Tutorial Z: MBD exchange through STEP AP242

Books	Drake, Dimensioning and Tolerancing Handbook, 5.9.7 (degrees of freedom of a datum reference frame); the plate is ours
Standards	ISO 10303-242 (STEP AP242: semantic PMI), ISO 5459 (datums), ISO 1101 (geometrical tolerances), ISO 286
You learn	the Inspection Plan’s datum reference frames, STEP with PMI, Import STEP with PMI, planning an inspection from the file alone
Sizes	A plate 120 × 80 × 10 with four Ø8 holes

Model-based definition means the model carries the tolerances, and they travel with it as data. Here they go out to a supplier in a STEP file and come back into an empty part as PMI, ready for the inspection plan.

Step by step

1. The plate and its PMI

The plate and its PMI are made by script, as tutorials T and Y make them with the ribbon: datums A (underside), B (left side), C (front side), the hole Ø8 H11 positioned Ø0.2 Ⓜ to A|B|C, side B perpendicular 0.05 to A, the thickness 10 ±0.1.

2. The datum reference frames

PMI › Inspection Plan. Below the characteristics:

A | B | C arrests 6 of 6 degrees of freedom (A 3, B 2, C 1)
A arrests 3 of 6 degrees of freedom (A 3); free: translation along X; translation along Y; rotation about Z

The position needs all six; the perpendicularity of B needs only A.

The datum reference frames in the Inspection Plan

3. Out: STEP with PMI

PMI › STEP with PMI, a file name, OK: datums A, B and C, two datum systems, the size with H11 and the thickness with ±0.1, the position and the perpendicularity.

4. In: Import STEP with PMI

Ctrl+N, PMI › Import STEP with PMI, the file, OK. The plate comes in with seven PMI, the same as were written, on the same faces.

What came in: the part and its seven PMI

5. The supplier’s inspection plan

Inspection Plan on the imported part: the same characteristics, limits and datum reference frames as at the source.

The replay

#	In the book (NX)	In FreeCAD NX-Style	Result	Notes
Z1	The mounting plate and its PMI: datums A, B, C; the holes Ø8 H11 positioned Ø0.2 (M) to A\|B\|C; B perpendicular to A; thickness 10 ±0.1 (a count such as 4X has no AP242 form in OpenCASCADE, so it is left off)	modelled by script, the PMI made as in tutorials T and Y	differs	10.000 ±0.100; datum feature A; datum feature B; datum feature C; perpendicularity \| 0.050 \| A; position \| Ø0.200 (M) \| A \| B \| C; Ø8.000 H11 (+0.090/0)
Z2	Inspection Plan: the datum reference frames, degrees of freedom arrested (Drake 5.9.7)	ribbon 'PMI › Inspection > Inspection Plan'	differs	Datum reference frames (degrees of freedom, Drake 5.9.7: a plane arrests 3, 2 or 1 in order of precedence, an axis up to 4): / A \| B \| C arrests 6 of 6 degrees of freedom (A 3, B 2, C 1) / A arrests 3 of 6 degrees of freedom (A 3); free: translation along X; translation along Y; rotation about Z. NX has no such check; a position to A\|B\|C fixes all six, the perpendicularity to A alone leaves the plate free to slide and turn on A, which is all it needs
Z3	PMI > STEP with PMI: the file for the supplier	ribbon 'PMI › Exchange > STEP with PMI', file name typed, MB2 = OK	differs	schema AP242_MANAGED_MODEL_BASED_3D_ENGINEERING_MIM_LF; datums A, B, C (2 datum systems); sizes: 1 diameter, 1 thickness; locations: 0; with ± tolerances: 2; fits: H11; geometric tolerances: 1 perpendicularity, 1 position
Z4	New part, PMI > Import STEP with PMI: the same PMI on the same faces	Ctrl+N, ribbon 'PMI › Exchange > Import STEP with PMI', the file typed, MB2 = OK	differs	parts ['Mounting plate']; 7 PMI, identical to what was written: True. NX: File > Import > STEP with PMI; FreeCAD’s own STEP import drops the PMI
Z5	The supplier’s Inspection Plan from the imported PMI	ribbon 'PMI > Inspection Plan'	differs	the same characteristics and datum reference frames as at the source: the inspection can be planned from the STEP file alone
Z6	The imported plate with its PMI	render of the graphics window	same	5.5% of the view shows the part

In the book (NX)

In FreeCAD NX-Style

Result

Notes

The mounting plate and its PMI: datums A, B, C; the holes Ø8 H11 positioned Ø0.2 (M) to A|B|C; B perpendicular to A; thickness 10 ±0.1 (a count such as 4X has no AP242 form in OpenCASCADE, so it is left off)

modelled by script, the PMI made as in tutorials T and Y

differs

10.000 ±0.100; datum feature A; datum feature B; datum feature C; perpendicularity | 0.050 | A; position | Ø0.200 (M) | A | B | C; Ø8.000 H11 (+0.090/0)

Inspection Plan: the datum reference frames, degrees of freedom arrested (Drake 5.9.7)

ribbon 'PMI › Inspection > Inspection Plan'

differs

Datum reference frames (degrees of freedom, Drake 5.9.7: a plane arrests 3, 2 or 1 in order of precedence, an axis up to 4): / A | B | C arrests 6 of 6 degrees of freedom (A 3, B 2, C 1) / A arrests 3 of 6 degrees of freedom (A 3); free: translation along X; translation along Y; rotation about Z. NX has no such check; a position to A|B|C fixes all six, the perpendicularity to A alone leaves the plate free to slide and turn on A, which is all it needs

PMI > STEP with PMI: the file for the supplier

ribbon 'PMI › Exchange > STEP with PMI', file name typed, MB2 = OK

differs

schema AP242_MANAGED_MODEL_BASED_3D_ENGINEERING_MIM_LF; datums A, B, C (2 datum systems); sizes: 1 diameter, 1 thickness; locations: 0; with ± tolerances: 2; fits: H11; geometric tolerances: 1 perpendicularity, 1 position

New part, PMI > Import STEP with PMI: the same PMI on the same faces

Ctrl+N, ribbon 'PMI › Exchange > Import STEP with PMI', the file typed, MB2 = OK

differs

parts ['Mounting plate']; 7 PMI, identical to what was written: True. NX: File > Import > STEP with PMI; FreeCAD’s own STEP import drops the PMI

The supplier’s Inspection Plan from the imported PMI

ribbon 'PMI > Inspection Plan'

differs

the same characteristics and datum reference frames as at the source: the inspection can be planned from the STEP file alone

The imported plate with its PMI

render of the graphics window

same

5.5% of the view shows the part

Result	Means
same	The book’s NX steps work as written.
differs	It works, but the FreeCAD way is different; the notes say how.
limit	The book’s way fails in FreeCAD itself; a workaround follows in the next steps.
missing	FreeCAD has no such function; a stand-in follows.
skipped	Not replayed; the notes give the reason.
FAILED	Did not work.

Result

Means

same

The book’s NX steps work as written.

differs

It works, but the FreeCAD way is different; the notes say how.

limit

The book’s way fails in FreeCAD itself; a workaround follows in the next steps.

missing

FreeCAD has no such function; a stand-in follows.

skipped

Not replayed; the notes give the reason.

FAILED

Did not work.

What differs from NX

NX exchanges PMI through STEP AP242 and JT, with graphical PMI and saved views; NX-Style’s files carry the semantic PMI only.
A count (4X), the envelope Ⓔ and the ISO 2768 note have no AP242 form in OpenCASCADE, so this plate is dimensioned without them.
The report of the degrees of freedom a datum system arrests is NX-Style’s.
The file carries the shape and its PMI; tutorial AL sends the history, the sketch constraints and the parameters too.