Working with SolidWorks, Inventor, AutoCAD, Rhino and Blender Users

Overview#

Very few teams use a single tool. A Fusion user sends brackets to a SolidWorks shop, receives enclosures from an Inventor-based customer, hands flat patterns to an AutoCAD drafter, trades surfaces with a Rhino designer, and gets organic shapes from a Blender artist. Each pairing has its own habits, its own preferred formats and its own typical failures. This page gives you a recipe for each.

Everything here rests on three principles:

1. Exchange the lowest-common-denominator that preserves what the other person needs. Usually STEP for solids, DXF for 2D, 3MF/OBJ for meshes.
2. Agree conventions up front: units, origin, orientation, file naming, and revision flow.
3. Never let a translated copy replace your master. The master stays in its native system.

Which native formats Fusion can read or write depends on release and license; Autodesk groups formats into tiers, and a few (such as DWG) are not available on Personal use. Verify in your version.

Where to find it#

Step by step#

Collaborating with a SolidWorks user#

Receiving.

1. Ask for the part or assembly in native SLDPRT/SLDASM with all referenced files (use SolidWorks' Pack and Go to collect everything into one folder or zip), plus a STEP file as a backup.
2. Upload the folder to Fusion. Select the top-level assembly when prompted.
3. Check units, compare mass properties with the sender's values, and verify that components are present.
4. Expect no mates and no feature tree. Rebuild joints if you need motion. Configurations in SolidWorks parts typically translate as the active configuration only. Ask the sender for each configuration you need as a separate file.

Sending.

1. Export STEP (AP214 if the sender specifically asks; otherwise whatever Fusion writes by default; verify in your version).
2. Mention units and origin. Tell them it contains no feature history.
3. For sheet metal, include a flat pattern DXF; SolidWorks will not interpret Fusion's sheet metal intelligence.
4. SolidWorks reads STEP into a part or assembly; it may create a single imported body with no features. If they expect to edit it, advise them to use their Feature Recognition tool or rebuild.

Collaborating with an Inventor user#

Inventor is the closest relation: it is an Autodesk product, and Fusion reads IPT and IAM files, and may export to Inventor-compatible formats on some tiers.

Receiving.

1. Ask for an IAM with Pack and Go (Inventor's equivalent) so that all referenced files and the project context are included.
2. Upload the folder. The translator handles the Inventor project's relative paths when the folder structure is preserved.
3. Expect geometry and assembly structure; do not expect iMates, iLogic, derived components, or parametric relationships to survive.
4. For sheet metal parts, flat patterns can be recomputed in Fusion's sheet metal workspace when the part imports with its sheet metal features; often it imports as a plain solid. Verify in your version.

Sending.

1. STEP is safest. SMT or SAT also work well between Autodesk kernels.
2. If an Inventor-format export is offered in your tier, test it with the recipient before relying on it.
3. Tell the recipient to use the Import option in Inventor with Convert to solid / Reference to keep the model lightweight.

Collaborating with an AutoCAD user#

AutoCAD users generally want 2D: DWG or DXF.

1. For a profile, right-click the sketch and Export DXF. Ask the recipient which AutoCAD release (the DXF version) they need; some modern exporters write recent versions that older AutoCAD cannot open. If Fusion offers no version choice, ask the recipient to open it in a newer viewer such as Autodesk's free tooling and save down.
2. For drawings, use Export DWG or Export DXF from the Drawing workspace. Layers, line types and dimension styles are partially preserved; see the drawings section for detail. DWG output availability depends on license; verify in your version.
3. Units: DXF header units are unreliable. State them in your message ("millimeters, 1:1").
4. Receiving DWG: use Insert DXF (or Insert > Insert DXF/DWG if labeled) to bring 2D geometry into a sketch. 3D DWG solids (ACIS) may come in through Upload; test.
5. For 3D, AutoCAD can read SAT and STEP (from recent versions). Check with the recipient's release.

Collaborating with a Rhino user#

Rhino is NURBS-surface oriented. Designers love it for freeform surfaces, and then need solids from you or want your solids for rendering.

Receiving.

1. Ask for STEP or IGES, or a 3DM through Upload if your tier supports it. Ask them to ensure surfaces are joined into closed polysurfaces (the Rhino command Join, then ShowEdges to find naked edges).
2. In Fusion the result may arrive as surfaces. Use Stitch with a suitable tolerance to make solids.
3. Rhino's file tolerance is often looser than manufacturing CAD expects; expect to repair gaps.
4. Untrimmed or highly degree NURBS surfaces can be heavy. Ask for rebuilt or lighter surfaces if performance suffers.

Sending.

1. Send STEP for solids; they'll arrive as polysurfaces in Rhino.
2. For rendering in Rhino, a mesh export (OBJ) may be better.
3. IGES is accepted by Rhino and sometimes handles surface sets more gracefully than STEP; try both.

Collaborating with a Blender user#

Blender is a mesh application. Its users deal in OBJ, FBX, glTF, STL and sometimes USD.

Sending to Blender.

1. Right-click the body and Save As Mesh to OBJ (or use File > Export for FBX).
2. Choose refinement high enough that curved surfaces do not show facets after smoothing.
3. State the unit. Blender by default uses meters; scale at import if your file is millimeters (scale factor 0.001).
4. Expect to need to fix orientation: Blender is Z-up, and Fusion's default modeling orientation is also Z up; if you changed it to Y up, tell the artist or change it back before exporting.
5. For photorealistic work, many people render in Fusion first. If Blender is required, consider exporting each material region as separate bodies so materials can be assigned.

Receiving from Blender.

1. Ask for an applied-modifier mesh, scaled (apply scale), in meters or millimeters as agreed, with normals consistent and manifold geometry if it will be printed (Blender's 3D-Print Toolbox add-on helps).
2. Insert as a mesh; repair; use for reference or print. Converting artistic meshes to solid CAD is rarely sensible.

Options reference#

Tips and pitfalls#

Tip: A one-page "exchange spec" saves hours: file formats, unit, origin, revision naming, return channel. Include it in the first email.

Tip: Ask for both native and neutral. If both open well, compare them; if only one opens well, you have your answer.

Tip: Document critical dimensions in a drawing PDF. Even if geometry translates perfectly, the PDF is the contract.

Warning: Do not trust assembly motion or constraints to travel. Rebuild or document them.

Warning: Sending native Fusion files to non-Fusion users is useless; sending F3D to a Fusion user is fine, and often better than STEP. Don't forget that Fusion users can use shared links to view, comment and download.

Warning: Beware of version skew. A SolidWorks 2026 file may not translate if Autodesk's translator lags behind. Ask for an older save-as or a neutral file. Verify supported versions in the current help.

Warning: Check licensing and confidentiality before uploading a client's native files to a cloud service, particularly under export-control or NDA terms.

Practice exercise#

1. Pick one pairing relevant to you (for example, SolidWorks).
2. Write an exchange spec of five lines covering formats, units, origin, orientation and revision naming.
3. Using a sample part, export from Fusion in the recommended format, then open it with the other tool or a free viewer for that ecosystem (FreeCAD, an eDrawings viewer, Blender, a DXF viewer).
4. Record three differences you notice and one fix.

Expected result: a reusable, tested exchange spec for that pairing.

Related#

• STEP best practices (step-best-practices)
• Mesh vs BRep exchange (mesh-vs-brep-exchange)
• Format cheat sheet (format-cheat-sheet)
• Export PDF, DWG, DXF from drawings (10-drawings-documentation/export-pdf-dwg-dxf)