STEP File Format — AP203 vs AP214 vs AP242, How CAD Kernels Differ, and Which Version to Export

The Universal Language of CAD Data Exchange

Picture this: an aerospace engineer in Seattle needs to share a turbine blade design with a manufacturer in Germany, or a product development team needs to collaborate across multiple CAD platforms. They all rely on one file format that every system understands—STEP.

STEP files have become the backbone of modern engineering collaboration, making it possible to exchange data seamlessly between different CAD systems, manufacturers, and engineering teams worldwide. Yet many engineers use STEP files daily without really understanding how they work or how to get the most out of them.

This guide covers everything you need to know about STEP files—from the technical details to practical tips that can make your engineering workflows smoother.

What Is a STEP File?

STEP (Standard for the Exchange of Product Data) is a neutral file format that lets you share 3D CAD data between different software applications. Unlike proprietary formats locked to specific CAD systems, STEP files give you a vendor-independent way to share both geometric shapes and manufacturing details.

The format follows ISO 10303, an international standard that sets the rules for representing and exchanging industrial product data. When you save a part or assembly as a STEP file, you’re translating your design into a standardized language that any STEP-compatible CAD system can read.

STEP files use .stp or .step extensions and pack in both geometric data (surfaces, solids, curves) and metadata (material properties, tolerances, manufacturing specs). This combination makes STEP especially valuable for manufacturing handoffs where you need both the shape and the specifications.

The Technical Foundation: ISO 10303 Standard

STEP emerged from decades of international work to solve CAD compatibility problems. ISO 10303, first published in 1994, defines more than just a file format—it’s an entire framework for representing product data.

The standard uses EXPRESS modeling language to define data structures, which means a cylindrical feature created in SolidWorks will keep its geometric properties and relationships when you open it in Autodesk Inventor or Siemens NX.

Application Protocols: The STEP Variants

STEP isn’t one format but a family of related standards called Application Protocols (APs). Each targets specific industry needs:

AP203 (Configuration Controlled 3D Design) handles mechanical design data exchange. It covers 3D geometry, basic annotations, and design history but skips manufacturing-specific details. Most general CAD-to-CAD transfers use AP203.

AP214 (Core Data for Automotive Mechanical Design) builds on AP203 with automotive industry requirements. It includes materials, tolerances, surface finishes, and manufacturing processes. Despite the automotive name, AP214 works well for any precision manufacturing.

AP242 (Managed Model Based 3D Engineering) is the latest version, supporting advanced features like parametric models, product manufacturing information (PMI), and model-based definition (MBD) workflows.

Your choice of AP affects what information travels with your geometry. AP203 gives you reliable geometric exchange for most jobs, while AP214 and AP242 preserve more manufacturing context but create more complex files.

STEP File Structure and Data Organization

Knowing how STEP files are built helps you troubleshoot transfer problems and optimize your workflows. STEP files use a text-based format with distinct sections:

Header Section

Contains file metadata like originating software, creation date, author, and units. This helps receiving systems interpret the geometric data correctly.

Data Section

Holds the actual geometric and product information using numbered entities. Each entity represents a specific geometric element (point, curve, surface) or relationship (assembly structure, material assignment). This entity-based approach lets complex products be reconstructed accurately in the receiving system.

Entity Relationships

STEP files maintain connections between geometric elements, preserving design intent during transfer. A hole feature stays linked to its parent surface, and assembly constraints are kept where the receiving application supports them.

Three Kernels, Three STEP Translators

Every major CAD system delegates geometry to a geometric kernel — the engine that actually creates and manipulates B-Rep topology. When you export a STEP file, you’re not just “saving” — you’re translating from one kernel’s internal representation into a standardized format. And each kernel does this translation differently.

If you’ve read our deep dive into how SolidWorks, Inventor, and FreeCAD handle fillets, you’ve already seen how the same operation — “round this edge” — produces fundamentally different geometry depending on whether Parasolid, ShapeManager/ACIS, or OpenCASCADE does the work. Those same architectural differences carry directly into STEP export. The kernel that built the geometry is the kernel that serializes it.

SolidWorks: Parasolid → Dassault STEP Translator

When you call SaveAs with a .stp extension in SolidWorks, the export flows through a specific DLL chain:

1. pskernel.dll (Parasolid) serializes the B-Rep geometry via its PK_PART_transmit functions — the same transmit pipeline used for native .x_t export
2. sldstepu.dll (SolidWorks’ STEP translator, 2.8 MB) orchestrates the conversion through RunSldStepDLL / RunSldStepDLLWithData entry points
3. catssdstepform.dll (a Dassault Systèmes component) handles ISO 10303-21 file serialization — writing the header, entity instances, and exchange structure via WriteExchangeStructure

The catssdstepform.dll is significant. It contains CATStepExchangeStructure, CATStepFileHeader, CATStepFileName, and CATStepFileSchema classes — the same CATIA-derived STEP infrastructure that Dassault uses across its product family. SolidWorks’ STEP translator is not a Parasolid-native tool; it’s a Dassault data exchange layer that reads Parasolid geometry and writes STEP entities.

SolidWorks exposes several export preferences through its API:

For AP242 with MBD data, SolidWorks provides a dedicated method — IModelDocExtension.PublishSTEP242File — that bypasses the generic SaveAs path entirely and requires the MBD add-in license.

Autodesk Inventor: ShapeManager/ACIS → ATF STEP Producer

Inventor’s STEP export uses an entirely different architecture. The translator is registered as a COM AddIn ({90AF7F40-0C01-11D5-8E83-0010B541CD80}) implemented in Trans.dll, but the actual STEP generation happens in the Autodesk Translation Framework (ATF):

1. Trans.dll receives the SaveCopyAs call and reads export options via transOptionsManager
2. atf_step_producer.dll (1.3 MB) contains ATF::STEPProducer and ATF::STEPProducerOptions — the actual STEP generation engine
3. stp_aim_x64_vc15.dll (13.6 MB, 59,111 exports) implements the complete STEP schema entity classes — every stp_cartesian_point, stp_face_surface, stp_edge_curve, and stp_product_definition entity is a C++ class in this DLL
4. ASMKERN231.dll (the ShapeManager/ACIS kernel) provides the source B-Rep geometry

The ATF producer has an interesting typo preserved across the entire API: ApplicationProtocalEnum (misspelling “Protocol”). The producer supports AP203, AP203E2, AP214, and AP242.

Inventor’s ATF::STEPProducerOptions exposes options that SolidWorks doesn’t:

Inventor also ships atf_step_extension_data.dll (418 exports) with validation property classes — GeomValidationProperties, SurfaceGeomValidationProperties, BoundingBoxValidationProperties — that embed geometric checksums into the STEP file for import verification.

FreeCAD: OpenCASCADE → STEPControl_Writer

FreeCAD’s STEP export is fully readable in source code. There are two paths:

Simplified path (src/Mod/Part/App/TopoShape.cpp, line 900):

STEPControl_Writer aWriter;
aWriter.Transfer(this->_Shape, STEPControl_AsIs);
aWriter.Write(encodeFilename(fileName).c_str());

Assembly path (src/Mod/Import/App/WriterStep.cpp, line 47):

STEPCAFControl_Writer writer(hDoc->Get());
writer.Transfer(hDoc, STEPControl_AsIs);

Both paths use STEPControl_AsIs — telling OCCT to preserve the shape type as-is during conversion. Solids stay as manifold_solid_brep, shells as shell_based_surface_model. FreeCAD doesn’t force any shape type conversion.

The AP protocol is set via Interface_Static::SetCVal("write.step.schema", ...) with five options: AP203, AP214CD (1996), AP214DIS (1998), AP214IS (2002, the default), and AP242DIS.

Why the Same Part Produces Different STEP Geometry

This is the question that matters for manufacturing: if you model the same part in SolidWorks and FreeCAD and export both as STEP, will the files contain identical geometry?

No. They won’t. And the differences go deeper than rounding errors.

Different tolerance regimes

Each kernel maintains its own internal precision model, and these are not identical:

When these tolerances get written to STEP, they become UNCERTAINTY_MEASURE_WITH_UNIT entities — the STEP standard’s way of declaring how precisely the geometry should be interpreted. But each kernel computes this value differently:

Parasolid derives uncertainty from its per-edge tolerance values. An edge where two surfaces don’t quite meet carries a tolerance reflecting the gap size. The STEP translator typically writes the maximum edge tolerance as the file’s uncertainty.

ACIS/ShapeManager uses a fixed maximum uncertainty of 0.1 mm in Inventor’s STEP export — a value users cannot change. This is considerably looser than what Parasolid typically writes.

OpenCASCADE provides explicit control through write.precision.mode:

• Least (-1): uncertainty = minimum tolerance across the shape
• Average (0): uncertainty = average tolerance (the default)
• Greatest (1): uncertainty = maximum tolerance
• Session (2): uses write.precision.val (default 0.0001 mm)

A Parasolid model with 1e-6 mm edge tolerances can create micro-gaps when imported into an ACIS-based system set to 1e-4 mm tolerance. The geometry is “the same,” but the tolerance regime interprets it differently — faces that were airtight in Parasolid might register as having gaps in ACIS.

Analytic surfaces vs. NURBS: the fillet problem

This is where kernel-level differences in fillet implementation directly affect STEP export quality.

The STEP standard supports both analytic surface types (PLANE, CYLINDRICAL_SURFACE, CONICAL_SURFACE, SPHERICAL_SURFACE, TOROIDAL_SURFACE) and NURBS types (B_SPLINE_SURFACE, RATIONAL_B_SPLINE_SURFACE). A cylinder can be represented either as a CYLINDRICAL_SURFACE with a center, axis, and radius, or as a B_SPLINE_SURFACE with control points and knot vectors. Both are valid STEP. But they are not equivalent in practice.

The problem starts during modeling, not during export. When Parasolid creates a fillet using PK_EDGE_set_blend_constant (one of its 21 dedicated blend functions), it creates a rolling-ball blend surface. If that surface is a simple torus (constant-radius fillet on a straight edge between two planar faces), Parasolid can represent it analytically. But if the fillet intersects with other features — a boss, a rib, or another fillet — Parasolid’s boolean engine trims the surface. That trimming often converts a clean analytic surface into a NURBS approximation.

The same fillet in OpenCASCADE’s BRepFilletAPI_MakeFillet (which uses the ChFi3d_FilBuilder spine-based algorithm) may produce a different NURBS representation — different degree, different knot vectors, different control point placement — because the kernel’s blend algorithm marched along the edge differently and chose different surface representations (ChFi3d_Rational, ChFi3d_QuasiAngular, or ChFi3d_Polynomial).

When these surfaces hit the STEP file, what was once a clean analytic surface — a cylinder for a hole, a torus for a fillet — becomes a general-purpose B-spline surface that looks like a cylinder but behaves like a NURBS. The receiving system’s feature recognition module might try to recover the analytic type, but this is heuristic and imperfect. A hole that was a clean CYLINDRICAL_SURFACE in the original kernel might arrive as a B_SPLINE_SURFACE that the receiving system doesn’t recognize as a hole at all.

SolidWorks explicitly offers a “convert analytic geometry into NURBS geometry” option in its STEP export settings. When enabled, every plane, cylinder, cone, and sphere gets converted to B-spline surfaces — deliberately sacrificing recognizability for consistency. When disabled (the default), analytic surfaces are preserved where possible.

FreeCAD does not set OCCT’s write.convertsurface.mode parameter, so analytic surfaces are preserved as-is by default. But the surfaces that were already NURBS from the kernel’s boolean operations stay as NURBS — and those NURBS representations differ from what Parasolid or ACIS would have produced for the same nominal geometry.

Trimming curves and pcurves

Every trimmed surface in a B-Rep model has trimming curves — the boundaries that define where the surface stops. In the kernel’s internal representation, these exist as both 3D edge curves and 2D parametric curves (pcurves) in the surface’s UV space. How these get written to STEP varies:

OCCT controls pcurve export through write.surfacecurve.mode:

• Mode 1 (default): writes pcurves to the STEP file
• Mode 0: omits pcurves to minimize file size (documented as OCCT bug #25654)

FreeCAD exposes this as a “Write surface curve mode” checkbox. Omitting pcurves reduces file size but forces the receiving system to recompute them — and different kernels may compute slightly different pcurves for the same 3D edge, introducing micro-discrepancies.

Parasolid and ACIS both include pcurves by default, but their parameterizations differ. The same trimming curve on the same surface may have different UV-space representations because each kernel parameterizes its surfaces differently. A cylinder in Parasolid may be parameterized 0→2π in one direction while ACIS parameterizes it -π→π. The STEP file preserves whatever parameterization the source kernel used.

OCCT converts all trimmed_curve entities to Geom2d_BSplineCurve during import — and only supports curves trimmed by parameters, not by Cartesian points. This means trimming information that one kernel exports cleanly may get approximated during import into another.

The dimensional impact: is it real?

Yes, but the magnitude depends on the geometry.

For simple prismatic parts — boxes, holes, slots — the dimensional differences between kernels’ STEP exports are typically within 1e-6 mm. Well within manufacturing tolerance. The analytic surfaces transfer cleanly, and tolerance regime differences don’t matter because the geometry is exact.

For complex curved geometry — fillets, blends, lofted surfaces, swept features — the differences can be measurable. A fillet surface that one kernel represents as a degree-3 B-spline with 12 control points might be represented as a degree-5 B-spline with 8 control points by another kernel. Both approximate the same nominal shape, but at different points along the surface they may disagree by microns. In extreme cases documented in manufacturing contexts, dimensions have shown 0.005-inch (0.127 mm) discrepancies between the design model and the STEP file interpretation.

For thread geometry, the degradation is worse. A helix modeled analytically becomes NURBS in STEP, and the receiving system sees “just a set of abstract mathematical values, having nothing to do with manufacturing” — the thread pitch, diameter, and form are lost as semantic information even though the geometry approximates them.

Compatibility Across CAD Systems

STEP’s vendor-neutral design enables broad compatibility, though the kernel-level differences described above mean “compatible” doesn’t always mean “identical.” Each system’s STEP translator reflects its kernel’s assumptions:

SolidWorks uses Parasolid geometry through Dassault’s STEP infrastructure (sldstepu.dll + catssdstepform.dll). It handles AP203 and AP214 well, with a dedicated AP242 path for MBD. The swStepExportSplitPeriodic option splits cylindrical and toroidal faces at seam lines — important because some receiving systems can’t handle periodic surfaces. For a complete walkthrough of the export process, see our guide on how to convert SolidWorks files to STEP format.

Autodesk Inventor routes through the ATF (Autodesk Translation Framework) and its 59,111-export STEP schema library (stp_aim_x64_vc15.dll). Inventor’s fixed 0.1 mm maximum uncertainty in STEP export is notably loose — parts with tight tolerances may need verification after import into Parasolid-based systems. The ConvertFacetedBrepToBrep option can upgrade faceted geometry to full B-rep during export.

Siemens NX shares Parasolid with SolidWorks, so NX-to-SolidWorks STEP transfers tend to be the most reliable — the source and target kernel speak the same geometric language. NX supports advanced AP242 features including semantic PMI.

CATIA helped develop the STEP standard, and SolidWorks’ STEP translator inherits Dassault’s CATIA-derived infrastructure. CATIA limits revolved surfaces to 180 degrees, which forces trimmed or partial representations that other systems may interpret differently.

FreeCAD uses OCCT’s STEPCAFControl_Writer with explicit control over precision, pcurves, and surface conversion. FreeCAD does not yet support AP242 Edition 2/3/4 (tracked as OCCT issue), creating compatibility gaps with newer STEP files from commercial systems. A known bug requires setting a dummy color on hidden assembly components to avoid a crash in STEPCAFControl_Writer.

Success with STEP exchange comes from understanding that “neutral” doesn’t mean “lossless” — each kernel’s tolerance regime, surface representation choices, and trimming curve parameterizations leave fingerprints on the STEP file.

Common Use Cases and Applications

STEP files shine in scenarios requiring reliable geometric data exchange:

Manufacturing Handoffs

When designs move from engineering to manufacturing, STEP files carry both geometric and specification data. A machined part exported as AP214 STEP can include surface finish requirements, tolerances, and material specifications with the 3D geometry. Our CAD file conversion for manufacturing guide covers format selection and metadata preservation in detail.

Multi-CAD Collaboration

Teams using different CAD systems depend on STEP for design reviews and collaborative development. An automotive supplier using CATIA can share components with an OEM using NX through STEP exchange without losing geometric accuracy.

Supplier Communication

STEP files create clear communication with external suppliers who may use different CAD systems. The standardized format reduces misinterpretation and ensures manufacturers get complete geometric information.

Design Archives

STEP provides a future-proof archival format independent of specific CAD software versions. Designs stored as STEP files stay accessible even if the original CAD system becomes obsolete.

Simulation and Analysis

Many FEA and CFD packages accept STEP files directly, enabling smooth transfer from design to analysis without geometric cleanup or rebuilding.

Working with STEP Files: Best Practices

Effective STEP workflows need attention to export settings, file organization, and quality checks:

Export Configuration

Pick the right Application Protocol for your needs. Use AP203 for general geometric exchange and AP214 when manufacturing information matters. Keep units consistent between export and import systems to avoid scaling problems.

Quality Verification

Always check STEP file quality after export. Open the file in your CAD system to confirm geometry transferred correctly. Look for missing features, simplified surfaces, or broken assembly relationships that could affect downstream work.

File Management

Create naming conventions that identify STEP file content and revision level. Include AP version in filenames when working with multiple protocols. Keep STEP files organized alongside native CAD files to maintain design history.

Batch Processing Considerations

For teams handling multiple STEP exports regularly, automation tools can reduce manual work and ensure consistent export settings. This proves especially valuable in manufacturing environments where design changes trigger multiple supplier updates. Learn how CadShift helps engineering teams automate repetitive workflows including STEP export.

Advantages and Limitations

STEP files offer significant benefits but have inherent limitations — and some of those limitations are more nuanced than they appear:

Key Advantages

Universal compatibility enables exchange between any STEP-supporting CAD systems without vendor lock-in. Standardized format ensures consistent interpretation across different platforms and software versions. Rich data support allows transfer of both geometric and manufacturing information in one file. Future-proof archival provides long-term accessibility independent of specific software. Analytic surface preservation — unlike mesh formats, STEP can carry exact geometric definitions (CYLINDRICAL_SURFACE, TOROIDAL_SURFACE) that maintain dimensional precision across systems.

Notable Limitations

Parametric loss happens during STEP export — parametric relationships and design history don’t transfer, leaving you with static geometry. A fillet that was a single parametric feature with a radius value becomes a trimmed B-spline surface with no memory of what created it.

Kernel-dependent geometry means the same nominal shape produces different STEP files depending on which kernel exported it. The NURBS representation of a fillet surface from Parasolid will have different control points, knot vectors, and degree than the same fillet from OpenCASCADE — both approximate the same shape, but they’re not bit-identical.

Tolerance regime mismatch is the root cause of most STEP interoperability failures. A model that’s airtight in Parasolid (1e-6 mm edge tolerance) may have detectable gaps when imported into an ACIS-based system with coarser tolerance. The STEP file’s UNCERTAINTY_MEASURE_WITH_UNIT declares precision, but each kernel computes and interprets this value differently.

Feature simplification may convert complex parametric features into basic surfaces or solids. Conic-profile fillets (SolidWorks’ rho parameter) export as NURBS surfaces — if the receiving system tries to edit the fillet, the conic shape information is lost and it reverts to a standard circular profile. (See our kernel fillet comparison for why this happens.)

File size can grow large for complex assemblies due to the text-based format structure. STEP files are ASCII, and the numerical representation of B-spline surfaces with many control points can be verbose.

Version compatibility issues may arise when newer AP versions aren’t supported by older CAD systems. FreeCAD’s OCCT backend doesn’t yet support AP242 Edition 2/3/4, creating gaps with files from commercial systems.

What Happens After Import: Geometry Healing

Because different kernels write STEP files with different tolerance regimes and surface representations, every major CAD system includes geometry healing tools that run during or after STEP import. Understanding what these tools do — and why they exist — explains many “my STEP file looks wrong” problems.

OpenCASCADE’s ShapeFix framework (used by FreeCAD) runs several repair passes:

• ShapeFix_Wire::FixConnected() forces adjacent edges to share vertices, increasing tolerance up to read.maxprecision.val (default 1.0 mm)
• ShapeFix_Wire::FixLacking() detects gaps between parametric curves and compensates through tolerance increase or degenerated edge insertion
• ShapeFix_Wire::FixSelfIntersection() increases vertex tolerance or cuts edges at intersection points
• ShapeFix_Edge handles incorrect SameParameter flags where curve deviation exceeds edge tolerance

The read.maxprecision.mode setting is critical: in “preferred” mode (the default), OCCT can exceed the stated maximum tolerance to ensure shape validity. In “forced” mode, tolerance is rigidly capped — which may produce geometrically invalid shapes with gaps.

SolidWorks’ Import Diagnostic Tool detects and repairs faulty faces, gaps between faces, and invalid edges in imported STEP geometry. The tool runs after Parasolid’s own import healing, catching issues that the kernel’s automatic repair missed.

Inventor’s ATF consumer uses ATF::STEPConsumerOptions::SetTolerance() and the SplitAllPeriodicSurfaces option during import. The consumer-side tolerance setting is separate from the producer-side uncertainty written to the file — import tolerance can be tighter or looser than what the STEP file declares.

The fact that every CAD system ships geometry healing tools for STEP import tells you everything about the state of “neutral” format interoperability. A solid that displays correctly after import may still have topological defects invisible on screen — gaps between faces, self-intersections, degenerated edges — that only surface during FEA meshing, CNC toolpath generation, or further boolean operations.

STEP vs. Other CAD Formats

Understanding when to use STEP versus alternatives helps optimize your data exchange strategy — especially now that you understand the kernel-level translation that STEP export involves:

STEP vs. IGES: STEP provides better data integrity and supports newer geometric types. IGES remains useful for legacy system compatibility but offers less robust data transfer. Both formats involve kernel-to-neutral translation, but STEP’s entity-based structure preserves topology more reliably than IGES’s geometry-only approach.

STEP vs. Parasolid (.x_t): Parasolid files maintain machine-precision geometry with per-edge tolerances — no translation loss, because SolidWorks and NX read Parasolid natively. But only Parasolid-based systems (SolidWorks, NX, Solid Edge) can read them. If your downstream tool uses Parasolid, .x_t avoids the entire kernel-to-STEP translation problem. If it doesn’t, you need STEP. The tradeoff is between geometric fidelity and compatibility.

STEP vs. STL: STL files work well for 3D printing and rapid prototyping but contain only mesh data. STEP preserves exact geometric definitions needed for manufacturing and further design work.

STEP vs. Native Formats: Native CAD formats (.sldprt, .ipt, .prt) maintain full parametric capability within their ecosystem but can’t be opened by other CAD systems.

For a deeper comparison of these formats, see our complete guide to converting CAD files between formats.

Future of STEP Format

The STEP standard keeps evolving to meet modern engineering needs. AP242, the latest major revision, introduces support for model-based definition (MBD) workflows where 3D models carry complete manufacturing information without separate 2D drawings.

New developments include better support for additive manufacturing data, enhanced material property definitions, and improved integration with PLM systems. These advances position STEP to stay relevant as engineering workflows become increasingly digital and collaborative.

The format’s standardized foundation and international governance ensure continued development aligned with industry needs, making STEP a reliable long-term choice for CAD data exchange.

Optimizing Your STEP Workflow

Successful STEP implementation requires a systematic approach to file handling and quality management. Start by standardizing export settings across your team to ensure consistent results. Document which Application Protocol works best for different use cases in your workflow.

Set up verification procedures that catch transfer issues early. This might include automated geometry checking or manual review protocols depending on your quality requirements. For high-volume operations, consider tools that can batch-process STEP exports with consistent settings.

Regular training on STEP capabilities helps teams leverage the format’s full potential while avoiding common pitfalls. Understanding when STEP provides the best solution versus alternative formats prevents unnecessary complications in your data exchange workflows.

Conclusion

STEP files represent one of engineering’s most successful standardization efforts, but “standard” doesn’t mean “identical.” The same part modeled in SolidWorks, Inventor, and FreeCAD will produce three different STEP files — not because the standard is broken, but because each geometric kernel (Parasolid, ShapeManager/ACIS, OpenCASCADE) makes different decisions about surface representation, tolerance, and trimming curve parameterization during the translation from internal B-Rep to ISO 10303 entities.

For simple prismatic geometry, these differences are negligible — well within any reasonable manufacturing tolerance. For complex curved surfaces — fillets, blends, lofted features — the differences can be measurable. Understanding that a STEP file carries the fingerprints of the kernel that created it helps you make better decisions about export settings, import verification, and when to use kernel-native formats (like Parasolid .x_t) instead.

Whether you’re coordinating with suppliers, archiving designs, or collaborating across different CAD systems, the practical advice is: always verify critical dimensions after STEP import, understand your sending and receiving kernel’s tolerance regimes, and use the appropriate AP protocol for your data requirements. The format’s continued evolution — particularly AP242’s MBD capabilities — ensures STEP will stay relevant, but it will never be truly lossless as long as different kernels have different ideas about what “the same shape” means.

For engineering teams looking to streamline their CAD workflows and reduce manual export processes, automated solutions can help maintain consistent STEP file quality while reducing repetitive tasks. Learn more at Cadshift.com.

This analysis draws on decompilation of SolidWorks 2025 (pskernel.dll, sldstepu.dll, catssdstepform.dll), Autodesk Inventor 2026 (Trans.dll, atf_step_producer.dll, stp_aim_x64_vc15.dll, ASMKERN231.dll), and FreeCAD source code (STEPControl_Writer, STEPCAFControl_Writer, ExportOCAF2). For more on how kernel differences affect specific operations, see our fillet kernel comparison and our guide to converting CAD files without losing data integrity.