Heidenhain TNC Series Guide

Heidenhain has been shipping shop-floor TNC controls since the 1980s, and machines running everything from a TNC 124 to a TNC7 are still cutting parts today. The fastest way to identify what you are standing in front of is not the badge on the pendant — it is the NC software number, an ID like 340590-18 that names both the control family and the firmware release. This guide maps every series in the lineup: which number family belongs to which control, what class of machine it runs on, whether it does mill-turn, which probing-cycle generation it has, and which manual answers which question.

Reading the NC Software Number

On TNC 640 / 620 / 320 / 128 and iTNC 530, press the MOD key and open General Information → Version Information: the control displays the control model, the NC-SW number, and the PLC software (the PLC number belongs to your machine builder, not Heidenhain). On a TNC7 the same information lives in the Settings application, which also shows in the SIK menu item which software options are enabled. Legacy controls like the TNC 124 show their NC and PLC software numbers on screen at switch-on.

NC-SW:  340590-18
340590 = product: TNC 640 (the machine-side control)
-18 = software version / release period

Family notation: 34059x  ("x" = last digit varies by variant)
340590 = TNC 640          340591 = TNC 640 E (export)
340595 = TNC 640 Programming Station

Two conventions to know. First, the last digit encodes the variant, not the product: 0 is the machine control, 1 the export version (suffix E, limited to 4-axis interpolation under dual-use rules), 5 the PC programming station — which is why documentation writes families as 34059x or 81762x. Second, starting with NC software version 16 Heidenhain simplified the version schema: the release period determines the version number and all control models of a publication period share the same version number — a TNC7 at -18, a TNC 640 at -18, and a TNC 320 at -18 all shipped in the same documentation cycle (10/2023).

Master Table — the TNC Lineup

Number families verified against the Heidenhain manual library (TNCguide, 07/2026). “Probing generation” refers to the automatic touch-probe cycles: the classic 4xx cycles (Cycle 400 basic rotation, 410–419 presetting, 420–427 inspection) versus the newer 14xx cycles (1400/1401/1402 probing, 1410/1411/1412/1416 alignment, 1420 plane) that current controls run alongside them.

Watch out for the number-family traps. TNC7 and TNC7 basic share 81762x — only the control-model line in Version Information tells them apart. 81760x is the TNC 620, 81762x is the TNC7 — two digits apart, two generations apart. And a TNC 620 can carry three different families depending on age (34056x → 73498x → 81760x), just as a TNC 320 can be 340551 or 771851 and an iTNC 530 can be 34049x or 60642x. Always read the number, not the model badge, before ordering options, posting programs, or downloading a manual.

Capability Checkpoints That Bite

Three questions settle most “will this program run here?” arguments:

Mill-turn? Only the TNC 640 (option 50, or Turning v2 option 158) and the TNC7 run milling and turning on one control; the TNC 640 also added jig grinding (option 156) and gear cutting (option 157). A TNC 620/320 program that switches to turning mode has nowhere to go. On the iTNC 530 the closest thing is optional interpolation turning (Cycle 290).

Which probing generation? If a setup sheet calls CYCL DEF 1410 PROBING ON EDGE, it needs a TNC 640/620/320 on recent software or a TNC7. An iTNC 530 only knows the 4xx cycles — the equivalent there is Cycle 400/419 territory, and error 280-046F “Touch probe cycle is not supported by this NC software” is what you get for guessing wrong. The current controls still run the full 4xx set alongside 14xx, so old programs migrate forward; new ones don't migrate back.

Klartext or DIN/ISO? Every contouring TNC from the TNC 426 up runs both Heidenhain Klartext (conversational) and DIN/ISO G-code — on TNC 640/620/320 they even get separate programming manuals. The two exceptions are the straight-cut controls: the TNC 128 is Klartext-only, and the TNC 124 predates the modern file system entirely. Note that many software options gate what either language can do — tilting the working plane (PLANE / Cycle 19) is option 8 (Advanced Function Set 1), 5-axis TCPM is option 9, and the export “E” models cap interpolation at 4 axes.

How the Manual Set Is Organized

Heidenhain splits each control's documentation into per-topic books, and knowing the split saves you from paging through the wrong 700-page PDF. Since roughly the version-16/-18 releases the set looks like this (each book has a per-control ID number; -xx is the edition):

Older releases combined the two cycles books into one Cycle Programming manual (e.g. iTNC 530: 670388-xx, covering fixed and touch-probe cycles), and the iTNC 530 additionally has a User's Manual in each language flavor (Klartext 737759-xx, DIN/ISO 737760-xx) plus a smarT.NC pilot (533191-xx). The whole library ships as the TNCguide — a complete-edition PDF/HTML export that is also installed on the control itself (on the TNC7, the built-in Help application is the TNCguide, with context-sensitive lookup). Everything is a free download from Heidenhain's TNCguide portal. Supplementary references worth knowing: the Overview of Machine Parameters, Error Numbers and System Data (1445456-xx, covers FN 14 error numbers and FN 18 system data) and the NC Error Messages list — see Heidenhain TNC Error Messages.

TNC 128 and the Straight-Cut / Legacy Family

The TNC 128 is easy to misjudge because it looks like its contouring siblings. It is a workshop-oriented straight-cut control: paraxial moves on up to 3 axes plus programmed spindle orientation — no arbitrary contour milling. Within that envelope it is surprisingly modern: full Klartext dialog programming with programming graphics and simulation, subprograms and program-section repeats, Q-parameter programming, drilling and pocket cycles, a CAD viewer, and background editing while another program runs. Probing is the sharp edge: software option 17 buys manual presetting with a touch probe and automatic tool measurement, but there are no automatic workpiece-probing cycles — do not plan a probed in-process inspection routine on one. Its manual set is just two books: Klartext Programming (819494-xx) and Setup (1263174-xx).

Its ancestor, the TNC 124, is a different century: straight-cut, dialog-prompted programming with teach-in, drilling cycles, hole patterns, rectangular pockets, and subprogram repeats — but no Q parameters, no probing, and file transfer over a serial data interface. Heidenhain's own compatibility note in the TNC 128 manual says TNC 124 programs “may not always run” on a TNC 128 — invalid blocks get flagged as ERROR blocks on import. The 1990s contouring controls (TNC 310, 406/416, 410, 426/430) sit between these worlds: real Klartext contouring with cycles and early touch-probe support (the 280 476 TNC 426/430 release already had thread-milling cycles 262–267 and TT tool measurement), but no preset-table workflow as you know it from current controls, no 14xx probing, no USB — treat any feature newer than the early 2000s as absent until the manual proves otherwise.

Going Deeper Per Series

Once you know which control you have, these are the detailed references:

For error numbers and the diagnostics workflow on any TNC, see Heidenhain TNC Error Messages & Diagnostics.

References

• Heidenhain, TNC7 User's Manual for Programming and Testing, NC SW 81762x-20, 10/2025, ID 1358773-24; TNC7 basic ID 1409856-22; TNC7 go Complete Edition ID 1441440; vTNC7 Complete Edition ID 1505672.
• Heidenhain, TNC 640 / TNC 620 / TNC 320 Setup, Testing and Running NC Programs, NC SW -18, 10/2023, IDs 1261174-25 / 1263172-25 / 1263173-21.
• Heidenhain, TNC 128 Klartext Programming User's Manual, NC SW 77184x-18, 10/2023, ID 819494-26.
• Heidenhain, iTNC 530 User's Manual (Conversational), NC SW 60642x-04 SP8, ID 737759-24.
• Heidenhain legacy manuals: TNC 426/430 (280 476-xx, 340 135-22), TNC 410 (309 740-25), TNC 406/416 (291 016-24), TNC 310 (331 645-22), TNC 124 (284 679-24).