Heidenhain TNC 640: Touch-Probe Cycles

The TNC 640 ships its probing as built-in TCH PROBE cycles — no Renishaw macro pack, no G65 argument lists. Workpiece probes (TS series, spindle-mounted) get cycles for alignment, presetting, and inspection in two generations: the classic 4xx set and the newer 14xx set, which adds tolerance parsing and semi-automatic setup. Tool probes (TT, table-mounted) get the 48x measurement cycles. Every cycle drops its results into fixed, globally effective Q parameters. This reference is verified against the TNC 640 measuring-cycles manual for NC software 34059x-18 — cycle inventories differ between Heidenhain series and firmware levels.

How TNC Probing Differs from Fanuc-Style G65 Macros

On a Fanuc or Haas you call vendor macros (G65 P9810 X.. Y..) with letter arguments and read #135-series results. On the TNC 640:

• Cycles are part of the control. Press the TOUCH PROBE key in Programming mode, pick the group, and the control walks you through a dialog with a help graphic highlighting each parameter.
• Parameters are named Q numbers, consistent across cycles: Q260 is always clearance height, Q261 measuring height, Q320 set-up clearance.
• Touch-probe cycles are DEF-active: they execute the moment the control reads the definition. There is no CYCL CALL and no M99 — a big difference from machining cycles and from G65 habits.
• Results land in fixed global Q parameters (Q150–Q199 for 4xx, Q950–Q997 for 14xx) and in an HTML log (TCHPRAUTO.html in automatic mode, TCHPRMAN.html for manual probing).
• The probe is a tool: it needs a tool-table row plus a matching row in the touch-probe table (both numbers must agree), and a TOOL CALL defining the probe axis must precede the cycle definition.

Behavior common to all cycles: the probe approaches paraxially (even under a basic rotation or tilted plane), stops at stylus deflection, stores the trigger point, and retracts at rapid. No trigger within the DIST distance from the touch-probe table → error message. Pre-positioning distance = ball radius + SET_UP (touch-probe table) + Q320 from the cycle; positioning logic pivots on Q260 CLEARANCE HEIGHT. Probing feed is column F, positioning feed FMAX, and F_PREPOS selects true rapid vs FMAX. TRACK = ON orients an infrared probe to the probing direction before each touch (recalibrate after changing it).

Manual Probing Functions

In Manual Operation and Electronic Handwheel modes the probing soft keys offer: probe calibration, a 3-D basic rotation via plane probing, a basic rotation via a line, preset on any axis, corner as preset, circle center as preset, centerline as preset, plus touch-probe data management. Measured values can be written straight to the preset table (or a datum table). Notes from the Setup manual: in Turning mode all manual functions work except Probe in plane and Intersection probing (X values read as diameters, and the probe must be calibrated separately for turning); with no probe inserted you can still capture actual position with NC Start. The machine parameter chkTiltingAxes decides whether the control verifies that rotary-axis positions match the active 3D-ROT angles when presetting — unset, it checks always.

Calibrating the Workpiece Probe (TS)

Calibration determines the effective stylus length (referenced to the tool reference point, usually the spindle nose) and effective ball radius; length/radius go to the tool table, center offset to columns CAL_OF1/CAL_OF2 of the touch-probe table. Recalibrate after commissioning, a broken or swapped stylus, a change of probing feed rate, thermal drift, or a change of active tool axis. Calibration values apply immediately — no new tool call needed. L-shaped styli (L-TYPE, supported by cycles 444 and 14xx) should be calibrated with 460 (radius) and 461 (length) at the same feed rate used for probing.

Workpiece Cycles I — Measuring Misalignment (Rotation)

Two generations coexist on this firmware. The 14xx cycles know the machine kinematics, accept nominal dimensions with tolerances (e.g. 10H7, 10+0.01-0.015), support 3-D calibration data, and can measure rotation and position simultaneously; compensation can go into the preset table as basic rotation or as a rotary-axis offset (Q1126 ALIGN ROTARY AXIS, Q1121 CONFIRM ROTATION).

Semi-automatic mode (14xx only)

If you don’t know where the part sits, program nominal positions as strings with a leading ? — the control stops, lets you jog the probe near the feature, and takes it from there. Manual example, edge alignment with unknown positions:

11 TCH PROBE 1410 PROBING ON EDGE ~
QS1100= "?"    ;1ST POINT REF AXIS ~     ; unknown - jog to it
QS1101= "?0"   ;1ST POINT MINOR AXIS ~   ; nominal 0, workpiece position unknown
QS1102= "?"    ;1ST POINT TOOL AXIS ~
QS1103= "?"    ;2ND POINT REF AXIS ~
QS1104= "?0"   ;2ND POINT MINOR AXIS ~
QS1105= "?"    ;2ND POINT TOOL AXIS ~
Q372=+2        ;PROBING DIRECTION ~      ; Y+
Q320=+0        ;SET-UP CLEARANCE ~
Q260=+100      ;CLEARANCE HEIGHT ~
Q1125=+2       ;CLEAR. HEIGHT MODE ~
Q309=+0        ;ERROR REACTION ~         ; 0 no stop, 1 stop on rework/scrap, 2 stop on scrap
Q1126=+0       ;ALIGN ROTARY AXIS ~
Q1120=+0       ;TRANSER POSITION ~
Q1121=+0       ;CONFIRM ROTATION

Workpiece Cycles II — Presetting

Where the calculated preset goes is controlled by Q303 (MEAS. VALUE TRANSFER) and Q305 (NUMBER IN TABLE) in every 4xx presetting cycle:

Workpiece Cycles III — Inspection (Measuring)

The 42x cycles measure a feature, compare against nominal limits you define, optionally write a log (Q281: 0 none, 1 file, 2 screen/stop), optionally stop the program out of tolerance (Q309), and optionally correct the tool that cut the feature (Q330, see below).

Tool monitoring (Q330): reference the milling tool by number or name and the control writes the measured deviation into that tool’s DR column — always, even inside tolerance — and checks it against RBREAK for breakage (tool locked, TL = L, program stops). Q181 tells your program whether rework is needed. For an indexed tool by name, the manual’s recipe: QS0 = "TOOL NAME", FN 18: SYSREAD Q0 = ID990 NR10 IDX0, add the index as a decimal (Q0 = Q0 + 0.2), then Q330 = Q0.

Tool Measurement with the TT (Cycles 480–485)

TT cycles measure stationary or rotating tools, or individual teeth, against a table-mounted tool probe. They require TOOL.T active and the tool called before measuring. First measurement writes geometry; wear values compare against LTOL/RTOL and breakage against LBREAK/RBREAK (tool locked at TL on violation). Speed and probing feed for rotating measurement are computed by the control from maxPeriphSpeedMeas and the measuring-tolerance machine parameters.

Cycles 31–33 and 481–483 are functionally identical; 481–483 exist as G481–G483 in ISO and always report status in the fixed parameter Q199 instead of a selectable one. Tool-table columns that feed the TT cycles: CUT (teeth), DIRECT (rotation direction), R-OFFS (radial offset for length measurement — default = tool radius), L-OFFS (axial offset for radius measurement). Manual guidance: drill → R-OFFS 0 (measure the tip); end mill → R-OFFS = R; 10 mm ball cutter → L-OFFS 5 so the diameter isn’t measured at the south pole.

Result Q-Parameters

Worked Example from the Manual — Measure & Rework a Stud

Rough a rectangular stud with allowance, measure it with Cycle 424, shrink the programmed side lengths by the measured deviations (Q164/Q165), and finish — the whole measure-and-correct loop in one program:

0 BEGIN PGM TOUCHPROBE MM
1 TOOL CALL 5 Z S6000              ; Tool call: roughing
2 Q1 = 81                          ; Rectangle length in X (roughing dimension)
3 Q2 = 61                          ; Rectangle length in Y (roughing dimension)
4 L Z+100 R0 FMAX M3
5 CALL LBL 1                       ; Machine (subprogram)
6 L Z+100 R0 FMAX
7 TOOL CALL 600 Z                  ; Call the touch probe
8 TCH PROBE 424 MEAS. RECTAN. OUTS. ~
Q273=+50   ;CENTER IN 1ST AXIS ~
Q274=+50   ;CENTER IN 2ND AXIS ~
Q282=+80   ;FIRST SIDE LENGTH ~
Q283=+60   ;2ND SIDE LENGTH ~
Q261=-5    ;MEASURING HEIGHT ~
Q320=+0    ;SET-UP CLEARANCE ~
Q260=+30   ;CLEARANCE HEIGHT ~
Q301=+0    ;MOVE TO CLEARANCE ~
Q284=+0    ;MAX. LIMIT 1ST SIDE ~
Q285=+0    ;MIN. LIMIT 1ST SIDE ~
Q286=+0    ;MAX. LIMIT 2ND SIDE ~
Q287=+0    ;MIN. LIMIT 2ND SIDE ~
Q279=+0    ;TOLERANCE 1ST CENTER ~
Q280=+0    ;TOLERANCE 2ND CENTER ~
Q281=+0    ;MEASURING LOG ~
Q309=+0    ;PGM STOP TOLERANCE ~
Q330=+0    ;TOOL
9 Q1 = Q1 - Q164                   ; Correct X length by measured deviation
10 Q2 = Q2 - Q165                  ; Correct Y length by measured deviation
11 L Z+100 R0 FMAX
12 TOOL CALL 25 Z S8000            ; Tool call: finishing
13 L Z+100 R0 FMAX M3
14 CALL LBL 1                      ; Machine again with corrected Q1/Q2
15 L Z+100 R0 FMAX
16 M30
17 LBL 1                           ; Subprogram: CYCL DEF 256 RECTANGULAR STUD
18 CYCL DEF 256 RECTANGULAR STUD ~
Q218=+Q1   ;FIRST SIDE LENGTH ~
Q219=+Q2   ;2ND SIDE LENGTH ~
...
19 L X+50 Y+50 R0 FMAX M99
20 LBL 0
21 END PGM TOUCHPROBE MM

Common Gotchas

• Kill your transformations first. Cycles 400–499 must run with all coordinate-transformation cycles inactive (Cycle 7 DATUM SHIFT, 8 MIRRORING, 10 ROTATION, 11/26 SCALING). For 444 and 14xx the ban covers mirroring, scaling, and TRANS MIRROR. Collision warning straight from the manual.
• DEF-active means it runs now. The probe moves the instant the cycle definition is read — position safely before the TCH PROBE block.
• 4xx resets your basic rotation. Cycles 40x–43x reset an active basic rotation at cycle start.
• Q115–Q119 are raw. No stylus length or radius compensation — use the cycle result parameters (Q15x/Q95x) for real coordinates.
• Units follow the main program in logs and result parameters — but anything read via FN 18: SYSREAD is always metric.
• Tool number = probe number. The row number in the touch-probe table must match the probe’s tool number in TOOL.T, in manual and automatic modes alike.
• Q305=0 rewrites row 0. Presetting cycles with Q305=0/Q303=1 overwrite and activate preset row 0 — fine for setup, surprising mid-program.
• Calibrate like you probe. Same feed for calibration and probing, especially with L-shaped styli; recalibrate after changing TRACK or the probing feed.
• 14xx deviations reference the mean tolerance (Q98x/Q99x), not the nominal, whenever a toleranced dimension was programmed.

References

• HEIDENHAIN, TNC 640 Programming of Measuring Cycles for Workpieces and Tools User’s Manual, NC software 34059x-18, 10/2023, ID 1303409-23.
• HEIDENHAIN, TNC 640 Setup, Testing and Running NC Programs User’s Manual, NC software 34059x-18, 10/2023, ID 1261174-25 (manual probing functions, calibration in manual mode).
• HEIDENHAIN, TNC 640 Klartext Programming User’s Manual, 34059x-11, 01/2021, ID 892903-29 (preassigned Q-parameter reference).