STEP AP203 vs AP214 vs AP242 — Which Version to Send Your Supplier (and the AP242 PMI Trap)

When SolidWorks shows you the Save As dialog, three STEP variants appear in the dropdown: AP203, AP214, and AP242. Most engineers pick one, never change it, and assume the output is correct. Sometimes it is. Sometimes half the data you expected to transfer isn’t in the file at all, and you find out when the supplier calls.

This post explains what each version actually carries, what SolidWorks and Inventor write for each, and which one to choose based on what your recipient needs on the other end.

What “AP” Actually Means

STEP stands for Standard for the Exchange of Product model data — ISO 10303. The standard is enormous: 45+ parts covering geometry, drawing views, kinematics, process planning, composite materials, and more.

Application Protocol (AP) is the specific subset of the STEP schema that a given software implementation targets. Each AP defines:

• Which ISO 10303 entity types must be written
• Which are optional
• Conformance classes (what a claiming implementation must handle)

The AP number isn’t a version in the usual sense — AP242 isn’t “STEP 3.0.” It’s a different scope from AP203 and AP214. AP242 merges and supersedes both of them, but systems that only need geometry can still produce valid AP203 output and be fully conformant.

AP203 — Configuration Controlled Design (1994)

ISO 10303-203 was published in 1994 and targets mechanical part and assembly geometry transfer. It covers:

• Solid B-Rep geometry (faces, edges, vertices, surfaces)
• Assembly structure (product, product definition, next assembly usage occurrence)
• Configuration management constructs (product definition with config context)

What it does not carry:

• Colors or visual attributes
• Layer assignments
• Surface finish codes
• GD&T or PMI (tolerances, datum references, annotations)
• Drawing views
• Kinematics

AP203 is the minimum viable STEP file. If you open an AP203 file in FreeCAD, Inventor, or Fusion 360, you get geometry and assembly tree — nothing else.

When to use AP203:

• The recipient explicitly asks for “plain STEP” or “maximum compatibility”
• You’re sending to a CAM system or CNC post-processor from the early 2000s (Mastercam 8 era, older ACIS-based importers)
• Only geometry matters — no color coding, no surface finish callouts, no annotations
• You don’t know what STEP version the recipient’s system handles

When to avoid AP203:

• Your assembly uses component colors for anything meaningful (color goes away)
• Your downstream user needs GD&T to arrive with the geometry
• You’re sending to a modern simulation or fabrication system — they handle AP214 and AP242 just as easily

AP214 — Core Data for Automotive Mechanical Design (1998/2010)

ISO 10303-214 was built for the automotive supply chain and is a substantial superset of AP203. In practice it became the dominant STEP flavor across all of manufacturing, not just automotive.

Additional data over AP203:

• Colors (colour_rgb and draughting_model_item_association)
• Layer categories and layer membership
• Surface finish codes (roughness values via surface_texture_representation)
• Some drawing revision and engineering change metadata
• Constraint relationships between assembly components
• Extended product structure attributes (design and product context flags)

AP214 does not carry GD&T, PMI, or 3D model annotations. Those require AP242.

When to use AP214:

• Your assembly uses component colors for visual organization (BOM color coding, interference zone highlights, subsystem grouping)
• You’re sending to a machining or fabrication supplier — every major CAM system (Mastercam, HSMWorks, EdgeCAM, Hypermill, PowerMill) reads AP214 cleanly
• You want colors and surface finishes to arrive without attaching a PDF callout sheet
• You’re unsure between AP203 and AP214: use AP214. Any system that reads AP203 also reads AP214 — the entity types are backward-compatible

Practical note: AP214 is the most widely deployed STEP version in the manufacturing supply chain. If a machine shop says “send me STEP,” they mean AP214.

AP242 — Managed Model-Based 3D Engineering (2014, Amendment 1: 2020)

ISO 10303-242 is the current standard. It merges AP203 and AP214 into a single unified schema and adds a substantial layer of product manufacturing information capability.

Additional data over AP214:

• Full PMI (Product and Manufacturing Information) — geometric dimensioning and tolerancing annotations, datum feature symbols, tolerancing notes
• 3D annotations embedded in the model geometry space (the core of Model-Based Definition)
• Feature-based GD&T associations (tolerance → specific geometric feature, not just floating annotation)
• Validation properties — geometric checksums that allow the recipient to verify the STEP file round-tripped correctly
• Composite material lay-up definitions
• Kinematics and motion linkage
• Supplemental geometry (datum targets, measurement reference geometry)
• Assembly of alternative shape representations

AP242 Edition 2 (Amendment 1, 2020) adds electrical harness, additive manufacturing process, and composite fiber path data — niche use cases, but the schema is there.

When to use AP242:

• Your model has GD&T that the recipient needs for CNC setup, CMM programming, or inspection planning — not just for visual reference, but as actual machine-readable data
• You’re following a Model-Based Definition (MBD) workflow where the annotated 3D model replaces 2D drawings
• Your customer or contract specifies AP242 explicitly
• You’re sending to a simulation system (Ansys, Abaqus, Nastran) that can consume PMI for automated boundary condition setup
• You’re in an aerospace or defense supply chain where AS9102 inspection data must be machine-readable

When AP242 silently produces AP214 output from SolidWorks: This is the most important gotcha. SolidWorks exports PMI in AP242 only if your annotations exist as 3D annotations created with DimXpert or the MBD module. GD&T added in 2D drawing views (the traditional workflow) stays in the drawing file and does not appear in the STEP output regardless of which AP version you select. If your team uses 2D drawings for tolerancing and tries to send AP242 “with GD&T,” the recipient gets a geometrically identical file to AP214 — no annotations. The AP242 label in the file header is accurate (it’s a valid AP242 file with no PMI entities), but the PMI isn’t there.

To use AP242 as intended, DimXpert or MBD must be the source of tolerance data, not 2D drawing annotations.

What SolidWorks Writes for Each Version

SolidWorks’ STEP translation pipeline: Parasolid serializes B-Rep via PK_PART_transmit, then sldstepu.dll converts to STEP entities, then catssdstepform.dll (Dassault’s ISO 10303-21 serializer, inherited from CATIA) writes the final file. The AP selection controls which entity types sldstepu.dll emits.

SolidWorks STEP API settings (for automation via GetUserPreferenceIntegerValue):

• swStepAP (integer 75) — value 1 = AP203, 2 = AP214, 3 = AP242
• swStepExportSplitPeriodic (396) — splits cylindrical/toroidal faces at seam lines; helps with older ACIS importers
• swStepExportFaceEdgeProps (397) — face/edge colors and transparency
• swStepExport3DCurveFeatures (497) — includes 3D curve geometry, not just surfaces
• swStepExportConfigurationData (403) — includes configuration context data

For batch export automation across an assembly tree, these preferences can be set programmatically before calling SaveAs3 with the swSaveAsOptions_e.swSaveAsOptions_Silent flag.

What Inventor Writes for Each Version

Inventor’s STEP translator uses the ATF (Autodesk Translation Framework), not Parasolid or CATIA. This produces different STEP output characteristics from SolidWorks for nominally identical geometry:

• Inventor AP214 color transfer is generally more reliable than SolidWorks because Inventor tracks display colors as explicit model attributes (iProperties), not visual overrides. Colors that are set via “Appearances” in SolidWorks sometimes fail to transfer; Inventor’s attribute-level color model avoids this.
• Inventor AP242 support was added in Inventor 2022. Older versions default to AP214 even if AP242 is selected, with no warning.
• Inventor exports PMI from 3D annotations created in the Model Annotation environment. Like SolidWorks, 2D drawing annotations do not appear in STEP output.

Inventor API: The Document.FileSaveAs method with FileType set to kStepFileType and the Options object’s StepApplicationProtocol property (values: StepAP203, StepAP214, StepAP242).

Choosing the Right Version: Decision Guide

Sending pure geometry to a machinist or fabricator: → AP214. Colors arrive if you’ve used them; the supplier’s CAM system reads it without issues.

Sending to an older CAM system or uncertain recipient: → AP203. Maximum compatibility, no risk of the recipient’s old ACIS importer choking on AP214 entity types.

Sending GD&T for inspection or machine setup: → AP242, but only if your tolerances are in DimXpert/MBD 3D annotations. Otherwise AP214 and a PDF drawing.

Sending to a simulation tool: → AP242 if the solver supports PMI boundary conditions (Ansys Mechanical 2023+ does). AP214 otherwise — most FEA pre-processors treat STEP as geometry input only.

Sending for long-term archival: → AP242. The validation properties give you a checksum to verify the geometry hasn’t drifted over years of format migration.

Export settings checklist regardless of AP version:

• Run Tools > Evaluate > Check on your SolidWorks part before exporting. Geometry errors in the model produce invalid STEP entities.
• Enable “Export 3D curve data” if the downstream tool needs wire geometry (sweep paths, routing curves) not just surfaces.
• Enable “Split periodic faces” if sending to an older ACIS-based system (Inventor, some CAM systems pre-2015).
• Verify the output in a neutral viewer — eDrawings, FreeCAD, or an online viewer — before sending. SolidWorks can produce syntactically valid STEP files with missing geometry when suppressed or lightweight components aren’t fully resolved.

For teams running batch STEP exports across large assemblies, see our guide to converting SolidWorks files to STEP for API automation and the batch export setup. For teams evaluating which CAD platform handles STEP export best as part of a broader tool comparison, the SolidWorks vs Fusion 360 vs Inventor comparison covers STEP translator differences alongside pricing and workflow factors.