# IGES files

Exchanging IGES geometry with explicit translator settings, units, body expectations and post-import checks.

Reviewed: 2026-11-01

Tags: parts-and-design, file-formats, cad

IGES exchanges curves, surfaces and solids. Check which representations the exporter and receiver support.

IGES is not limited to disconnected surfaces. SOLIDWORKS **2025** documentation describes import/export of surfaces and BREP solids. Its entity list includes rational B-spline curves (126), rational B-spline surfaces (128), trimmed parametric surfaces (144) and manifold solid B-rep objects (186). Some entities are import-only in that translator. The presence of an entity in the specification therefore does not establish two-way support in a particular application. [SOLIDWORKS 2025, IGES Files](https://help.solidworks.com/2025/English/SolidWorks/sldworks/c_IGES_Files_igs_iges.htm?id=921109670b424a4093082c036aecc98a)

Version matters, but translator support matters too. NIST's **April 2003 NISTIR 6972**, *Initial Graphics Exchange Specification, Volume 2: Application Protocols*, lists IGES 5.3 as the 1996 version. The current OCCT 8.0.1 translator guide explicitly identifies its writer output as IGES 5.3, ANS US PRO/IPO-100-1996. Do not read a file's recent creation date as a new specification edition. [NISTIR 6972](https://nvlpubs.nist.gov/nistpubs/Legacy/IR/nistir6972.pdf), [Open CASCADE Technology 8.0.1, IGES Translator](https://occt3d.com/dev/doc/overview/html/occt_user_guides__iges.html)

## Geometry representation and entity support

| Representation | What the receiver must establish |
| --- | --- |
| Wireframe curves | Intended curve content, continuity and coordinates |
| Individual/trimmed surfaces | Complete boundaries, valid trims and expected surface count |
| Sewn shell or solid | Closure, orientation, valid topology and intended body count |
| Multiple components | Correct inclusion, placement and required separation |

A collection of surfaces may visually enclose a volume without forming a valid closed solid in the receiving kernel. Conversely, a valid surface model may be exactly the required deliverable. State the expected result instead of treating every surface body as a translation failure.

The OCCT guide says its processor recognizes IGES 5.3 definitions but translates only 3D geometric entities; unhandled data is ignored with diagnostic messages. Colors and names use its XDE facilities, while administrative Global-section data is not transferred into the resulting OCCT geometry. This is a concrete translator limitation, not a statement that IGES itself cannot contain such information. [OCCT 8.0.1, IGES Translator](https://occt3d.com/dev/doc/overview/html/occt_user_guides__iges.html)

## Agree export options with the recipient

SOLIDWORKS 2025 offers trimmed-surface output (144), manifold-solid B-rep output (186) and 3D wireframe output. Its system-preference choices change the exported entity mix. A high trim-curve accuracy option can help a receiving system knit surfaces but increases file size. Record the chosen representation and recipient preference rather than assuming all IGES exports from the same CAD model are equivalent. [SOLIDWORKS 2025, Setting IGES Export Options](https://help.solidworks.com/2025/English/SolidWorks/sldworks/HIDD_EXPORT_OPTION_IGES.htm)

That documentation also provides assembly packaging and hierarchy-flattening options. SOLIDWORKS's IGES overview separately explains that resolving hidden/suppressed components during export determines whether they are included. Inspect the exported content; a complete-looking top-level assembly can still omit a hidden part. [SOLIDWORKS 2025, Setting IGES Export Options](https://help.solidworks.com/2025/English/SolidWorks/sldworks/HIDD_EXPORT_OPTION_IGES.htm), [IGES Files](https://help.solidworks.com/2025/English/SolidWorks/sldworks/c_IGES_Files_igs_iges.htm?id=921109670b424a4093082c036aecc98a)

Onshape's export help provides an IGES compatibility mode for surfaces and curves intended for legacy CAD/CAM systems. It also states that downloaded exports do not contain features or parametric history. A recipient may subsequently create new features from imported geometry, but that is not restoration of the original modeling sequence. Keep the native source if future design changes depend on sketches, constraints or feature relationships. [Onshape, Exporting Files](https://cad.onshape.com/help/Content/File/exporting_files.htm)

## Units, origin and precision

Record intended units, a known reference dimension and the coordinate-system convention with the delivery. Verify both geometry size and its position/orientation after import. A length-unit setting and an origin transform answer different questions: a correctly sized part can still be misplaced in an assembly or CAM setup.

OCCT's guide states that non-millimeter lengths are converted to millimeters during its IGES translation. It also explains that a user precision setting is a target for shape construction and cannot improve the original file's geometry quality. Increasing numerical precision or changing an import tolerance does not recreate missing design information. [OCCT 8.0.1, IGES Translator](https://occt3d.com/dev/doc/overview/html/occt_user_guides__iges.html)

**Original scale check:** suppose the source drawing identifies a reference edge as **2 inches**, or **50.8 mm**. After translation, measure that edge in the receiving application's declared units. A result of **2 mm** indicates a 25.4-fold scale discrepancy; a result of **50.8 mm** passes this one scale check. It does not establish that all faces, holes, placements or tolerances transferred correctly. Do not repair a suspected units problem merely by relabeling display units without checking what the operation does to geometry.

## Application-specific exclusions

Autodesk's **28 October 2026** Fusion support article states that its STEP/IGES exchange recognizes solids and surfaces, while sketches, mesh bodies and T-splines are not transferred through that route. This is Fusion's documented behavior, not a universal prohibition on IGES curves. SOLIDWORKS's separate curve support above illustrates the difference. A file that imports incompletely may reflect unsupported source content rather than a damaged file. [Autodesk Support, Exported STEP/IGES files with missing splines and sketches](https://www.autodesk.com/support/technical/article/caas/sfdcarticles/sfdcarticles/STEP-file-exported-from-an-OBJ-design-converted-in-Fusion-360-is-empty-or-incomplete.html)

Agree a supported representation before conversion. Converting a faceted mesh to a B-rep changes its data structure; it does not automatically restore the original analytic cylinders, smooth design surfaces or manufacturing intent.

## Translation and release checks

A practical handoff uses five checks:

1. Identify source revision, source/target applications and required transferred content.
2. Record IGES representation, relevant export/import options, units and coordinate convention.
3. Reopen the actual delivered file in the receiving system and inspect warnings or omissions.
4. Check known dimensions, placements, body/component count, surface closure and critical interfaces.
5. Compare repaired geometry with the intended design before releasing it for downstream work.

Keep the original file when healing or sewing. A repaired model may be useful, but changed trims, removed sliver faces or joined boundaries require review where they affect function. Visual similarity alone is insufficient for a tight-fit or sealing interface. If import yields only surfaces where a solid is required, diagnose missing faces, trimming and sewing conditions before repeatedly relaxing tolerances.

The file should accompany an unambiguous revision and the drawing or other agreed manufacturing requirements. Do not infer material grade, heat treatment, finish, geometric tolerances or inspection acceptance from geometry or color. Where product/manufacturing information must transfer digitally, agree and demonstrate the receiving workflow explicitly, using a different deliverable where necessary.

## Source versions

NISTIR 6972 prints April 2003. The cited SOLIDWORKS help is versioned 2025. OCCT's retrieved guide identifies **8.0.1**. Onshape help displays a last-updated date of **30 October 2026**. The Autodesk support article displays **28 October 2026**. These document versions define the examples, not every installed translator's behavior.

## Related reference

[Drawing and model file references](index.md)