PMI and technical product documentation

Each PMI is attached to its faces by a link that FreeCAD’s topological naming keeps on the same face. It is drawn at a constant size with a leader to the face; frames and datum symbols use the same drawing as NX-Style’s Drafting dialogs. Its values are properties: change the Fit, the Envelope or a tolerance in the property view and everything that uses it follows, the stack-ups too.

A PMI that cannot be measured from its faces at a recompute becomes invalid: its face was deleted, it became a different kind of surface (a diameter on what is now a plane), or a distance lost one of its two faces. Its Valid property turns false, its label turns red and says why, and nothing uses its last good values: * the inspection plan and the functional gauge leave it out, and the checks report it as an error; * Pin Location, Position Evaluation, Gauge Study and the stack-ups refuse it; * STEP with PMI does not write it; * Inherit PMI skips it; * a release package fails. Reattach it to the right face and it is valid again.

A deviation of zero is written as the digit 0, without a sign (ISO 129-1, and ASME Y14.5 for metric drawings): 4X Ø5.000 +0.200/0, Ø16.000 H7 (+0.018/0).

Dimensions and frames also have a Measurement uncertainty U, the uncertainty of the method that checks them. The inspection plan turns it into a TUR and the ISO 14253-1 acceptance limits (Inspection).

A pattern of holes often needs its holes held to each other more tightly than the pattern is held to the datums. ASME Y14.5 states this with a two-row frame (Cogorno ch. 12; Drake ch. 5). In the Feature Control Frame dialog, choose a Frame Style and fill in the lower row: its tolerance, its Ⓜ or Ⓛ, and its datums.

The checks require a two-row frame to be position or profile, the lower row to be tighter than the upper one, and a composite lower row to repeat the upper row’s datums in their order. Under ISO GPS, a two-row frame gets a note: ISO states a pattern requirement with ISO 5458 (two frames, combined zone CZ). The inspection plan lists each row as a characteristic with its own bonus and method. The functional gauge has one gauge per row: the FRTZF gauge’s pins float, with no stops for the location datums (Cogorno ch. 13). STEP AP242 receives the rows as two position tolerances, because OpenCASCADE’s XCAF has no relationship that ties them together; the Information window says so. Inherit PMI draws the two-row frame on the sheet. Position Evaluation decides from CMM data whether a measured pattern passes both rows.

As in NX, PMI belongs to model views. The part’s first PMI command (Tolerancing, Rapid Dimension …) adds a Model Views folder to the Part Navigator with NX’s eight: Front, Top, Right, Back, Bottom, Left, Isometric and Trimetric. They look as FreeCAD’s standard views do.

The release package’s pmi.json lists the model views, and each annotation’s views.

Tutorial Y works through it.

The two differ where it matters for a fit:

Inspection Plan checks the PMI as an experienced checker would:

For a frame at MMC on a feature of size, the plan gives the gauge element at its virtual condition: a gauge pin of the hole’s MMC minus its tolerance, a gauge hole of the pin’s MMC plus its tolerance. A datum feature of size referenced at MMC is simulated at its maximum material boundary, its orientation tolerance’s virtual condition. The unit tests reproduce Cogorno’s hole-pattern plate (ch. 13): pins of .250 for the four holes, .500 for datum D.

In Drafting, select a view and click Inherit PMI:

A PMI is placed once per sheet, in the first view that shows it. The drawing follows the PMI. When a PMI’s callout changes (its fit, tolerance, datum letter, modifier or lower row), its inherited annotation is made again from it, where you had placed it. When a PMI is deleted, its annotation goes. An annotation whose PMI is invalid stays as it is, and a release package refuses the drawing until the PMI is fixed. Inherit PMI also updates what is already on the sheet. Annotations inherited before 2026-10-26 do not record what they were made from: inherit them again once to have them follow. Dimensions covered by the general tolerance show no tolerance of their own, as on a drawing.

Which PMI a view inherits is its NX_InheritPMI property, NX’s Settings › Common › PMI › Inherit PMI (Wünsch, Pilz and Vajna, 6.10):

PMI › STEP with PMI writes the part and its PMI into one STEP AP242 file (ISO 10303-242). The PMI goes in as data that CAM, CMM software and other CAD systems read, not as pictures:

FreeCAD’s own STEP export drops PMI. Its Windows and conda builds ship pythonocc, which reaches OpenCASCADE’s dimension and tolerance tools and its AP242 writer; NX-Style maps its PMI onto them (nxstyle/ap242.py). After writing, OpenCASCADE reads the file back, and the Information window reports what it found. Without pythonocc the command writes plain STEP and says why.

Not written, because OpenCASCADE has no semantic slot for them: the envelope Ⓔ, theoretically exact dimensions, a count such as 4X, the ISO 2768 general tolerance, notes and centerlines. The Information window lists each one; they stay in pmi.json, the inspection plan and on the drawing.

OpenCASCADE 7.8 writes the IT grade of LIMITS_AND_FITS two too high (IT7 as '9'), and its own reader then returns IT9. NX-Style writes the grade each dimension has; the unit tests and the self-test check it.

OpenCASCADE also takes a dimension’s lower tolerance as the size below nominal and writes its negative as the lower bound. The first two NX-Style versions with STEP with PMI (commits 8b05383 and e217d17, 2026-10-14) passed it signed, so their files gave lower bounds the wrong sign (±0.1 as +0.1/+0.1); write such parts again.

PMI › Import STEP with PMI reads an AP242 file into the open part (or a new one): each part as a solid, and its semantic PMI as NX-Style PMI on the same faces, which the Inspection Plan, the stack-ups, Pin Location and Inherit PMI then use as if they had been made here. A supplier receives the model and its tolerances in one file, and plans the inspection from it (tutorial Z).

What comes in: datums, diameters, radii, widths and distances with their deviations or ISO 286 class, and the frames NX-Style has, with their zone, Ⓜ/Ⓛ and datum system (MMB/LMB). What does not: dimension types and tolerances NX-Style’s PMI has no form for (they are listed), saved views, and the graphical PMI. OpenCASCADE’s reader returns only the size of a lower tolerance; NX-Style takes its sign from the file’s own TOLERANCE_VALUE, so +0.050/+0.020 comes back as written.

The Inspection Plan ends with every datum system the frames refer to, and the degrees of freedom it arrests (Drake, Dimensioning and Tolerancing Handbook, 5.9.7): a planar primary datum arrests three, a planar secondary two, a tertiary the last one; a cylinder’s axis up to four.

What stays free is named: the plate on A can still slide and turn on it, which is all a perpendicularity to A needs, but a position to A alone would not be located. A face and a hole perpendicular to it leave the turn about the hole: the report says rotation about Z through (25, 25, 0).

FreeCAD has planned a PMI workbench of its own (issues 29772 and 29773): an annotation set per part, model views, datums, dimensions and geometrical tolerances to ISO GPS, validation and AP242 exchange. NX-Style writes its PMI through the OpenCASCADE enumerations the plan maps its objects to (its appendix A). Tolerance analysis is outside that plan’s scope; here it is the stack-up and pin location analyses, which read the PMI.

The MBD Workbench add-on (LGPL-2.1, an early preview) also writes semantic AP242 through pythonocc, and reads it back into FreeCAD objects. NX-Style does not use it. The Tolerancing page of the FreeCAD wiki collects the earlier attempts.