 Thread depth Q201 (incremental): Distance between workpiece surface and root of thread. Input range -99999.9999 to 99999.
4 Fixed Cycles: Tapping / Thread Milling 4.7 4.7 THREAD MILLING/COUNTERSINKING (Cycle 263, DIN/ISO:G263) THREAD MILLING/ COUNTERSINKING (Cycle 263, DIN/ ISO:G263) Cycle run 1 The TNC positions the tool in the tool axis at rapid traverse FMAX to the entered set-up clearance above the workpiece surface. Countersinking 2 The tool moves at the feed rate for pre-positioning to the countersinking depth minus the set-up clearance, and then at the feed rate for countersinking to the countersinking depth.
4 THREAD MILLING/COUNTERSINKING (Cycle 263, DIN/ISO:G263) 4.7 Please note while programming: Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0. The algebraic sign of the cycle parameters depth of thread, countersinking depth or sinking depth at front determines the working direction. The working direction is defined in the following sequence: 1. Thread depth 2. Countersinking depth 3.
4 Fixed Cycles: Tapping / Thread Milling 4.7 THREAD MILLING/COUNTERSINKING (Cycle 263, DIN/ISO:G263) Cycle parameters Nominal diameter Q335: Nominal thread diameter. Input range 0 to 99999.9999 Thread pitch Q239: Pitch of the thread. The algebraic sign differentiates between right-hand and left-hand threads: + = right-hand thread –= left-hand thread Input range -99.9999 to 99.9999 Thread depth Q201 (incremental): Distance between workpiece surface and root of thread. Input range -99999.9999 to 99999.
4 THREAD MILLING/COUNTERSINKING (Cycle 263, DIN/ISO:G263) 4.7 Coordinate of workpiece surface Q203 (absolute): Coordinate of the workpiece surface. Input range -99999.9999 to 99999.9999 2nd set-up clearance Q204 (incremental): Coordinate in the spindle axis at which no collision between tool and workpiece (fixtures) can occur. Input range 0 to 99999.9999 Feed rate for countersinking Q254: Traversing speed of the tool during countersinking in mm/min. Input range 0 to 99999.
4 Fixed Cycles: Tapping / Thread Milling 4.8 4.8 THREAD DRILLING/MILLING (Cycle 264, DIN/ISO: G264) THREAD DRILLING/MILLING (Cycle 264, DIN/ISO: G264) Cycle run 1 The TNC positions the tool in the tool axis at rapid traverse FMAX to the entered set-up clearance above the workpiece surface. Drilling 2 The tool drills to the first plunging depth at the programmed feed rate for plunging. 3 If you have programmed chip breaking, the tool then retracts by the entered retraction value.
4 THREAD DRILLING/MILLING (Cycle 264, DIN/ISO: G264) 4.8 Please note while programming: Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0. The algebraic sign of the cycle parameters depth of thread, countersinking depth or sinking depth at front determines the working direction. The working direction is defined in the following sequence: 1. Thread depth 2. Countersinking depth 3.
4 Fixed Cycles: Tapping / Thread Milling 4.8 THREAD DRILLING/MILLING (Cycle 264, DIN/ISO: G264) Cycle parameters Nominal diameter Q335: Nominal thread diameter. Input range 0 to 99999.9999 Thread pitch Q239: Pitch of the thread. The algebraic sign differentiates between right-hand and left-hand threads: + = right-hand thread –= left-hand thread Input range -99.9999 to 99.9999 Thread depth Q201 (incremental): Distance between workpiece surface and root of thread. Input range -99999.9999 to 99999.
4 THREAD DRILLING/MILLING (Cycle 264, DIN/ISO: G264) Upper advanced stop distance Q258 (incremental): Set-up clearance for rapid traverse positioning when the TNC moves the tool again to the current plunging depth after retraction from the hole. Input range 0 to 99999.9999 Infeed depth for chip breaking Q257 (incremental): Depth at which the TNC carries out chip breaking. No chip breaking if 0 is entered. Input range 0 to 99999.
4 Fixed Cycles: Tapping / Thread Milling 4.9 4.9 HELICAL THREAD DRILLING/MILLING (Cycle 265, DIN/ISO: G265) HELICAL THREAD DRILLING/ MILLING (Cycle 265, DIN/ISO: G265) Cycle run 1 The TNC positions the tool in the tool axis at rapid traverse FMAX to the entered set-up clearance above the workpiece surface. Countersinking at front 2 If countersinking occurs before thread milling, the tool moves at the feed rate for countersinking to the sinking depth at front.
4 HELICAL THREAD DRILLING/MILLING (Cycle 265, DIN/ISO: G265) 4.9 Please note while programming: Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0. The algebraic sign of the cycle parameters depth of thread or sinking depth at front determines the working direction. The working direction is defined in the following sequence: 1. Thread depth 2. Depth at front If you program a depth parameter to be 0, the TNC does not execute that step.
4 Fixed Cycles: Tapping / Thread Milling 4.9 HELICAL THREAD DRILLING/MILLING (Cycle 265, DIN/ISO: G265) Cycle parameters Nominal diameter Q335: Nominal thread diameter. Input range 0 to 99999.9999 Thread pitch Q239: Pitch of the thread. The algebraic sign differentiates between right-hand and left-hand threads: + = right-hand thread –= left-hand thread Input range -99.9999 to 99.9999 Thread depth Q201 (incremental): Distance between workpiece surface and root of thread. Input range -99999.9999 to 99999.
4 HELICAL THREAD DRILLING/MILLING (Cycle 265, DIN/ISO: G265) 4.9 2nd set-up clearance Q204 (incremental): Coordinate in the spindle axis at which no collision between tool and workpiece (fixtures) can occur. Input range 0 to 99999.9999 Feed rate for countersinking Q254: Traversing speed of the tool during countersinking in mm/min. Input range 0 to 99999.9999 alternatively FAUTO, FU Feed rate for milling Q207: Traversing speed of the tool in mm/min while milling. Input range 0 to 99999.
4 Fixed Cycles: Tapping / Thread Milling 4.10 OUTSIDE THREAD MILLING (Cycle 267, DIN/ISO: G267) 4.10 OUTSIDE THREAD MILLING (Cycle 267, DIN/ISO: G267) Cycle run 1 The TNC positions the tool in the tool axis at rapid traverse FMAX to the entered set-up clearance above the workpiece surface. Countersinking at front 2 The TNC moves on the reference axis of the working plane from the center of the stud to the starting point for countersinking at front.
4 OUTSIDE THREAD MILLING (Cycle 267, DIN/ISO: G267) 4.10 Please note while programming: Program a positioning block for the starting point (stud center) in the working plane with radius compensation R0. The offset required before countersinking at the front should be determined ahead of time. You must enter the value from the center of the stud to the center of the tool (uncorrected value).
4 Fixed Cycles: Tapping / Thread Milling 4.10 OUTSIDE THREAD MILLING (Cycle 267, DIN/ISO: G267) Cycle parameters Nominal diameter Q335: Nominal thread diameter. Input range 0 to 99999.9999 Thread pitch Q239: Pitch of the thread. The algebraic sign differentiates between right-hand and left-hand threads: + = right-hand thread –= left-hand thread Input range -99.9999 to 99.9999 Thread depth Q201 (incremental): Distance between workpiece surface and root of thread. Input range -99999.9999 to 99999.
4 OUTSIDE THREAD MILLING (Cycle 267, DIN/ISO: G267) 4.10 Coordinate of workpiece surface Q203 (absolute): Coordinate of the workpiece surface. Input range -99999.9999 to 99999.9999 2nd set-up clearance Q204 (incremental): Coordinate in the spindle axis at which no collision between tool and workpiece (fixtures) can occur. Input range 0 to 99999.9999 Feed rate for countersinking Q254: Traversing speed of the tool during countersinking in mm/min. Input range 0 to 99999.
4 Fixed Cycles: Tapping / Thread Milling 4.11 Programming Examples 4.11 Programming Examples Example: Thread milling The drill hole coordinates are stored in the point table TAB1.PNT and are called by the TNC with CYCL CALL PAT. The tool radii are selected so that all work steps can be seen in the test graphics. Program sequence Centering Drilling Tapping 0 BEGIN PGM 1 MM 1 BLK FORM 0.1 Z X+0 Y+0 Z-20 Definition of workpiece blank 2 BLK FORM 0.
4 Programming Examples 4.11 Q204=0 ;2ND SET-UP CLEARANCE Q211=0.2 ;DWELL TIME AT DEPTH Q395=0 ;DEPTH REFERENCE 0 must be entered here, effective as defined in point table 15 CYCL CALL PAT F5000 M3 Cycle call in connection with point table TAB1.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.1 Fundamentals 5.
5 RECTANGULAR POCKET (Cycle 251) 5.2 5.2 RECTANGULAR POCKET (Cycle 251, DIN/ISO: G251) Cycle run Use Cycle 251 RECTANGULAR POCKET to completely machine rectangular pockets.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.2 RECTANGULAR POCKET (Cycle 251) Please note while programming: With an inactive tool table you must always plunge vertically (Q366=0) because you cannot define a plunging angle. Pre-position the tool in the machining plane to the starting position with radius compensation R0. Note parameter Q367 (position). The TNC automatically pre-positions the tool in the tool axis. Note the 2nd set-up clearance Q204.
5 RECTANGULAR POCKET (Cycle 251) 5.2 Cycle parameters Machining operation (0/1/2) Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing Side finishing and floor finishing are only machined when the specific allowance (Q368, Q369) is defined 1st side length Q218 (incremental): Pocket length, parallel to the reference axis of the working plane. Input range 0 to 99999.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.2 RECTANGULAR POCKET (Cycle 251) Finishing allowance for floor Q369 (incremental value): Finishing allowance in the tool axis. Input range 0 to 99999.9999 Feed rate for plunging Q206: Traversing speed of the tool while moving to depth in mm/min. Input range 0 to 99999.999; alternatively FAUTO, FU, FZ Infeed for finishing Q338 (incremental): Infeed per cut. Q338=0: Finishing in one infeed. Input range 0 to 99999.
5 CIRCULAR POCKET (Cycle 252, DIN/ISO: G252) 5.3 5.3 CIRCULAR POCKET (Cycle 252, DIN/ ISO: G252) Cycle run Use Cycle 252 CIRCULAR POCKET to machine circular pockets.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.3 CIRCULAR POCKET (Cycle 252, DIN/ISO: G252) Finishing 1 Inasmuch as finishing allowances are defined, the TNC then finishes the pocket walls, in multiple infeeds if so specified. 2 The TNC positions the tool in the tool axis in front of the pocket wall, taking the finishing allowance Q368 and the set-up clearance Q200 into account. 3 The TNC clears the pocket from the inside out until the diameter Q223 is reached.
5 CIRCULAR POCKET (Cycle 252, DIN/ISO: G252) 5.3 Please note while programming: With an inactive tool table you must always plunge vertically (Q366=0) because you cannot define a plunging angle. Pre-position the tool in the machining plane to the starting position (circle center) with radius compensation R0. The TNC automatically pre-positions the tool in the tool axis. Note the 2nd set-up clearance Q204. The algebraic sign for the cycle parameter DEPTH determines the working direction.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.3 CIRCULAR POCKET (Cycle 252, DIN/ISO: G252) Cycle parameters Machining operation (0/1/2) Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing Side finishing and floor finishing are only machined when the specific allowance (Q368, Q369) is defined Circle diameter Q223: Diameter of the finished pocket. Input range 0 to 99999.
5 CIRCULAR POCKET (Cycle 252, DIN/ISO: G252) 5.3 Infeed for finishing Q338 (incremental): Infeed per cut. Q338=0: Finishing in one infeed. Input range 0 to 99999.9999 Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Input range 0 to 99999.9999; alternatively PREDEF Coordinate of workpiece surface Q203 (absolute): Coordinate of the workpiece surface. Input range -99999.9999 to 99999.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.4 5.4 SLOT MILLING (Cycle 253, DIN/ISO: G253) SLOT MILLING (Cycle 253, DIN/ISO: G253) Cycle run Use Cycle 253 to completely machine a slot.
5 SLOT MILLING (Cycle 253, DIN/ISO: G253) 5.4 Please note while programming: With an inactive tool table you must always plunge vertically (Q366=0) because you cannot define a plunging angle. Pre-position the tool in the machining plane to the starting position with radius compensation R0. Note parameter Q367 (position). The TNC automatically pre-positions the tool in the tool axis. Note the 2nd set-up clearance Q204.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.4 SLOT MILLING (Cycle 253, DIN/ISO: G253) Cycle parameters Machining operation (0/1/2) Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing Side finishing and floor finishing are only machined when the specific allowance (Q368, Q369) is defined Slot length Q218 (value parallel to the reference axis of the working plane): Enter the length of the slot. Input range 0 to 99999.
5 SLOT MILLING (Cycle 253, DIN/ISO: G253) Finishing allowance for floor Q369 (incremental value): Finishing allowance in the tool axis. Input range 0 to 99999.9999 Feed rate for plunging Q206: Traversing speed of the tool while moving to depth in mm/min. Input range 0 to 99999.999; alternatively FAUTO, FU, FZ Infeed for finishing Q338 (incremental): Infeed per cut. Q338=0: Finishing in one infeed. Input range 0 to 99999.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.5 5.5 CIRCULAR SLOT (Cycle 254, DIN/ISO: G254) CIRCULAR SLOT (Cycle 254, DIN/ISO: G254) Cycle run Use Cycle 254 to completely machine a circular slot.
5 CIRCULAR SLOT (Cycle 254, DIN/ISO: G254) 5.5 Please note while programming: With an inactive tool table you must always plunge vertically (Q366=0) because you cannot define a plunging angle. Pre-position the tool in the machining plane to the starting position with radius compensation R0. Note parameter Q367 (position). The TNC automatically pre-positions the tool in the tool axis. Note the 2nd set-up clearance Q204.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.5 CIRCULAR SLOT (Cycle 254, DIN/ISO: G254) Cycle parameters Machining operation (0/1/2) Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing Side finishing and floor finishing are only machined when the specific allowance (Q368, Q369) is defined Slot width Q219 (value parallel to the secondary axis of the working plane): Enter the slot width.
5 CIRCULAR SLOT (Cycle 254, DIN/ISO: G254) 5.5 Feed rate for milling Q207: Traversing speed of the tool in mm/min while milling. Input range 0 to 99999.999 alternatively FAUTO, FU, FZ Climb or up-cut Q351: Type of milling operation with M3 +1 = climb –1 = up-cut PREDEF: The TNC uses the value from the GLOBAL DEF block (If you enter 0, climb milling is used for machining) Depth Q201 (incremental): Distance between workpiece surface and bottom of slot. Input range -99999.9999 to 99999.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.5 CIRCULAR SLOT (Cycle 254, DIN/ISO: G254) Plunging strategy Q366: Type of plunging strategy: 0: vertical plunging. The plunging angle (ANGLE) in the tool table is not evaluated. 1, 2: reciprocal plunging. In the tool table, the plunging angle ANGLE for the active tool must be defined as not equal to 0.
5 RECTANGULAR STUD (Cycle 256) 5.6 5.6 RECTANGULAR STUD (Cycle 256, DIN/ISO: G256) Cycle run Use Cycle 256 to machine a rectangular stud. If a dimension of the workpiece blank is greater than the maximum possible stepover, then the TNC performs multiple stepovers until the finished dimension has been machined. 1 The tool moves from the cycle starting position (stud center) to the starting position for stud machining. Specify the starting position with parameter Q437.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.6 RECTANGULAR STUD (Cycle 256) Please note while programming: Pre-position the tool in the machining plane to the starting position with radius compensation R0. Note parameter Q367 (position). The TNC automatically pre-positions the tool in the tool axis. Note the 2nd set-up clearance Q204. The algebraic sign for the cycle parameter DEPTH determines the working direction. If you program DEPTH=0, the cycle will not be executed.
5 RECTANGULAR STUD (Cycle 256) 5.6 Cycle parameters 1st side length Q218: Stud length, parallel to the reference axis of the working plane. Input range 0 to 99999.9999 Workpiece blank side length 1 Q424: Length of the stud blank, parallel to the reference axis of the working plane. Enter Workpiece blank side length 1 greater than 1st side length.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.6 RECTANGULAR STUD (Cycle 256) Climb or up-cut Q351: Type of milling operation with M3 +1 = climb –1 = up-cut PREDEF: The TNC uses the value from the GLOBAL DEF block (If you enter 0, climb milling is used for machining) Depth Q201 (incremental): Distance between workpiece surface and bottom of stud. Input range -99999.9999 to 99999.9999 Plunging depth Q202 (incremental): Infeed per cut. Enter a value greater than 0. Input range 0 to 99999.
5 CIRCULAR STUD (Cycle 257, DIN/ISO: G257) 5.7 5.7 CIRCULAR STUD (Cycle 257, DIN/ISO: G257) Cycle run Use Cycle 257 to machine a circular stud. The TNC mills the circular stud with a helical infeed motion starting from the workpiece blank diameter. 1 If the tool is below the 2nd set-up clearance, the TNC retracts the tool to the 2nd set-up clearance. 2 The tool moves from the stud center to the starting position for stud machining.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.7 CIRCULAR STUD (Cycle 257, DIN/ISO: G257) Please note while programming: Pre-position the tool in the machining plane to the starting position (stud center) with radius compensation R0. The TNC automatically pre-positions the tool in the tool axis. Note the 2nd set-up clearance Q204. The algebraic sign for the cycle parameter DEPTH determines the working direction. If you program DEPTH=0, the cycle will not be executed.
5 CIRCULAR STUD (Cycle 257, DIN/ISO: G257) 5.7 Cycle parameters Finished part diameter Q223: Diameter of the completely machined stud. Input range 0 to 99999.9999 Workpiece blank diameter Q222: Diameter of the workpiece blank. Enter the workpiece blank diameter greater than the finished diameter. The TNC performs multiple stepovers if the difference between the workpiece blank diameter and finished diameter is greater than the permitted stepover (tool radius multiplied by path overlap Q370).
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.7 CIRCULAR STUD (Cycle 257, DIN/ISO: G257) Coordinate of workpiece surface Q203 (absolute): Coordinate of the workpiece surface. Input range -99999.9999 to 99999.9999 2nd set-up clearance Q204 (incremental): Coordinate in the spindle axis at which no collision between tool and workpiece (fixtures) can occur. Input range 0 to 99999.
5 CIRCULAR STUD (cycle 258, DIN/ISO: G258) 5.8 5.8 CIRCULAR STUD (cycle 258, DIN/ISO: G258) Cycle run With the cycle POLYGON STUD you can create an even polygon by machining the contour outside. The milling operation is carried out on a spiral path, based on the diameter of the workpiece blank. 1 If, at the beginning of machining, the work piece is positioned below the 2nd set-up clearance, the TNC will retract the tool back to the 2nd setup clearance.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.8 CIRCULAR STUD (cycle 258, DIN/ISO: G258) Please note while programming: Before the start of the cycle you will have to preposition the tool on the machining plane. In order to do so, move the tool with radius compensation R0 to the center of the stud. The TNC automatically pre-positions the tool in the tool axis. Note the 2nd set-up clearance Q204. The algebraic sign for the cycle parameter DEPTH determines the working direction.
5 CIRCULAR STUD (cycle 258, DIN/ISO: G258) 5.8 Cycle parameters Reference circuit Q573: Definition of whether the dimensioning shall reference to the inscribed circle or to the perimeter: 0= dimensioning refers to the inscribed circle 1= dimensioning refers to the perimeter Reference circuit diameter Q571: Definition of the diameter of the reference circuit. Specify in parameter Q573 whether the diameter references to the inscribed circle or the perimeter. Input range: 0 to 99999.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.8 CIRCULAR STUD (cycle 258, DIN/ISO: G258) Radius/Chamfer Q220: Enter the value for the input form radius or chamfer. When entering a positive value between 0 and +99999.9999 the TNC creates a polygon with round corners. The radius refers to the value you entered. If you enter a negative value between 0 and -99999.9999 all corners of the contour are chamfered and the value entered refers to the length of the chamfer.
5 CIRCULAR STUD (cycle 258, DIN/ISO: G258) Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Input range 0 to 99999.9999; alternatively PREDEF Coordinate of workpiece surface Q203 (absolute): Coordinate of the workpiece surface. Input range -99999.9999 to 99999.9999 2nd set-up clearance Q204 (incremental): Coordinate in the spindle axis at which no collision between tool and workpiece (fixtures) can occur. Input range 0 to 99999.9999; alternatively PREDEF 5.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.9 5.9 FACE MILLING (Cycle 233) FACE MILLING (Cycle 233, DIN/ISO: G233) Cycle run Cycle 233 is used to face mill a level surface in multiple infeeds while taking the finishing allowance into account. You can also define side walls in the cycle, which are then taken into account when machining the level surface.
5 FACE MILLING (Cycle 233) 5.9 Strategies Q389=0 and Q389 =1 The strategies Q389=0 and Q389=1 differ in the overtravel during face milling. If Q389=0, the end point lies outside of the surface. If Q389=1, it lies at the edge of the surface. The TNC calculates the end point 2 from the side length and the safety clearance to the side. If the strategy Q389=0 is used, the TNC additionally moves the tool beyond the level surface by the tool radius.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.9 FACE MILLING (Cycle 233) Strategies Q389=2 and Q389 =3 The strategies Q389=2 and Q389=3 differ in the overtravel during face milling. If Q389=2, the end point lies outside of the surface. If Q389=3, it lies at the edge of the surface. The TNC calculates the end point 2 from the side length and the safety clearance to the side. If the strategy Q389=2 is used, the TNC additionally moves the tool beyond the level surface by the tool radius.
5 FACE MILLING (Cycle 233) 5.9 Strategy Q389=4 4 The tool subsequently approaches the starting point of the milling path on a tangential arc at the programmed feed rate for milling. 5 The TNC machines the level surface at the feed rate for milling from the outside toward the inside with ever-shorter milling paths. The constant stepover results in the tool being continuously engaged. 6 The process is repeated until the programmed surface has been completed.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.9 FACE MILLING (Cycle 233) Please note while programming: Pre-position the tool in the machining plane to the starting position with radius compensation R0. Keep in mind the machining direction. The TNC automatically pre-positions the tool in the tool axis. Note the 2nd set-up clearance Q204. Enter the 2nd set-up clearance in Q204 so that no collision with the workpiece or the fixtures can occur.
5 FACE MILLING (Cycle 233) 5.
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.9 FACE MILLING (Cycle 233) Starting point in 3rd axis Q227 (absolute): Coordinate of the workpiece surface used to calculate the infeeds. Input range -99999.9999 to 99999.9999 End point in 3rd axis Q386 (absolute): Coordinate in the spindle axis to which the surface is to be face milled. Input range -99999.9999 to 99999.9999 Allowance for floor Q369 (incremental): Distance used for the last infeed. Input range 0 to 99999.
5 FACE MILLING (Cycle 233) 5.9 2nd set-up clearance Q204 (incremental): Coordinate in the spindle axis at which no collision between tool and workpiece (fixtures) can occur. Input range 0 to 99999.9999; alternatively PREDEF 1st limit Q347:Select the workpiece side on which the level surface is limited by a side wall (not possible for helical machining).
5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling 5.10 Programming Examples 5.10 Programming Examples Example: Milling pockets, studs and slots 0 BEGINN PGM C210 MM 1 BLK FORM 0.1 Z X+0 Y+0 Z-40 Definition of workpiece blank 2 BLK FORM 0.2 X+100 Y+100 Z+0 3 TOOL CALL 1 Z S3500 Call the tool for roughing/finishing 4 L Z+250 R0 FMAX Retract the tool 5 CYCL DEF 256 RECTANGULAR STUD Define cycle for machining the contour outside Q218=90 ;FIRST SIDE LENGTH Q424=100 ;WORKPC.
5 Programming Examples 5.10 Q351=+1 ;CLIMB OR UP-CUT Q201=-30 ;DEPTH Q202=5 ;PLUNGING DEPTH Q369=0.
6 Fixed Cycles: Pattern Definitions
6 Fixed Cycles: Pattern Definitions 6.1 Fundamentals 6.1 Fundamentals Overview The TNC provides two cycles for machining point patterns directly: Soft key Cycle Page 220 POLAR PATTERN 187 221 CARTESIAN PATTERN 190 You can combine Cycle 220 and Cycle 221 with the following fixed cycles: If you have to machine irregular point patterns, use CYCL CALL PAT (see "Point tables", page 71) to develop point tables.
6 POLAR PATTERN (Cycle 220) 6.2 6.2 POLAR PATTERN (Cycle 220, DIN/ ISO: G220) Cycle run 1 At rapid traverse, the TNC moves the tool from its current position to the starting point for the first machining operation. Sequence: Move to the 2nd set-up clearance (spindle axis) Approach the starting point in the spindle axis. Move to the set-up clearance above the workpiece surface (spindle axis). 2 From this position, the TNC executes the last defined fixed cycle.
6 Fixed Cycles: Pattern Definitions 6.2 POLAR PATTERN (Cycle 220) Cycle parameters Center in 1st axis Q216 (absolute): Center of the pitch circle in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 Center in 2nd axis Q217 (absolute): Center of the pitch circle in the minor axis of the working plane. Input range -99999.9999 to 99999.9999 Pitch circle diameter Q244: Diameter of the pitch circle. Input range 0 to 99999.
6 POLAR PATTERN (Cycle 220) 2nd set-up clearance Q204 (incremental): Coordinate in the spindle axis at which no collision between tool and workpiece (fixtures) can occur. Input range 0 to 99999.
6 Fixed Cycles: Pattern Definitions 6.3 6.3 LINEAR PATTERN (Cycle 221) LINEAR PATTERN (Cycle 221, DIN/ ISO: G221) Cycle run 1 The TNC automatically moves the tool from its current position to the starting point for the first machining operation. Sequence: Move to the set-up clearance (spindle axis) Approach the starting point in the machining plane Move to the set-up clearance above the workpiece surface (spindle axis) 2 From this position, the TNC executes the last defined fixed cycle.
6 LINEAR PATTERN (Cycle 221) 6.3 Cycle parameters Starting point in 1st axis Q225 (absolute): Coordinate of the starting point in the reference axis of the working plane.
6 Fixed Cycles: Pattern Definitions 6.4 6.4 Programming Examples Programming Examples Example: Polar hole patterns 0 BEGIN PGM HOLEPAT MM 1 BLK FORM 0.1 Z X+0 Y+0 Z-40 Definition of workpiece blank 2 BLK FORM 0.
6 Programming Examples Q301=1 ;MOVE TO CLEARANCE Q365=0 ;TYPE OF TRAVERSE 7 CYCL DEF 220 POLAR PATTERN Q216=+90 ;CENTER IN 1ST AXIS Q217=+25 ;CENTER IN 2ND AXIS Q244=70 ;PITCH CIRCLE DIA. Q245=+90 ;STARTING ANGLE Q246=+360 ;STOPPING ANGLE Q247=+30 ;STEPPING ANGLE Q241=5 ;NR OF REPETITIONS Q200=2 ;SET-UP CLEARANCE Q203=+0 ;SURFACE COORDINATE Q204=100 ;2ND SET-UP CLEARANCE Q301=1 ;MOVE TO CLEARANCE Q365=0 ;TYPE OF TRAVERSE 8 L Z+250 R0 FMAX M2 6.
7 Fixed Cycles: Contour Pocket
7 Fixed Cycles: Contour Pocket 7.1 7.1 SL Cycles SL Cycles Fundamentals SL cycles enable you to form complex contours by combining up to 12 subcontours (pockets or islands). You define the individual subcontours in subprograms. The TNC calculates the total contour from the subcontours (subprogram numbers) that you enter in Cycle 14 CONTOUR GEOMETRY. Program structure: Machining with SL cycles 0 BEGIN PGM SL2 MM ... 12 CYCL DEF 14 CONTOUR... The memory capacity for programming an SL cycle is limited.
7 SL Cycles Characteristics of the fixed cycles The TNC automatically positions the tool to the set-up clearance before each cycle–position the tool to a safe position before the cycle call. Each level of infeed depth is milled without interruptions since the cutter traverses around islands instead of over them.
7 Fixed Cycles: Contour Pocket 7.2 7.2 CONTOUR (Cycle 14, DIN/ISO: G37) CONTOUR (Cycle 14, DIN/ISO: G37) Please note while programming: All subprograms that are superimposed to define the contour are listed in Cycle 14 CONTOUR GEOMETRY. Cycle 14 is DEF active which means that it becomes effective as soon as it is defined in the part program. You can list up to 12 subprograms (subcontours) in Cycle 14.
7 Superimposed contours 7.3 7.3 Superimposed contours Fundamentals Pockets and islands can be overlapped to form a new contour. You can thus enlarge the area of a pocket by another pocket or reduce it by an island. NC blocks 12 CYCL DEF 14.0 CONTOUR 13 CYCL DEF 14.1 CONTOUR LABEL 1/2/3/4 Subprograms: overlapping pockets The subsequent programming examples are contour subprograms that are called by Cycle 14 CONTOUR GEOMETRY in a main program. Pockets A and B overlap.
7 Fixed Cycles: Contour Pocket 7.3 Superimposed contours Area of inclusion Both surfaces A and B are to be machined, including the overlapping area: The surfaces A and B must be pockets. The first pocket (in Cycle 14) must start outside the second pocket.
7 Superimposed contours 7.3 Area of exclusion Surface A is to be machined without the portion overlapped by B: Surface A must be a pocket and B an island. A must start outside of B. B must start inside of A.
7 Fixed Cycles: Contour Pocket 7.3 Superimposed contours Area of intersection Only the area where A and B overlap is to be machined. (The areas covered by A or B alone are to be left unmachined.) A and B must be pockets. A must start inside of B.
7 CONTOUR DATA (Cycle 20, DIN/ISO: G120) 7.4 7.4 CONTOUR DATA (Cycle 20, DIN/ISO: G120) Please note while programming: Machining data for the subprograms describing the subcontours are entered in Cycle 20. Cycle 20 is DEF active, which means that it becomes effective as soon as it is defined in the part program. The machining data entered in Cycle 20 are valid for Cycles 21 to 24. The algebraic sign for the cycle parameter DEPTH determines the working direction.
7 Fixed Cycles: Contour Pocket 7.4 CONTOUR DATA (Cycle 20, DIN/ISO: G120) Cycle parameters Milling depth Q1 (incremental): Distance between workpiece surface and bottom of pocket. Input range -99999.9999 to 99999.9999 Path overlap factor Q2: Q2 x tool radius = stepover factor k. Input range -0.0001 to 1.9999 Finishing allowance for side Q3 (incremental): Finishing allowance in the working plane. Input range -99999.9999 to 99999.
7 PILOT DRILLING (Cycle 21, DIN/ISO: G121) 7.5 7.5 PILOT DRILLING (Cycle 21, DIN/ISO: G121) Cycle run Use Cycle 21 PILOT DRILLING if you will subsequently rough out the contour with a tool other than a center-cut end mill (ISO 1641). This cycle drills a hole in the area that is to be roughed out with a cycle such as Cycle 22. Cycle 21 takes the allowance for side and the allowance for floor as well as the radius of the rough-out tool into account for the cutter infeed points.
7 Fixed Cycles: Contour Pocket 7.5 PILOT DRILLING (Cycle 21, DIN/ISO: G121) Please note while programming: When calculating the infeed points, the TNC does not account for the delta value DR programmed in a TOOL CALL block. In narrow areas, the TNC may not be able to carry out pilot drilling with a tool that is larger than the rough-out tool. If Q13=0, the TNC uses the data of the tool that is currently in the spindle.
7 ROUGHING (Cycle 22, DIN/ISO: G122) 7.6 7.6 ROUGHING (Cycle 22, DIN/ ISO: G122) Cycle run Use Cycle 22 ROUGHING to define the technology data for roughing. Before calling Cycle 22 you need to program further cycles: Cycle 14 CONTOUR GEOMETRY or SEL CONTOUR Cycle 20 CONTOUR DATA Cycle 21 PILOT DRILLING, if necessary Cycle run 1 The TNC positions the tool over the cutter infeed point, taking the allowance for side into account.
7 Fixed Cycles: Contour Pocket 7.6 ROUGHING (Cycle 22, DIN/ISO: G122) Please note while programming: This cycle requires a center-cut end mill (ISO 1641) or pilot drilling with Cycle 21. You define the plunging behavior of Cycle 22 with parameter Q19 and with the tool table in the ANGLE and LCUTS columns: If Q19=0 is defined, the TNC always plunges perpendicularly, even if a plunge angle (ANGLE) is defined for the active tool. If you define the ANGLE=90°, the TNC plunges perpendicularly.
7 ROUGHING (Cycle 22, DIN/ISO: G122) 7.6 Cycle parameters Plunging depth Q10 (incremental): Infeed per cut. Input range -99999.9999 to 99999.9999 Feed rate for plunging Q11: Traversing speed of the tool in the spindle axis. Input range 0 to 99999.9999, alternatively FAUTO, FU, FZ Feed rate for milling Q12: Traversing speed of the tool in the working plane. Input range 0 to 99999.
7 Fixed Cycles: Contour Pocket 7.6 ROUGHING (Cycle 22, DIN/ISO: G122) Feed rate factor in % Q401: Percentage factor by which the TNC reduces the machining feed rate (Q12) as soon as the tool moves within the material over its entire circumference during roughing. If you use the feed rate reduction, then you can define the feed rate for roughing so large that there are optimum cutting conditions with the path overlap (Q2) specified in Cycle 20.
7 FLOOR FINISHING (Cycle 23, DIN/ISO: G123) 7.7 7.7 FLOOR FINISHING (Cycle 23, DIN/ISO: G123) Cycle run With Cycle 23 FLOOR FINISHING, you can clear the finishing allowance for floor that is programmed in Cycle 20. The tool approaches the machining plane smoothly (on a vertically tangential arc) if there is sufficient room. If there is not enough room, the TNC moves the tool to depth vertically. The tool then clears the finishing allowance remaining from rough-out.
7 Fixed Cycles: Contour Pocket 7.7 FLOOR FINISHING (Cycle 23, DIN/ISO: G123) Please note while programming: The TNC automatically calculates the starting point for finishing. The starting point depends on the available space in the pocket. The approaching radius for pre-positioning to the final depth is permanently defined and independent of the plunging angle of the tool. If M110 is activated during operation, the feed rate of compensated circular arcs within will be reduced accordingly.
7 SIDE FINISHING (Cycle 24, DIN/ISO: G124) 7.8 7.8 SIDE FINISHING (Cycle 24, DIN/ISO: G124) Cycle run With Cycle 24 SIDE FINISHING, you can clear the finishing allowance for side that is programmed in Cycle 20. You can run this cycle in climb or up-cut milling.
7 Fixed Cycles: Contour Pocket 7.8 SIDE FINISHING (Cycle 24, DIN/ISO: G124) Please note while programming: The sum of allowance for side (Q14) and the radius of the finish mill must be smaller than the sum of allowance for side (Q3, Cycle 20) and the radius of the rough mill. If no allowance has been defined in Cycle 20, the control issues the error message "Tool radius too large". The allowance for side Q14 is left over after finishing. Therefore, it must be smaller than the allowance in Cycle 20.
7 SIDE FINISHING (Cycle 24, DIN/ISO: G124) 7.8 Cycle parameters Direction of rotation Q9: Machining direction: +1: Rotation counterclockwise –1: Rotation clockwise Plunging depth Q10 (incremental): Infeed per cut. Input range -99999.9999 to 99999.9999 Feed rate for plunging Q11: Traversing speed of the tool when plunging into the workpiece in mm/ min. Input range 0 to 99999.9999 alternatively FAUTO, FU, FZ Feed rate for milling Q12: Traversing speed of the tool in the working plane.
7 Fixed Cycles: Contour Pocket 7.9 7.9 CONTOUR TRAIN (Cycle 25, DIN/ISO: G125) CONTOUR TRAIN (Cycle 25, DIN/ISO: G125) Cycle run In conjunction with Cycle 14 CONTOUR GEOMETRY, this cycle facilitates the machining of open and closed contours. Cycle 25 CONTOUR TRAIN offers considerable advantages over machining a contour using positioning blocks: The TNC monitors the operation to prevent undercuts and surface blemishes. It is recommended that you run a graphic simulation of the contour before execution.
7 CONTOUR TRAIN (Cycle 25, DIN/ISO: G125) 7.9 Danger of collision! To avoid collisions, Do not program positions in incremental dimensions immediately after Cycle 25 since they are referenced to the position of the tool at the end of the cycle. Move the tool to defined (absolute) positions in all main axes, since the position of the tool at the end of the cycle is not identical to the position of the tool at the start of the cycle.
7 Fixed Cycles: Contour Pocket 7.10 7.10 CONTOUR TRAIN DATA (Cycle 270, DIN/ISO: G270) CONTOUR TRAIN DATA (Cycle 270, DIN/ISO: G270) Please note while programming: You can use this cycle to specify various properties of Cycle 25 CONTOUR TRAIN. Cycle 270 is DEF active, which means that it becomes effective as soon as it is defined in the part program. If Cycle 270 is used, do not define any radius compensation in the contour subprogram. Define Cycle 270 before Cycle 25.
7 TROCHOIDAL SLOT (Cycle 275, DIN ISO G275) 7.11 7.11 TROCHOIDAL SLOT (Cycle 275, DIN ISO G275) Cycle run In conjunction with Cycle 14 CONTOUR GEOMETRY, this cycle facilitates the complete machining of open and closed slots or contour slots using trochoidal milling. With trochoidal milling, large cutting depths and high cutting speeds are possible because the equally distributed cutting conditions prevent wear-increasing influences on the tool.
7 Fixed Cycles: Contour Pocket 7.11 TROCHOIDAL SLOT (Cycle 275, DIN ISO G275) Roughing with open slots The contour description of an open slot must always start with an approach block (APPR). 1 Following the positioning logic, the tool moves to the starting point of the machining operation as defined by the parameters in the APPR block and positions there perpendicular to the first plunging depth. 2 The TNC roughs the slot in circular motions to the contour end point.
7 TROCHOIDAL SLOT (Cycle 275, DIN ISO G275) 7.11 Cycle parameters Machining operation (0/1/2) Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing Side finishing and floor finishing are only machined when the specific allowance (Q368, Q369) is defined Slot width Q219 (value parallel to the secondary axis of the working plane): Enter the slot width.
7 Fixed Cycles: Contour Pocket 7.11 TROCHOIDAL SLOT (Cycle 275, DIN ISO G275) Plunging depth Q202 (incremental): Infeed per cut. Enter a value greater than 0. Input range 0 to 99999.9999 Feed rate for plunging Q206: Traversing speed of the tool while moving to depth in mm/min. Input range 0 to 99999.999; alternatively FAUTO, FU, FZ 8 CYCL DEF 275 TROCHOIDAL SLOT Q215=0 ;MACHINING OPERATION Q219=12 ;SLOT WIDTH Infeed for finishing Q338 (incremental): Infeed per cut. Q338=0: Finishing in one infeed.
7 Programming Examples 7.12 7.12 Programming Examples Example: Roughing-out and fine-roughing a pocket 0 BEGIN PGM C20 MM 1 BLK FORM 0.1 Z X-10 Y-10 Z-40 2 BLK FORM 0.2 X+100 Y+100 Z+0 Definition of workpiece blank 3 TOOL CALL 1 Z S2500 Tool call: coarse roughing tool, diameter 30 4 L Z+250 R0 FMAX Retract the tool 5 CYCL DEF 14.0 CONTOUR GEOMETRY Define contour subprogram 6 CYCL DEF 14.
7 Fixed Cycles: Contour Pocket 7.
7 Programming Examples 7.12 Example: Pilot drilling, roughing-out and finishing overlapping contours 0 BEGIN PGM C21 MM 1 BLK FORM 0.1 Z X+0 Y+0 Z-40 Definition of workpiece blank 2 BLK FORM 0.2 X+100 Y+100 Z+0 3 TOOL CALL 1 Z S2500 Tool call: Drill, diameter 12 4 L Z+250 R0 FMAX Retract the tool 5 CYCL DEF 14.0 CONTOUR GEOMETRY Define contour subprogram 6 CYCL DEF 14.1 CONTOUR LABEL 1 /2 /3 /4 7 CYCL DEF 20 CONTOUR DATA Q1=-20 ;MILLING DEPTH Q2=1 ;TOOL PATH OVERLAP Q3=+0.
7 Fixed Cycles: Contour Pocket 7.
7 Programming Examples 7.12 Example: Contour train 0 BEGIN PGM C25 MM 1 BLK FORM 0.1 Z X+0 Y+0 Z-40 Definition of workpiece blank 2 BLK FORM 0.2 X+100 Y+100 Z+0 3 TOOL CALL 1 Z S2000 Tool call: Diameter 20 4 L Z+250 R0 FMAX Retract the tool 5 CYCL DEF 14.0 CONTOUR GEOMETRY Define contour subprogram 6 CYCL DEF 14.
8 Fixed Cycles: Cylindrical Surface
8 Fixed Cycles: Cylindrical Surface 8.1 Fundamentals 8.
8 CYLINDER SURFACE (Cycle 27, DIN/ISO: G127, software option 1) 8.2 8.2 CYLINDER SURFACE (Cycle 27, DIN/ISO: G127, software option 1) Cycle run This cycle enables you to program a contour in two dimensions and then roll it onto a cylindrical surface for 3-D machining. Use Cycle 28 if you want to mill guideways on the cylinder. The contour is described in a subprogram identified in Cycle 14 CONTOUR GEOMETRY.
8 Fixed Cycles: Cylindrical Surface 8.2 CYLINDER SURFACE (Cycle 27, DIN/ISO: G127, software option 1) Please note while programming: The machine and TNC must be prepared for cylinder surface interpolation by the machine tool builder. Refer to your machine manual. In the first NC block of the contour program, always program both cylinder surface coordinates. The memory capacity for programming an SL cycle is limited. You can program up to 16384 contour elements in one SL cycle.
8 CYLINDER SURFACE (Cycle 27, DIN/ISO: G127, software option 1) 8.2 Cycle parameters Milling depth Q1 (incremental): Distance between the cylindrical surface and the floor of the contour. Input range -99999.9999 to 99999.9999 Finishing allowance for side Q3 (incremental): Finishing allowance in the plane of the unrolled cylindrical surface. This allowance is effective in the direction of the radius compensation. Input range -99999.9999 to 99999.
8 Fixed Cycles: Cylindrical Surface 8.3 8.3 CYLINDER SURFACE Slot milling (Cycle 28, DIN/ISO: G128, software option 1) CYLINDER SURFACE Slot milling (Cycle 28, DIN/ISO: G128, software option 1) Cycle run With this cycle you can program a guide notch in two dimensions and then transfer it onto a cylindrical surface. Unlike Cycle 27, this cycle enables the TNC to adjust the tool so that, with radius compensation active, the walls of the slot are nearly parallel.
8 CYLINDER SURFACE Slot milling (Cycle 28, DIN/ISO: G128, software option 1) 8.3 Please note while programming: This cycle performs an inclined 5-axis machining operation. To run this cycle, the first machine axis below the machine table must be a rotary axis. In addition, it must be possible to position the tool perpendicular to the cylinder surface.
8 Fixed Cycles: Cylindrical Surface 8.3 CYLINDER SURFACE Slot milling (Cycle 28, DIN/ISO: G128, software option 1) Cycle parameters Milling depth Q1 (incremental): Distance between the cylindrical surface and the floor of the contour. Input range -99999.9999 to 99999.9999 Finishing allowance for side Q3 (incremental): Finishing allowance on the slot wall. The finishing allowance reduces the slot width by twice the entered value. Input range -99999.9999 to 99999.
8 CYLINDER SURFACE Ridge milling (Cycle 29, DIN/ISO: G129, software option 1) 8.4 8.4 CYLINDER SURFACE Ridge milling (Cycle 29, DIN/ISO: G129, software option 1) Cycle run This cycle enables you to program a ridge in two dimensions and then transfer it onto a cylindrical surface. With this cycle the TNC adjusts the tool so that, with radius compensation active, the walls of the slot are always parallel. Program the midpoint path of the ridge together with the tool radius compensation.
8 Fixed Cycles: Cylindrical Surface 8.4 CYLINDER SURFACE Ridge milling (Cycle 29, DIN/ISO: G129, software option 1) Please note while programming: This cycle performs an inclined 5-axis machining operation. To run this cycle, the first machine axis below the machine table must be a rotary axis. In addition, it must be possible to position the tool perpendicular to the cylinder surface. In the first NC block of the contour program, always program both cylinder surface coordinates.
8 CYLINDER SURFACE Ridge milling (Cycle 29, DIN/ISO: G129, software option 1) 8.4 Cycle parameters Milling depth Q1 (incremental): Distance between the cylindrical surface and the floor of the contour. Input range -99999.9999 to 99999.9999 Finishing allowance for side Q3 (incremental): Finishing allowance on the ridge wall. The finishing allowance increases the ridge width by twice the entered value. Input range -99999.9999 to 99999.
8 Fixed Cycles: Cylindrical Surface 8.5 8.5 CYLINDER SURFACE (Cycle 39, DIN/ISO: G139, software option 1) CYLINDER SURFACE (Cycle 39, DIN/ISO: G139, software option 1) Cycle run This cycle enables you to machine a contour on a cylindrical surface. The contour to be machined is programmed on the unrolled surface of the cylinder. With this cycle the TNC adjusts the tool so that, with radius compensation active, the wall of the open contour is always parallel to the cylinder axis.
8 CYLINDER SURFACE (Cycle 39, DIN/ISO: G139, software option 1) 8.5 Please note while programming: This cycle performs an inclined 5-axis machining operation. To run this cycle, the first machine axis below the machine table must be a rotary axis. In addition, it must be possible to position the tool perpendicular to the cylinder surface. In the first NC block of the contour program, always program both cylinder surface coordinates.
8 Fixed Cycles: Cylindrical Surface 8.5 CYLINDER SURFACE (Cycle 39, DIN/ISO: G139, software option 1) Cycle parameters Milling depth Q1 (incremental): Distance between the cylindrical surface and the floor of the contour. Input range -99999.9999 to 99999.9999 Finishing allowance for side Q3 (incremental): Finishing allowance in the plane of the unrolled cylindrical surface. This allowance is effective in the direction of the radius compensation. Input range -99999.9999 to 99999.
8 Programming Examples 8.6 8.6 Programming Examples Example: Cylinder surface with Cycle 27 Machine with B head and C table Cylinder centered on rotary table Datum is on the underside, in the center of the rotary table Y (Z) X (C) 0 BEGIN PGM C27 MM 1 TOOL CALL 1 Z S2000 Tool call: Diameter 7 2 L Z+250 R0 FMAX Retract the tool 3 L X+50 Y0 R0 FMAX Pre-position tool at rotary table center 4 PLANE SPATIAL SPA+0 SPB+90 SPC+0 TURN MBMAX FMAX Positioning 5 CYCL DEF 14.
8 Fixed Cycles: Cylindrical Surface 8.6 Programming Examples 21 RND R7.
8 Programming Examples 8.6 Example: Cylinder surface with Cycle 28 Y (Z) Cylinder centered on rotary table Machine with B head and C table Datum at center of rotary table Description of the midpoint path in the contour subprogram X (C) 0 BEGIN PGM C28 MM 1 TOOL CALL 1 Z S2000 Tool call, tool axis Z, diameter 7 2 L Z+250 R0 FMAX Retract the tool 3 L X+50 Y+0 R0 FMAX Position tool at rotary table center 4 PLANE SPATIAL SPA+0 SPB+90 SPC+0 TURN FMAX Tilting 5 CYCL DEF 14.
9 Fixed Cycles: Contour Pocket with Contour Formula
9 Fixed Cycles: Contour Pocket with Contour Formula 9.1 9.1 SL cycles with complex contour formula SL cycles with complex contour formula Fundamentals SL cycles and the complex contour formula enable you to form complex contours by combining subcontours (pockets or islands). You define the individual subcontours (geometry data) as separate programs. In this way, any subcontour can be used any number of times.
9 SL cycles with complex contour formula Properties of the subcontours By default, the TNC assumes that the contour is a pocket. Do not program a radius compensation. The TNC ignores feed rates F and miscellaneous functions M. Coordinate transformations are allowed. If they are programmed within the subcontour they are also effective in the following subprograms, but they need not be reset after the cycle call.
9 Fixed Cycles: Contour Pocket with Contour Formula 9.
9 SL cycles with complex contour formula 9.1 Entering a complex contour formula You can use soft keys to interlink various contours in a mathematical formula. Show the soft-key row with special functions Select the menu for functions for contour and point machining Press the CONTOUR FORMULA soft key. The TNC then displays the following soft keys: Soft key Mathematical function cut with e.g. QC10 = QC1 & QC5 joined with e.g. QC25 = QC7 | QC18 joined with, but without cut e.g. QC12 = QC5 ^ QC25 without e.
9 Fixed Cycles: Contour Pocket with Contour Formula 9.1 SL cycles with complex contour formula Superimposed contours By default, the TNC considers a programmed contour to be a pocket. With the functions of the contour formula, you can convert a contour from a pocket to an island. Pockets and islands can be overlapped to form a new contour. You can thus enlarge the area of a pocket by another pocket or reduce it by an island.
9 SL cycles with complex contour formula 9.1 Area of inclusion Both areas A and B are to be machined, including the overlapping area: The areas A and B must be entered in separate programs without radius compensation. In the contour formula, the areas A and B are processed with the "joined with" function. Contour definition program: 50 ... 51 ... 52 DECLARE CONTOUR QC1 = "POCKET_A.H" 53 DECLARE CONTOUR QC2 = "POCKET_B.H" 54 QC10 = QC1 | QC2 55 ... 56 ...
9 Fixed Cycles: Contour Pocket with Contour Formula 9.1 SL cycles with complex contour formula Area of intersection Only the area where A and B overlap is to be machined. (The areas covered by A or B alone are to be left unmachined.) The areas A and B must be entered in separate programs without radius compensation. In the contour formula, the areas A and B are processed with the "intersection with" function. Contour definition program: 50 ... 51 ... 52 DECLARE CONTOUR QC1 = "POCKET_A.
9 SL cycles with complex contour formula 9.1 Example: Roughing and finishing superimposed contours with the contour formula 0 BEGIN PGM CONTOUR MM 1 BLK FORM 0.1 Z X+0 Y+0 Z-40 Definition of workpiece blank 2 BLK FORM 0.2 X+100 Y+100 Z+0 3 TOOL DEF 1 L+0 R+2.
9 Fixed Cycles: Contour Pocket with Contour Formula 9.
9 SL cycles with complex contour formula 9.
9 Fixed Cycles: Contour Pocket with Contour Formula 9.2 9.2 SL cycles with simple contour formula SL cycles with simple contour formula Fundamentals SL cycles and the simple contour formula enable you to form contours by combining up to 9 subcontours (pockets or islands) in a simple manner. You define the individual subcontours (geometry data) as separate programs. In this way, any subcontour can be used any number of times. The TNC calculates the contour from the selected subcontours.
9 SL cycles with simple contour formula 9.2 Properties of the subcontours Do not program a radius compensation. The TNC ignores feed rates F and miscellaneous functions M. Coordinate transformations are allowed. If they are programmed within the subcontour they are also effective in the following subprograms, but they need not be reset after the cycle call. Although the subprograms can contain coordinates in the spindle axis, such coordinates are ignored.
9 Fixed Cycles: Contour Pocket with Contour Formula 9.2 SL cycles with simple contour formula Entering a simple contour formula You can use soft keys to interlink various contours in a mathematical formula. Show the soft-key row with special functions Select the menu for functions for contour and point machining Press the CONTOUR DEF soft key. The TNC opens the dialog for entering the contour formula Enter the name of the first subcontour. The first subcontour must always be the deepest pocket.
10 Cycles: Coordinate Transformations
10 Cycles: Coordinate Transformations 10.1 Fundamentals 10.1 Fundamentals Overview Once a contour has been programmed, you can position it on the workpiece at various locations and in different sizes through the use of coordinate transformations.
10 DATUM SHIFT (Cycle 7) 10.2 10.2 DATUM SHIFT (Cycle 7, DIN/ISO: G54) Effect A DATUM SHIFT allows machining operations to be repeated at various locations on the workpiece. When the DATUM SHIFT cycle is defined, all coordinate data is based on the new datum. The TNC displays the datum shift in each axis in the additional status display. Input of rotary axes is also permitted. Resetting Program a datum shift to the coordinates X=0, Y=0 etc. directly with a cycle definition.
10 Cycles: Coordinate Transformations 10.3 DATUM SHIFT with datum tables (Cycle 7) 10.3 DATUM SHIFT with datum tables (Cycle 7, DIN/ISO: G53) Effect Datum tables are used for: Frequently recurring machining sequences at various locations on the workpiece Frequent use of the same datum shift Within a program, you can either program datum points directly in the cycle definition or call them from a datum table. Resetting Call a datum shift to the coordinates X=0; Y=0 etc. from a datum table.
10 DATUM SHIFT with datum tables (Cycle 7) 10.3 Please note while programming: Danger of collision! Datums from a datum table are always and exclusively referenced to the current datum (preset). If you are using datum shifts with datum tables, then use the SEL TABLE function to activate the desired datum table from the NC program. If you work without SEL TABLE, then you must activate the desired datum table before the test run or the program run. (This applies also to the programming graphics).
10 Cycles: Coordinate Transformations 10.3 DATUM SHIFT with datum tables (Cycle 7) Selecting a datum table in the part program With the SEL TABLE function you select the table from which the TNC takes the datums: Select the functions for program call: Press the PGM CALL key Press the DATUM TABLE soft key Select the complete path name of the datum table or the file with the SELECT soft key and confirm your entry with the END key Program a SEL TABLE block before Cycle 7 Datum Shift.
10 DATUM SHIFT with datum tables (Cycle 7) 10.
10 Cycles: Coordinate Transformations 10.3 DATUM SHIFT with datum tables (Cycle 7) Configuring the datum table If you do not wish to define a datum for an active axis, press the DEL key. Then the TNC clears the numerical value from the corresponding input field. You can change the properties of tables. Enter the code number 555343 in the MOD menu. The TNC then offers the EDIT FORMAT soft key if a table is selected.
10 DATUM SETTING (Cycle 247) 10.4 10.4 DATUM SETTING (Cycle 247, DIN/ ISO: G247) Effect With the DATUM SETTING cycle you can activate as the new datum a preset defined in a preset table. After a DATUM SETTING cycle definition, all of the coordinate inputs and datum shifts (absolute and incremental) are referenced to the new preset. Status display In the status display the TNC shows the active preset number behind the datum symbol.
10 Cycles: Coordinate Transformations 10.5 MIRRORING (Cycle 8) 10.5 MIRRORING (Cycle 8, DIN/ISO: G28) Effect The TNC can machine the mirror image of a contour in the working plane. The mirroring cycle becomes effective as soon as it is defined in the program. It is also effective in the Positioning with MDI mode of operation. The active mirrored axes are shown in the additional status display. If you mirror only one axis, the machining direction of the tool is reversed (except in SL cycles).
10 MIRRORING (Cycle 8) 10.5 Please note while programming: If you work in a tilted system with Cycle 8 the following procedure is recommended: First program the tilting movement and then call Cycle 8 MIRRORING! Cycle parameters Mirrored axis?: Enter the axis to be mirrored. You can mirror all axes except for the spindle axis— including rotary axes—with the exception of the spindle axis and its associated auxiliary axis. You can enter up to three axes.
10 Cycles: Coordinate Transformations 10.6 ROTATION (Cycle 10, DIN/ISO: G73) 10.6 ROTATION (Cycle 10, DIN/ISO: G73) Effect The TNC can rotate the coordinate system about the active datum in the working plane within a program. The ROTATION cycle becomes effective as soon as it is defined in the program. It is also effective in the Positioning with MDI mode of operation. The active rotation angle is shown in the additional status display.
10 ROTATION (Cycle 10, DIN/ISO: G73) 10.6 Please note while programming: An active radius compensation is canceled by defining Cycle 10 and must therefore be reprogrammed, if necessary. After defining Cycle 10, you must move both axes of the working plane to activate rotation for all axes. Cycle parameters Rotation: Enter the rotation angle in degrees (°). Input range –360.000° to +360.000° (absolute or incremental) NC blocks 12 CALL LBL 1 13 CYCL DEF 7.0 DATUM SHIFT 14 CYCL DEF 7.1 X+60 15 CYCL DEF 7.
10 Cycles: Coordinate Transformations 10.7 SCALING (Cycle 11 10.7 SCALING (Cycle 11, DIN/ISO: G72 Effect The TNC can increase or reduce the size of contours within a program, enabling you to program shrinkage and oversize allowances. The SCALING FACTOR becomes effective as soon as it is defined in the program. It is also effective in the Positioning with MDI mode of operation. The active scaling factor is shown in the additional status display.
10 AXIS-SPECIFIC SCALING (Cycle 26) 10.8 10.8 AXIS-SPECIFIC SCALING (Cycle 26) Effect With Cycle 26 you can account for shrinkage and oversize factors for each axis. The SCALING FACTOR becomes effective as soon as it is defined in the program. It is also effective in the Positioning with MDI mode of operation. The active scaling factor is shown in the additional status display. Resetting Program the SCALING cycle once again with a scaling factor of 1 for the same axis.
10 Cycles: Coordinate Transformations 10.8 AXIS-SPECIFIC SCALING (Cycle 26) Cycle parameters Axis and scaling factor: Select the coordinate axis/ axes by soft key and enter the factor(s) involved in enlarging or reducing. Input range 0.000001 to 99.999999 Center coordinates: Enter the center of the axisspecific enlargement or reduction. Input range -99999.9999 to 99999.9999 NC blocks 25 CALL LBL 1 26 CYCL DEF 26.0 AXIS-SPECIFIC SCALING 27 CYCL DEF 26.1 X 1.4 Y 0.
10 WORKING PLANE (Cycle 19, DIN/ISO: G80, software option 1) 10.9 10.9 WORKING PLANE (Cycle 19, DIN/ISO: G80, software option 1) Effect In Cycle 19 you define the position of the working plane—i.e. the position of the tool axis referenced to the machine coordinate system—by entering tilt angles. There are two ways to determine the position of the working plane: Enter the position of the rotary axes directly.
10 Cycles: Coordinate Transformations 10.9 WORKING PLANE (Cycle 19, DIN/ISO: G80, software option 1) Please note while programming: The functions for tilting the working plane are interfaced to the TNC and the machine tool by the machine tool builder. With some swivel heads and tilting tables, the machine tool builder determines whether the entered angles are interpreted as coordinates of the rotary axes or as angular components of a tilted plane. Refer to your machine manual.
10 WORKING PLANE (Cycle 19, DIN/ISO: G80, software option 1) 10.9 Resetting To cancel the tilt angle, redefine the WORKING PLANE cycle and enter an angular value of 0° for all axes of rotation. You must then program the WORKING PLANE cycle once again and respond to the dialog question with the NO ENT key to disable the function.
10 Cycles: Coordinate Transformations 10.9 WORKING PLANE (Cycle 19, DIN/ISO: G80, software option 1) Automatic positioning of rotary axes If the rotary axes are positioned automatically in Cycle 19: The TNC can position only controlled axes In order for the tilted axes to be positioned, you must enter a feed rate and a set-up clearance in addition to the tilting angles, during cycle definition. Use only preset tools (the full tool length must be defined).
10 WORKING PLANE (Cycle 19, DIN/ISO: G80, software option 1) 10.9 Positioning in a tilted coordinate system With the miscellaneous function M130 you can move the tool, while the coordinate system is tilted, to positions that are referenced to the non-tilted coordinate system. Positioning movements with straight lines that are referenced to the machine coordinate system (blocks with M91 or M92) can also be executed in a tilted working plane. Constraints: Positioning is without length compensation.
10 Cycles: Coordinate Transformations 10.9 WORKING PLANE (Cycle 19, DIN/ISO: G80, software option 1) Procedure for working with Cycle 19 WORKING PLANE 1 Write the program Define the tool (not required if TOOL.T is active), and enter the full tool length. Call the tool. Retract the tool in the tool axis to a position where there is no danger of collision with the workpiece or clamping devices during tilting.
10 Programming Examples 10.10 10.10 Programming Examples Example: Coordinate transformation cycles Program sequence Program the coordinate transformations in the main program Machining within a subprogram 0 BEGIN PGM COTRANS MM 1 BLK FORM 0.1 Z X+0 Y+0 Z-20 Definition of workpiece blank 2 BLK FORM 0.2 X+130 Y+130 Z+0 3 TOOL CALL 1 Z S4500 Tool call 4 L Z+250 R0 FMAX Retract the tool 5 CYCL DEF 7.0 DATUM SHIFT Shift datum to center 6 CYCL DEF 7.1 X+65 7 CYCL DEF 7.
10 Cycles: Coordinate Transformations 10.
11 Cycles: Special Functions
11 Cycles: Special Functions 11.1 Fundamentals 11.
11 DWELL TIME (Cycle 9) 11.2 11.2 DWELL TIME (Cycle 9, DIN/ISO: G04) Function This causes the execution of the next block within a running program to be delayed by the programmed DWELL TIME. A dwell time can be used for such purposes as chip breaking. The cycle becomes effective as soon as it is defined in the program. Modal conditions such as spindle rotation are not affected. NC blocks 89 CYCL DEF 9.0 DWELL TIME 90 CYCL DEF 9.1 DWELL 1.
11 Cycles: Special Functions 11.3 11.3 PROGRAM CALL (Cycle 12) PROGRAM CALL (Cycle 12, DIN/ISO: G39) Cycle function Routines that you have programmed (such as special drilling cycles or geometrical modules) can be written as main programs. These can then be called like fixed cycles. Please note while programming: The program you are calling must be stored in the internal memory of your TNC.
11 PROGRAM CALL (Cycle 12) 11.
11 Cycles: Special Functions 11.4 11.4 SPINDLE ORIENTATION (Cycle 13) SPINDLE ORIENTATION (Cycle 13, DIN/ISO: G36) Cycle function Machine and TNC must be specially prepared by the machine tool builder for use of this cycle. The TNC can control the machine tool spindle and rotate it to a given angular position.
11 TOLERANCE (Cycle 32, DIN/ISO: G62) 11.5 11.5 TOLERANCE (Cycle 32, DIN/ISO: G62) Cycle function Machine and TNC must be specially prepared by the machine tool builder for use of this cycle. With the entries in Cycle 32 you can influence the result of HSC machining with respect to accuracy, surface definition and speed, inasmuch as the TNC has been adapted to the machine’s characteristics. The TNC automatically smoothens the contour between two path elements (whether compensated or not).
11 Cycles: Special Functions 11.5 TOLERANCE (Cycle 32, DIN/ISO: G62) Please note while programming: With very small tolerance values the machine cannot cut the contour without jerking. These jerking movements are not caused by poor processing power in the TNC, but by the fact that, in order to machine the contour element transitions very exactly, the TNC might have to drastically reduce the speed. Cycle 32 is DEF active which means that it becomes effective as soon as it is defined in the part program.
11 TOLERANCE (Cycle 32, DIN/ISO: G62) 11.5 Cycle parameters Tolerance value T: Permissible contour deviation in mm (or inches with inch programming). Input range 0 to 99999.9999 HSC MODE, Finishing=0, Roughing=1: Activate filter: Input value 0: Milling with increased contour accuracy. The TNC uses internally defined finishing filter settings Input value 1: Milling at an increased feed rate.
11 Cycles: Special Functions 11.6 11.6 CONTOUR TURNING INTERPOLATION (Cycle 292, DIN/ISO: G292, software option 96) CONTOUR TURNING INTERPOLATION (Cycle 292, DIN/ ISO: G292, software option 96) Cycle run Cycle 292 CONTOUR TURNING INTERPOLATION couples the tool spindle to the position of the linear axes. This cycle enables you to machine specific rotationally symmetrical contours in the active working plane. You can also run this cycle in the tilted working plane.
11 CONTOUR TURNING INTERPOLATION (Cycle 292, DIN/ISO: G292, software option 96) 11.6 Cycle run, Q560=0: Contour milling 1 The M3/M4 function programmed before the cycle call remains in effect. 2 No spindle stop and no spindle orientation are performed. Q336 is not taken into account. 3 The TNC positions the tool to the contour start radius Q491, taking the selected machining operation inside/outside Q529 and the clearance to side Q357 into account.
11 Cycles: Special Functions 11.6 CONTOUR TURNING INTERPOLATION (Cycle 292, DIN/ISO: G292, software option 96) Please note while programming: A programming example is provided at the end of this chapter, see page 322. Program the contour either with monotonically decreasing or monotonically increasing coordinates. When programming, remember to use only positive radius values. Program the turning contour without tool radius compensation (RR/RL) and without APPR or DEP movements.
11 CONTOUR TURNING INTERPOLATION (Cycle 292, DIN/ISO: G292, software option 96) 11.6 The described contour is not automatically extended by a set-up clearance. An extension of the contour must be programmed in the subprogram.
11 Cycles: Special Functions 11.6 CONTOUR TURNING INTERPOLATION (Cycle 292, DIN/ISO: G292, software option 96) Cycle parameters Spindle coupling (0, 1) Q560: Define whether the spindle is to be coupled. 0: Spindle coupling off (contour milling) 1: Spindle coupling on (contour turning) Angle of spindle Q336: The TNC orients the tool to this angle before starting the machining operation. If you work with a milling tool, enter the angle in such a way that a tooth is turned towards the center of rotation.
11 CONTOUR TURNING INTERPOLATION (Cycle 292, DIN/ISO: G292, software option 96) 11.6 Machining variants Before using Cycle 292, you first need to define the desired turning contour in a subprogram and refer to this contour with Cycle 14 or SEL CONTOUR. Describe the turning contour on the cross section of a rotationally symmetrical body.
11 Cycles: Special Functions 11.6 CONTOUR TURNING INTERPOLATION (Cycle 292, DIN/ISO: G292, software option 96) Outside machining The center of rotation is the position of the tool in the working plane at the time the cycle is called 1 After the cycle is started, neither the indexable insert nor the spindle center must be moved into the center of rotation. Keep this in mind when describing the contour! 2 The described contour is not automatically extended by a set-up clearance.
11 CONTOUR TURNING INTERPOLATION (Cycle 292, DIN/ISO: G292, software option 96) 11.6 Defining the tool Overview Depending on the setting of the parameter Q560, you can mill (Q560=0) or turn (Q560=1) the contour. For each of the two machining modes, there are different possibilities to define the tool in the tool table.
11 Cycles: Special Functions 11.
11 COUPLING INTERPOLATION TURNING (cycle 291, DIN/ISO: G291, software option 96) 11.7 11.7 COUPLING INTERPOLATION TURNING (cycle 291, DIN/ISO: G291, software option 96) Cycle run Cycle 291 COUPLING TURNING INTERPOLATION couples the tool spindle to the position of the linear axes or deactivates this spindle coupling. In interpolation turning the cutting edge is oriented to the center of a circle. The center of rotation is defined in the cycle by entering the coordinates Q216 and Q217.
11 Cycles: Special Functions 11.7 COUPLING INTERPOLATION TURNING (cycle 291, DIN/ISO: G291, software option 96) Cycle 291 is CALL-active. Programming of M3/M4 is not required. In order to describe the circular motions of the linear axes, you can use CC and C coordinates, for example. If you specify the turning tool in the turning tool table (toolturn.trn), we recommend to work with parameter Q561=1.
11 COUPLING INTERPOLATION TURNING (cycle 291, DIN/ISO: G291, software option 96) 11.7 Cycle parameters Spindle coupling (0, 1) Q560: Define whether the tool spindle is coupled to the position of the linear axes. When spindle coupling is active, a cutting edge of the tool is oriented to the center of rotation. 0: Spindle coupling off 1: Spindle coupling on Angle of spindle Q336: The TNC orients the tool to this angle before starting the machining operation.
11 Cycles: Special Functions 11.7 COUPLING INTERPOLATION TURNING (cycle 291, DIN/ISO: G291, software option 96) Defining the tool Overview Depending on the setting of the parameter Q560, you can activate (Q560=1) or deactivate (Q560=0) the COUPLING TURNING INTERPOLATION cycle. Spindle coupling off, Q560=0 The tool spindle is not coupled to the position of the linear axes.
11 COUPLING INTERPOLATION TURNING (cycle 291, DIN/ISO: G291, software option 96) 11.7 Define a turning tool in the turning tool table (toolturn.trn) If you are working with option 50, you can define the turning tool in the turning tool table (toolturn.trn).
11 Cycles: Special Functions 11.
11 ENGRAVING (Cycle 225, DIN/ISO: G225) 11.8 11.8 ENGRAVING (Cycle 225, DIN/ISO: G225) Cycle run This cycle is used to engrave texts on a flat surface of the workpiece. The texts can be arranged in a straight line or along an arc. 1 The TNC positions the tool in the working plane to the starting point of the first character. 2 The tool plunges perpendicularly to the engraving floor and mills the character. The TNC retracts the tool to the set-up clearance between the characters when required.
11 Cycles: Special Functions 11.8 ENGRAVING (Cycle 225, DIN/ISO: G225) Cycle parameters Engraving text QS500: Text to be engraved inside quotation marks. Assignment of a string variable through the Q key of the numerical keypad. The Q key on the ASCI keyboard represents normal text input. Allowed entry characters: see "Engraving system variables", page 312 Character height Q513 (absolute): Height of the characters to be engraved in mm. Input range 0 to 99999.
11 ENGRAVING (Cycle 225, DIN/ISO: G225) 11.8 Allowed engraving characters The following special characters are allowed in addition to lowercase letters, uppercase letters and numbers: ! # $ % & ‘ ( ) * + , - . / : ; < = > ? @ [ \ ] _ ß CE The TNC uses the special characters % and \ for special functions. These characters must be indicated twice in the text to be engraved (e.g. %%) if you want to engrave them.
11 Cycles: Special Functions 11.8 ENGRAVING (Cycle 225, DIN/ISO: G225) Engraving system variables In addition to the standard characters, you can engrave the contents of certain system variables. Enter % before the system variable. You can also engrave the current date or time. Enter %time. defines the format, e.g. 08 for DD.MM.YYYY.
11 FACE MILLING (Cycle 232, DIN/ISO: G232) 11.9 11.9 FACE MILLING (Cycle 232, DIN/ISO: G232) Cycle run Cycle 232 is used to face mill a level surface in multiple infeeds while taking the finishing allowance into account.
11 Cycles: Special Functions 11.9 FACE MILLING (Cycle 232, DIN/ISO: G232) Strategy Q389=1 3 The tool subsequently advances to the end point 2 at the programmed feed rate for milling. The end point lies at the edge of the surface. The TNC calculates the end point from the programmed starting point, the programmed length and the tool radius. 4 The TNC offsets the tool to the starting point in the next pass at the pre-positioning feed rate.
11 FACE MILLING (Cycle 232, DIN/ISO: G232) 11.9 Please note while programming: Enter the 2nd set-up clearance in Q204 so that no collision with the workpiece or the fixtures can occur. If the starting point in the 3rd axis Q227 and the end point in the 3rd axis Q386 are entered as equal values, the TNC does not run the cycle (depth = 0 has been programmed). Program Q227 greater than Q386. Otherwise, the TNC will display an error message.
11 Cycles: Special Functions 11.
11 FACE MILLING (Cycle 232, DIN/ISO: G232) 11.9 Max. path overlap factor Q370: Maximum stepover factor k. The TNC calculates the actual stepover from the second side length (Q219) and the tool radius so that a constant stepover is used for machining. If you have entered a radius R2 in the tool table (e.g. tooth radius when using a face-milling cutter), the TNC reduces the stepover accordingly. Input range 0.1 to 1.9999 Feed rate for milling Q207: Traversing speed of the tool in mm/min while milling.
11 Cycles: Special Functions 11.10 ASCERTAIN THE LOAD (Cycle 239, DIN/ISO: G239, software option 143) 11.10 ASCERTAIN THE LOAD (Cycle 239, DIN/ISO: G239, software option 143) Cycle run The dynamic behavior of your machine may vary with different workpiece weights acting on the machine table. A change in the load has an influence on the friction forces, acceleration, holding torque and stick-slip friction of table axes.
11 ASCERTAIN THE LOAD (Cycle 239, DIN/ISO: G239, software option 11.10 143) Please note while programming: Cycle 239 becomes effective immediately after definition. If you are using the mid-program startup function and the TNC skips Cycle 239 in the block scan, the TNC will ignore this cycle—no weighing procedure will be performed. The machine must be prepared by the machine tool builder for this cycle. Cycle 239 can only be used with option 143 LAC (Load Adaptive Control).
Cycles: Special Functions 11.11 Programming examples 11.11 Programming examples 60 5 6 Cycle 291 COUPLING TURNING INTERPOLATION is used in the following program. This programming example illustrates the machining of an axial recess and a radial recess. Program sequence Turning tool as defined in toolturn.trn: tool No 10: TO:1, ORI:0, TYPE:ROUGH, tool for axial recesses Turning tool as defined in toolturn.
11 Programming examples 11.11 13 LBL 2 Retract from recess, step: 0.4 mm 14 CP IPA+360 IZ+0.4 DR+ 15 CALL LBL 2 REP15 16 L Z+200 R0 FMAX Retract to clearance height, deactivate radius compensation 17 CYCL DEF 291 COUPLG. TURNG. INTERP.
Cycles: Special Functions 11.11 Programming examples Q217=+0 ;CENTER IN 2ND AXIS Q561=+0 ;TURNING TOOL CONVERSION 42 CYCL CALL Call the cycle 43 TOOL CALL 11 Repeated TOOL CALL in order to override the conversion of parameter Q561 44 M30 45 END PGM 1 MM Example: Interpolation Turning Cycle 292 38 30 5 40 7 Cycle 292 CONTOUR TURNING INTERPOLATION is used in the following program. This programming example illustrates the machining of an outside contour with the milling spindle rotating.
11 Programming examples 11.
12 Cycles: Turning
12 Cycles: Turning 12.1 Turning Cycles (software option 50) 12.1 Turning Cycles (software option 50) Overview Defining turning cycles: The soft-key row shows the available groups of cycles Select the menu for cycle group TURNING Select cycle group, e.g. cycles for longitudinal turning Select cycle, e.g.
12 Turning Cycles (software option 50) 12.
12 Cycles: Turning 12.
12 Turning Cycles (software option 50) 12.1 Working with turning cycles You can only use turning cycles in Turning mode FUNCTION MODE TURN. In turning cycles the TNC takes into account the cutting geometry (TO, RS, P-ANGLE, T-ANGLE) of the tool so that damage to the defined contour elements is prevented. The TNC outputs a warning if complete machining of the contour with the active tool is not possible. You can use the turning cycles both for inside and outside machining.
12 Cycles: Turning 12.1 Turning Cycles (software option 50) Blank form update (FUNCTION TURNDATA) During turning operations workpieces must often be machined with several tools. Often a contour element cannot be completely finished because the tool form does not permit this (e.g. with a back cut). In this case, single sub-areas have to be reworked with other tools.
12 Turning Cycles (software option 50) 12.
12 Cycles: Turning 12.2 ADAPT ROTARY COORDINATE SYSTEM (Cycle 800, DIN/ISO: G800) 12.2 ADAPT ROTARY COORDINATE SYSTEM (Cycle 800, DIN/ISO: G800) Application This function must be adapted to the TNC by your machine manufacturer. Refer to your machine manual. You need to position the tool appropriately with respect to the turning spindle, in order to be able to perform a turning operation. You can use Cycle 800 ADAPT ROTARY COORDINATE SYSTEM for this.
12 ADAPT ROTARY COORDINATE SYSTEM 12.2 (Cycle 800, DIN/ISO: G800) If the axis of the milling spindle and the axis of the turning spindle are aligned parallel to each other, you can use PRECESSION ANGLE Q497 to define any desired rotation of the coordinate system around the spindle axis (Z axis). This may be necessary if you have to bring the tool into a specific position due to space restrictions or if you want to improve your ability to observe a machining process.
12 Cycles: Turning 12.2 ADAPT ROTARY COORDINATE SYSTEM (Cycle 800, DIN/ISO: G800) Eccentric turning Sometimes it is not possible to clamp a workpiece such that the axis of rotation is aligned with the axis of the turning spindle (e.g. if large or rotationally non-symmetrical workpieces are being used). The Q535 eccentric turning function in Cycle 800 enables you to perform turning operations in such cases as well. During eccentric turning more than one linear axis is coupled to the turning spindle.
12 ADAPT ROTARY COORDINATE SYSTEM 12.2 (Cycle 800, DIN/ISO: G800) Effect With Cycle 800 ADAPT ROTARY COORDINATE SYSTEM, the TNC aligns the workpiece coordinate system and orients the tool correspondingly. Cycle 800 is effective until it is reset by Cycle 801, or until Cycle 800 is defined again. Some cycle functions of Cycle 800 are additionally reset by other factors: The mirroring of the tool data (Q498 REVERSE TOOL) is reset by a TOOL CALL.
12 Cycles: Turning 12.2 ADAPT ROTARY COORDINATE SYSTEM (Cycle 800, DIN/ISO: G800) Cycle parameters PRECESSION ANGLE Q497: Angle to which the TNC aligns the tool. Input range 0 to 359.9999 REVERSE TOOL Q498: mirror tool for inside/ outside machining. Input range 0 and 1.
12 ADAPT ROTARY COORDINATE SYSTEM 12.2 (Cycle 800, DIN/ISO: G800) Eccentric turning Q535: Couple the axes for the eccentric turning operation: 0: Deactivate axis couplings 1: Activate axis couplings The center of rotation is located at the active preset 2: Activate axis couplings. The center of rotation is located at the active datum 3: Do not change axis couplings. Eccentric turning without stop Q536: Interrupt program run before the axes are coupled: 0: Stop before the axes are coupled again.
12 Cycles: Turning 12.3 RESET ROTARY COORDINATE SYSTEM (Cycle 801, DIN/ISO: G801) 12.3 RESET ROTARY COORDINATE SYSTEM (Cycle 801, DIN/ISO: G801) Please note while programming: The Cycle 801 RESET ROTARY COORDINATE SYSTEM is machine-dependent. Refer to your machine manual. With Cycle 801 RESET ROTARY COORDINATE SYSTEM you can reset the settings you have made with Cycle 800 ADAPT ROTARY COORDINATE SYSTEM. Cycle 800 limits the maximum spindle speed during eccentric turning.
12 Fundamentals of Turning Cycles 12.4 12.4 Fundamentals of Turning Cycles The pre-positioning of the tool decisively affects the workspace of the cycle and thus the machining time. During roughing, the starting point for cycles corresponds to the tool position when a cycle is called. When calculating the area to be machined, the TNC takes into account the starting point and the end point defined in the cycle or contour defined in the cycle.
12 Cycles: Turning 12.5 TURN SHOULDER LONGITUDINAL (Cycle 811, DIN/ISO: G811) 12.5 TURN SHOULDER LONGITUDINAL (Cycle 811, DIN/ISO: G811) Application This cycle enables you to carry out longitudinal turning of rightangled shoulders. You can use the cycle either for roughing, finishing or complete machining. Turning is run paraxially with roughing. The cycle can be used for inside and outside machining.
12 TURN SHOULDER LONGITUDINAL 12.5 (Cycle 811, DIN/ISO: G811) Finishing cycle run 1 The TNC traverses the tool in the Z coordinate by the set-up clearance Q460. The movement is performed at rapid traverse. 2 The TNC runs the paraxial infeed motion at rapid traverse. 3 The TNC finishes the finished part contour at the defined feed rate Q505. 4 The TNC returns the tool to set-up clearance at the defined feed rate. 5 The TNC positions the tool back at rapid traverse to the cycle starting point.
12 Cycles: Turning 12.5 TURN SHOULDER LONGITUDINAL (Cycle 811, DIN/ISO: G811) Cycle parameters Machining operation Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing to finished dimension 3: Only finishing to oversize Set-up clearance Q460 (incremental): Distance for retraction and pre-positioning.
12 TURN SHOULDER LONGITUDINAL EXTENDED 12.6 (Cycle 812, DIN/ISO: G812) 12.6 TURN SHOULDER LONGITUDINAL EXTENDED (Cycle 812, DIN/ISO: G812) Application This cycle enables you to run longitudinal turning of shoulders. Expanded scope of function: You can insert a chamfer or curve at the contour start and contour end.
12 Cycles: Turning 12.6 TURN SHOULDER LONGITUDINAL EXTENDED (Cycle 812, DIN/ISO: G812) Finishing cycle run If the starting point lies in the area to be machined, the TNC positions the tool beforehand to set-up clearance in the Z coordinate. 1 The TNC runs the paraxial infeed motion at rapid traverse. 2 The TNC finishes the finished part contour (contour starting point to contour end point) at the defined feed rate Q505. 3 The TNC returns the tool to set-up clearance at the defined feed rate.
12 TURN SHOULDER LONGITUDINAL EXTENDED 12.6 (Cycle 812, DIN/ISO: G812) Cycle parameters Machining operation Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing to finished dimension 3: Only finishing to oversize Set-up clearance Q460 (incremental): Distance for retraction and pre-positioning.
12 Cycles: Turning 12.6 TURN SHOULDER LONGITUDINAL EXTENDED (Cycle 812, DIN/ISO: G812) Type of starting element Q501: Define the type of element at the start of the contour (circumferential surface): 0: No additional element 1: Element is a chamfer 2: Element is a radius Size of starting element Q502: Size of the starting element (chamfer section) Radius of contour edge Q500: Radius of the inside contour edge. If no radius is specified, the radius of the cutting insert is generated.
12 TURN, LONGITUDINAL PLUNGE 12.7 (Cycle 813, DIN/ISO: G813) 12.7 TURN, LONGITUDINAL PLUNGE (Cycle 813, DIN/ISO: G813) Application This cycle enables you to run longitudinal turning of shoulders with plunge elements (undercuts). You can use the cycle either for roughing, finishing or complete machining. Turning is run paraxially with roughing. The cycle can be used for inside and outside machining. If the start diameter Q491 is larger than the end diameter Q493, the cycle runs outside machining.
12 Cycles: Turning 12.7 TURN, LONGITUDINAL PLUNGE (Cycle 813, DIN/ISO: G813) Finishing cycle run 1 The TNC runs the infeed motion at rapid traverse. 2 The TNC finishes the finished part contour (contour starting point to contour end point) at the defined feed rate Q505. 3 The TNC returns the tool to set-up clearance at the defined feed rate. 4 The TNC positions the tool back at rapid traverse to the cycle starting point.
12 TURN, LONGITUDINAL PLUNGE 12.7 (Cycle 813, DIN/ISO: G813) Cycle parameters Machining operation Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing to finished dimension 3: Only finishing to oversize Set-up clearance Q460 (incremental): Distance for retraction and pre-positioning.
12 Cycles: Turning 12.8 TURN, LONGITUDINAL PLUNGE EXTENDED (Cycle 814, DIN/ISO: G814) 12.8 TURN, LONGITUDINAL PLUNGE EXTENDED (Cycle 814, DIN/ISO: G814) Application This cycle enables you to run longitudinal turning of shoulders with plunge elements (undercuts). Expanded scope of function: You can insert a chamfer or curve at the contour start and contour end.
12 TURN, LONGITUDINAL PLUNGE EXTENDED 12.8 (Cycle 814, DIN/ISO: G814) Finishing cycle run 1 The TNC runs the infeed motion at rapid traverse. 2 The TNC finishes the finished part contour (contour starting point to contour end point) at the defined feed rate Q505. 3 The TNC returns the tool to set-up clearance at the defined feed rate. 4 The TNC positions the tool back at rapid traverse to the cycle starting point.
12 Cycles: Turning 12.8 TURN, LONGITUDINAL PLUNGE EXTENDED (Cycle 814, DIN/ISO: G814) Cycle parameters Machining operation Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing to finished dimension 3: Only finishing to oversize Set-up clearance Q460 (incremental): Distance for retraction and pre-positioning.
12 TURN, LONGITUDINAL PLUNGE EXTENDED 12.8 (Cycle 814, DIN/ISO: G814) Type of starting element Q501: Define the type of element at the start of the contour (circumferential surface): 0: No additional element 1: Element is a chamfer 2: Element is a radius Size of starting element Q502: Size of the starting element (chamfer section) Radius of contour edge Q500: Radius of the inside contour edge. If no radius is specified, the radius of the cutting insert is generated.
12 Cycles: Turning 12.9 TURN CONTOUR LONGITUDINAL (Cycle 810, DIN/ISO: G810) 12.9 TURN CONTOUR LONGITUDINAL (Cycle 810, DIN/ISO: G810) Application This cycle enables you to run longitudinal turning of workpieces with any turning contours. The contour description is in a subprogram. You can use the cycle either for roughing, finishing or complete machining. Turning is run paraxially with roughing. The cycle can be used for inside and outside machining.
12 TURN CONTOUR LONGITUDINAL 12.9 (Cycle 810, DIN/ISO: G810) Finishing cycle run If the Z coordinate of the starting point is less than the contour starting point, the TNC positions the tool in the Z coordinate to setup clearance and begins the cycle there. 1 The TNC runs the infeed motion at rapid traverse. 2 The TNC finishes the finished part contour (contour starting point to contour end point) at the defined feed rate Q505. 3 The TNC returns the tool to set-up clearance at the defined feed rate.
12 Cycles: Turning 12.9 TURN CONTOUR LONGITUDINAL (Cycle 810, DIN/ISO: G810) Cycle parameters Machining operation Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing to finished dimension 3: Only finishing to oversize Set-up clearance Q460 (incremental): Distance for retraction and pre-positioning.
12 TURN CONTOUR LONGITUDINAL 12.9 (Cycle 810, DIN/ISO: G810) Oversize in Z Q484 (incremental): Oversize for the defined contour in axial direction Finishing feed rate Q505: Feed rate during finishing. If M136 has been programmed, the value is interpreted by the TNC in millimeters per revolution, without M136 in millimeters per minute.
12 Cycles: Turning 12.10 TURN CONTOUR-PARALLEL (Cycle 815, DIN/ISO: G815) 12.10 TURN CONTOUR-PARALLEL (Cycle 815, DIN/ISO: G815) Application This cycle enables you to machine workpieces with any turning contours. The contour description is in a subprogram. You can use the cycle either for roughing, finishing or complete machining. Turning with roughing is contour-parallel. The cycle can be used for inside and outside machining.
12 TURN CONTOUR-PARALLEL 12.10 (Cycle 815, DIN/ISO: G815) Finishing cycle run If the Z coordinate of the starting point is less than the contour starting point, the TNC positions the tool in the Z coordinate to setup clearance and begins the cycle there. 1 The TNC runs the infeed motion at rapid traverse. 2 The TNC finishes the finished part contour (contour starting point to contour end point) at the defined feed rate Q505. 3 The TNC returns the tool to set-up clearance at the defined feed rate.
12 Cycles: Turning 12.10 TURN CONTOUR-PARALLEL (Cycle 815, DIN/ISO: G815) Cycle parameters Machining operation Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing to finished dimension 3: Only finishing to oversize Set-up clearance Q460 (incremental): Distance for retraction and pre-positioning.
12 TURN CONTOUR-PARALLEL 12.10 (Cycle 815, DIN/ISO: G815) Roughing feed rate Q478: Feed rate during roughing. If M136 has been programmed, the value is interpreted by the TNC in millimeters per revolution, without M136 in millimeters per minute. Oversize in diameter Q483 (incremental): Diameter oversize for the defined contour Oversize in Z Q484 (incremental): Oversize for the defined contour in axial direction Finishing feed rate Q505: Feed rate during finishing.
12 Cycles: Turning 12.11 TURN SHOULDER FACE (Cycle 821, DIN/ISO: G821) 12.11 TURN SHOULDER FACE (Cycle 821, DIN/ISO: G821) Application This cycle enables you to face turn right-angled shoulders. You can use the cycle either for roughing, finishing or complete machining. Turning is run paraxially with roughing. The cycle can be used for inside and outside machining. If the tool is outside the contour to be machined when the cycle is called, the cycle runs outside machining.
12 TURN SHOULDER FACE 12.11 (Cycle 821, DIN/ISO: G821) Finishing cycle run 1 The TNC traverses the tool in the Z coordinate by the set-up clearance Q460. The movement is performed at rapid traverse. 2 The TNC runs the paraxial infeed motion at rapid traverse. 3 The TNC finishes the finished part contour at the defined feed rate Q505. 4 The TNC returns the tool to set-up clearance at the defined feed rate. 5 The TNC positions the tool back at rapid traverse to the cycle starting point.
12 Cycles: Turning 12.11 TURN SHOULDER FACE (Cycle 821, DIN/ISO: G821) Cycle parameters Machining operation Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing to finished dimension 3: Only finishing to oversize Set-up clearance Q460 (incremental): Distance for retraction and pre-positioning.
12 TURN SHOULDER FACE EXTENDED 12.12 (Cycle 822, DIN/ISO: G822) 12.12 TURN SHOULDER FACE EXTENDED (Cycle 822, DIN/ISO: G822) Application This cycle enables you to face turn shoulders. Expanded scope of function: You can insert a chamfer or curve at the contour start and contour end. In the cycle you can define angles for the face and circumferential surfaces You can insert a radius in the contour edge You can use the cycle either for roughing, finishing or complete machining.
12 Cycles: Turning 12.12 TURN SHOULDER FACE EXTENDED (Cycle 822, DIN/ISO: G822) Finishing cycle run 1 The TNC runs the paraxial infeed motion at rapid traverse. 2 The TNC finishes the finished part contour (contour starting point to contour end point) at the defined feed rate Q505. 3 The TNC returns the tool to set-up clearance at the defined feed rate. 4 The TNC positions the tool back at rapid traverse to the cycle starting point.
12 TURN SHOULDER FACE EXTENDED 12.12 (Cycle 822, DIN/ISO: G822) Cycle parameters Machining operation Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing to finished dimension 3: Only finishing to oversize Set-up clearance Q460 (incremental): Distance for retraction and pre-positioning.
12 Cycles: Turning 12.12 TURN SHOULDER FACE EXTENDED (Cycle 822, DIN/ISO: G822) Size of starting element Q502: Size of the starting element (chamfer section) Radius of contour edge Q500: Radius of the inside contour edge. If no radius is specified, the radius of the cutting insert is generated.
12 TURN, TRANSVERSE PLUNGE 12.13 (Cycle 823, DIN/ISO: G823) 12.13 TURN, TRANSVERSE PLUNGE (Cycle 823, DIN/ISO: G823) Application This cycle enables you to face turn plunge elements (undercuts). You can use the cycle either for roughing, finishing or complete machining. Turning is run paraxially with roughing. The cycle can be used for inside and outside machining. If the start diameter Q491 is larger than the end diameter Q493, the cycle runs outside machining.
12 Cycles: Turning 12.13 TURN, TRANSVERSE PLUNGE (Cycle 823, DIN/ISO: G823) Finishing cycle run The TNC uses the tool position as cycle starting point when a cycle is called. If the Z coordinate of the starting point is less than the contour starting point, the TNC positions the tool in the Z coordinate to set-up clearance and begins the cycle there. 1 The TNC runs the infeed motion at rapid traverse.
12 TURN, TRANSVERSE PLUNGE 12.13 (Cycle 823, DIN/ISO: G823) Cycle parameters Machining operation Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing to finished dimension 3: Only finishing to oversize Set-up clearance Q460 (incremental): Distance for retraction and pre-positioning.
12 Cycles: Turning 12.14 TURN, TRANSVERSE PLUNGE EXTENDED (Cycle 824, DIN/ISO: G824) 12.14 TURN, TRANSVERSE PLUNGE EXTENDED (Cycle 824, DIN/ISO: G824) Application This cycle enables you to face turn plunge elements (undercuts). Expanded scope of function: You can insert a chamfer or curve at the contour start and contour end. In the cycle you can define an angle for the face and a radius for the contour edge You can use the cycle either for roughing, finishing or complete machining.
12 TURN, TRANSVERSE PLUNGE EXTENDED 12.14 (Cycle 824, DIN/ISO: G824) Finishing cycle run The TNC uses the tool position as cycle starting point when a cycle is called. If the Z coordinate of the starting point is less than the contour starting point, the TNC positions the tool in the Z coordinate to set-up clearance and begins the cycle there. 1 The TNC runs the infeed motion at rapid traverse.
12 Cycles: Turning 12.14 TURN, TRANSVERSE PLUNGE EXTENDED (Cycle 824, DIN/ISO: G824) Cycle parameters Machining operation Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing to finished dimension 3: Only finishing to oversize Set-up clearance Q460 (incremental): Distance for retraction and pre-positioning.
12 TURN, TRANSVERSE PLUNGE EXTENDED 12.14 (Cycle 824, DIN/ISO: G824) Size of starting element Q502: Size of the starting element (chamfer section) Radius of contour edge Q500: Radius of the inside contour edge. If no radius is specified, the radius of the cutting insert is generated.
12 Cycles: Turning 12.15 TURN CONTOUR FACE (Cycle 820, DIN/ISO: G820) 12.15 TURN CONTOUR FACE (Cycle 820, DIN/ISO: G820) Application This cycle enables you to face turn workpieces with any turning contours. The contour description is in a subprogram. You can use the cycle either for roughing, finishing or complete machining. Turning is run paraxially with roughing. The cycle can be used for inside and outside machining.
12 TURN CONTOUR FACE 12.15 (Cycle 820, DIN/ISO: G820) Finishing cycle run If the Z coordinate of the starting point is less than the contour starting point, the TNC positions the tool in the Z coordinate to setup clearance and begins the cycle there. 1 The TNC runs the infeed motion at rapid traverse. 2 The TNC finishes the finished part contour (contour starting point to contour end point) at the defined feed rate Q505. 3 The TNC returns the tool to set-up clearance at the defined feed rate.
12 Cycles: Turning 12.15 TURN CONTOUR FACE (Cycle 820, DIN/ISO: G820) Cycle parameters Machining operation Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing to finished dimension 3: Only finishing to oversize Set-up clearance Q460 (incremental): Distance for retraction and pre-positioning.
12 TURN CONTOUR FACE 12.15 (Cycle 820, DIN/ISO: G820) Oversize in Z Q484 (incremental): Oversize for the defined contour in axial direction Finishing feed rate Q505: Feed rate during finishing. If M136 has been programmed, the value is interpreted by the TNC in millimeters per revolution, without M136 in millimeters per minute.
12 Cycles: Turning 12.16 SIMPLE RADIAL RECESSING (Cycle 841, DIN/ISO: G841) 12.16 SIMPLE RADIAL RECESSING (Cycle 841, DIN/ISO: G841) Application This cycle enables you to recess right-angled slots in longitudinal direction. With recess turning, a recessing traverse to plunging depth and then a roughing traverse is alternatively machined. The machining process thus requires a minimum of retraction and infeed movements. You can use the cycle either for roughing, finishing or complete machining.
12 SIMPLE RADIAL RECESSING 12.16 (Cycle 841, DIN/ISO: G841) Finishing cycle run 1 The TNC positions the tool at rapid traverse to the first slot side. 2 The TNC finishes the side wall of the slot at the defined feed rate Q505. 3 The TNC finishes the slot floor at the defined feed rate. 4 The TNC returns the tool at rapid traverse. 5 The TNC positions the tool at rapid traverse to the second slot side. 6 The TNC finishes the side wall of the slot at the defined feed rate Q505.
12 Cycles: Turning 12.
12 RADIAL RECESSING EXTENDED 12.17 (Cycle 842, DIN/ISO: G842) 12.17 RADIAL RECESSING EXTENDED (Cycle 842, DIN/ISO: G842) Application This cycle enables you to recess right-angled slots in longitudinal direction. With recess turning, a recessing traverse to plunging depth and then a roughing traverse is alternatively machined. The machining process thus requires a minimum of retraction and infeed movements. Expanded scope of function: You can insert a chamfer or curve at the contour start and contour end.
12 Cycles: Turning 12.17 RADIAL RECESSING EXTENDED (Cycle 842, DIN/ISO: G842) Finishing cycle run The TNC uses the tool position as cycle starting point when a cycle is called. If the Z coordinate of the starting point is less than Q491 DIAMETER AT CONTOUR START, the TNC positions the tool in the X coordinate to Q491 and begins the cycle there. 1 The TNC positions the tool at rapid traverse to the first slot side. 2 The TNC finishes the side wall of the slot at the defined feed rate Q505.
12 RADIAL RECESSING EXTENDED 12.
12 Cycles: Turning 12.17 RADIAL RECESSING EXTENDED (Cycle 842, DIN/ISO: G842) Type of starting element Q501: Define the type of element at the start of the contour (circumferential surface): 0: No additional element 1: Element is a chamfer 2: Element is a radius Size of starting element Q502: Size of the starting element (chamfer section) Radius of contour edge Q500: Radius of the inside contour edge. If no radius is specified, the radius of the cutting insert is generated.
12 RADIAL RECESSING EXTENDED 12.17 (Cycle 842, DIN/ISO: G842) Turning depth compensation Q509: Depending on factors such as workpiece material or feed rate, the tool tip is displaced during a turning operation. You can correct the resulting infeed error with the turning depth compensation factor. Feed rate for plunging Q488: Feed rate for machining of plunging elements. This input value is optional. If it is not programmed, the feed rate defined for turning is effective.
12 Cycles: Turning 12.18 RECESSING CONTOUR RADIAL (Cycle 840, DIN/ISO: G840) 12.18 RECESSING CONTOUR RADIAL (Cycle 840, DIN/ISO: G840) Application This cycle enables you to recess right-angled slots of any form in longitudinal direction. With recess turning, a recessing traverse to plunging depth and then a roughing traverse is alternatively machined. You can use the cycle either for roughing, finishing or complete machining. Turning is run paraxially with roughing.
12 RECESSING CONTOUR RADIAL 12.18 (Cycle 840, DIN/ISO: G840) Finishing cycle run 1 The TNC positions the tool at rapid traverse to the first slot side. 2 The TNC finishes the side walls of the slot at the defined feed rate Q505. 3 The TNC finishes the slot floor at the defined feed rate. 4 The TNC positions the tool back at rapid traverse to the cycle starting point. Please note while programming: The cutting limit defines the contour range to be machined.
12 Cycles: Turning 12.18 RECESSING CONTOUR RADIAL (Cycle 840, DIN/ISO: G840) Cycle parameters Machining operation Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing to finished dimension 3: Only finishing to oversize Set-up clearance Q460: Reserved, currently without function Roughing feed rate Q478: Feed rate during roughing. If M136 has been programmed, the value is interpreted by the TNC in millimeters per revolution, without M136 in millimeters per minute.
12 RECESSING CONTOUR RADIAL 12.18 (Cycle 840, DIN/ISO: G840) Finishing feed rate Q505: Feed rate during finishing. If M136 has been programmed, the value is interpreted by the TNC in millimeters per revolution, without M136 in millimeters per minute.
12 Cycles: Turning 12.19 SIMPLE AXIAL RECESSING (Cycle 851, DIN/ISO: G851) 12.19 SIMPLE AXIAL RECESSING (Cycle 851, DIN/ISO: G851) Application This cycle enables you to recess right-angled slots in traverse direction. With recess turning, a recessing traverse to plunging depth and then a roughing traverse is alternatively machined. The machining process thus requires a minimum of retraction and infeed movements. You can use the cycle either for roughing, finishing or complete machining.
12 SIMPLE AXIAL RECESSING 12.19 (Cycle 851, DIN/ISO: G851) Finishing cycle run 1 The TNC positions the tool at rapid traverse to the first slot side. 2 The TNC finishes the side wall of the slot at the defined feed rate Q505. 3 The TNC finishes the slot floor at the defined feed rate. 4 The TNC returns the tool at rapid traverse. 5 The TNC positions the tool at rapid traverse to the second slot side. 6 The TNC finishes the side wall of the slot at the defined feed rate Q505.
12 Cycles: Turning 12.
12 AXIAL RECESSING EXTENDED 12.20 (Cycle 852, DIN/ISO: G852) 12.20 AXIAL RECESSING EXTENDED (Cycle 852, DIN/ISO: G852) Application This cycle enables you to recess right-angled slots in traverse direction. With recess turning, a recessing traverse to plunging depth and then a roughing traverse is alternatively machined. The machining process thus requires a minimum of retraction and infeed movements. Expanded scope of function: You can insert a chamfer or curve at the contour start and contour end.
12 Cycles: Turning 12.20 AXIAL RECESSING EXTENDED (Cycle 852, DIN/ISO: G852) Finishing cycle run The TNC uses the tool position as cycle starting point when a cycle is called. If the Z coordinate of the starting point is less than Q492 CONTOUR START IN Z, the TNC positions the tool in the Z coordinate to Q492 and begins the cycle there. 1 The TNC positions the tool at rapid traverse to the first slot side. 2 The TNC finishes the side wall of the slot at the defined feed rate Q505.
12 AXIAL RECESSING EXTENDED 12.
12 Cycles: Turning 12.20 AXIAL RECESSING EXTENDED (Cycle 852, DIN/ISO: G852) Type of starting element Q501: Define the type of element at the start of the contour (circumferential surface): 0: No additional element 1: Element is a chamfer 2: Element is a radius Size of starting element Q502: Size of the starting element (chamfer section) Radius of contour edge Q500: Radius of the inside contour edge. If no radius is specified, the radius of the cutting insert is generated.
12 AXIAL RECESSING EXTENDED 12.20 (Cycle 852, DIN/ISO: G852) Turning depth compensation Q509: Depending on factors such as workpiece material or feed rate, the tool tip is displaced during a turning operation. You can correct the resulting infeed error with the turning depth compensation factor. Feed rate for plunging Q488: Feed rate for machining of plunging elements. This input value is optional. If it is not programmed, the feed rate defined for turning is effective.
12 Cycles: Turning 12.21 AXIAL RECESSING (Cycle 850, DIN/ISO: G850) 12.21 AXIAL RECESSING (Cycle 850, DIN/ISO: G850) Application This cycle enables you to recess right-angled slots of any form in longitudinal direction. With recess turning, a recessing traverse to plunging depth and then a roughing traverse is alternatively machined. You can use the cycle either for roughing, finishing or complete machining. Turning is run paraxially with roughing. The cycle can be used for inside and outside machining.
12 AXIAL RECESSING 12.21 (Cycle 850, DIN/ISO: G850) Finishing cycle run The TNC uses the tool position as cycle starting point when a cycle is called. 1 The TNC positions the tool at rapid traverse to the first slot side. 2 The TNC finishes the side walls of the slot at the defined feed rate Q505. 3 The TNC finishes the slot floor at the defined feed rate. 4 The TNC positions the tool back at rapid traverse to the cycle starting point.
12 Cycles: Turning 12.21 AXIAL RECESSING (Cycle 850, DIN/ISO: G850) Cycle parameters Machining operation Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing to finished dimension 3: Only finishing to oversize Set-up clearance Q460: Reserved, currently without function Roughing feed rate Q478: Feed rate during roughing. If M136 has been programmed, the value is interpreted by the TNC in millimeters per revolution, without M136 in millimeters per minute.
12 AXIAL RECESSING 12.21 (Cycle 850, DIN/ISO: G850) Finishing feed rate Q505: Feed rate during finishing. If M136 has been programmed, the value is interpreted by the TNC in millimeters per revolution, without M136 in millimeters per minute.
12 Cycles: Turning 12.22 RADIAL RECESSING (Cycle 861, DIN/ISO: G861) 12.22 RADIAL RECESSING (Cycle 861, DIN/ISO: G861) Application This cycle enables you to radially cut in right-angled slots. You can use the cycle either for roughing, finishing or complete machining. Turning is run paraxially with roughing. The cycle can be used for inside and outside machining. If the tool is outside the contour to be machined when the cycle is called, the cycle runs outside machining.
12 RADIAL RECESSING 12.22 (Cycle 861, DIN/ISO: G861) Finishing cycle run 1 The TNC positions the tool at rapid traverse to the first slot side. 2 The TNC finishes the side wall of the slot at the defined feed rate Q505. 3 The TNC finishes half the slot width at the defined feed rate. 4 The TNC returns the tool at rapid traverse. 5 The TNC positions the tool at rapid traverse to the second slot side. 6 The TNC finishes the side wall of the slot at the defined feed rate Q505.
12 Cycles: Turning 12.
12 RADIAL RECESSING EXTENDED 12.23 (Cycle 862, DIN/ISO: G862) 12.23 RADIAL RECESSING EXTENDED (Cycle 862, DIN/ISO: G862) Application This cycle enables you to radially cut in slots. Expanded scope of function: You can insert a chamfer or curve at the contour start and contour end. In the cycle you can define angles for the side walls of the slot You can insert radii in the contour edges You can use the cycle either for roughing, finishing or complete machining. Turning is run paraxially with roughing.
12 Cycles: Turning 12.23 RADIAL RECESSING EXTENDED (Cycle 862, DIN/ISO: G862) Finishing cycle run 1 The TNC positions the tool at rapid traverse to the first slot side. 2 The TNC finishes the side wall of the slot at the defined feed rate Q505. 3 The TNC finishes half the slot width at the defined feed rate. 4 The TNC returns the tool at rapid traverse. 5 The TNC positions the tool at rapid traverse to the second slot side. 6 The TNC finishes the side wall of the slot at the defined feed rate Q505.
12 RADIAL RECESSING EXTENDED 12.
12 Cycles: Turning 12.23 RADIAL RECESSING EXTENDED (Cycle 862, DIN/ISO: G862) Type of starting element Q501: Define the type of element at the start of the contour (circumferential surface): 0: No additional element 1: Element is a chamfer 2: Element is a radius Size of starting element Q502: Size of the starting element (chamfer section) Radius of contour edge Q500: Radius of the inside contour edge. If no radius is specified, the radius of the cutting insert is generated.
12 RECESSING CONTOUR RADIAL 12.24 (Cycle 860, DIN/ISO: G860) 12.24 RECESSING CONTOUR RADIAL (Cycle 860, DIN/ISO: G860) Application This cycle enables you to radially cut in slots of any form. You can use the cycle either for roughing, finishing or complete machining. Turning is run paraxially with roughing. The cycle can be used for inside and outside machining. If the starting point of the contour is larger than the end point of the contour, the cycle runs outside machining.
12 Cycles: Turning 12.24 RECESSING CONTOUR RADIAL (Cycle 860, DIN/ISO: G860) Finishing cycle run 1 The TNC positions the tool at rapid traverse to the first slot side. 2 The TNC finishes the side wall of the slot at the defined feed rate Q505. 3 The TNC finishes one half of the slot at the defined feed rate. 4 The TNC returns the tool at rapid traverse. 5 The TNC positions the tool at rapid traverse to the second slot side. 6 The TNC finishes the side wall of the slot at the defined feed rate Q505.
12 RECESSING CONTOUR RADIAL 12.24 (Cycle 860, DIN/ISO: G860) Cycle parameters Machining operation Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing to finished dimension 3: Only finishing to oversize Set-up clearance Q460: Reserved, currently without function Roughing feed rate Q478: Feed rate during roughing. If M136 has been programmed, the value is interpreted by the TNC in millimeters per revolution, without M136 in millimeters per minute.
12 Cycles: Turning 12.24 RECESSING CONTOUR RADIAL (Cycle 860, DIN/ISO: G860) Finishing feed rate Q505: Feed rate during finishing. If M136 has been programmed, the value is interpreted by the TNC in millimeters per revolution, without M136 in millimeters per minute.
12 AXIAL RECESSING 12.25 (Cycle 871, DIN/ISO: G871) 12.25 AXIAL RECESSING (Cycle 871, DIN/ISO: G871) Application This cycle enables you to axially cut in right-angled slots (face recessing). You can use the cycle either for roughing, finishing or complete machining. Turning is run paraxially with roughing. Roughing cycle run The TNC uses the tool position as cycle starting point when a cycle is called. The cycle processes only the area from the cycle starting point to the end point defined in the cycle.
12 Cycles: Turning 12.25 AXIAL RECESSING (Cycle 871, DIN/ISO: G871) Please note while programming: Program a positioning block to the starting position with radius compensation R0 before the cycle call. The tool position at cycle call defines the size of the area to be machined (cycle starting point).
12 AXIAL RECESSING EXTENDED 12.26 (Cycle 872, DIN/ISO: G872) 12.26 AXIAL RECESSING EXTENDED (Cycle 872, DIN/ISO: G872) Application This cycle enables you to axially cut in slots (face recessing). Expanded scope of function: You can insert a chamfer or curve at the contour start and contour end. In the cycle you can define angles for the side walls of the slot You can insert radii in the contour edges You can use the cycle either for roughing, finishing or complete machining.
12 Cycles: Turning 12.26 AXIAL RECESSING EXTENDED (Cycle 872, DIN/ISO: G872) Finishing cycle run The TNC uses the tool position as cycle starting point when a cycle is called. If the Z coordinate of the starting point is less than Q492 CONTOUR START IN Z, the TNC positions the tool in the Z coordinate to Q492 and begins the cycle there. 1 The TNC positions the tool at rapid traverse to the first slot side. 2 The TNC finishes the side wall of the slot at the defined feed rate Q505.
12 AXIAL RECESSING EXTENDED 12.
12 Cycles: Turning 12.26 AXIAL RECESSING EXTENDED (Cycle 872, DIN/ISO: G872) Size of end element Q504: Size of the end element (chamfer section) Roughing feed rate Q478: Feed rate during roughing. If M136 has been programmed, the value is interpreted by the TNC in millimeters per revolution, without M136 in millimeters per minute.
12 AXIAL RECESSING 12.27 (Cycle 870, DIN/ISO: G870) 12.27 AXIAL RECESSING (Cycle 870, DIN/ISO: G870) Application This cycle enables you to axially cut in slots of any form (face recessing). You can use the cycle either for roughing, finishing or complete machining. Turning is run paraxially with roughing. Roughing cycle run The TNC uses the tool position as cycle starting point when a cycle is called.
12 Cycles: Turning 12.27 AXIAL RECESSING (Cycle 870, DIN/ISO: G870) Finishing cycle run The TNC uses the tool position as cycle starting point when a cycle is called. 1 The TNC positions the tool at rapid traverse to the first slot side. 2 The TNC finishes the side wall of the slot at the defined feed rate Q505. 3 The TNC finishes one half of the slot at the defined feed rate. 4 The TNC returns the tool at rapid traverse. 5 The TNC positions the tool at rapid traverse to the second slot side.
12 AXIAL RECESSING 12.27 (Cycle 870, DIN/ISO: G870) Cycle parameters Machining operation Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing to finished dimension 3: Only finishing to oversize Set-up clearance Q460: Reserved, currently without function Roughing feed rate Q478: Feed rate during roughing. If M136 has been programmed, the value is interpreted by the TNC in millimeters per revolution, without M136 in millimeters per minute.
12 Cycles: Turning 12.28 THREAD LONGITUDINAL (Cycle 831, DIN/ISO: G831) 12.28 THREAD LONGITUDINAL (Cycle 831, DIN/ISO: G831) Application This cycle enables you to run longitudinal turning of threads. You can process single threads or multi-threads with the cycle. If you do not enter a thread depth, the cycle uses thread depth in accordance with the ISO1502 standard. The cycle can be used for inside and outside machining.
12 THREAD LONGITUDINAL 12.28 (Cycle 831, DIN/ISO: G831) Please note while programming: Program a positioning block to the starting position with radius compensation R0 before the cycle call. The TNC uses the set-up clearance Q460 as approach path. The approach path must be long enough for the feed axes to be accelerated to the required velocity. The TNC uses the thread pitch as overrun path. The overrun path must be long enough to decelerate the feed axes.
12 Cycles: Turning 12.28 THREAD LONGITUDINAL (Cycle 831, DIN/ISO: G831) Cycle parameters Thread position Q471: Define the position of the thread: 0: External thread 1: Internal thread Set-up clearance Q460: Set-up clearance in radial and axial direction. In axial direction, the set-up clearance is used for acceleration (approach path) to the synchronized feed rate. Thread diameter Q491: Define the nominal diameter of the thread. Thread pitch Q472: Pitch of the thread.
12 THREAD EXTENDED (Cycle 832, DIN/ISO: G832) 12.29 12.29 THREAD EXTENDED (Cycle 832, DIN/ ISO: G832) Application This cycle enables you to run both face turning and longitudinal turning of threads or tapered threads. Expanded scope of function: Selection of longitudinal thread or face thread. The parameters for dimension type of taper, taper angle and contour starting point X enable the definition of various tapered threads.
12 Cycles: Turning 12.29 THREAD EXTENDED (Cycle 832, DIN/ISO: G832) Please note while programming: Program a positioning block to a safe position with radius compensation R0 before the cycle call. The approach path (Q465) must be long enough for the feed axes to be accelerated to the required velocity. The overrun path (Q466) must be long enough to decelerate the feed axes. When the TNC runs a thread cut, the feed-rate override knob is disabled.
12 THREAD EXTENDED (Cycle 832, DIN/ISO: G832) 12.29 Cycle parameters Thread position Q471: Define the position of the thread: 0: External thread 1: Internal thread Thread orientationQ461: Define the direction of the thread pitch: 0: Longitudinal (parallel to the rotary axis) 1: Lateral (perpendicular to the rotary axis) Set-up clearance Q460: Set-up clearance perpendicular to thread pitch. Thread pitch Q472: Pitch of the thread. Depth of thread Q473 (incremental): Depth of the thread.
12 Cycles: Turning 12.29 THREAD EXTENDED (Cycle 832, DIN/ISO: G832) Angle of infeed Q467: Angle for the infeed Q463. The reference angle is formed by the parallel line to the thread pitch. Type of infeed Q468: Define the type of infeed: 0: Constant chip cross section (infeed lessens with depth) 1: Constant plunging depth Starting angle Q470: Angle of the turning spindle at which the thread start is to be made.
12 CONTOUR-PARALLEL THREAD 12.30 (Cycle 830, DIN/ISO: G830) 12.30 CONTOUR-PARALLEL THREAD (Cycle 830, DIN/ISO: G830) Application This cycle enables you to run both face turning and longitudinal turning of threads with any form. You can process single threads or multi-threads with the cycle. If you do not enter a thread depth in the cycle, the cycle uses a standardized thread depth. The cycle can be used for inside and outside machining.
12 Cycles: Turning 12.30 CONTOUR-PARALLEL THREAD (Cycle 830, DIN/ISO: G830) Please note while programming: Program a positioning block to the starting position with radius compensation R0 before the cycle call. The approach path (Q465) must be long enough for the feed axes to be accelerated to the required velocity. The overrun path (Q466) must be long enough to decelerate the feed axes. Both the approach and overrun take place outside the defined contour.
12 CONTOUR-PARALLEL THREAD 12.30 (Cycle 830, DIN/ISO: G830) Cycle parameters Thread position Q471: Define the position of the thread: 0: External thread 1: Internal thread Thread orientationQ461: Define the direction of the thread pitch: 0: Longitudinal (parallel to the rotary axis) 1: Lateral (perpendicular to the rotary axis) Set-up clearance Q460: Set-up clearance perpendicular to thread pitch. Thread pitch Q472: Pitch of the thread.
12 Cycles: Turning 12.30 CONTOUR-PARALLEL THREAD (Cycle 830, DIN/ISO: G830) Approach path Q465 (incremental): Length of the path in pitch direction on which the feed axes are accelerated to the required velocity. The approach path is outside of the defined thread contour. Overrun path Q466: Length of the path in pitch direction on which the feed axes are decelerated. The overrun path is within the defined thread contour.
12 GEAR HOBBING (Cycle 880, DIN/ISO: G880) 12.31 12.31 GEAR HOBBING (Cycle 880, DIN/ISO: G880) Cycle run With Cycle 880 Gear Hobbing you can machine external cylindrical gears or helical gears with any angles. In the cycle you first define the gear and then the tool with which the gear is to be machined. You can select the machining strategy and the machining side in the cycle. The machining process for gear hobbing is performed with a synchronized rotary motion of the tool spindle and rotary table.
12 Cycles: Turning 12.31 GEAR HOBBING (Cycle 880, DIN/ISO: G880) Please note while programming: The values entered for module, number of teeth and outside diameter are monitored. If these values are not consistent, an error message is displayed. It is also possible to make entries for only 2 of these 3 parameters. In this case, enter the value 0 for either the module or the number of teeth or the outside diameter. The TNC then calculates the missing value. Program FUNCTION TURNDATA SPIN VCONST:OFF.
12 GEAR HOBBING (Cycle 880, DIN/ISO: G880) 12.31 Cycle parameters Machining operation Q215: Define machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing to finished dimension 3: Only finishing to oversize Module Q540: Define the gear: Module of the gear wheel. Input range 0 to 99.9999 Number of teeth Q541: Define the gear: Number of teeth. Input range 0 to 99999 Outside diameter Q542: Define the gear: Outside diameter of the finished part. Input range 0 to 99999.
12 Cycles: Turning 12.31 GEAR HOBBING (Cycle 880, DIN/ISO: G880) Inclined machining Q530: Position the tilting axes for inclined machining: 1: Position the tilting axis automatically, thereby orienting the tool tip (MOVE). The relative position between the tool and workpiece remains unchanged. The TNC performs a compensating movement with the linear axes 2: Position the tilting axis automatically without orienting the tool tip (TURN).
12 GEAR HOBBING (Cycle 880, DIN/ISO: G880) 12.31 Roughing feed rate Q478: Feed rate during roughing. If M136 has been programmed, the value is interpreted by the TNC in millimeters per revolution, without M136 in millimeters per minute. Oversize in diameter Q483 (incremental): Diameter oversize for the defined contour . Finishing feed rate Q505: Feed rate during finishing. If M136 has been programmed, the value is interpreted by the TNC in millimeters per revolution, without M136 in millimeters per minute.
12 Cycles: Turning 12.32 CHECK UNBALANCE (Cycle 892, DIN/ISO: G892) 12.32 CHECK UNBALANCE (Cycle 892, DIN/ ISO: G892) Application When turning a nonsymmetrical workpiece, such as a pump body, an unbalance may occur. This may cause a high load on the machine, depending on the rotational speed, mass and shape of the workpiece. With Cycle 892 CHECK UNBALANCE the TNC checks the unbalance of the turning spindle. This cycle uses two parameters. Q450 describes the maximum unbalance and Q451 the maximum speed.
12 CHECK UNBALANCE (Cycle 892, DIN/ISO: G892) 12.32 Please note while programming: Check the unbalance whenever you clamp a new workpiece. If required, use balancing weights to compensate any imbalance. The removal of material during machining will change the mass distribution within the workpiece. This may also have an influence on workpiece unbalance. Therefore, unbalance checks should also be carried out between machining steps.
12 Cycles: Turning 12.32 CHECK UNBALANCE (Cycle 892, DIN/ISO: G892) Cycle parameters Maximum runout Q450: (mm) Specifies the maximum amplitude of a sinusoidal unbalance signal. The signal results from the following error of the measuring axis and from the spindle revolutions. Speed Q451: (rpm) The unbalance check starts at a low rotational speed (e.g. 50 rpm). It is automatically increased by specified increments (e.g. 25 rpm) until the defined maximum speed is reached. Spindle override is not effective.
12 Example program 12.33 12.33 Example program Example: Shoulder with recess 0 BEGIN PGM SHOULDER MM 1 BLK FORM 0.1 Y X+0 Y-10 Z-35 Definition of workpiece blank 2 BLK FORM 0.
12 Cycles: Turning 12.33 Example program Q484=+0.2 ;OVERSIZE IN Z Q505=+0.
12 Example program 12.33 Example: Gear hobbing Cycle 880 GEAR HOBBING is used in the following program. This programming example illustrates the machining of a helical gear, with Module=2.1.
12 Cycles: Turning 12.33 Example program Q488=+1 ;PLUNGING FEED RATE Q478=+2 ;ROUGHING FEED RATE Q483=+0.
13 Using Touch Probe Cycles
13 Using Touch Probe Cycles 13.1 General information about touch probe cycles 13.1 General information about touch probe cycles HEIDENHAIN only warrants the function of the touch probe cycles if HEIDENHAIN touch probes are used. The TNC must be specially prepared by the machine tool builder for the use of a 3-D touch probe. Refer to your machine manual. Method of function Whenever the TNC runs a touch probe cycle, the 3-D touch probe approaches the workpiece in one linear axis.
13 General information about touch probe cycles 13.1 Touch probe cycles for automatic operation Besides the touch probe cycles, which you can use in the Manual and El.
13 Using Touch Probe Cycles 13.1 General information about touch probe cycles Defining the touch probe cycle in the Programming and Editing mode of operation The soft-key row shows all available touch probe functions divided into groups. Select the desired probe cycle group, for example datum setting. Cycles for automatic tool measurement are available only if your machine has been prepared for them. Select a cycle, e.g. datum setting at pocket center.
13 Before You Start Working with Touch Probe Cycles 13.2 13.2 Before You Start Working with Touch Probe Cycles To make it possible to cover the widest possible range of applications, machine parameters enable you to determine the behavior common to all touch probe cycles. Maximum traverse to touch point: DIST in touch probe table If the stylus is not deflected within the path defined in DIST, the TNC outputs an error message.
13 Using Touch Probe Cycles 13.2 Before You Start Working with Touch Probe Cycles Touch trigger probe, probing feed rate: F in touch probe table In F you define the feed rate at which the TNC is to probe the workpiece. Touch trigger probe, rapid traverse for positioning: FMAX In FMAX you define the feed rate at which the TNC pre-positions the touch probe, or positions it between measuring points.
13 Before You Start Working with Touch Probe Cycles 13.2 Multiple measurements To increase measuring certainty, the TNC can run each probing process up to three times in sequence. Define the number of measurements in machine parameter ProbeSettings > Configuration of probe behavior > Automatic mode: Multiple measurements with probe function. If the measured position values differ too greatly, the TNC outputs an error message (the limit value is defined in Confidence interval of multiple measurements).
13 Using Touch Probe Cycles 13.2 Before You Start Working with Touch Probe Cycles Executing touch probe cycles All touch probe cycles are DEF active. This means that the TNC runs the cycle automatically as soon as the TNC executes the cycle definition in the program run. Danger of collision! When running touch probe cycles, no cycles must be active for coordinate transformation (Cycle 7 DATUM, Cycle 8 MIRROR IMAGE, Cycle 10 ROTATION, Cycles 11 SCALING and 26 AXISSPECIFIC SCALING).
13 Touch probe table 13.3 13.3 Touch probe table General information Various data is stored in the touch probe table that defines the probe behavior during the probing process. If you run several touch probes on your machine tool, you can save separate data for each touch probe.
13 Using Touch Probe Cycles 13.3 Touch probe table Touch probe data Abbr. Inputs Dialog NO Number of the touch probe: Enter this number in the tool table (column: TP_NO) under the appropriate tool number – TYPE Selection of the touch probe used Selection of touch probe? CAL_OF1 Offset of the touch probe axis to the spindle axis for the reference axis TS center misalignmt. ref. axis? [mm] CAL_OF2 Offset of the touch probe axis to the spindle axis for the minor axis TS center misalignmt. aux.
14 Touch Probe Cycles: Automatic Measurement of Workpiece Misalignment
14 Touch Probe Cycles: Automatic Measurement of Workpiece Misalignment 14.1 Fundamentals 14.1 Fundamentals Overview When running touch probe cycles, Cycle 8 MIRROR IMAGE, Cycle 11 SCALING and Cycle 26 AXISSPECIFIC SCALING must not be active. HEIDENHAIN only warrants the function of the touch probe cycles if HEIDENHAIN touch probes are used. The TNC must be specially prepared by the machine tool builder for the use of a 3-D touch probe. Refer to your machine manual.
14 Fundamentals 14.1 Characteristics common to all touch probe cycles for measuring workpiece misalignment For Cycles 400, 401 and 402 you can define through parameter Q307 Default setting for basic rotation whether the measurement result is to be corrected by a known angle # (see figure at right). This enables you to measure the basic rotation against any straight line 1 of the workpiece and to establish the reference to the actual 0° direction 2.
14 Touch Probe Cycles: Automatic Measurement of Workpiece Misalignment 14.2 BASIC ROTATION (Cycle 400, DIN/ISO: G400) 14.2 BASIC ROTATION (Cycle 400, DIN/ISO: G400) Cycle run Touch probe cycle 400 determines a workpiece misalignment by measuring two points, which must lie on a straight surface. With the basic rotation function the TNC compensates the measured value.
14 BASIC ROTATION (Cycle 400, DIN/ISO: G400) 14.2 Cycle parameters 1st meas. point 1st axis Q263 (absolute): Coordinate of the first touch point in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 1st meas. point 2nd axis Q264 (absolute): Coordinate of the first touch point in the minor axis of the working plane. Input range -99999.9999 to 99999.9999 2nd meas. point 1st axis Q265 (absolute): Coordinate of the second touch point in the reference axis of the working plane.
14 Touch Probe Cycles: Automatic Measurement of Workpiece Misalignment 14.
14 BASIC ROTATION over two holes (Cycle 401, DIN/ISO: G401) 14.3 14.3 BASIC ROTATION over two holes (Cycle 401, DIN/ISO: G401) Cycle run The Touch Probe Cycle 401 measures the centers of two holes. Then the TNC calculates the angle between the reference axis in the working plane and the line connecting the hole centers. With the basic rotation function, the TNC compensates the calculated value. As an alternative, you can also compensate the determined misalignment by rotating the rotary table.
14 Touch Probe Cycles: Automatic Measurement of Workpiece Misalignment 14.3 BASIC ROTATION over two holes (Cycle 401, DIN/ISO: G401) Cycle parameters 1st hole: Center in 1st axis Q268 (absolute): Center of the first hole in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 1st hole: Center in 2nd axis Q269 (absolute): Center of the first hole in the minor axis of the working plane. Input range -99999.9999 to 99999.
14 BASIC ROTATION over two holes (Cycle 401, DIN/ISO: G401) 14.3 Compensation Q402: Define whether the TNC should set the measured misalignment as basic rotation or should align via rotating the rotary table: 0: Set basic rotation 1: Rotate the rotary table If you specify rotating the rotary table, the TNC does not save the measured misalignment, even if you have defined a table row in parameter Q305.
14 Touch Probe Cycles: Automatic Measurement of Workpiece Misalignment 14.4 BASIC ROTATION over two studs (Cycle 402, DIN/ISO: G402) 14.4 BASIC ROTATION over two studs (Cycle 402, DIN/ISO: G402) Cycle run The Touch Probe Cycle 402 measures the centers of two studs. Then the TNC calculates the angle between the reference axis in the working plane and the line connecting the two stud centers. With the basic rotation function, the TNC compensates the calculated value.
14 BASIC ROTATION over two studs (Cycle 402, DIN/ISO: G402) 14.4 Cycle parameters 1st stud: Center in 1st axis Q268 (absolute): Center of the first stud in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 1st stud: Center in 2nd axis Q269 (absolute): Center of the first stud in the minor axis of the working plane. Input range -99999.9999 to 99999.9999 Diameter of stud 1 Q313: Approximate diameter of the 1st stud.
14 Touch Probe Cycles: Automatic Measurement of Workpiece Misalignment 14.4 BASIC ROTATION over two studs (Cycle 402, DIN/ISO: G402) Preset value for rotation angle Q307 (absolute): If the misalignment is to be measured against a straight line other than the reference axis, enter the angle of this reference line. The TNC will then calculate the difference between the value measured and the angle of the reference line for the basic rotation. Input range -360.000 to 360.
14 BASIC ROTATION compensation via rotary axis (Cycle 403, DIN/ 14.5 ISO: G403) 14.5 BASIC ROTATION compensation via rotary axis (Cycle 403, DIN/ ISO: G403) Cycle run Touch probe cycle 403 determines a workpiece misalignment by measuring two points, which must lie on a straight line. The TNC compensates the determined misalignment by rotating the A, B or C axis. The workpiece can be clamped in any position on the rotary table.
14 Touch Probe Cycles: Automatic Measurement of Workpiece Misalignment 14.5 BASIC ROTATION compensation via rotary axis (Cycle 403, DIN/ ISO: G403) Cycle parameters 1st meas. point 1st axis Q263 (absolute): Coordinate of the first touch point in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 1st meas. point 2nd axis Q264 (absolute): Coordinate of the first touch point in the minor axis of the working plane. Input range -99999.9999 to 99999.9999 2nd meas.
14 BASIC ROTATION compensation via rotary axis (Cycle 403, DIN/ 14.
14 Touch Probe Cycles: Automatic Measurement of Workpiece Misalignment 14.6 SET BASIC ROTATION (Cycle 404, DIN/ISO: G404) 14.6 SET BASIC ROTATION (Cycle 404, DIN/ISO: G404) Cycle run With Touch Probe Cycle 404, during program run you can automatically set any basic rotation or save it to the preset table. You can also use Cycle 404 if you want to reset an active basic rotation. NC blocks 5 TCH PROBE 404 BASIC ROTATION Q307=+0 ;PRESET ROTATION ANG. Q305=-1 ;NO.
14 Compensating workpiece misalignment by rotating the C axis 14.7 (Cycle 405, DIN/ISO: G405) 14.7 Compensating workpiece misalignment by rotating the C axis (Cycle 405, DIN/ISO: G405) Cycle run With Touch Probe Cycle 405, you can measure the angular offset between the positive Y axis of the active coordinate system and the center of a hole, or the angular offset between the nominal position and the actual position of a hole center.
14 Touch Probe Cycles: Automatic Measurement of Workpiece Misalignment 14.7 Compensating workpiece misalignment by rotating the C axis (Cycle 405, DIN/ISO: G405) Please note while programming: Danger of collision! To prevent a collision between the touch probe and the workpiece, enter a low estimate for the nominal diameter of the pocket (or hole).
14 Compensating workpiece misalignment by rotating the C axis 14.7 (Cycle 405, DIN/ISO: G405) Cycle parameters Center in 1st axis Q321 (absolute): Center of the hole in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 Center in 2nd axis Q322 (absolute value): Center of the hole in the minor axis of the working plane. If you program Q322 = 0, the TNC aligns the hole center to the positive Y axis.
14 Touch Probe Cycles: Automatic Measurement of Workpiece Misalignment 14.7 Compensating workpiece misalignment by rotating the C axis (Cycle 405, DIN/ISO: G405) Set to zero after alignment Q337: definition of whether the TNC should set the display of the Caxis to zero, or write the angular misalignment in column C of the datum table: 0: Set the display of the C-axis to zero >0: Write the measured angular misalignment with correct algebraic signs in the datum table. Line number = value of Q337.
14 Example: Determining a basic rotation from two holes 14.8 14.
15 Touch Probe Cycles: Automatic Datum Setting
15 Touch Probe Cycles: Automatic Datum Setting 15.1 Fundamentals 15.1 Fundamentals Overview When running touch probe cycles, Cycle 8 MIRROR IMAGE, Cycle 11 SCALING and Cycle 26 AXISSPECIFIC SCALING must not be active. HEIDENHAIN only warrants the function of the touch probe cycles if HEIDENHAIN touch probes are used. The TNC must be specially prepared by the machine tool builder for the use of a 3-D touch probe. Refer to your machine manual.
15 Fundamentals 15.1 Soft key Cycle Page 408 SLOT CENTER REF PT. Measuring the inside width of a slot, and defining the slot center as datum 484 409 RIDGE CENTER REF PT.
15 Touch Probe Cycles: Automatic Datum Setting 15.1 Fundamentals Characteristics common to all touch probe cycles for datum setting You can also run the Touch Probe Cycles 408 to 419 during an active rotation (basic rotation or Cycle 10). Datum point and touch probe axis From the touch probe axis that you have defined in the measuring program the TNC determines the working plane for the datum.
15 Fundamentals 15.1 This combination can only occur if you read in programs containing Cycles 410 to 418 created on a TNC 4xx read in programs containing Cycles 410 to 418 created with an older software version on an iTNC 530 did not specifically define the measured-value transfer with parameter Q303 when defining the cycle. In these cases the TNC outputs an error message, since the complete handling of REF-referenced datum tables has changed.
15 Touch Probe Cycles: Automatic Datum Setting 15.2 DATUM SLOT CENTER (Cycle 408, DIN/ISO: G408) 15.2 DATUM SLOT CENTER (Cycle 408, DIN/ISO: G408) Cycle run Touch Probe Cycle 408 finds the center of a slot and defines its center as datum. If desired, the TNC can also enter the coordinates into a datum table or the preset table. 1 Following the positioning logic, the TNC positions the touch probe at rapid traverse (value from FMAX column) (see "Executing touch probe cycles", page 454) to touch point 1.
15 DATUM SLOT CENTER (Cycle 408, DIN/ISO: G408) 15.2 Please note while programming: Danger of collision! To prevent a collision between touch probe and workpiece, enter a low estimate for the slot width. If the slot width and the safety clearance do not permit pre-positioning in the proximity of the touch points, the TNC always starts probing from the center of the slot. In this case the touch probe does not return to the clearance height between the two measuring points.
15 Touch Probe Cycles: Automatic Datum Setting 15.2 DATUM SLOT CENTER (Cycle 408, DIN/ISO: G408) Cycle parameters Center in 1st axis Q321 (absolute): Center of the slot in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 Center in 2nd axis Q322 (absolute): Center of the slot in the minor axis of the working plane. Input range -99999.9999 to 99999.9999 Width of slot Q311 (incremental): Width of the slot, regardless of its position in the working plane. Input range 0 to 99999.
15 DATUM SLOT CENTER (Cycle 408, DIN/ISO: G408) 15.2 Probe in TS axis Q381: Specify whether the TNC should also set the datum in the touch probe axis: 0: Do not set the datum in the touch probe axis 1: Set the datum in the touch probe axis Probe TS axis: Coord. 1st axis Q382 (absolute): Coordinate of the probe point in the reference axis of the working plane at which point the datum is to be set in the touch probe axis. Only effective if Q381 = 1st input range -99999.9999 to 99999.
15 Touch Probe Cycles: Automatic Datum Setting 15.3 DATUM RIDGE CENTER (Cycle 409, DIN/ISO: G409) 15.3 DATUM RIDGE CENTER (Cycle 409, DIN/ISO: G409) Cycle run Touch Probe Cycle 409 finds the center of a ridge and defines its center as datum. If desired, the TNC can also enter the coordinates into a datum table or the preset table.
15 DATUM RIDGE CENTER (Cycle 409, DIN/ISO: G409) 15.3 Cycle parameters Center in 1st axis Q321 (absolute): Center of the ridge in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 Center in 2nd axis Q322 (absolute): Center of the ridge in the minor axis of the working plane. Input range -99999.9999 to 99999.9999 Width of ridge Q311 (incremental): Width of the ridge, regardless of its position in the working plane. Input range 0 to 99999.
15 Touch Probe Cycles: Automatic Datum Setting 15.3 DATUM RIDGE CENTER (Cycle 409, DIN/ISO: G409) Probe TS axis: Coord. 1st axis Q382 (absolute): Coordinate of the probe point in the reference axis of the working plane at which point the datum is to be set in the touch probe axis. Only effective if Q381 = 1st input range -99999.9999 to 99999.9999 Probe TS axis: Coord.
15 DATUM FROM INSIDE OF RECTANGLE (Cycle 410, DIN/ISO: G410) 15.4 15.4 DATUM FROM INSIDE OF RECTANGLE (Cycle 410, DIN/ ISO: G410) Cycle run Touch Probe Cycle 410 finds the center of a rectangular pocket and defines its center as datum. If desired, the TNC can also enter the coordinates into a datum table or the preset table. 1 Following the positioning logic, the TNC positions the touch probe at rapid traverse (value from FMAX column) (see "Executing touch probe cycles", page 454) to touch point 1.
15 Touch Probe Cycles: Automatic Datum Setting 15.4 DATUM FROM INSIDE OF RECTANGLE (Cycle 410, DIN/ISO: G410) Please note while programming: Danger of collision! To prevent a collision between touch probe and workpiece, enter low estimates for the lengths of the first and second sides. If the dimensions of the pocket and the safety clearance do not permit pre-positioning in the proximity of the touch points, the TNC always starts probing from the center of the pocket.
15 DATUM FROM INSIDE OF RECTANGLE (Cycle 410, DIN/ISO: G410) 15.4 Cycle parameters Center in 1st axis Q321 (absolute): Center of the pocket in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 Center in 2nd axis Q322 (absolute): Center of the pocket in the minor axis of the working plane. Input range -99999.9999 to 99999.9999 1st side length Q323 (incremental): Pocket length, parallel to the reference axis of the working plane. Input range 0 to 99999.
15 Touch Probe Cycles: Automatic Datum Setting 15.4 DATUM FROM INSIDE OF RECTANGLE (Cycle 410, DIN/ISO: G410) New datum for reference axis Q331 (absolute): Coordinate in the reference axis at which the TNC should set the pocket center. Default setting = 0. Input range -99999.9999 to 99999.9999 New datum for minor axis Q332 (absolute): Coordinate in the minor axis at which the TNC should set the pocket center. Default setting = 0 input range -99999.9999 to 99999.
15 DATUM FROM OUTSIDE OF RECTANGLE (Cycle 411, DIN/ISO: G411) 15.5 15.5 DATUM FROM OUTSIDE OF RECTANGLE (Cycle 411, DIN/ ISO: G411) Cycle run Touch Probe Cycle 411 finds the center of a rectangular stud and defines its center as datum. If desired, the TNC can also enter the coordinates into a datum table or the preset table. 1 Following the positioning logic, the TNC positions the touch probe at rapid traverse (value from FMAX column) (see "Executing touch probe cycles", page 454) to touch point 1.
15 Touch Probe Cycles: Automatic Datum Setting 15.5 DATUM FROM OUTSIDE OF RECTANGLE (Cycle 411, DIN/ISO: G411) Cycle parameters Center in 1st axis Q321 (absolute): Center of the stud in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 Center in 2nd axis Q322 (absolute): Center of the stud in the minor axis of the working plane. Input range -99999.9999 to 99999.
15 DATUM FROM OUTSIDE OF RECTANGLE (Cycle 411, DIN/ISO: G411) 15.5 Measured-value transfer (0, 1) Q303: Specify whether the determined datum is to be saved in the datum table or in the preset table: -1: Do not use! Is entered by the TNC when old programs are read in (see "Characteristics common to all touch probe cycles for datum setting", page 482) 0: Write the measured datum into the active datum table.
15 Touch Probe Cycles: Automatic Datum Setting 15.6 DATUM FROM INSIDE OF CIRCLE (Cycle 412, DIN/ISO: G412) 15.6 DATUM FROM INSIDE OF CIRCLE (Cycle 412, DIN/ISO: G412) Cycle run Touch Probe Cycle 412 finds the center of a circular pocket (or of a hole) and defines its center as datum. If desired, the TNC can also enter the coordinates into a datum table or the preset table.
15 DATUM FROM INSIDE OF CIRCLE (Cycle 412, DIN/ISO: G412) 15.6 Please note while programming: Danger of collision! To prevent a collision between the touch probe and the workpiece, enter a low estimate for the nominal diameter of the pocket (or hole). If the dimensions of the pocket and the safety clearance do not permit pre-positioning in the proximity of the touch points, the TNC always starts probing from the center of the pocket.
15 Touch Probe Cycles: Automatic Datum Setting 15.6 DATUM FROM INSIDE OF CIRCLE (Cycle 412, DIN/ISO: G412) Cycle parameters Center in 1st axis Q321 (absolute): Center of the pocket in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 Center in 2nd axis Q322 (absolute): Center of the pocket in the minor axis of the working plane. If you program Q322 = 0, the TNC aligns the hole center to the positive Y axis.
15 DATUM FROM INSIDE OF CIRCLE (Cycle 412, DIN/ISO: G412) 15.6 New datum for reference axis Q331 (absolute): Coordinate in the reference axis at which the TNC should set the pocket center. Default setting = 0. Input range -99999.9999 to 99999.9999 New datum for minor axis Q332 (absolute): Coordinate in the minor axis at which the TNC should set the pocket center. Default setting = 0 input range -99999.9999 to 99999.
15 Touch Probe Cycles: Automatic Datum Setting 15.6 DATUM FROM INSIDE OF CIRCLE (Cycle 412, DIN/ISO: G412) New datum in TS axis Q333 (absolute): Coordinate in the touch probe axis at which the TNC should set the datum. Default setting = 0. Input range -99999.9999 to 99999.9999 No.
15 DATUM FROM OUTSIDE OF CIRCLE (Cycle 413, DIN/ISO: G413) 15.7 15.7 DATUM FROM OUTSIDE OF CIRCLE (Cycle 413, DIN/ISO: G413) Cycle run Touch Probe Cycle 413 finds the center of a circular stud and defines it as datum. If desired, the TNC can also enter the coordinates into a datum table or the preset table. 1 Following the positioning logic, the TNC positions the touch probe at rapid traverse (value from FMAX column) (see "Executing touch probe cycles", page 454) to touch point 1.
15 Touch Probe Cycles: Automatic Datum Setting 15.7 DATUM FROM OUTSIDE OF CIRCLE (Cycle 413, DIN/ISO: G413) Cycle parameters Center in 1st axis Q321 (absolute): Center of the stud in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 Center in 2nd axis Q322 (absolute): Center of the stud in the minor axis of the working plane. If you program Q322 = 0, the TNC aligns the hole center to the positive Y axis.
15 DATUM FROM OUTSIDE OF CIRCLE (Cycle 413, DIN/ISO: G413) 15.7 Datum number in table Q305: Enter the number in the datum/preset table in which the TNC is to save the coordinates of the stud center. If Q303=1: If you enter Q305=0, the TNC automatically sets the display so that the new datum is on the stud center. If Q303=0: If you enter Q305=0, the TNC writes to line 0 of the datum table.
15 Touch Probe Cycles: Automatic Datum Setting 15.7 DATUM FROM OUTSIDE OF CIRCLE (Cycle 413, DIN/ISO: G413) Probe TS axis: Coord. 3rd axis Q384 (absolute): Coordinate of the probe point in the touch probe axis, at which point the datum is to be set in the touch probe axis. Only effective if Q381 = 1. Input range -99999.9999 to 99999.9999 New datum in TS axis Q333 (absolute): Coordinate in the touch probe axis at which the TNC should set the datum. Default setting = 0. Input range -99999.9999 to 99999.
15 DATUM FROM OUTSIDE OF CORNER (Cycle 414, DIN/ISO: G414) 15.8 15.8 DATUM FROM OUTSIDE OF CORNER (Cycle 414, DIN/ISO: G414) Cycle run Touch Probe Cycle 414 finds the intersection of two lines and defines it as the datum. If desired, the TNC can also enter the intersection into a datum table or preset table.
15 Touch Probe Cycles: Automatic Datum Setting 15.8 DATUM FROM OUTSIDE OF CORNER (Cycle 414, DIN/ISO: G414) Please note while programming: Danger of collision! If you set a datum (Q303 = 0) with the touch probe cycle and also use probe in TS axis (Q381 = 1), then no coordinate transformation must be active. Before a cycle definition you must have programmed a tool call to define the touch probe axis. The TNC always measures the first line in the direction of the minor axis of the working plane.
15 DATUM FROM OUTSIDE OF CORNER (Cycle 414, DIN/ISO: G414) 15.8 Cycle parameters 1st meas. point 1st axis Q263 (absolute): Coordinate of the first touch point in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 1st meas. point 2nd axis Q264 (absolute): Coordinate of the first touch point in the minor axis of the working plane. Input range -99999.9999 to 99999.
15 Touch Probe Cycles: Automatic Datum Setting 15.8 DATUM FROM OUTSIDE OF CORNER (Cycle 414, DIN/ISO: G414) Execute basic rotation Q304: Definition of whether the TNC should compensate workpiece misalignment with a basic rotation: 0: Do not execute basic rotation 1: Execute basic rotation Datum number in table Q305: Enter the datum number in the datum or preset table in which the TNC is to save the coordinates of the corner.
15 DATUM FROM OUTSIDE OF CORNER (Cycle 414, DIN/ISO: G414) 15.8 Probe TS axis: Coord. 2nd axis Q383 (absolute): Coordinate of the probe point in the minor axis of the working plane at which point the datum is to be set in the touch probe axis. Only effective if Q381 = 1. Input range -99999.9999 to 99999.9999 Probe TS axis: Coord. 3rd axis Q384 (absolute): Coordinate of the probe point in the touch probe axis, at which point the datum is to be set in the touch probe axis. Only effective if Q381 = 1.
15 Touch Probe Cycles: Automatic Datum Setting 15.9 DATUM FROM INSIDE OF CORNER (Cycle 415, DIN/ISO: G415) 15.9 DATUM FROM INSIDE OF CORNER (Cycle 415, DIN/ISO: G415) Cycle run Touch Probe Cycle 415 finds the intersection of two lines and defines it as the datum. If desired, the TNC can also enter the intersection into a datum table or preset table.
15 DATUM FROM INSIDE OF CORNER (Cycle 415, DIN/ISO: G415) 15.9 Please note while programming: Danger of collision! If you set a datum (Q303 = 0) with the touch probe cycle and also use probe in TS axis (Q381 = 1), then no coordinate transformation must be active. Before a cycle definition you must have programmed a tool call to define the touch probe axis. The TNC always measures the first line in the direction of the minor axis of the working plane.
15 Touch Probe Cycles: Automatic Datum Setting 15.9 DATUM FROM INSIDE OF CORNER (Cycle 415, DIN/ISO: G415) Cycle parameters 1st meas. point 1st axis Q263 (absolute): Coordinate of the first touch point in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 1st meas. point 2nd axis Q264 (absolute): Coordinate of the first touch point in the minor axis of the working plane. Input range -99999.9999 to 99999.
15 DATUM FROM INSIDE OF CORNER (Cycle 415, DIN/ISO: G415) 15.9 New datum for reference axis Q331 (absolute): Coordinate in the reference axis at which the TNC should set the corner. Default setting = 0 input range -99999.9999 to 99999.9999 New datum for minor axis Q332 (absolute): Coordinate in the minor axis at which the TNC should set the calculated corner. Default setting = 0 input range -99999.9999 to 99999.
15 Touch Probe Cycles: Automatic Datum Setting 15.10 DATUM CIRCLE CENTER (Cycle 416, DIN/ISO: G416) 15.10 DATUM CIRCLE CENTER (Cycle 416, DIN/ISO: G416) Cycle run Touch Probe Cycle 416 finds the center of a bolt hole circle and defines its center as datum. If desired, the TNC can also enter the coordinates into a datum table or the preset table.
15 DATUM CIRCLE CENTER (Cycle 416, DIN/ISO: G416) 15.10 Please note while programming: Danger of collision! If you set a datum (Q303 = 0) with the touch probe cycle and also use probe in TS axis (Q381 = 1), then no coordinate transformation must be active. Before a cycle definition you must have programmed a tool call to define the touch probe axis.
15 Touch Probe Cycles: Automatic Datum Setting 15.10 DATUM CIRCLE CENTER (Cycle 416, DIN/ISO: G416) Cycle parameters Center in 1st axis Q273 (absolute): Bolt hole circle center (nominal value) in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 Center in 2nd axis Q274 (absolute): Bolt hole circle center (nominal value) in the minor axis of the working plane. Input range -99999.9999 to 99999.9999 Nominal diameter Q262: Enter the approximate bolt hole circle diameter.
15 DATUM CIRCLE CENTER (Cycle 416, DIN/ISO: G416) 15.10 Measured-value transfer (0, 1) Q303: Specify whether the determined datum is to be saved in the datum table or in the preset table: -1: Do not use! Is entered by the TNC when old programs are read in (see "Characteristics common to all touch probe cycles for datum setting", page 482) 0: Write the measured datum into the active datum table. The reference system is the active workpiece coordinate system 1: Write the measured datum into the preset table.
15 Touch Probe Cycles: Automatic Datum Setting 15.11 DATUM IN TOUCH PROBE AXIS (Cycle 417, DIN/ISO: G417) 15.11 DATUM IN TOUCH PROBE AXIS (Cycle 417, DIN/ISO: G417) Cycle run Touch Probe Cycle 417 measures any coordinate in the touch probe axis and defines it as datum. If desired, the TNC can also enter the measured coordinate in a datum table or preset table.
15 DATUM IN TOUCH PROBE AXIS (Cycle 417, DIN/ISO: G417) 15.11 Cycle parameters 1st meas. point 1st axis Q263 (absolute): Coordinate of the first touch point in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 1st meas. point 2nd axis Q264 (absolute): Coordinate of the first touch point in the minor axis of the working plane. Input range -99999.9999 to 99999.9999 1st meas. point 3rd axis Q294 (absolute): Coordinate of the first touch point in the touch probe axis.
15 Touch Probe Cycles: Automatic Datum Setting 15.12 DATUM AT CENTER OF 4 HOLES (Cycle 418, DIN/ISO: G418) 15.12 DATUM AT CENTER OF 4 HOLES (Cycle 418, DIN/ISO: G418) Cycle run Touch Probe Cycle 418 calculates the intersection of the lines connecting opposite holes and sets the datum at the intersection. If desired, the TNC can also enter the intersection into a datum table or preset table.
15 DATUM AT CENTER OF 4 HOLES (Cycle 418, DIN/ISO: G418) 15.12 Please note while programming: Danger of collision! If you set a datum (Q303 = 0) with the touch probe cycle and also use probe in TS axis (Q381 = 1), then no coordinate transformation must be active. Before a cycle definition you must have programmed a tool call to define the touch probe axis.
15 Touch Probe Cycles: Automatic Datum Setting 15.12 DATUM AT CENTER OF 4 HOLES (Cycle 418, DIN/ISO: G418) Cycle parameters 1st hole: Center in 1st axis Q268 (absolute): Center of the first hole in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 1st hole: Center in 2nd axis Q269 (absolute): Center of the first hole in the minor axis of the working plane. Input range -99999.9999 to 99999.
15 DATUM AT CENTER OF 4 HOLES (Cycle 418, DIN/ISO: G418) 15.12 New datum for minor axis Q332 (absolute): Coordinate in the minor axis at which the TNC should set the calculated intersection of the connecting lines. Default setting = 0 input range -99999.9999 to 99999.
15 Touch Probe Cycles: Automatic Datum Setting 15.13 DATUM IN ONE AXIS (Cycle 419, DIN/ISO: G419) 15.13 DATUM IN ONE AXIS (Cycle 419, DIN/ISO: G419) Cycle run Touch Probe Cycle 419 measures any coordinate in any axis and defines it as datum. If desired, the TNC can also enter the measured coordinate in a datum table or preset table.
15 DATUM IN ONE AXIS (Cycle 419, DIN/ISO: G419) 15.13 Cycle parameters 1st meas. point 1st axis Q263 (absolute): Coordinate of the first touch point in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 1st meas. point 2nd axis Q264 (absolute): Coordinate of the first touch point in the minor axis of the working plane. Input range -99999.9999 to 99999.
15 Touch Probe Cycles: Automatic Datum Setting 15.13 DATUM IN ONE AXIS (Cycle 419, DIN/ISO: G419) Traverse direction 1 Q267: Direction in which the probe is to approach the workpiece: -1: Negative Traverse direction +1: Positive traverse direction Datum number in table Q305: Enter the number in the datum or preset table in which the TNC is to save the coordinate. If Q303=1: If you enter Q305=0, the TNC automatically sets the display so that the new datum is on the probed surface.
15 Example: Datum setting in center of a circular segment and on top 15.14 surface of workpiece 15.
15 Touch Probe Cycles: Automatic Datum Setting 15.15 Example: Datum setting on top surface of workpiece and in center of a bolt hole circle 15.15 Example: Datum setting on top surface of workpiece and in center of a bolt hole circle The measured bolt hole center shall be written in the preset table so that it may be used at a later time.
15 Example: Datum setting on top surface of workpiece and in center 15.15 of a bolt hole circle Q303=+1 ;MEAS. VALUE TRANSFER In the preset table PRESET.PR, save the calculated datum referenced to the machine-based coordinate system (REF system) Q381=0 ;PROBE IN TS AXIS Do not set a datum in the touch probe axis Q382=+0 ;1ST CO. FOR TS AXIS No function Q383=+0 ;2ND CO. FOR TS AXIS No function Q384=+0 ;3RD CO.
16 Touch Probe Cycles: Automatic Workpiece Inspection
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.1 Fundamentals 16.1 Fundamentals Overview When running touch probe cycles, Cycle 8 MIRROR IMAGE, Cycle 11 SCALING and Cycle 26 AXISSPECIFIC SCALING must not be active. HEIDENHAIN only warrants the function of the touch probe cycles if HEIDENHAIN touch probes are used. The TNC must be specially prepared by the machine tool builder for the use of a 3-D touch probe. Refer to your machine manual.
16 Fundamentals 16.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.1 Fundamentals Example: Measuring log for touch probe cycle 421: Measuring log for Probing Cycle 421 Hole Measuring Date: 30-06-2005 Time: 6:55:04 Measuring program: TNC:\GEH35712\CHECK1.H Nominal values: Center in reference axis: Center in minor axis: Diameter: 50.0000 65.0000 12.0000 Given limit values: Maximum limit for center in reference axis: 50.1000 Minimum limit for center in reference axis: 49.
16 Fundamentals 16.1 Measurement results in Q parameters The TNC saves the measurement results of the respective touch probe cycle in the globally effective Q parameters Q150 to Q160. Deviations from the nominal value are saved in the parameters Q161 to Q166. Note the table of result parameters listed with every cycle description. During cycle definition the TNC also shows the result parameters for the respective cycle in a help graphic (see figure at upper right).
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.1 Fundamentals Tool monitoring For some cycles for workpiece inspection you can have the TNC perform tool monitoring. The TNC then monitors whether The tool radius should be compensated because of the deviations from the nominal value (values in Q16x). The deviations from the nominal value (values in Q16x) are greater than the tool breakage tolerance. Tool compensation This function works only: If the tool table is active.
16 Fundamentals 16.1 Tool breakage monitoring This function works only: If the tool table is active. If tool monitoring is switched on in the cycle (enter Q330 not equal to 0). If the breakage tolerance RBREAK for the tool number entered in the table is greater than 0 (see also the User's Manual, section 5.2 "Tool Data"). The TNC will output an error message and stop program run if the measured deviation is greater than the breakage tolerance of the tool.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.2 DATUM PLANE (Cycle 0, DIN/ISO: G55) 16.2 DATUM PLANE (Cycle 0, DIN/ISO: G55) Cycle run 1 The touch probe moves at rapid traverse (value from FMAX column) to the starting position 1 programmed in the cycle. 2 Then the touch probe runs the probing process at the probing feed rate (column F). The probing direction is defined in the cycle.
16 POLAR DATUM PLANE (Cycle 1) 16.3 16.3 POLAR DATUM PLANE (Cycle 1) Cycle run Touch Probe Cycle 1 measures any position on the workpiece in any direction. 1 The touch probe moves at rapid traverse (value from FMAX column) to the starting position 1 programmed in the cycle. 2 Then the touch probe runs the probing process at the probing feed rate (column F). During probing the TNC moves simultaneously in two axes (depending on the probing angle).
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.4 MEASURE ANGLE (Cycle 420, DIN/ISO: G420) 16.4 MEASURE ANGLE (Cycle 420, DIN/ISO: G420) Cycle run Touch Probe Cycle 420 measures the angle that any straight surface on the workpiece describes with respect to the reference axis of the working plane. 1 Following the positioning logic, the TNC positions the touch probe at rapid traverse (value from FMAX column) (see "Executing touch probe cycles", page 454) to the programmed touch point 1.
16 MEASURE ANGLE (Cycle 420, DIN/ISO: G420) 16.4 Cycle parameters 1st meas. point 1st axis Q263 (absolute): Coordinate of the first touch point in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 1st meas. point 2nd axis Q264 (absolute): Coordinate of the first touch point in the minor axis of the working plane. Input range -99999.9999 to 99999.9999 2nd meas. point 1st axis Q265 (absolute): Coordinate of the second touch point in the reference axis of the working plane.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.4 MEASURE ANGLE (Cycle 420, DIN/ISO: G420) Measuring log Q281: Define whether the TNC should create a measuring log: 0: Do not create a measuring log 1: Create a measuring log: The TNC saves the log file TCHPR420.TXT as standard in the directory TNC:\. 2: Interrupt program run and output measuring log to the TNC screen. Resume program run with NC Start.
16 MEASURE HOLE (Cycle 421, DIN/ISO: G421) 16.5 16.5 MEASURE HOLE (Cycle 421, DIN/ISO: G421) Cycle run Touch Probe Cycle 421 measures the center and diameter of a hole (or circular pocket). If you define the corresponding tolerance values in the cycle, the TNC makes a nominal-to-actual value comparison and saves the deviation value in system parameters.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.5 MEASURE HOLE (Cycle 421, DIN/ISO: G421) Please note while programming: Before a cycle definition you must have programmed a tool call to define the touch probe axis. The smaller the angle, the less accurately the TNC can calculate the hole dimensions.
16 MEASURE HOLE (Cycle 421, DIN/ISO: G421) 16.5 Cycle parameters Center in 1st axis Q273 (absolute): Center of the hole in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 Center in 2nd axis Q274 (absolute value): Center of the hole in the minor axis of the working plane. Input range -99999.9999 to 99999.9999 Nominal diameter Q262: Enter the diameter of the hole. Input range 0 to 99999.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.5 MEASURE HOLE (Cycle 421, DIN/ISO: G421) Measuring log Q281: Definition of whether TNC should create a measuring log: 0: Create no measuring log 1: Create measuring log: The TNC will save the log file TCHPR421.TXT by default in the directory that also contains the associated NC program. 2: Interrupt the program run and display the measuring log on the TNC screen. Resume program run with NC Start.
16 MEASURE HOLE (Cycle 421, DIN/ISO: G421) 16.5 Reverse tool (0=no/1=yes)? Q498: Only relevant if you have entered a turning tool in parameter Q330 before. For proper monitoring of the turning tool, the TNC requires the exact working condition. Therefore, enter the following: 1: Turning tool is mirrored (rotated by 180°) e.g. by Cycle 800 and parameter Reverse the tool Q498=1 0: Turning tool matches the description of the turning tool table toolturn.trn, no modifications, e.g.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.6 MEASURE HOLE OUTSIDE (Cycle 422, DIN/ISO: G422) 16.6 MEASURE HOLE OUTSIDE (Cycle 422, DIN/ISO: G422) Cycle run Touch Probe Cycle 422 measures the center and diameter of a circular stud. If you define the corresponding tolerance values in the cycle, the TNC makes a nominal-to-actual value comparison and saves the deviation value in system parameters.
16 MEASURE HOLE OUTSIDE (Cycle 422, DIN/ISO: G422) 16.6 Please note while programming: Before a cycle definition you must have programmed a tool call to define the touch probe axis. The smaller the angle, the less accurately the TNC can calculate the dimensions of the stud.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.6 MEASURE HOLE OUTSIDE (Cycle 422, DIN/ISO: G422) Cycle parameters Center in 1st axis Q273 (absolute): Center of the stud in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 Center in 2nd axis Q274 (absolute): Center of the stud in the minor axis of the working plane. Input range -99999.9999 to 99999.9999 Nominal diameter Q262: Enter the diameter of the stud. Input range 0 to 99999.
16 MEASURE HOLE OUTSIDE (Cycle 422, DIN/ISO: G422) 16.6 Tolerance for center 1st axis Q279: Permissible position deviation in the reference axis of the working plane. Input range 0 to 99999.9999 Tolerance for center 2nd axis Q280: Permissible position deviation in the minor axis of the working plane. Input range 0 to 99999.9999 Measuring log Q281: Define whether the TNC should create a measuring log: 0: Do not create a measuring log 1: Create a measuring log: The TNC saves the log file TCHPR422.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.6 MEASURE HOLE OUTSIDE (Cycle 422, DIN/ISO: G422) Reverse tool (0=no/1=yes)? Q498: Only relevant if you have entered a turning tool in parameter Q330 before. For proper monitoring of the turning tool, the TNC requires the exact working condition. Therefore, enter the following: 1: Turning tool is mirrored (rotated by 180°) e.g.
16 MEASURE RECTANGLE INSIDE (Cycle 423, DIN/ISO: G423) 16.7 16.7 MEASURE RECTANGLE INSIDE (Cycle 423, DIN/ISO: G423) Cycle run Touch Probe Cycle 423 finds the center, length and width of a rectangular pocket. If you define the corresponding tolerance values in the cycle, the TNC makes a nominal-to-actual value comparison and saves the deviation value in system parameters.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.7 MEASURE RECTANGLE INSIDE (Cycle 423, DIN/ISO: G423) Cycle parameters Center in 1st axis Q273 (absolute): Center of the pocket in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 Center in 2nd axis Q274 (absolute): Center of the pocket in the minor axis of the working plane. Input range -99999.9999 to 99999.9999 1st side length Q282: Pocket length, parallel to the reference axis of the working plane.
16 MEASURE RECTANGLE INSIDE (Cycle 423, DIN/ISO: G423) 16.7 Measuring log Q281: Define whether the TNC should create a measuring log: 0: Do not create a measuring log 1: Create a measuring log: The TNC saves the log file TCHPR423.TXT as standard in the directory TNC:\. 2: Interrupt program run and output measuring log to the TNC screen. Resume program run with NC Start.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.8 MEASURE RECTANGLE OUTSIDE (Cycle 424, DIN/ISO: G424) 16.8 MEASURE RECTANGLE OUTSIDE (Cycle 424, DIN/ISO: G424) Cycle run Touch Probe Cycle 424 finds the center, length and width of a rectangular stud. If you define the corresponding tolerance values in the cycle, the TNC makes a nominal-to-actual value comparison and saves the deviation value in system parameters.
16 MEASURE RECTANGLE OUTSIDE (Cycle 424, DIN/ISO: G424) 16.8 Cycle parameters Center in 1st axis Q273 (absolute): Center of the stud in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 Center in 2nd axis Q274 (absolute): Center of the stud in the minor axis of the working plane. Input range -99999.9999 to 99999.9999 1st side length Q282: Stud length, parallel to the reference axis of the working plane. Input range 0 to 99999.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.8 MEASURE RECTANGLE OUTSIDE (Cycle 424, DIN/ISO: G424) Tolerance for center 1st axis Q279: Permissible position deviation in the reference axis of the working plane. Input range 0 to 99999.9999 Tolerance for center 2nd axis Q280: Permissible position deviation in the minor axis of the working plane. Input range 0 to 99999.
16 MEASURE INSIDE WIDTH (Cycle 425, DIN/ISO: G425) 16.9 16.9 MEASURE INSIDE WIDTH (Cycle 425, DIN/ISO: G425) Cycle run Touch Probe Cycle 425 measures the position and width of a slot (or pocket). If you define the corresponding tolerance values in the cycle, the TNC makes a nominal-to-actual value comparison and saves the deviation value in a system parameter.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.9 MEASURE INSIDE WIDTH (Cycle 425, DIN/ISO: G425) Cycle parameters Starting point in 1st axis Q328 (absolute): Starting point for probing in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 Starting point in 2nd axis Q329 (absolute): Starting point for probing in the minor axis of the working plane. Input range -99999.9999 to 99999.
16 MEASURE INSIDE WIDTH (Cycle 425, DIN/ISO: G425) 16.9 Tool for monitoring Q330: Definition of whether the TNC is to monitor the tool (see "Tool monitoring", page 538). Enter 0 to 32767.9, optionally the tool name with up to 16 characters 0: Monitoring not active >0: Number or name of the tool the TNC used to perform the operation with. You are able to apply a tool via soft key directly from the tool table. Set-up clearance Q320 (incremental): Additional distance between measuring point and ball tip.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.10 MEASURE RIDGE WIDTH (Cycle 426, DIN/ISO: G426) 16.10 MEASURE RIDGE WIDTH (Cycle 426, DIN/ISO: G426) Cycle run Touch Probe Cycle 426 measures the position and width of a ridge. If you define the corresponding tolerance values in the cycle, the TNC makes a nominal-to-actual value comparison and saves the deviation value in system parameters.
16 MEASURE RIDGE WIDTH (Cycle 426, DIN/ISO: G426) 16.10 Cycle parameters 1st meas. point 1st axis Q263 (absolute): Coordinate of the first touch point in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 1st meas. point 2nd axis Q264 (absolute): Coordinate of the first touch point in the minor axis of the working plane. Input range -99999.9999 to 99999.9999 2nd meas. point 1st axis Q265 (absolute): Coordinate of the second touch point in the reference axis of the working plane.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.10 MEASURE RIDGE WIDTH (Cycle 426, DIN/ISO: G426) PGM stop if tolerance error Q309: Definition of whether in the event of a violation of tolerance limits the TNC is to interrupt program run and output an error message: 0: Do not interrupt program run, do not output an error message 1: Interrupt program run and output an error message Tool for monitoring Q330: Definition of whether the TNC is to monitor the tool (see "Tool monitoring", page 538).
16 MEASURE COORDINATE (Cycle 427, DIN/ISO: G427) 16.11 16.11 MEASURE COORDINATE (Cycle 427, DIN/ISO: G427) Cycle run Touch Probe Cycle 427 finds a coordinate in a selectable axis and saves the value in a system parameter. If you define the corresponding tolerance values in the cycle, the TNC makes a nominal-to-actual value comparison and saves the deviation value in system parameters.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.11 MEASURE COORDINATE (Cycle 427, DIN/ISO: G427) Cycle parameters 1st meas. point 1st axis Q263 (absolute): Coordinate of the first touch point in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 1st meas. point 2nd axis Q264 (absolute): Coordinate of the first touch point in the minor axis of the working plane. Input range -99999.9999 to 99999.
16 MEASURE COORDINATE (Cycle 427, DIN/ISO: G427) 16.11 Maximum limit of size Q288: Maximum permissible measured value. Input range 0 to 99999.9999 Minimum limit of size Q289: Minimum permissible measured value. Input range 0 to 99999.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.12 MEASURE BOLT HOLE CIRCLE (Cycle 430, DIN/ISO: G430) 16.12 MEASURE BOLT HOLE CIRCLE (Cycle 430, DIN/ISO: G430) Cycle run Touch Probe Cycle 430 finds the center and diameter of a bolt hole circle by probing three holes. If you define the corresponding tolerance values in the cycle, the TNC makes a nominal-toactual value comparison and saves the deviation value in system parameters.
16 MEASURE BOLT HOLE CIRCLE (Cycle 430, DIN/ISO: G430) 16.12 Please note while programming: Before a cycle definition you must have programmed a tool call to define the touch probe axis. Cycle 430 only monitors for tool breakage; there is no automatic tool compensation. Cycle parameters Center in 1st axis Q273 (absolute): Bolt hole circle center (nominal value) in the reference axis of the working plane. Input range -99999.9999 to 99999.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.12 MEASURE BOLT HOLE CIRCLE (Cycle 430, DIN/ISO: G430) Tolerance for center 2nd axis Q280: Permissible position deviation in the minor axis of the working plane. Input range 0 to 99999.9999 Measuring log Q281: Define whether the TNC should create a measuring log: 0: Do not create a measuring log 1: Create a measuring log: The TNC saves the log file TCHPR430.TXT as standard in the directory TNC:\.
16 MEASURE PLANE (Cycle 431, DIN/ISO: G431) 16.13 16.13 MEASURE PLANE (Cycle 431, DIN/ ISO: G431) Cycle run Touch Probe Cycle 431 finds the angle of a plane by measuring three points. It saves the measured values in system parameters. 1 Following the positioning logic, the TNC positions the touch probe at rapid traverse (value from FMAX column) (see "Executing touch probe cycles", page 454) to the programmed touch point 1 and measures the first point of the plane.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.13 MEASURE PLANE (Cycle 431, DIN/ISO: G431) Please note while programming: Before a cycle definition you must have programmed a tool call to define the touch probe axis. For the TNC to be able to calculate the angular values, the three measuring points must not be positioned on one straight line. The spatial angles that are needed for tilting the working plane are saved in parameters Q170 – Q172.
16 MEASURE PLANE (Cycle 431, DIN/ISO: G431) 16.13 3rd meas. point 1st axis Q296 (absolute): Coordinate of the third touch point in the reference axis of the working plane. Input range -99999.9999 to 99999.9999 3rd meas. point 2nd axis Q297 (absolute): Coordinate of the third touch point in the minor axis of the working plane. Input range -99999.9999 to 99999.9999 3rd meas. point 3rd axis Q298 (absolute): Coordinate of the third touch point in the touch probe axis. Input range -99999.9999 to 99999.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.14 Programming Examples 16.14 Programming Examples Example: Measuring and reworking a rectangular stud Program sequence Roughing with 0.
16 Programming Examples 16.
16 Touch Probe Cycles: Automatic Workpiece Inspection 16.14 Programming Examples Example: Measuring a rectangular pocket and recording the results 0 BEGIN PGM BSMEAS MM 1 TOOL CALL 1 Z Tool call for touch probe 2 L Z+100 R0 FMAX Retract the touch probe 3 TCH PROBE 423 MEAS. RECTAN.
17 Touch Probe Cycles: Special Functions
17 Touch Probe Cycles: Special Functions 17.1 Fundamentals 17.1 Fundamentals Overview When running touch probe cycles, Cycle 8 MIRROR IMAGE, Cycle 11 SCALING and Cycle 26 AXISSPECIFIC SCALING must not be active. HEIDENHAIN grants a warranty for the function of the touch probe cycles only if HEIDENHAIN touch probes are used. The TNC must be specially prepared by the machine tool builder for the use of a 3-D touch probe.
17 MEASURE (Cycle 3) 17.2 17.2 MEASURE (Cycle 3) Cycle run Touch Probe Cycle 3 measures any position on the workpiece in a selectable direction. Unlike other measuring cycles, Cycle 3 enables you to enter the measuring range SET UP and feed rate F directly. Also, the touch probe retracts by a definable value after determining the measured value MB. 1 The touch probe moves from the current position at the entered feed rate in the defined probing direction.
17 Touch Probe Cycles: Special Functions 17.2 MEASURE (Cycle 3) Cycle parameters Parameter number for result: Enter the number of the Q parameter to which you want the TNC to assign the first measured coordinate (X). The values Y and Z are in the immediately following Q parameters. Input range: 0 to 1999 Probing axis: Enter the axis in whose direction the probe is to move and confirm with the ENT key.
17 MEASURING IN 3-D (Cycle 4) 17.3 17.3 MEASURING IN 3-D (Cycle 4) Cycle run Cycle 4 is an auxiliary cycle that can be used for probing with any touch probe (TS, TT or TL). The TNC does not provide a cycle for calibrating the TS touch probe in any probing direction. Touch probe cycle 4 measures any position on the workpiece in the probing direction defined by a vector. Unlike other measuring cycles, Cycle 4 enables you to enter the measuring distance and feed rate directly.
17 Touch Probe Cycles: Special Functions 17.3 MEASURING IN 3-D (Cycle 4) Cycle parameters Parameter number for result: Enter the number of the Q parameter to which you want the TNC to assign the first measured coordinate (X). The values Y and Z are in the immediately following Q parameters. Input range: 0 to 1999 Relative measuring path in X: X component of the direction vector defining the direction in which the touch probe is to move. Input range -99999.9999 to 99999.
17 Calibrating a touch trigger probe 17.4 17.4 Calibrating a touch trigger probe In order to precisely specify the actual trigger point of a 3-D touch probe, you must calibrate the touch probe, otherwise the TNC cannot provide precise measuring results.
17 Touch Probe Cycles: Special Functions 17.5 17.5 Displaying calibration values Displaying calibration values The TNC saves the effective length and effective radius of the touch probe in the tool table. The TNC saves the ball-tip center offset of the touch probe in the touch-probe table in the CAL_OF1 (principal axis) and CAL_OF2 (secondary axis) columns. You can display the values on the screen by pressing the TOUCH PROBE TABLE soft key. A measuring log is created automatically during calibration.
17 CALIBRATE TS (Cycle 460, DIN/ISO: G460) 17.6 17.6 CALIBRATE TS (Cycle 460, DIN/ISO: G460) With Cycle 460 you can calibrate a triggering 3-D touch probe automatically on an exact calibration sphere. You can do radius calibration alone, or radius and length calibration. A measuring log is created automatically during calibration. The log file is named TCHPRAUTO.html. This file is stored in the same location as the original file. The measuring log can be displayed in the browser on the control.
17 Touch Probe Cycles: Special Functions 17.6 CALIBRATE TS (Cycle 460, DIN/ISO: G460) Exact calibration sphere radius Q407: Enter the exact radius of the calibration sphere used. Input range 0.0001 to 99.9999 Set-up clearance Q320 (incremental): Additional distance between measuring point and ball tip. Q320 is added to SET_UP in the touch probe table. Input range 0 to 99999.
17 CALIBRATE TS LENGTH (Cycle 461, DIN/ISO: G461) 17.7 17.7 CALIBRATE TS LENGTH (Cycle 461, DIN/ISO: G461) Cycle run Before starting the calibration cycle, you must set the datum in the spindle axis so that Z=0 on the machine table; you must also preposition the touch probe over the calibration ring. A measuring log is created automatically during calibration. The log file is named TCHPRAUTO.html. This file is stored in the same location as the original file.
17 Touch Probe Cycles: Special Functions 17.7 CALIBRATE TS LENGTH (Cycle 461, DIN/ISO: G461) Please note while programming: HEIDENHAIN only warrants the function of the touch probe cycles if HEIDENHAIN touch probes are used. The effective length of the touch probe is always referenced to the tool datum. The machine tool builder usually defines the spindle tip as the tool datum. Before a cycle definition you must have programmed a tool call to define the touch probe axis.
17 CALIBRATE TS RADIUS INSIDE (Cycle 462, DIN/ISO: G462) 17.8 17.8 CALIBRATE TS RADIUS INSIDE (Cycle 462, DIN/ISO: G462) Cycle run Before starting the calibration cycle, you need to preposition the touch probe in the center of the calibration ring and at the required measuring height. When calibrating the ball tip radius, the TNC executes an automatic probing routine.
17 Touch Probe Cycles: Special Functions 17.8 CALIBRATE TS RADIUS INSIDE (Cycle 462, DIN/ISO: G462) Please note while programming: HEIDENHAIN only warrants the function of the touch probe cycles if HEIDENHAIN touch probes are used. Before a cycle definition you must have programmed a tool call to define the touch probe axis. The center offset can be determined only with a suitable touch probe. A measuring log is created automatically during calibration. The log file is named TCHPRAUTO.html.
17 CALIBRATE TS RADIUS OUTSIDE (Cycle 463, DIN/ISO: G463) 17.9 17.9 CALIBRATE TS RADIUS OUTSIDE (Cycle 463, DIN/ISO: G463) Cycle run Before starting the calibration cycle, you need to preposition the touch probe above the center of the calibration pin. Position the touch probe in the touch probe axis by approximately the set-up clearance (value from touch probe table + value from cycle) above the calibration pin. When calibrating the ball tip radius, the TNC executes an automatic probing routine.
17 Touch Probe Cycles: Special Functions 17.9 CALIBRATE TS RADIUS OUTSIDE (Cycle 463, DIN/ISO: G463) Please note while programming: HEIDENHAIN only warrants the function of the touch probe cycles if HEIDENHAIN touch probes are used. Before a cycle definition you must have programmed a tool call to define the touch probe axis. The center offset can be determined only with a suitable touch probe. A measuring log is created automatically during calibration. The log file is named TCHPRAUTO.html.
18 Visual Setup Control VSC (software option 136)
18 Visual Setup Control VSC (software option 136) 18.1 Camera-based monitoring of the setup situation VSC (option number136) 18.
18 Camera-based monitoring of the setup situation VSC (option 18.1 number136) Term Explanation Error If you take a picture that shows a poor situation (e.g.workpiece wrongly clamped), you can create what is known as an error image. It is not advisable to highlight an error image as a reference image. Monitoring area Denotes an area that you highlight with the mouse. When evaluating new images, the control only refers to this area.
18 Visual Setup Control VSC (software option 136) 18.1 Camera-based monitoring of the setup situation VSC (option number136) Produce live image In the Manual operation mode, you can display and save the current camera view as a live image. The control only uses the picture taken here for automatic monitoring of the setup situation. Images produced in this menu may be used for documentation and traceability. For example, you could record the current setup situation.
18 Camera-based monitoring of the setup situation VSC (option 18.1 number136) Manage monitoring data In the Manual operation mode you can manage images from cycles 600 and 601.
18 Visual Setup Control VSC (software option 136) 18.1 Camera-based monitoring of the setup situation VSC (option number136) Features of the monitoring data management Soft key Function Mark selected image as a reference image Please note: A reference image shows a situation in the working space that you regard as safe. All reference images are used as part of the evaluation process. If you add or remove an image as a reference image, this has an effect on the results of image evaluation.
18 Camera-based monitoring of the setup situation VSC (option 18.1 number136) Overview The TNC provides two cycles you can use for visual setup control in the Programming mode of operation: The soft-key row shows all available touch probe functions divided into groups.
18 Visual Setup Control VSC (software option 136) 18.1 Camera-based monitoring of the setup situation VSC (option number136) Results of the image evaluation The results of the image evaluation depend on the monitoring area and the reference images. When evaluating all images, each image is evaluated according to the current configuration and the results are compared with the data last saved.
18 Camera-based monitoring of the setup situation VSC (option 18.1 number136) You are able to click on the image and draw up a rectangular frame. This way you define the monitoring area. (More information, see "Fundamentals", page 596.) If you define monitoring areas in a setting that is always exposed or in which differences in contrast are to be expected, false alerts will be displayed.
18 Visual Setup Control VSC (software option 136) 18.1 Camera-based monitoring of the setup situation VSC (option number136) Defining the monitoring area The monitoring area is defined with the modes of operation Single Block or Block Scan. The TNC will prompt you to define a monitoring area. The TNC will display this prompt on the screen after you have started the cycle for the first time in the modes of operation Single Block or Block Scan.
18 Camera-based monitoring of the setup situation VSC (option 18.1 number136) Possible queries The cycles of the workspace monitoring enter a value in parameter Q601. The following values are possible: Q601 = 1: No error Q601 = 2: Error Q601 = 3: You have yet not defined a monitoring area or you did not save enough reference images Q601 = 10: Internal error (no signal, faulty camera, etc.) You can use parameter Q601 for internal queries.
18 Visual Setup Control VSC (software option 136) 18.2 Workspace Global (Cycle 600) 18.2 Workspace Global (Cycle 600) Application With Cycle 600, Workspace Global, you monitor the workspace of your tooling machine. The TNC will generate an image of the current workspace from a position determined by your machine tool builder. Then, the TNC will match the image with previously generated reference images and enforce a program stop, if required.
18 Workspace Global (Cycle 600) 18.2 The TNC will save the current image and return to the program run screen. If you changed the configuration, the TNC will perform an image evaluation. (More information, "Results of the image evaluation") The status display at the top right displays the word "Reference". You have marked the current image as the reference image. Because a reference image can never be an error image at the same time, the soft key ERROR IMAGE is gray.
18 Visual Setup Control VSC (software option 136) 18.2 Workspace Global (Cycle 600) Defining the monitoring area The monitoring area is defined with the modes of operation Single Block or Block Scan. The TNC will prompt you to define a monitoring area. The TNC will display this prompt on the screen after you have started the cycle for the first time in the modes of operation Single Block or Block Scan. A monitoring area consists of one or more windows that you draw with your mouse.
18 Workspace Global (Cycle 600) 18.2 Monitoring phase Cycle run: Monitoring phase 1 The camera will be mounted by the machine tool builder onto the main spindle. The main spindle moves to a position defined by the machine tool builder. 2 After the TNC has reached this position, it will automatically open the camera lid. 3 The TNC will generate an image of the current condition. 4 Then it will match the image against the mean value and the variance image (more information, see "Fundamentals", page 596).
18 Visual Setup Control VSC (software option 136) 18.2 Workspace Global (Cycle 600) Danger of contaminating the camera due to open camera lid with parameter Q613. This could lead to blurred images, the camera may be damaged. Close the camera lid before continuing with the process. Danger of collision during automatic positioning of the camera. The camera and your machine may be damaged. Consult your machine tool builder, at which point the TNC will preposition the camera.
18 Workspace Local (Cycle 601) 18.3 18.3 Workspace Local (Cycle 601) Application With Cycle 601, Workspace Local, you monitor the workspace of your tooling machine. The TNC will generate an image of the current workspace from the position of the spindle at the point in time of the cycle call. Then, the TNC will match the image against previously generated reference images and enforce a program stop, if required.
18 Visual Setup Control VSC (software option 136) 18.3 Workspace Local (Cycle 601) The TNC will save the current image and return to the program run screen. If you changed the configuration, the TNC will perform an image evaluation. (More information, "Results of the image evaluation") The status display at the top right displays the word "Reference". You have marked the current image as the reference image.
18 Workspace Local (Cycle 601) 18.3 Defining the monitoring area The monitoring area is defined with the modes of operation Single Block or Block Scan. The TNC will prompt you to define a monitoring area. The TNC will display this prompt on the screen after you have started the cycle for the first time in the modes of operation Single Block or Block Scan. A monitoring area consists of one or more windows that you draw with your mouse. The TNC will only scan these areas of the image.
18 Visual Setup Control VSC (software option 136) 18.3 Workspace Local (Cycle 601) Monitoring phase The monitoring phase starts as soon as the TNC has generated enough reference images. Cycle run: Monitoring phase 1 The camera will be mounted by the machine tool builder onto the main spindle. 2 The TNC automatically opens the camera lid. 3 The TNC will generate an image of the current condition.
18 Workspace Local (Cycle 601) 18.3 Danger of contaminating the camera due to open camera lid with parameter Q613. This could lead to blurred images, the camera may be damaged. Close the camera lid before continuing with the process! Cycle parameters Monitoring point QS600 (string parameter): Enter the name of your monitoring file PGM stop if error Q309: (0/1) Definition of whether the TNC will stop the program after detecting an error. 0: Program will not stop after detecting an error.
19 Touch Probe Cycles: Automatic Kinematics Measurement
19 Touch Probe Cycles: Automatic Kinematics Measurement 19.1 Kinematics Measurement with TS Touch Probes (KinematicsOpt option) 19.1 Kinematics Measurement with TS Touch Probes (KinematicsOpt option) Fundamentals Accuracy requirements are becoming increasingly stringent, particularly in the area of 5-axis machining. Complex parts need to be manufactured with precision and reproducible accuracy even over long periods.
19 Kinematics Measurement with TS Touch Probes (KinematicsOpt 19.
19 Touch Probe Cycles: Automatic Kinematics Measurement 19.2 Prerequisites 19.2 Prerequisites The following are prerequisites for using the KinematicsOpt option: The software options 48 (KinematicsOpt), 8 (Software option 1) and 17 (Touch Probe function) must be enabled. The 3-D touch probe used for the measurement must be calibrated. The cycles can only be carried out with the tool axis Z.
19 SAVE KINEMATICS (Cycle 450, DIN/ISO: G450, option) 19.3 19.3 SAVE KINEMATICS (Cycle 450, DIN/ISO: G450, option) Cycle run With the touch probe cycle 450 you can save the active machine kinematic configuration or restore a previously saved one. The saved data can be displayed and deleted. 16 memory spaces in total are available. Please note while programming: Always save the active kinematics configuration before running a kinematics optimization.
19 Touch Probe Cycles: Automatic Kinematics Measurement 19.3 SAVE KINEMATICS (Cycle 450, DIN/ISO: G450, option) Cycle parameters Mode (0/1/2/3) Q410: Define if you wish to backup or restore the kinematics: 0: Backup active kinematics 1: Restore saved kinematics 2: Display current memory status 3: Delete a data record Memory designation Q409/QS409: Number or name of the data block designator. For a number, enter a value from 0 to 99999; for a name, enter a maximum of 16 characters.
19 SAVE KINEMATICS (Cycle 450, DIN/ISO: G450, option) 19.3 Notes on data management The TNC stores the saved data in the file TNC:\table\DATA450.KD. This file can be backed up on an external PC with TNCREMO, for example. If the file is deleted, the stored data are removed, too. If the data in the file are changed manually, the data records can become corrupted so that they cannot be used anymore. If the TNC:\table\DATA450.KD file does not exist, it is generated automatically when Cycle 450 is executed.
19 Touch Probe Cycles: Automatic Kinematics Measurement 19.4 MEASURE KINEMATICS (Cycle 451, DIN/ISO: G451, option) 19.4 MEASURE KINEMATICS (Cycle 451, DIN/ISO: G451, option) Cycle run The touch probe cycle 451 enables you to check and, if required, optimize the kinematics of your machine. Use the 3-D TS touch probe to measure a HEIDENHAIN calibration sphere that you have attached to the machine table.
19 MEASURE KINEMATICS (Cycle 451, DIN/ISO: G451, option) 19.
19 Touch Probe Cycles: Automatic Kinematics Measurement 19.4 MEASURE KINEMATICS (Cycle 451, DIN/ISO: G451, option) Positioning direction The positioning direction of the rotary axis to be measured is determined from the start angle and the end angle that you define in the cycle. A reference measurement is automatically performed at 0°. Specify the start and end angles to ensure that the same position is not measured twice. A duplicated point measurement (e.g.
19 MEASURE KINEMATICS (Cycle 451, DIN/ISO: G451, option) 19.4 Machines with Hirth-coupled axes Danger of collision! In order to be positioned, the axis must move out of the Hirth grid. So remember to leave a large enough safety clearance to prevent any risk of collision between the touch probe and calibration sphere. Also ensure that there is enough space to reach the safety clearance (software limit switch).
19 Touch Probe Cycles: Automatic Kinematics Measurement 19.4 MEASURE KINEMATICS (Cycle 451, DIN/ISO: G451, option) Choice of number of measuring points To save time you can make a rough optimization with a small number of measuring points (1 or 2), for example during commissioning. You then make a fine optimization with a medium number of measuring points (recommended value = approx. 4). Higher numbers of measuring points do not usually improve the results.
19 MEASURE KINEMATICS (Cycle 451, DIN/ISO: G451, option) 19.4 Choice of the calibration sphere position on the machine table In principle, you can fix the calibration sphere to any accessible position on the machine table and also on fixtures or workpieces. The following factors should positively influence the result of measurement: On machine with rotary tables/tilting tables: Clamp the calibrating ball as far as possible away from the center of rotation.
19 Touch Probe Cycles: Automatic Kinematics Measurement 19.4 MEASURE KINEMATICS (Cycle 451, DIN/ISO: G451, option) Notes on various calibration methods Rough optimization during commissioning after entering approximate dimensions. Number of measuring points between 1 and 2 Angular step of the rotary axes: Approx. 90° Fine optimization over the entire range of traverse Number of measuring points between 3 and 6 The start and end angles should cover the largest possible traverse range of the rotary axes.
19 MEASURE KINEMATICS (Cycle 451, DIN/ISO: G451, option) 19.4 Backlash Backlash is a small amount of play between the rotary or angle encoder and the table that occurs when the traverse direction is reversed. If the rotary axes have backlash outside of the control loop, for example because the angle measurement is made with the motor encoder, this can result in significant error during tilting. With input parameter Q432 you can activate backlash measurement.
19 Touch Probe Cycles: Automatic Kinematics Measurement 19.4 MEASURE KINEMATICS (Cycle 451, DIN/ISO: G451, option) Please note while programming: Note that all functions for tilting in the working plane are reset. M128 and FUNCTION TCPM are deactivated. Position the calibration sphere on the machine table so that there can be no collisions during the measuring process.
19 MEASURE KINEMATICS (Cycle 451, DIN/ISO: G451, option) 19.4 Cycle parameters Mode (0=Check/1=Measure) Q406: Specify whether the TNC should check or optimize the active kinematics: 0: Check active kinematics. The TNC measures the kinematics in the rotary axes you have defined, but it does not make any changes to it. The TNC displays the results of measurement in a measurement log. 1: Optimize active kinematics.
19 Touch Probe Cycles: Automatic Kinematics Measurement 19.4 MEASURE KINEMATICS (Cycle 451, DIN/ISO: G451, option) Reference angle Q380 (absolute): Reference angle (basic rotation) for measuring the measuring points in the active workpiece coordinate system. Defining a reference angle can considerably enlarge the measuring range of an axis. Input range 0 to 360.0000 Start angle A axis Q411 (absolute): Starting angle in the A axis at which the first measurement is to be made. Input range -359.999 to 359.
19 MEASURE KINEMATICS (Cycle 451, DIN/ISO: G451, option) 19.4 Number meas. points (3-8) Q423: Number of probe measurements with which the TNC is to measure the calibration sphere in the plane. Input range 3 to 8. Less measuring points increase speed and more measuring points increase measurement precision.
19 Touch Probe Cycles: Automatic Kinematics Measurement 19.4 MEASURE KINEMATICS (Cycle 451, DIN/ISO: G451, option) Various modes (Q406) Test mode Q406 = 0 The TNC measures the rotary axes in the positions defined and calculates the static accuracy of the tilting transformation. The TNC records the results of a possible position optimization but does not make any adjustments.
19 MEASURE KINEMATICS (Cycle 451, DIN/ISO: G451, option) 19.4 Logging function After running Cycle 451, the TNC creates a measuring log (TCHPR451.
19 Touch Probe Cycles: Automatic Kinematics Measurement 19.5 PRESET COMPENSATION (Cycle 452, DIN/ISO: G452, option) 19.5 PRESET COMPENSATION (Cycle 452, DIN/ISO: G452, option) Cycle run Touch probe cycle 452 optimizes the kinematic transformation chain of your machine (see "MEASURE KINEMATICS (Cycle 451, DIN/ISO: G451, option)", page 624).
19 PRESET COMPENSATION (Cycle 452, DIN/ISO: G452, option) 19.
19 Touch Probe Cycles: Automatic Kinematics Measurement 19.5 PRESET COMPENSATION (Cycle 452, DIN/ISO: G452, option) Please note while programming: In order to be able to perform a preset compensation, the kinematics must be specially prepared. The machine manual provides further information. Note that all functions for tilting in the working plane are reset. M128 and FUNCTION TCPM are deactivated.
19 PRESET COMPENSATION (Cycle 452, DIN/ISO: G452, option) 19.5 Cycle parameters Exact calibration sphere radius Q407: Enter the exact radius of the calibration sphere used. Input range 0.0001 to 99.9999 Set-up clearance Q320 (incremental): Additional distance between measuring point and ball tip. Q320 is added to SET_UP. Input range 0 to 99999.9999; alternatively PREDEF Retraction height Q408 (absolute): Input range 0.0001 to 99999.9999 Input 0: Do not move to any retraction height.
19 Touch Probe Cycles: Automatic Kinematics Measurement 19.5 PRESET COMPENSATION (Cycle 452, DIN/ISO: G452, option) Angle of incid. in B axis Q417: Angle of incidence in the B axis at which the other rotary axes are to be measured. Input range -359.999 to 359.999 Number meas. points B axis Q418: Number of probe measurements with which the TNC is to measure the B axis. If the input value = 0, the TNC does not measure the respective axis.
19 PRESET COMPENSATION (Cycle 452, DIN/ISO: G452, option) 19.5 Adjustment of interchangeable heads The goal of this procedure is for the workpiece preset to remain unchanged after changing rotary axes (head exchange). In the following example, a fork head is adjusted to the A and C axes. The A axis is changed, whereas the C axis continues being a part of the basic configuration. Insert the interchangeable head that will be used as a reference head.
19 Touch Probe Cycles: Automatic Kinematics Measurement 19.
19 PRESET COMPENSATION (Cycle 452, DIN/ISO: G452, option) 19.5 Drift compensation During machining various machine components are subject to drift due to varying ambient conditions. If the drift remains sufficiently constant over the range of traverse, and if the calibration sphere can be left on the machine table during machining, the drift can be measured and compensated with Cycle 452.
19 Touch Probe Cycles: Automatic Kinematics Measurement 19.5 PRESET COMPENSATION (Cycle 452, DIN/ISO: G452, option) Measure the drift of the axes at regular intervals. Insert the touch probe Activate the preset in the calibration sphere. Use Cycle 452 to measure the kinematics. The preset and the position of the calibration sphere must not be changed during the complete process This procedure can also be performed on machines without rotary axes.
19 PRESET COMPENSATION (Cycle 452, DIN/ISO: G452, option) 19.5 Logging function After running Cycle 452, the TNC creates a measuring log (TCHPR452.
20 Touch Probe Cycles: Automatic Tool Measurement
20 Touch Probe Cycles: Automatic Tool Measurement 20.1 Fundamentals 20.1 Fundamentals Overview When running touch probe cycles, Cycle 8 MIRROR IMAGE, Cycle 11 SCALING and Cycle 26 AXISSPECIFIC SCALING must not be active. HEIDENHAIN only gives warranty for the function of the probing cycles if HEIDENHAIN touch probes are used. The TNC and the machine tool must be set up by the machine tool builder for use of the TT touch probe. Some cycles and functions may not be provided on your machine tool.
20 Fundamentals 20.1 You can program the cycles for tool measurement in the Programming mode of operation using the TOUCH PROBE key.
20 Touch Probe Cycles: Automatic Tool Measurement 20.1 Fundamentals Setting machine parameters Before you start working with the measuring cycles, check all machine parameters defined in ProbeSettings > CfgToolMeasurement and CfgTTRoundStylus. The TNC uses the feed rate for probing defined in probingFeed when measuring a tool at standstill. When measuring a rotating tool, the TNC automatically calculates the spindle speed and feed rate for probing.
20 Fundamentals 20.1 probingFeedCalc determines the calculation of the probing feed rate: probingFeedCalc = ConstantTolerance: The measuring tolerance remains constant regardless of the tool radius. With very large tools, however, the feed rate for probing is reduced to zero. The smaller you set the maximum permissible rotational speed (maxPeriphSpeedMeas) and the permissible tolerance (measureTolerance1), the sooner you will encounter this effect.
20 Touch Probe Cycles: Automatic Tool Measurement 20.1 Fundamentals Entries in the tool table TOOL.T Abbr. Inputs Dialog CUT Number of teeth (20 teeth maximum) Number of teeth? LTOL Permissible deviation from tool length L for wear detection. If the entered value is exceeded, the TNC locks the tool (status L). Input range: 0 to 0.9999 mm Wear tolerance: length? RTOL Permissible deviation from tool radius R for wear detection. If the entered value is exceeded, the TNC locks the tool (status L).
20 Fundamentals 20.1 Input examples for common tool types Tool type CUT TT:R_OFFS Drill – (no function) 0 (no offset required because tool tip is to be measured) End mill with diameter of < 19 mm 4 (4 teeth) 0 (no offset required because tool diameter is smaller than the contact plate diameter of the TT) 0 (no additional offset required during radius measurement.
20 Touch Probe Cycles: Automatic Tool Measurement 20.2 Calibrate the TT (Cycle 480,) 20.2 Calibrate the TT (Cycle 30 or 480, DIN/ISO: G480 Option 17) Cycle run The TT is calibrated with the measuring cycle TCH PROBE 30 or TCH PROBE 480 (see "Differences between Cycles 31 to 33 and Cycles 481 to 483", page 651). The calibration process is automatic.
20 Calibrating the wireless TT 449 (Cycle 484, DIN/ISO: G484) 20.3 20.3 Calibrating the wireless TT 449 (Cycle 484, DIN/ISO: G484, DIN/ISO: G484) Fundamentals With Cycle 484, you can calibrate your tool touch probe, e.g the wireless infrared TT 449 tool touch probe. The calibration process is either fully automatic or semi-automatic, depending on the parameter setting.
20 Touch Probe Cycles: Automatic Tool Measurement 20.3 Calibrating the wireless TT 449 (Cycle 484, DIN/ISO: G484) Please note while programming: Danger of collision! To avoid collisions, the tool must be pre-positioned before the cycle call if Q536 is set to 1! In the calibration process, the TNC also measures the center misalignment of the calibrating tool by rotating the spindle by 180° after the first half of the calibration cycle.
20 Measuring tool length (Cycle 481) 20.4 20.4 Measuring tool length (Cycle 31 or 481, DIN/ISO: G481) Cycle run In order to measure the tool length program the measurement cycles TCH PROBE 31 or TCH PROBE 481 (see "Differences between Cycles 31 to 33 and Cycles 481 to 483"). Via input parameters you can measure the length of a tool by three methods: If the tool diameter is larger than the diameter of the measuring surface of the TT, you measure the tool while it is rotating.
20 Touch Probe Cycles: Automatic Tool Measurement 20.4 Measuring tool length (Cycle 481) Please note while programming: Before measuring a tool for the first time, enter the following data on the tool into the tool table TOOL.T: the approximate radius, the approximate length, the number of teeth, and the cutting direction. You can run an individual tooth measurement of tools with up to 20 teeth.
20 Measuring tool radius (Cycle 482) 20.5 20.5 Measuring tool radius (Cycle 32 or 482, DIN/ISO: G482) Cycle run To measure the tool radius, program the measuring cycle TCH PROBE 32 or TCH PROBE 482 (see "Differences between Cycles 31 to 33 and Cycles 481 to 483", page 651). Select via input parameters by which of two methods the radius of a tool is to be measured: Measuring the tool while it is rotating Measuring the tool while it is rotating and subsequently measuring the individual teeth.
20 Touch Probe Cycles: Automatic Tool Measurement 20.5 Measuring tool radius (Cycle 482) Cycle parameters Measure tool=0 / Check tool=1: Select whether the tool is to be measured for the first time or whether a tool that has already been measured is to be inspected. If the tool is being measured for the first time, the TNC overwrites the tool radius R in the central tool file TOOL.T by the delta value DR = 0.
20 Measuring tool length and radius (Cycle 483) 20.6 20.6 Measuring tool length and radius (Cycle 33 or 483, DIN/ISO: G483) Cycle run To measure both the length and radius of a tool, program the measuring cycle TCH PROBE 33 or TCH PROBE 483 (see "Differences between Cycles 31 to 33 and Cycles 481 to 483", page 651). This cycle is particularly suitable for the first measurement of tools, as it saves time when compared with individual measurement of length and radius.
20 Touch Probe Cycles: Automatic Tool Measurement 20.6 Measuring tool length and radius (Cycle 483) Cycle parameters Measure tool=0 / Check tool=1: Select whether the tool is to be measured for the first time or whether a tool that has already been measured is to be inspected. If the tool is being measured for the first time, the TNC overwrites the tool radius R and the tool length L in the central tool file TOOL.T by the delta values DR = 0 and DL = 0.
21 Tables of Cycles
21 Tables of Cycles 21.1 Overview 21.
21 Overview 21.
21 Tables of Cycles 21.
21 Overview 21.
21 Tables of Cycles 21.
Index 3 3D Touch Probes...................... 448 3-D touch probes....................... 52 A Adapt rotary coordinate system..................................... 332 Automatic datum setting.......... 480 At center of 4 holes............... 522 Center of a bolt hole circle..... 516 Center of a circular pocket (hole)...................................... 498 Center of a circular stud......... 503 Center of a rectangular pocket.................................... 491 Center of a rectangular stud...
Index S Scaling...................................... 274 Set a basic rotation.................. 472 Side finishing............................ 213 Single-lip deep-hole drilling......... 99 SL Cycles................. 196, 231, 240 Contour cycle......................... 198 Contour data.......................... 203 Contour train.................. 216, 218 Floor finishing......................... 211 SL cycles Fundamentals......................... 196 Fundamentals.........................
