Heidenhain TNC7 Touch-Probe Cycles

Probing on a TNC7 (and the TNC7 basic / TNC7 go, which run the same software platform) needs no vendor macro package: workpiece and tool measurement cycles ship in the control, programmed as TCH PROBE blocks and filled out through forms with help graphics. Results land in globally effective Q parameters and an automatic TCHPRAUTO.html log, and measured misalignment can flow straight into the preset table, a basic rotation, or a rotary-axis move. This reference is based on the TNC7 Measuring Cycles manual for NC software 81762x-20 (10/2025).

How TNC7 Probing Differs from Fanuc-Style G65 Packs

On a Fanuc or Haas you call Renishaw macros (G65 P9810…) with letter arguments and read #185-series variables. On a TNC7 the cycles are control firmware: you insert TCH PROBE 1411 PROBING TWO CIRCLES, the editor shows every parameter with a dialog question and picture, and cycles with numbers above 400 use Q-parameter transfer values that are consistent across cycles — Q260 is always clearance height, Q261 always measuring height, Q320 always set-up clearance. Two more differences worth internalizing:

All touch probe cycles are DEF-active — they run as soon as the control reads the definition. No CYCL CALL, no M99. And probing always happens parallel to a machine axis (also under an active basic rotation or tilted plane), with pre-positioning driven by the touch probe table rather than by arguments: the probe approaches at FMAX from the pre-position (offset = ball radius + SET_UP column + Q320), probes at the F column feed rate, and alarms if the stylus isn't deflected within DIST. Positioning logic: if the current position is above Q260, the probe moves in the plane first, then down; if below, it goes to clearance height first.

The machine manufacturer must prepare the control for a touch probe, HEIDENHAIN only guarantees the cycles with HEIDENHAIN probes, and the full feature set requires tool axis Z. Machine-specific probe cycles, if your builder added any, occupy numbers 500–599.

Before You Probe — Rules & Gotchas

These are the ones the manual flags with collision warnings:

Calibration Cycles

Calibration determines the effective stylus length and ball radius; length and radius go to the tool table, the center offset to columns CAL_OF1/CAL_OF2 of the touch probe table tchprobe.tp. Every calibration writes a TCHPRAUTO.html log. Make sure the probe number in the tool table matches the number in the touch probe table.

The Modern 14xx Workpiece Cycles

The 14xx generation is what HEIDENHAIN steers you toward — the manual explicitly recommends them over the old equivalents (e.g. 1410/1412 instead of 400, 1400 instead of Cycle 0). They account for the active machine kinematics and 3D calibration data, measure rotation and position simultaneously, and add three killer features:

Semi-automatic mode: put a ? before a nominal position (QS1100= "?30") and the control stops so you can jog the probe near the touch point, then presses on from there — for parts whose position is simply unknown. Machine modes only, not simulation. Tolerance evaluation: program nominal dimensions with tolerances — QS1116="+8-2-1", 10H7 (ISO 286-2) or 10m (ISO 2768-1) — and the control monitors the band, writes pass/rework/scrap to Q183, and per Q309 either continues (0), stops on rework-or-scrap (1), or stops on scrap only (2). Actual-position transfer: append @ + actual value (QS1100="10+0.02@10.0123") and no probing occurs — the cycle just computes compensation from nominal vs. supplied actual (all three axes required; Q1900–Q1999 can supply the values).

Common closing parameters decide what happens with the result: Q1120 TRANSFER POSITION (correct the active preset-table row), Q1121 CONFIRM ROTATION (set a basic rotation), Q1126 align rotary axes. If Cycle 1493 EXTRUSION PROBING was defined beforehand, the touch points repeat along a programmed direction/length.

The Classic 4xx Cycles (Still Fully Documented)

With inspection cycles 42x you get tolerance monitoring (enter limit values in the cycle) and tool monitoring via Q330 (tool number or name): measured deviations are written to the tool's DR (milling) or DXL/DZL (turning, cycles 421/422/427), and if the deviation exceeds the breakage tolerance RBREAK/LBREAK, the tool is locked (TL = L) and program run stops. For an indexed tool by name: QS0 = "TOOL NAME", then FN 18: SYSREAD Q0 = ID990 NR10 IDX0 and Q0 = Q0 + 0.2 before assigning Q330 = Q0.

Tool Measurement on the TT (481–485)

With a table-mounted tool touch probe the control measures tools automatically and writes the compensation into the tool table — stationary, rotating, or tooth-by-tooth (up to 20 teeth). Prerequisites in tool.t: approximate radius and length, number of teeth CUT, cutting direction DIRECT.; wear tolerances LTOL/RTOL, breakage tolerances LBREAK/RBREAK, and offsets R-OFFS (rotating-length measurement; 0 = stationary over center) and L-OFFS (radial measurement). For rotating measurement the control computes speed and probing feed itself from maxPeriphSpeedMeas (no. 122712) and measureTolerance1 (no. 122715).

The Q340 mode decides where results go: 0 writes the measured value to L/R and zeroes DL/DR; 1 compares to the stored value and puts the difference into DL/DR (also into Q115/Q116), locking the tool if the wear/break tolerance is exceeded; 2 only reports into Q115/Q116 without touching the table. The measurement status lands in Q199: 0 within LTOL/RTOL, 1 outside wear tolerance (tool locked), 2 outside LBREAK/RBREAK (tool locked). Leave stopOnCheck (no. 122717) at TRUE or the control won't stop on breakage. Tools defined with L=0 can be measured only if the builder set maxToolLengthTT (no. 122607).

11 TOOL CALL 12 Z
12 TCH PROBE 481 CAL. TOOL LENGTH ~
Q340=+1            ;ENTER DELTA VALUES ~
Q260=+100          ;CLEARANCE HEIGHT ~
Q341=+1            ;MEASURE INDIVIDUAL TEETH

Kinematics Measurement (450–453)

With option #48 (KinematicsOpt) the control measures its own rotary-axis kinematics on a calibration sphere: 450 SAVE KINEMATICS (backup/restore), 451 MEASURE KINEMATICS (measure and optionally optimize), 452 PRESET COMPENSATION (align head-change / drift situations), 453 KINEMATICS GRID (grid compensation). These are setup-crew cycles rather than part-program cycles, but they share the touch probe, calibration requirements, and DEF-active behavior described above.

Where the Results Go — Q-Parameter Map

Worked Example — Basic Rotation from Two Holes

Straight from the manual: measure two hole centers with Cycle 401, compensate the misalignment by rotating the table (Q402=1), zero the rotary display (Q337=1), then call the part program.

0 BEGIN PGM TOUCHPROBE MM
1 TOOL CALL 600 Z                 ; Touch probe call
2 TCH PROBE 401 ROT OF 2 HOLES ~
Q268=+25   ;1ST CENTER 1ST AXIS ~
Q269=+15   ;1ST CENTER 2ND AXIS ~
Q270=+80   ;2ND CENTER 1ST AXIS ~
Q271=+35   ;2ND CENTER 2ND AXIS ~
Q261=-5    ;MEASURING HEIGHT ~
Q260=+20   ;CLEARANCE HEIGHT ~
Q307=+0    ;PRESET ROTATION ANG. ~
Q305=+0    ;NUMBER IN TABLE ~
Q402=+1    ;SET ROTATION OF ROTARY TABLE ~
Q337=+1    ;SET A PRESET
3 CALL PGM 35                     ; Call the part program
4 END PGM TOUCHPROBE MM

The 14xx version of the same job chains 1420 PROBING IN PLANE (Q1120=+4 compensate to the mean touch point, Q1121=+1 set basic rotation) with 1411 PROBING TWO CIRCLES (Q1120=+3, Q1121=+1) — plane first, then the two holes. And the closed-loop classic: Cycle 424 measures a roughed rectangular stud, then Q1 = Q1 - Q164 / Q2 = Q2 - Q165 feed the measured deviations into the side lengths of the finishing pass with Cycle 256 — measure, correct, finish, all in one program.

References

• HEIDENHAIN, TNC7 User's Manual — Measuring Cycles for Workpieces and Tools, NC software 81762x-20, 10/2025, ID 1358777-24.
• HEIDENHAIN, TNC7 User's Manual — Setup and Program Run, 10/2025, ID 1358774-24 (touch probe table tchprobe.tp).