TNC 620 Touch-Probe Cycles

Probing on a TNC 620 is a control function, not a macro pack: with software option 17 (enabled automatically when a HEIDENHAIN probe with EnDat interface is plugged in) the control ships manual probing functions, calibration cycles, two full generations of workpiece cycles (classic 4xx and the newer 14xx), and TT tool-measurement cycles. Everything below is verified against the TNC 620 measuring-cycles manual for NC software 81760x-18.

How TNC Probing Differs from G65 Macro Packs

On a Fanuc or Haas you call vendor macros (G65 P9810…) with letter arguments and read #-variables back. On the TNC 620 you press the TOUCH PROBE key, pick the cycle from soft keys, and the control walks you through a dialog with a help graphic — the result is a TCH PROBE block whose parameters are named Q parameters (the same number always means the same thing: Q260 is always clearance height, Q261 measuring height). Three behavioral differences bite G65 veterans:

1. Touch-probe cycles are DEF-active. They run as soon as the control reads the definition — there is no CYCL CALL. 2. Pre-positioning is automatic. The control approaches each touch point axis-parallel using its positioning logic: if the probe sits above Q260 it moves at FMAX to the pre-position in the plane, then down the tool axis to measuring height; if below, it lifts to Q260 first. The pre-position stand-off = ball radius + SET_UP (probe table) + Q320 (cycle). 3. The probe data live in a table. tchprobe.tp holds the probing feed F, positioning feed FMAX, maximum deflection range DIST (error if nothing trips inside it), SET_UP, F_PREPOS (FMAX_PROBE vs machine rapid), and TRACK (orient an infrared probe to the probing direction — recalibrate after changing it). The tool number in TOOL.T and the probe row (TP_NO) must match.

Recurring parameters can be hoisted to the program head with GLOBAL DEF 120 PROBING and referenced in any cycle as PREDEF:

11 GLOBAL DEF 120 PROBING ~
Q320=+0    ;SET-UP CLEARANCE ~
Q260=+100  ;CLEARANCE HEIGHT ~
Q301=+1    ;MOVE TO CLEARANCE   (1 = clearance height between points)

Manual Probing & Where Results Can Go

In Manual Operation / Electronic Handwheel the control offers probing functions for calibrating the probe, measuring a basic rotation (workpiece misalignment — savable to the preset table, or compensated by rotating the table), and presetting on any axis, a corner, a circle center, or a center line. Every manual probing screen offers two write targets: ENTRY IN PRESET TABLE (machine/REF-referenced, into PRESET.PR) or ENTRY IN DATUM TABLE (workpiece coordinates, into a .D table). Manual results are also logged to TCHPRMAN.html; automatic 14xx and calibration cycles log to TCHPRAUTO.html.

The automatic 4xx presetting cycles use the same two targets, selected by two parameters that appear in every preset cycle: Q305 (row number) and Q303 (transfer mode): Q305=0, Q303=1 writes and activates preset row 0; Q305≠0, Q303=1 writes preset-table row Q305 (activate later with Cycle 247); Q305≠0, Q303=0 writes datum-table row Q305 (activate with TRANS DATUM).

Calibrating the Workpiece Probe (Cycles 460–463)

Calibration determines the effective stylus length (referenced to the tool reference point, usually the spindle nose) and effective ball radius, plus center misalignment. Length and radius land in the tool table; center offsets land in tchprobe.tp columns CAL_OF1/CAL_OF2. Values apply immediately — no repeated tool call needed. Recalibrate after: commissioning, a broken or replaced stylus, a probing-feed change, thermal drift, or a change of active tool axis. L-shaped styli (STYLUS = L-TYPE, supported by the 14xx cycles) need TRACK ON and should be calibrated at the same feed rate used for probing.

Workpiece Cycles — Two Generations Side by Side

The TNC 620 at 81760x-18 carries both cycle generations. The classic 4xx cycles are position-parameter driven and still fully supported; the newer 14xx cycles add consideration of the machine kinematics, semi-automatic mode (prefix a nominal position with “?” and the cycle pauses for you to pre-position by handwheel), tolerance-band inputs directly on nominal dimensions (10H7, 10+0.01-0.015 — status lands in Q183), 3D-calibration awareness, and simultaneous measurement of rotation and position. HEIDENHAIN’s own recommendation inside the manual: prefer 1410/1411/1412 over 400/401/402. Note the 4xx rotation/preset/inspection cycles do not work under 3D ROT — use 14xx on tilted planes.

Flavor of the 14xx semi-automatic mode — nominal positions prefixed with ? are supplied by jogging at runtime:

11 TCH PROBE 1411 PROBING TWO CIRCLES ~
QS1100= "?30"  ;1ST POINT REF AXIS ~     ; nominal 30, position unknown -> pause
QS1101= "?50"  ;1ST POINT MINOR AXIS ~
Q1116=+10      ;DIAMETER 1 ~
...
Q1121=+0       ;CONFIRM ROTATION

Tool Measurement with the TT (Cycles 480–484)

With a table-mounted TT probe (must be enabled by the machine builder; TOOL.T must be active and the tool called before the cycle), the control measures length and radius automatically and writes the results to the tool table. Each cycle exists in an old and a new numbering — identical behavior, except the 48x versions have ISO codes (G481…) and always report status in Q199.

The controlling parameter is Q340: 0 = write measured value into L/R and zero the delta; 1 = compare against the table, put the deviation into DL/DR (also into Q115/Q116) and lock the tool if it exceeds the wear or breakage tolerance; 2 = measure only. Wear/breakage gates and the probing offsets come from tool-table columns LTOL, RTOL, LBREAK, RBREAK, CUT, DIRECT, R-OFFS, L-OFFS. For rotating measurement the control computes speed and feed itself from maxPeriphSpeedMeas and the tolerance strategy in probingFeedCalc.

11 TOOL CALL 12 Z
12 TCH PROBE 483 MEASURE TOOL ~
Q340=+1        ;CHECK ~               ; 1 = deviation -> DL/DR, tolerance-gated
Q260=+100      ;CLEARANCE HEIGHT ~
Q341=+1        ;PROBING THE TEETH     ; 1 = individual tooth measurement

Where the Results Go — Q-Parameter Map

Inspection cycles write to global result parameters; every cycle description carries the exact per-cycle table, but the map is consistent:

Inspection cycles can additionally write a measuring log per cycle (Q281: 0 none, 1 file such as TCHPR431.TXT next to the NC program, 2 stop and display on screen) listing nominals, limits, actuals, and deviations.

Worked Example — Measure, Then Rework

The manual’s closed-loop pattern: rough a stud oversize, measure it with Cycle 424, shrink the target dimensions by the measured deviations (Q164/Q165), and finish. Abridged from the manual — the machining subprogram (Cycle 256 stud milling at LBL 1) is called before and after measurement:

0 BEGIN PGM TOUCHPROBE MM
1 TOOL CALL 5 Z S6000              ; roughing tool
2 Q1 = 81                          ; X length incl. 0.5 allowance
3 Q2 = 61                          ; Y length incl. 0.5 allowance
4 L Z+100 R0 FMAX M3
5 CALL LBL 1                       ; rough the stud (Cycle 256 in LBL 1)
6 L Z+100 R0 FMAX
7 TOOL CALL 600 Z                  ; 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 ~
Q281=+0    ;MEASURING LOG ~
Q330=+0    ;TOOL
9  Q1 = Q1 - Q164                  ; correct X target by measured deviation
10 Q2 = Q2 - Q165                  ; correct Y target by measured deviation
11 L Z+100 R0 FMAX
12 TOOL CALL 25 Z S8000            ; finishing tool
13 L Z+100 R0 FMAX M3
14 CALL LBL 1                      ; finish with corrected Q1/Q2
16 M30

And the two-hole basic rotation with table compensation, complete as printed in the manual:

0 BEGIN PGM TOUCHPROBE MM
1 TOOL CALL 600 Z
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 ~        ; 1 = align by rotating the table
Q337=+1    ;SET TO ZERO
3 CALL PGM 35                       ; call the part program
4 END PGM TOUCHPROBE MM

Common Gotchas

Transformations first. Before any 4xx cycle, Cycles 7/8/10/11/26 (datum shift, mirror, rotation, scaling) must all be inactive; the 14xx cycles tolerate a shift/rotation but not mirroring or scaling. The 40x–43x cycles also silently reset an active basic rotation at cycle start. Tool call before cycle. The probe axis comes from the last TOOL CALL — define it before any 14xx definition. DEF-active surprises. A TCH PROBE block probes the moment it is read; there is no separate call to forget. Units follow the main program in logs and return parameters — but raw FN 18/SQL reads stay metric. Semi-automatic mode ignores clearance-height modes 1/2 (Q1125) — retract manually after each touch. Tilted-plane checks: machine parameter chkTiltingAxes decides whether the control verifies rotary-axis positions against the 3D-ROT angles during probing/presetting. TT specifics: the cycles exist only if the builder enabled them (probingCapability can also restrict radius/tooth measurement); tools defined with L=0 are only searched for if maxToolLengthTT is set — otherwise the control pre-positions a zero-length tool straight at the probe.

References

• HEIDENHAIN, TNC 620 Programming of Measuring Cycles for Workpieces and Tools, NC software 81760x-18, 10/2023, ID 1303431-23.
• HEIDENHAIN, TNC 620 User’s Manual for Setup, Testing and Running NC Programs, NC software 81760x-18, 10/2023, ID 1263172-25 (manual probing, calibration, preset/datum table entry).