HEIDENHAIN TNC Conversational Programming for Beginners: One Minimal Program

3. The header trio: BEGIN / BLK FORM / TOOL CALL

① BEGIN PGM name unit

0 BEGIN PGM DEMO MM. Name is free; unit is MM or INCH. The last block must be END PGM DEMO MM to match.

② BLK FORM: blank definition (only affects the graphic simulation; it runs without it, but always define it)

• BLK FORM 0.1 Z X+0 Y+0 Z-40: Z is the spindle axis; the values are the MIN point (smallest X/Y/Z).
• BLK FORM 0.2 X+100 Y+100 Z+0: the MAX point.
• Cylindrical blank: BLK FORM CYLINDER Z R50 L105.

③ TOOL CALL: call the tool

TOOL CALL 5 Z S5000 = call tool 5, tool axis Z, spindle speed 5000. After a tool call, always retract to a safe position before feeding – avoid crashing at the change point.

4. Motion blocks: L / C / CR, plus R0·RL·RR and DR

Straight line L: L X+90 Y+90 R0 F200. X/Y/Z are target coordinates, F is feed, FMAX is rapid.

Arcs have two forms:

• C X... Y... DR+: give the end point and the arc centre (set the centre/pole first with CC); DR+ clockwise, DR- counter-clockwise.
• CR X... Y... R... DR+: give the end point, radius R and direction – no prior centre needed, and more common.
• Also CT (tangential arc), RND (corner rounding), CHF (chamfer).

Radius compensation R0 / RL / RR:

• R0 = no compensation (the example above runs on the centre line);
• RL = left, RR = right (when milling a contour, pick by whether the tool is on the left/right of the contour; the control offsets by the tool radius).

Incremental I: IX/IY/IZ mean “move this much further from the current position”, not an absolute coordinate. Common in drilling/patterns.

5. Approach and departure: APPR / DEP

Driving straight into the contour start with L leaves a mark and can even over-cut. The correct way is the approach/departure functions:

• Approach APPR: e.g. APPR LT (tangential straight-line approach) or APPR LCT (tangential arc approach), with the approach point and radius.
• Departure DEP: after machining, DEP ... leaves tangentially/straight, then retract.

This way the tool enters and exits while cutting – better corner quality and no gouge at the start point.

6. Fixed cycles: CYCL DEF 200 drilling, the easiest start

Do not hand-code repeated holes or pockets – use fixed cycles. For drilling:

3  TOOL CALL 5 Z S5000
4  L Z+250 R0 FMAX
5  PATTERN DEF POS1(X+10 Y+10 Z+0) POS2(X+90 Y+90 Z+0)
6  CYCL DEF 200 DRILLING
     Q200=2   ;set-up clearance
     Q201=-20 ;depth
     Q206=250 ;plunging feed rate
     Q202=5   ;plunging depth
     Q210=0   ;dwell at top
     Q203=0   ;surface coordinate
     Q204=20  ;2nd set-up clearance
7  CYCL CALL PAT FMAX M13
9  END PGM ...

• CYCL DEF defines the cycle (200 = drilling here); the Q parameters are the cycle’s “fill-in” values.
• PATTERN DEF defines the hole pattern; CYCL CALL PAT calls the cycle at every position.
• Cycle numbers vary by model (200/201/203…), so follow your machine’s cycle manual.

7. Six beginner mistakes

1. Forgetting to retract after TOOL CALL: feeding straight after a call can crash near the change point. Call tool -> retract to safety -> then position.
2. Mixing up R0/RL/RR: using R0 where RL/RR is needed means running on the tool centre – off by a tool radius.
3. DR+ / DR- reversed: the arc goes the other way, or over-cuts.
4. Using incremental I as absolute: IX+10 is “move 10 more”, not “go to X10”; in patterns the whole row shifts.
5. Forgetting M13/M9: M13 turns spindle+coolant on, M9 coolant off; plunge without the spindle on, or cut dry and smoke.
6. Wrong unit: typing imperial numbers into a MM program (or vice versa) scales dimensions by 25.4.

Frequently Asked Questions

How is conversational programming different from ISO/G-code?

Klartext is HEIDENHAIN’s “question-and-answer” language: each block describes the motion in words/parameters and the screen prompts you for what to enter – highly readable and hard to mistype; ISO/G-code is general text instructions. The TNC can also run ISO programs, but writing at the machine in Klartext is more intuitive and easier for the graphic simulation to check.

Do I have to define a BLK FORM?

Strictly, the program runs without it, but BLK FORM is the blank basis for the graphic simulation. Without it the simulation shows no workpiece and you cannot see over-cutting or collisions. Get into the habit of “define the blank first”, and debugging becomes much safer.

Why must R0 / RL / RR be distinguished?

They set how far the tool is offset from the programmed path: R0 no offset (centre line), RL/RR offsets by the tool radius to the left/right. If a contour or pocket needs compensation and you do not apply it, the actual contour is a tool radius too small (or large) and the part is scrap. Practise on the centre line with R0 first, then switch to RL/RR for real contours and check the tool radius.

Last updated: 2026-11-01

HEIDENHAIN TCH PROBE 31/481 cycles

HEIDENHAIN TNC tool management

HEIDENHAIN TNC block quick reference

HEIDENHAIN TNCremo / TNCcmd transfer