Heidenhain TNC 320: Touch-Probe Cycles

On a Fanuc or Haas you buy a Renishaw macro pack and call G65 P9810…. On the TNC 320 probing is part of the control: press the TOUCH PROBE key, pick a cycle from soft keys, and fill in Q parameters with a help graphic showing each one. This firmware (77185x-18) carries two generations side by side — the classic 4xx cycles and the newer 14xx cycles — plus calibration (46x) and TT tool-measurement (48x) cycles. Results land in globally effective Q parameters and an automatic HTML/ASCII log.

How TNC Probing Differs from G65 Macro Packs

Instead of macro-variable conventions, the TNC uses named cycle parameters that stay consistent across cycles — Q260 is always the clearance height, Q261 the measuring height, Q320 the set-up clearance. Probe behavior lives in the touch probe table tchprobe.tp rather than in macro commons: F probing feed, FMAX positioning feed, DIST maximum travel before the “no contact” error, SET_UP pre-position distance, TRACK spindle orientation per touch (recalibrate after changing it), CAL_OF1/2 center offset, STYLUS SIMPLE or L-TYPE. The probe is linked to its tool-table row via the TP_NO column — the numbers must match.

Three behaviors that trip up Fanuc-trained programmers:

1. Touch-probe cycles are DEF-active. They execute the moment the control reads TCH PROBE 4xx — there is no CYCL CALL. 2. Coordinate transformations must be off. Before 400–499 cycles, Cycle 7 DATUM SHIFT, 8 MIRRORING, 10 ROTATION, 11/26 SCALING must all be inactive; the 14xx cycles tolerate a datum shift but still forbid mirroring and scaling. The 40x–43x cycles also reset an active basic rotation at cycle start. 3. Pre-positioning is automatic. Cycles 400–499 and 1400–1499 use positioning logic around Q260 CLEARANCE HEIGHT; the pre-position distance is ball radius + SET_UP + Q320. Defaults for the recurring parameters can be set once per program with GLOBAL DEF 120 PROBING (Q320, Q260, Q301) and referenced in any cycle as PREDEF.

Manual Probing Functions

In Manual Operation / Electronic Handwheel mode (TOUCH PROBE soft key) the control offers: probe calibration, basic rotation from a line or a plane, preset on any axis, corner as preset, circle center as preset (hole, stud, or model circle with automatic probing routines, 3–8 touch points), and centerline as preset. Measured values can be written to the preset table or a datum table directly from the menu. No electronic probe? The same functions work with a mechanical probe or by touching off with a tool — you trigger each point manually with the actual-position-capture soft key. Manual probing results are logged to TCHPRMAN.html.

Calibration Cycles (46x)

Calibrate at commissioning, after a stylus break or swap, when the probing feed rate changes, and after changing the active tool axis or TRACK. Calibration stores the effective stylus length and ball radius in the probe's tool-table row (L and R) and the center offset in tchprobe.tp (CAL_OF1/CAL_OF2); values take effect immediately, no new tool call needed. Every calibration writes a log to TCHPRAUTO.html.

11 TCH PROBE 460 TS CALIBRATION OF TS ON A SPHERE ~
Q407=+12.5  ;SPHERE RADIUS ~
Q320=+0     ;SET-UP CLEARANCE ~
Q301=+1     ;MOVE TO CLEARANCE ~
Q423=+4     ;NO. OF PROBE POINTS ~
Q380=+0     ;REFERENCE ANGLE ~
Q433=+0     ;CALIBRATE LENGTH ~
Q434=-2.5   ;PRESET ~
Q455=+15    ;NO. POINTS 3-D CAL.

Workpiece Cycles — What Exists on the TNC 320

Verified against the cycle table of this manual (sw 77185x-18). For nearly every 4xx cycle, the manual now recommends its 14xx successor — but both remain available. Note what is not here: Cycle 444 PROBING IN 3-D and the KinematicsOpt 45x cycles are mentioned only in passing and do not appear in the TNC 320 cycle table — do not import them from TNC 620/640 documentation.

What the 14xx generation adds

Three input tricks, all typed via the ENTER TEXT soft key into the nominal-position parameters (Q1100…, entered as QS strings): semi-automatic mode — prefix ? (e.g. QS1100="?30") when you don't know where the part sits; the cycle stops, you jog the probe near the feature, press NC Start, and it measures from there. Tolerance monitoring — append a tolerance (QS1116="+8-2-1", or DIN EN ISO 286-2 like 10H7); the control classifies the result into Q183 (0 good / 1 rework / 2 scrap) and Q309 decides whether to stop. Actual-position transfer — append @ plus a measured value (QS1100="10+0.02@10.0123"): no probing occurs; the cycle just computes and applies the compensation. Where the 4xx presetting cycles steer output with Q303/Q305 (Q305=0 → row 0 + display; Q305>0 with Q303=1 → preset table, Q303=0 → datum table), the 14xx cycles use Q1120 TRANSFER POSITION and Q1121 CONFIRM ROTATION to correct the active preset, and Q1126 to align a rotary axis.

Where the Results Go — Q-Parameter Map

All result parameters are global. Units follow the main program; automatic logs go to the NC program's directory (4xx inspection cycles: e.g. TCHPR421.TXT, selected with Q281) or to TCHPRAUTO.html (14xx and calibration cycles).

TT Tool-Measurement Cycles

Enabled by the machine manufacturer (a table-mounted TT probe must be configured). Each cycle exists twice: old format 30–33 and new format 480–483 — functionally identical, but only 48x exist as G480–G483 in ISO, and 48x report status in the fixed parameter Q199 where Cycle 31–33 let you choose the result parameter. TOOL.T must be active, and the tool needs approximate L, R, CUT, and DIRECT entered before first measurement. R-OFFS/L-OFFS position the tool over the probe contact (drills: R-OFFS 0; end mills: offset by tool radius).

Q340 decides what happens with the measurement: 0 write L/R and zero the deltas, 1 compare and store the difference as wear DL/DR (locking the tool with status L if LTOL/RTOL/LBREAK/RBREAK are exceeded — deviation also lands in Q115/Q116), 2 just report into Q115/Q116, touch nothing. Rotating-tool speed and feed come from machine parameters (maxPeriphSpeedMeas, measureTolerance1, probingFeedCalc).

11 TOOL CALL 12 Z
12 TCH PROBE 481 CAL. TOOL LENGTH ~
Q340=+1    ;CHECK -- store deviation as wear DL ~
Q260=+100  ;CLEARANCE HEIGHT ~
Q341=+1    ;PROBING THE TEETH

Worked example — basic rotation from two holes (from the manual)

Probe two holes, compensate the misalignment by rotating the table (Q402=1), zero the rotary-axis display (Q337=1), then run the part program:

0 BEGIN PGM TOUCHPROBE MM
1 TOOL CALL 600 Z                      ; call the touch probe
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    ;COMPENSATION -- rotate the table ~
Q337=+1    ;SET TO ZERO
3 CALL PGM 35                          ; run the part program
4 END PGM TOUCHPROBE MM

And the measure-and-rework pattern with an inspection cycle — Cycle 424 measures a roughed stud, the measured side-length errors Q164/Q165 shrink the finish dimensions, and tool monitoring via Q330 can write the deviation straight into the milling cutter's DR column:

8  TCH PROBE 424 MEAS. RECTAN. OUTS. ...
9  Q1 = Q1 - Q164                      ; correct length X by measured deviation
10 Q2 = Q2 - Q165                      ; correct length Y
12 TOOL CALL 25 Z S8000                ; finishing tool
14 CALL LBL 1                          ; re-run the stud cycle with corrected Q1/Q2

Common Gotchas

References

• HEIDENHAIN, TNC 320 Programming of Measuring Cycles for Workpieces and Tools, NC software 77185x-18, 10/2023, ID 1303435-20.
• HEIDENHAIN, TNC 320 User's Manual for Setup, Testing and Running NC Programs, NC software 77185x-18, 10/2023, ID 1263173-21 (manual probing, touch probe table, preset management).