Why exporting to STEP or IGES doesn't hand the next engineer an editable copy of your model — it hands them the shape, not the recipe that built it.
A mechanical engineer emails a SolidWorks part to a supplier who runs CATIA, and is surprised when the imported file shows up as a single gray blob they can't edit — no sketches, no extrude, no fillet parameter to bump from 3 mm to 5 mm. Nothing went wrong. That is exactly what a neutral CAD format is supposed to do: carry the finished shapeacross a vendor boundary that has no shared understanding of how either company's CAD kernel builds features. The feature tree — the sequence of sketches, extrudes, fillets, and patterns that make a part editable and parametric — is native-format-only. STEP and IGES were never designed to carry it.
SolidWorks, CATIA, Creo, NX, and Inventor each build a solid using their own internal feature tree structure, their own sketch-solver, and often their own geometric kernel (Parasolid, ACIS, CGM, Granite). None of those vendors agree on how a "fillet feature" should be represented internally, so a format that tried to carry feature history across vendors would need every CAD kernel on earth to agree on a common feature language — which has never happened. STEP and IGES sidestep the problem entirely: instead of describing how the shape was built, they describe only whatthe shape is — a boundary representation (B-rep) made of trimmed surfaces, edges, and vertices that any kernel can rebuild geometrically, without needing to understand the other program's features at all. That is the entire trade being made: give up editable history, gain universal portability.
Neither half of that is right. First, STEP does not preserve design intent in the parametric sense — it preserves the finished geometry, not the sketches, dimensions, or feature order that produced it (some STEP AP242 files can carry PMI/GD&T annotations and semantic assembly structure, which is real progress, but that is still not an editable feature tree). Second, STEP and IGES are not equivalent neutral formats. IGES, standardized in the early 1980s, typically represents a part as a collection of independent trimmed surfaces rather than a single closed solid — surfaces frequently don't meet edge-to-edge with the numerical precision needed to form a watertight body, which is why IGES imports so often need "surface healing" or manual stitching before they behave like a solid at all. STEP (ISO 10303, especially AP203/AP214/AP242) represents a proper B-rep solid with defined topology, which is why it imports far more reliably as one clean, watertight body. For that reason most CAD teams now treat STEP as the default exchange format and IGES as a legacy fallback for old files or old partner systems that predate STEP support.
Explains the real distinguishing feature between native CAD files and neutral exchange formats like STEP and IGES — not file size or visual fidelity, but whether the editable feature tree survives the transfer — using a side-by-side comparison of a native round-trip (SolidWorks, Inventor, CATIA) and a STEP/IGES export-import cycle into a different CAD system.
Because a STEP file often looks identical to the native part on screen — same dimensions, same surfaces, same mass properties — it is easy to assume the file is functionally equivalent to the native one. It is not. Visual and dimensional fidelity is exactly what a good B-rep exchange format is supposed to deliver; parametric editability is a completely different property that neutral formats were never designed to carry. The confusion usually surfaces the first time someone tries to change a dimension on an imported STEP body and discovers there is no sketch to edit — only a "dumb solid" that supports direct face/edge editing at best.
Native formats (.SLDPRT/.SLDASM, .IPT/.IAM, .CATPart/.CATProduct, .PRT, .F3D) store the full parametric history: sketches with dimensional constraints, feature operations (extrude, revolve, fillet, pattern, shell), the order they were applied in, and often design tables, custom properties, and PMI.
STEP (ISO 10303, .stp/.step) stores a boundary-representation solid — the geometric result — plus, depending on the Application Protocol used (AP203 basic geometry, AP214 automotive/PMI, AP242 the current combined standard), optional assembly structure, part metadata, and semantic PMI/GD&T annotations. What it does not store, in any AP, is the feature tree.
IGES (.igs/.iges), an older ANS/US Product Data Association standard from the early 1980s, represents geometry as a set of independent trimmed surface and curve entities rather than a guaranteed single watertight solid. It is more prone to gaps between adjoining surfaces than STEP, which is why most modern CAD workflows have shifted to STEP as the default and keep IGES mainly for legacy compatibility.
Mesh formats like STL and OBJ are a further step down — they store only a triangulated approximation of the surface, with no true B-rep topology at all, which is fine for 3D printing but unsuitable for most downstream CAD or precision manufacturing work.
Anywhere two organizations on different CAD platforms need to exchange a design — an OEM sending a mating part to a supplier, a contract manufacturer receiving a customer's model for CAM programming, or an engineer archiving a design in a format that will still open in twenty years regardless of which CAD vendor still exists. The practical takeaway is to always keep the native file as the editable master and treat every STEP/IGES export as a disposable, re-generatable snapshot — never the only copy of a design that still needs to change.
No — not unless someone also sends you the native file. Once a model has been exported to STEP or IGES, the original sketches, extrude depths, and fillet radii are gone from that file; some CAD systems can auto-recognize features (fillets, holes, bosses) on an imported dumb solid to make it easier to edit, but that is a best-effort reconstruction, not the original parametric history.
It is a middle case. Parasolid is a geometric modeling kernel used natively inside several CAD systems (including SolidWorks and NX), so a .x_t file carries a clean B-rep solid similar to STEP — but because several major CAD products share that exact kernel, a Parasolid export can sometimes retain more fidelity between those specific programs than a STEP export would. It still does not carry a generic feature tree the way a native SLDPRT does.
IGES represents a part as independent trimmed surfaces rather than a topologically closed solid, so numerical tolerance mismatches between adjoining surface edges are common — the receiving CAD system has to stitch ("sew" or "heal") those surfaces back together within a tolerance, and sometimes cannot close every seam automatically. STEP's explicit solid topology makes this failure mode far less common, which is the main practical reason STEP has largely superseded IGES.
For basic geometry exchange, AP203 is the oldest and most universally supported. AP214 added color, layer, and some PMI support aimed at automotive workflows. AP242, the current combined standard, is the best choice when the receiving system needs semantic PMI/GD&T, assembly structure, or long-term archival — most modern CAD systems default to it or offer it as an explicit export option.
Not meaningfully for geometry — a well-formed STEP export preserves exact analytic surface definitions (planes, cylinders, NURBS) to the tolerance the exporting system used, so the resulting solid is not an approximation the way a mesh (STL) is. What is lost is not geometric accuracy but parametric structure: the "why" behind the shape, not the shape's dimensions.
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