3D Basic Rotation & Preset from Probing

You clamp a plate, probe it, and find it sitting a degree or two out of true. The slow answer is to loosen the vise and tap it in. The HEIDENHAIN answer is a touch-probe cycle that measures the misalignment and writes it straight into the active preset as a basic rotation — or, on a genuinely tilted setup, a 3D basic rotation. That value is a basic transformation: the control applies it automatically to every subsequent program, so a part written for the ideal position cuts correctly on the part as it actually sits. This is the HEIDENHAIN counterpart of Fanuc’s G54.4 workpiece-setting-error compensation. This page is derived from HEIDENHAIN’s TNC 640 Measuring Cycles for Workpieces and Tools (1303409-23, 10/2023), ch. 4, with the TNC7 term “3D basic rotation” from 1358773-24 §19.4.15.

Basic Rotation vs. 3D Basic Rotation

A basic rotation corrects a misalignment about the tool axis — the part is rotated flat on the table (a skew in the XY plane). A 3D basic rotation corrects a misalignment in space — the part is also tilted out of the table plane. The TNC7 uses the explicit term “3D basic rotation” for that spatial case; both are stored in the active row of the preset table as basic transformations. Because they live in the preset, they apply before and underneath everything else the program does, which is exactly why a probing cycle can write one and the rest of the program simply runs.

The manual is explicit about the two ways the correction can be realized: the control interprets a basic transformation as a basic rotation (a coordinate rotation) and an offset as a table rotation (physically turning the rotary table). The modern cycles let you choose.

The Modern 14xx Family (works with 3D-ROT and TCPM)

The 14xx cycles are the current, recommended way to measure and set a (3D) basic rotation. They write the required shifts as basic transformations in the preset table — rotations either as basic rotations or as axial offsets from the first rotary-table axis — and they integrate with the tilted-plane / TCPM world.

What Cycle 1420 returns and controls. Cycle 1420 finds the angles of a plane by measuring three points and saves them in Q parameters:

A skeleton call — define the cycle, then let Q1120/Q1121 decide whether the measured result is actually written:

11 TCH PROBE 1420 PROBING IN PLANE … Q1126=+0 ;ALIGN ROTARY AXIS … Q1120=+0 ;TRANSFER POSITION … Q1121=+0 ;CONFIRM ROTATION

The Legacy 400-Series (does NOT work with 3D-ROT)

The older 400-family still exists and still measures a basic rotation, but it predates 3D basic rotation and does not integrate with the 3D-ROT / tilted-plane workflow. HEIDENHAIN explicitly recommends the 14xx cycles instead of Cycle 400. Reach for the 400-series only for a plain flat-table skew or when maintaining old programs.

Rescinding a (3D) Basic Rotation: M143

A basic rotation lives in the preset, so it persists until something clears it. M143 clears the entries from the SPA, SPB and SPC columns in the preset table; when that preset row is next reactivated the basic rotation is 0 in all columns. Use it to drop a measured skew you no longer want — the counterpart of Fanuc canceling workpiece-setting-error compensation.

3D Basic Rotation vs. Fanuc G54.4 — Same Job

This is the HEIDENHAIN answer to Fanuc’s G54.4 Workpiece Setting Error Compensation (WSEC). Both take a probe-measured translation + rotation of a mis-set part and apply it as a coordinate transformation so the ideal-position program runs true. The difference is where the correction is stored and how it’s invoked: Fanuc keeps up to seven error sets on a dedicated screen and switches them in with G54.4 Pn; HEIDENHAIN writes the correction into the active preset row as a basic transformation that then applies automatically — no per-program command needed. And, exactly as on Fanuc, you first true the setup with this feature, then, if the feature itself is designed at an angle, tilt into it with the PLANE function and hold the tip on path with TCPM.

The Consistency Gotcha (and Where the Machine’s Own Error Lives)

Two things trip people up here. First, the working plane must be consistent while you probe: if you tilt before probing and then move a rotary axis so its position no longer matches the active 3D-ROT angles, the control alarms rather than measure garbage. With option 8 you may tilt the plane before probing; inclining the tool while probing needs options 8 and 9 together. Second, this whole page is about the workpiece being crooked — not the machine. A machine’s own rotary-axis position and angle errors are a separate problem, calibrated with KinematicsOpt (option 48, Cycle 451/452) against a sphere. Probe-to-preset trues the part; KinematicsOpt trues the machine — you often need both for a good 5-axis result.

Options & Machine Parameters

14xx-vs-4xx and 3D-ROT behaviour per 1303409-23; the consistency-while-probing rule and presetToAlignAxis from the TNC7 Setup manual 1358774-24 (TNC 640 Setup 1261174-25); KinematicsOpt from 1358777-24 §10.4. Touch-probe cycles require option 17.

See also: Tilting the working plane (PLANE) and FUNCTION TCPM / M128 — you true the setup here, then tilt into and machine the feature with those. The Fanuc equivalent is G54.4 Workpiece Setting Error Compensation; on Siemens the same job is done by measuring cycles that write a frame, e.g. CYCLE998 (align edge / plane) feeding a base or settable frame. For the concept across all three controls, see the 5-axis TWP & TCPM cross-control primer.

Sources: HEIDENHAIN TNC 640 Measuring Cycles for Workpieces and Tools, 1303409-23 (10/2023) — Cycle 1420 PROBING IN PLANE (p. 64), Cycle 1410 PROBING ON EDGE (p. 71), Cycles 1411/1412/1416, Cycle 400 BASIC ROTATION (p. 105) and Cycle 404 SET BASIC ROTATION (p. 128); and the TNC7 Measuring Cycles manual (1358777-24) plus TNC7 Klartext manual (1358773-24) §19.4.15 for the term “3D basic rotation”. M143 per the TNC 640 Klartext manual (892903-29).