iTNC 530 Touch-Probe Cycles

On a Fanuc/Haas machine, probing means a vendor macro pack (G65 P9810…) loaded into macro memory. On a Heidenhain iTNC 530 the probing cycles are part of the control: press the TOUCH PROBE key, pick a cycle from soft keys, and fill in a prompted dialog with a help graphic. Results land in fixed Q parameters (Q150–Q160 actuals, Q161–Q167 deviations) and can write the preset table or a datum table directly. This article covers the iTNC 530 generation only — the 4xx-numbered cycle set. The 14xx probing cycles found on newer TNC controls do not exist on this control.

How TNC Probing Differs from G65 Macro Packs

Cycles above 400 take Q parameters as transfer parameters with stable meanings across cycles — Q260 is always the clearance height, Q261 the measuring height, Q320 the set-up clearance. A cycle definition looks like this and is DEF-active: it runs as soon as the block executes, with no separate CYCL CALL:

5 TCH PROBE 410 DATUM INSIDE RECTAN.
Q321=+50 ;CENTER IN 1ST AXIS
Q322=+50 ;CENTER IN 2ND AXIS
Q323=60  ;1ST SIDE LENGTH
Q324=20  ;2ND SIDE LENGTH
Q261=-5  ;MEASURING HEIGHT
Q320=0   ;SET-UP CLEARANCE
Q260=+20 ;CLEARANCE HEIGHT
Q301=0   ;MOVE TO CLEARANCE
Q305=10  ;NO. IN TABLE
Q303=+1  ;MEAS. VALUE TRANSFER
...

Global probing behavior lives in machine parameters instead of macro variables:

Positioning logic for the 4xx cycles: if the stylus south pole is below the cycle’s clearance height, the TNC retracts in the probe axis first, then moves in the plane; otherwise plane first, then straight down to measuring height. Program a TOOL CALL before the cycle definition — that is how the TNC knows the touch-probe axis. Tool data must be active from calibration or the last TOOL CALL (MP7411 selects which).

Manual Probing Functions

In Manual Operation / El. Handwheel mode the TOUCH PROBE soft key opens the setup family: calibrate effective length, calibrate effective radius, basic rotation from a line (PROBING ROT), datum in any axis, corner as preset, circle center as preset, centerline as preset, plus basic rotation / preset from two or more holes or studs. Every manual function can hand its result off three ways: ENTER IN DATUM TABLE (workpiece coordinates), ENTER IN PRESET TABLE (REF/machine coordinates, file PRESET.PR), or the PRINT soft key, which appends the measured values to the ASCII file %TCHPRNT.A in TNC:\. Mind the manual’s collision warning: with an active datum shift, the probed value is referenced to the active datum even though the shift shows in the position display.

Raw Measuring Cycles — TCH PROBE 0, 1, 3

These are the building blocks OEM packs are made of — single touches with the result in a Q parameter of your choice. All three leave stylus length and ball radius uncompensated, and Cycles 0/1 additionally store the trigger position in Q115–Q119:

Cycle 4 MEASURING IN 3-D (FCL 3) probes along an I/J/K vector the same way but is flagged as an auxiliary cycle for external software.

Calibration — Cycles 2, 9, 460

5 TCH PROBE 2.0 CALIBRATE TS
6 TCH PROBE 2.1 HEIGHT: +50 R +25.003 DIRECTION: 0   ; 0=inside, 1=outside

5 TCH PROBE 460 CALIBRATE TS
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 ;DATUM

Manual-mode calibration (soft keys CAL. L / CAL. R) does the same job during setup and can manage multiple calibration data blocks per probe.

The Workpiece Cycle Set — Master Table

Where the Results Go

Datum-setting cycles (408–419) route their result with two parameters — this is the pattern to memorize:

Measured values land in globally effective Q parameters (each cycle’s description lists its exact set):

Inspection cycles can also write a measuring log (parameter Q281: 0 none, 1 to file — e.g. TCHPR421.TXT next to the program, 2 on-screen with program stop), stop the program on tolerance violation (Q309), and do tool monitoring (Q330 > 0): measured deviation goes into the tool’s DR column, and if it exceeds RBREAK the tool is locked (TL = L) with an error. Results are always referenced to the active (possibly shifted/rotated/tilted) coordinate system.

Tool Measurement with the TT — Cycles 30–33 / 480–484

TT table-probe cycles exist in two formats with identical behavior: the old numbers 30–33 (selectable status parameter) and the new 480–483 (DIN/ISO G480–G483, status always in Q199). Cycle 30/480 calibrates the TT (measuring the calibration tool’s center misalignment via a 180° spindle turn); Cycle 484 calibrates the wireless TT 449. Cycles 31/481, 32/482, 33/483 measure tool length, radius, or both — rotating (finds the longest tooth, offset by TT:R-OFFS), at standstill (drills, tools smaller than the probe contact), or tooth-by-tooth (up to 99 teeth). Speed and feed for rotating measurement are computed from MP6570 (max cutting speed) and MP6510/MP6507 (measuring tolerance strategy); standstill probing uses MP6520. Requirements: TOOL.T active, and approximate L, R, CUT, and DIRECT. entered before first measurement. First measurement writes the geometry (DL/DR = 0); check mode writes the deviation into DL/DR and locks the tool if LTOL/RTOL/LBREAK/RBREAK is exceeded.

; Old format - measure a rotating tool for the first time
6 TOOL CALL 12 Z
7 TCH PROBE 31.0 TOOL LENGTH
8 TCH PROBE 31.1 CHECK: 0
9 TCH PROBE 31.2 HEIGHT: +120
10 TCH PROBE 31.3 PROBING THE TEETH: 0

; New format - inspect a tool, probing the individual teeth
6 TOOL CALL 12 Z
7 TCH PROBE 481 TOOL LENGTH
Q340=1    ;CHECK (0 = first measurement)
Q260=+100 ;CLEARANCE HEIGHT
Q341=1    ;PROBING THE TEETH

Worked Example — Measure, Then Finish to Size

The manual’s BEAMS program is the classic adaptive loop: rough a stud oversize, measure it with Cycle 424, subtract the measured deviations (Q164/Q165) from the target lengths, and finish with the corrected dimensions:

0 BEGIN PGM BEAMS MM
1 TOOL CALL 69 Z                     ; roughing tool
3 FN 0: Q1 = +81                     ; X length, roughing (1 mm over)
4 FN 0: Q2 = +61                     ; Y length, roughing
5 CALL LBL 1                         ; rough the stud
7 TOOL CALL 99 Z                     ; touch probe
8 TCH PROBE 424 MEAS. RECTAN. OUTS.
Q273=+50 ;CENTER IN 1ST AXIS
Q274=+50 ;CENTER IN 2ND AXIS
Q282=80  ;1ST SIDE LENGTH       ; nominal finished size
Q283=60  ;2ND SIDE LENGTH
Q261=-5  ;MEASURING HEIGHT
Q260=+30 ;CLEARANCE HEIGHT
Q301=0   ;MOVE TO CLEARANCE
...
9  FN 2: Q1 = +Q1 - +Q164            ; correct X by measured deviation
10 FN 2: Q2 = +Q2 - +Q165            ; correct Y by measured deviation
12 TOOL CALL 1 Z S5000               ; finishing tool
13 CALL LBL 1                        ; finish with corrected Q1/Q2
15 LBL 1                             ; subprogram: Cycle 213 stud finishing
16 CYCL DEF 213 STUD FINISHING
Q218=Q1  ;FIRST SIDE LENGTH     ; variable dimensions
Q219=Q2  ;SECOND SIDE LENGTH
...
17 CYCL CALL M3
18 LBL 0
19 END PGM BEAMS MM

The same pattern with datum setting: probe a bolt-hole circle with Cycle 416 into preset line 1 (Q305=1, Q303=+1), activate it with CYCL DEF 247 Q339=1, then call the machining program.

Common Gotchas

References

• HEIDENHAIN, iTNC 530 Cycle Programming User's Manual, NC software 606 42x-04, 670388-25 (chapters 13–19).
• HEIDENHAIN, iTNC 530 Touch Probe Cycles User's Manual, NC software 340 49x generation.
• HEIDENHAIN, iTNC 530 Conversational Programming User's Manual, 737759-24 (manual probing, chapter 14).