Heidenhain TNC 640: Klartext & Q-Parameters

The TNC 640’s answer to Fanuc Macro B is Q-parameter programming: variables named Q/QL/QR/QS plus a set of numbered FN functions for assignment, math, jumps, and I/O. Combined with labels, subprograms, and external program calls, this is everything you need to write parametric part families and probing/utility macros in HEIDENHAIN Klartext (conversational) format. This reference is drawn from the TNC 640 Klartext Programming manual (NC software 34059x-11) — cycle and parameter numbers differ between Heidenhain series, so verify against your control’s manual if you run a TNC 620, iTNC 530, or TNC7.

Klartext Program Structure

A Klartext program is a numbered series of NC blocks. The first block is always BEGIN PGM with the program name and unit of measure; the last is END PGM with the same name and unit. Right after BEGIN PGM you normally define the workpiece blank with BLK FORM (needed only for graphic simulation) — rectangular (MIN/MAX corner points), cylindrical, rotationally symmetric, or an STL file. Klartext programs use the extension .H; DIN/ISO programs use .I.

0 BEGIN PGM NEW MM                 ; Program beginning, name, unit of measure
1 BLK FORM 0.1 Z X+0 Y+0 Z-40      ; Spindle axis, MIN point coordinates
2 BLK FORM 0.2 X+100 Y+100 Z+0     ; MAX point coordinates
3 END PGM NEW MM                   ; Program end, name, unit of measure

Labels, Subprograms & Program-Section Repeats

Subprograms and repeats both hang off labels (LBL), set with the LBL SET key. A label carries a number from 1 to 65535 or a name you define; each may be used only once per program. LBL 0 is reserved: it marks the end of a subprogram and may appear as often as needed (CALL LBL 0 is not permitted).

Maximum nesting depth is 19 for subprograms and 19 for external NC programs (a CYCL CALL counts as an external call); program-section repeats can be nested without limit. The PGM CALL key also holds the softkeys SEL TABLE (datum table), SEL PATTERN (point table), SEL CONTOUR, and SEL CYCLE.

Manual example — groups of holes via subprogram

0 BEGIN PGM UP1 MM
3 TOOL CALL 1 Z S5000              ; Tool call
5 CYCL DEF 200 DRILLING ...        ; Cycle definition: drilling
6 L X+15 Y+10 R0 FMAX M3           ; Move to starting point for group 1
7 CALL LBL 1                       ; Call the subprogram for the group
8 L X+45 Y+60 R0 FMAX
9 CALL LBL 1
12 L Z+250 R0 FMAX M2              ; End of main program
13 LBL 1                           ; Beginning of subprogram 1: group of holes
14 CYCL CALL                       ; Hole 1
15 L IX+20 R0 FMAX M99             ; Move to 2nd hole, call cycle
16 L IY+20 R0 FMAX M99             ; Move to 3rd hole, call cycle
17 L IX-20 R0 FMAX M99             ; Move to 4th hole, call cycle
18 LBL 0                           ; End of subprogram 1
19 END PGM UP1 MM

Q-Parameter Types & Ranges

The letter decides the type, the number decides who owns it. Stick to the recommended ranges — HEIDENHAIN cycles, OEM cycles, and your program all share the same Q space, and overlaps cause “reciprocal effects” the manual flags as a collision hazard.

Numeric values may range from −999 999 999 to +999 999 999, with 16 digits total of which 9 may precede the decimal point (internally the control calculates up to 10¹⁰, IEEE 754 binary — expect round-off on some decimals when comparing for jumps). A parameter can also be reset to the state Undefined with FN 0: Q5 SET UNDEFINED; a positioning block using an undefined Q parameter is simply ignored. Check values anytime with the Q INFO soft key, or pin a watch list in the QPARA status tab.

Assignments & Arithmetic — FN 0 to FN 5, FORMULA

The FORMULA soft key lets you skip the FN numbers entirely and write infix math in one block: operators + - * / ( ) ^ and functions SQ, SQRT, SIN, COS, TAN, ASIN, ACOS, ATAN, LN, LOG, EXP, NEG, INT, ABS, FRAC, SGN, % (modulo), and the constant PI. Normal precedence applies (parentheses, then functions, powers, multiply/divide, add/subtract); chained powers evaluate right-to-left. Beware: INT truncates — it does not round. To round, add 0.5 before truncating.

12 Q1 = 5 * 3 + 2 * 10             ; = 35
13 Q2 = SQ 10 - 3^3                ; = 73
37 Q25 = ATAN (Q12/Q13)            ; angle from opposite/adjacent sides
14 Q4 = SIN 30 ^ 2                 ; = 0.25 (function before power)

Jumps & If/Then Decisions — FN 9 to FN 12

A condition compares a Q parameter with another parameter or a value; if true, execution continues at the given label (by number, name, or QS parameter). If false, the next block runs. Unlike subprograms, jumps need no LBL 0 terminator — and they ignore return-jump labels entirely.

An unconditional jump is just a condition that is always true: FN 9: IF+10 EQU+10 GOTO LBL1. The manual’s counter idiom — loop a machining operation N times with a Q parameter as counter:

0 BEGIN PGM COUNTER MM
2 Q1 = 0                                 ; Initialize counter
3 Q2 = 3                                 ; Number of passes
5 LBL 99
6 Q1 = Q1 + 1                            ; New Q1 = old Q1 + 1
7 FN 12: IF +Q1 LT +Q2 GOTO LBL 99       ; Runs passes 1 and 2
8 FN 9: IF +Q1 EQU +Q2 GOTO LBL 99       ; Runs pass 3
10 END PGM COUNTER MM

String Processing — QS Parameters

QS parameters hold up to 255 characters and feed variable text into logs (FN 16), dynamic program calls (SEL PGM), and label targets. Assign with DECLARE STRING; process with the STRING FORMULA and FORMULA function groups:

FN 14: ERROR — and the Other Additional Functions

FN 14: ERROR raises an error message under program control and interrupts the program — the Klartext equivalent of Fanuc’s #3000 alarm. Numbers 0–999 call machine-builder dialogs; 1000–1199 are HEIDENHAIN-predefined messages (1000 = “Spindle?”, 1001 = “Tool axis is missing”, 1010 = “Feed rate is missing”, … up to 1191). Example from the manual — complain if the spindle is not on:

180 FN 14: ERROR = 1000            ; Displays "Spindle?" and stops the program

The rest of the DIVERSE FUNCTION menu, for completeness: FN 16: F-PRINT (formatted output), FN 18: SYSREAD (read system data), FN 19/FN 29: PLC (transfer two / eight values to the PLC — OEM territory), FN 20: WAIT FOR (NC/PLC sync; FN 20: WAIT FOR SYNC pauses look-ahead before real-time reads), FN 26/27/28 (freely definable tables), FN 37: EXPORT (return local QL/QS values from your own cycles), and FN 38: SEND (push text and up to seven variable values to the log or to StateMonitor over TCP/IP). FN 16, FN 18, and FN 26–28 are covered in depth in the Tables & System Data article.

Preassigned Q Parameters (Q100–Q199)

The control fills Q100–Q199 automatically — never write to them. Q108 and Q114–Q117 follow the unit of measure of the active program.

Worked Example from the Manual: Ellipse Macro

The classic Q-parameter demonstration — approximate an ellipse with short line segments, all geometry in parameters, machining inside a subprogram, loop closed with FN 12. Set the twelve header parameters and the same program cuts any ellipse:

0 BEGIN PGM ELLIPSE MM
1 FN 0: Q1 = +50                   ; Center in X axis
2 FN 0: Q2 = +50                   ; Center in Y axis
3 FN 0: Q3 = +50                   ; Semiaxis in X
4 FN 0: Q4 = +30                   ; Semiaxis in Y
5 FN 0: Q5 = +0                    ; Starting angle in the plane
6 FN 0: Q6 = +360                  ; End angle in the plane
7 FN 0: Q7 = +40                   ; Number of calculation steps
8 FN 0: Q8 = +0                    ; Rotational position of the ellipse
9 FN 0: Q9 = +5                    ; Milling depth
10 FN 0: Q10 = +100                ; Feed rate for plunging
11 FN 0: Q11 = +350                ; Feed rate for milling
12 FN 0: Q12 = +2                  ; Set-up clearance for pre-positioning
13 BLK FORM 0.1 Z X+0 Y+0 Z-20
14 BLK FORM 0.2 X+100 Y+100 Z+0
15 TOOL CALL 1 Z S4000
16 L Z+250 R0 FMAX
17 CALL LBL 10                     ; Call machining operation
18 L Z+100 R0 FMAX M2
19 LBL 10                          ; Subprogram 10: machining operation
20 CYCL DEF 7.0 DATUM SHIFT        ; Shift datum to center of ellipse
21 CYCL DEF 7.1 X+Q1
22 CYCL DEF 7.2 Y+Q2
23 CYCL DEF 10.0 ROTATION          ; Account for rotational position
24 CYCL DEF 10.1 ROT+Q8
25 Q35 = (Q6 - Q5) / Q7            ; Calculate angle increment
26 Q36 = Q5                        ; Copy starting angle
27 Q37 = 0                         ; Set counter
28 Q21 = Q3 * COS Q36              ; X coordinate of starting point
29 Q22 = Q4 * SIN Q36              ; Y coordinate of starting point
30 L X+Q21 Y+Q22 R0 FMAX M3        ; Move to starting point in the plane
31 L Z+Q12 R0 FMAX                 ; Pre-position to set-up clearance
32 L Z-Q9 R0 FQ10                  ; Move to working depth
33 LBL 1
34 Q36 = Q36 + Q35                 ; Update the angle
35 Q37 = Q37 + 1                   ; Update the counter
36 Q21 = Q3 * COS Q36              ; Current X coordinate
37 Q22 = Q4 * SIN Q36              ; Current Y coordinate
38 L X+Q21 Y+Q22 R0 FQ11           ; Move to next point
39 FN 12: IF +Q37 LT +Q7 GOTO LBL 1   ; Not finished? Loop
40 CYCL DEF 10.0 ROTATION          ; Reset the rotation
41 CYCL DEF 10.1 ROT+0
42 CYCL DEF 7.0 DATUM SHIFT        ; Reset the datum shift
43 CYCL DEF 7.1 X+0
44 CYCL DEF 7.2 Y+0
45 L Z+Q12 R0 FMAX                 ; Move to set-up clearance
46 LBL 0
47 END PGM ELLIPSE MM

DIN/ISO Equivalents: the D Functions

In the TNC 640’s ISO dialect the same machinery exists with D numbers instead of FN, and positional operands P01/P02/P03 instead of dialog prompts. Programs open with %NAME G71 (mm) and close with N99999999 %NAME G71; labels are set with G98 L1 and a subprogram is called with L1,0. The mapping is one-to-one: D00–D05 = FN 0–5, D09–D12 = FN 9–12, D14 = FN 14, D16 = FN 16, D18 = FN 18, D19/D29 = FN 19/29, D20 = FN 20, D26/D27/D28 = FN 26/27/28, D37 = FN 37, D38 = FN 38.

; Klartext                            ; DIN/ISO equivalent
16 FN 0: Q5 = +10                     N16 D00 Q5 P01 +10*
17 FN 3: Q12 = +Q5 * +7               N17 D03 Q12 P01 +Q5 P02 +7*
FN 12: IF +Q5 LT +0 GOTO LBL "ANYNAME"   D12 P01 +Q5 P02 +0 P03 "ANYNAME"*

References

• HEIDENHAIN, TNC 640 Klartext Programming User’s Manual, NC software 340590-11/340591-11/340595-11, 01/2021, ID 892903-29.
• HEIDENHAIN, TNC 640 ISO Programming User’s Manual, NC software 34059x-11, 01/2021, ID 892909-29.