Does model based definition mean a STEP file can replace the 2D drawing?

What does a STEP file actually carry to the machine shop?

A typical STEP export carries exact boundary geometry, the unit system, the part name and sometimes color, but every face sits at one nominal size with no tolerance attached. Whether it also carries tolerances depends on the application protocol used and on whether anyone authored them in the model.

STEP is ISO 10303, a family of standards for exchanging product data. The file you get from “Save as STEP” is written to one application protocol (AP). The older AP203 and AP214 exports that many CAD systems still default to are, in practice, geometry carriers: solids, surfaces, assemblies and a few attributes. Later editions of those protocols can hold some product and manufacturing information (PMI), but few exports use it. AP242, the protocol built for model based definition, is the one designed to carry PMI in full. According to NIST’s STEP File Analyzer documentation, PMI comes in two kinds: graphic PMI, which is only the visual appearance of the annotations, and semantic PMI, which is computer-interpretable tolerance, datum and dimension data that CAM and inspection software can read.

That distinction decides what a supplier can use. Graphic PMI is a picture of a feature control frame floating in 3D: a person can read it, but software cannot. Semantic PMI can drive a CMM program or a tolerance-aware CAM setup, but only if the exporting system wrote it correctly and the receiving system reads it. NIST runs a PMI validation and conformance testing project precisely because that round trip between CAD systems is not automatic. If you have never checked what your export contains, assume it is geometry only.

Native CAD files (a part file from your own CAD package) can hold more, including cosmetic threads, hole callouts and material properties. They are useful as an extra, but a supplier on a different CAD system, or a different version, may open them with those features silently stripped.

Why do parts made from a bare model come back at default tolerances?

Because a dimension with no stated tolerance has no limits anyone can inspect against, so the shop fills the gap with its own default. Per ASME Y14.5, every dimension other than a reference, minimum, maximum or stock dimension needs a tolerance, either stated directly or through a general note, and a bare model supplies neither.

When a programmer pulls geometry from a model with no tolerance information, the CAM toolpath targets the modeled surface. The machine then holds whatever its process normally holds, and the inspector, if there is one, checks against whatever the shop’s quality manual says is standard. That is not malice; it is the only basis available. The trouble comes later, when a part that met the shop’s default fails your assembly and neither side has a document that says who was wrong.

The most common version of this failure is the modeled-at-nominal trap. Designers usually model every feature at its nominal size. For a bore toleranced H7, that is harmless: per ISO 286-2, a 10 mm H7 bore runs from 0 to +0.015 mm, so nominal is the bottom of the band and still in tolerance. For a shaft toleranced g6 it is not: per ISO 286-2, a 10 mm g6 shaft runs from −0.005 mm to −0.014 mm, so a shaft machined exactly to the model is oversize and will not slide into its mating bore. Nothing in the STEP file warns anyone. Only the drawing callout, or semantic PMI, tells the shop to aim below nominal. The fit system itself is covered in clearance, transition and interference fits.

The same logic applies to general tolerances. A title-block note such as “ISO 2768-m” sets, per ISO 2768-1, a limit of 0.2 mm either side of nominal on any untoleranced length from over 6 mm up to 30 mm. Without that note, the same length has no stated limit at all. If you want the shop to read untoleranced model geometry at a known class, the class has to be written somewhere the shop will see it. How the classes work is explained in ISO 2768 and NADCA tolerances.

What should the drawing carry when the STEP file defines the geometry?

Everything the model cannot: the controlling tolerances, datums, thread and fit callouts, surface texture, material and finish notes, and a note saying which document governs. It does not need to repeat every nominal dimension the model already defines.

This hybrid is often called a reduced-dimension or limited-dimension drawing, and ASME Y14.41 covers data sets made of an annotated model with or without a drawing sheet. The drawing dimensions only what is controlled; every other surface takes its size from the model and its tolerance from the general note. Done well, it is shorter than a fully dimensioned print and harder to misread. A workable minimum, with example wording:

• Precedence note. “Untoleranced geometry per 3D model 1234-567 rev C. In case of conflict, this drawing governs.” Put the same revision letter on both files.
• General tolerance. “Unless otherwise specified, tolerances per ISO 2768-m,” or a decimal-place tolerance block. Name the GD&T standard too, for example “Dimensioning and tolerancing per ASME Y14.5-2018.” Why that matters is in ASME Y14.5 vs ISO GPS.
• Datums and the controlled features. Only the features that locate, mate, seal or carry load, each with its own tolerance or feature control frame against the datums.
• Fits as fits. Write “Ø10 g6” with the limits, not just the nominal size, so nobody machines to the modeled value. State whether the model shows nominal or mean-of-tolerance geometry.
• Every thread. Designation, class and depth, as in “1/4-20 UNC-2B, full thread depth .50 min.” The model shows a plain hole. Format guidance is in how to write a thread callout.
• Surface texture on the faces that need it, with a default for the rest. See how to write a surface finish symbol.
• Material, finish and masking. Alloy and temper by standard, the finish by name and standard, and which features stay bare.
• Edge and cosmetic notes. An edge-break note, which faces are cosmetic, and any part marking.
• Projection symbol and units in the title block, so the views are not read mirrored; see first angle vs third angle projection.

What does Saola do with a STEP file and a drawing at quote stage?

The quote form takes the model and the drawing together, and a STEP file plus a dimensioned PDF gets the fastest, most accurate quote. Every tolerance, callout and note on the drawing is read at drawing review, and you receive a marked-up copy of your own drawing.

The form accepts STEP, STP, IGES, IGS, DWG, DXF, PDF, ZIP, PNG or JPG files. If you send a model with no drawing, expect questions before a firm price, because the questions in this guide still need answers: which features are controlled, what the threads are, and what finish goes on. At first article, the first piece off new tooling is measured against every toleranced dimension on your drawing, and you receive that report; a requirement that exists only as an unannotated model surface has nothing to be measured against. If your drawing marks a dimension as a process-capability control point, it is watched through the run, not only at first article.

For turned parts on CNC turning, the tolerances on your drawing are reviewed feature by feature, and pipe threads are gauge-checked to ANSI/ASME B1.20.1, so the thread callout on the drawing is what the gauge is chosen from. Machined features on castings run on CNC milling, where the datum scheme on your drawing sets the fixture; simultaneous five-axis machining is not offered. If the drawing names a finish, check it against the menu on surface finishing before you send it. To start, send the STEP file and the PDF together.