About Importing Files from other CAD Systems

Files from other CAD systems can be imported for use in Inventor using the Import CAD Formats command. The file type determines the available options. For example, you can choose to import some file types as:

When you import a file, Inventor automatically detects whether the imported file is a part or assembly and creates a new document accordingly. You can then preview and select imported items. To import a 3rd party assembly file as a part, you must first create or have a part file open, and then import the 3rd party assembly file into the part file.

Some file types do not support the Reference model. Choose the workflow that works best for your design.

Note: Imported AutoCAD DWG files automatically maintain associativity to the corresponding DWG file in AutoCAD. When the original DWG file is updated in AutoCAD, the corresponding Inventor files will be updated accordingly, either for geometry change or position change.

Import as Reference Model: (Alias, CATIA, Solidworks, NX, and Pro-E/Creo files)

If the design is changing and you are not required to edit the referenced model, take control and improve performance by importing the design as a Reference Model.

Envision an engineering environment in which a standard keyboard design was created as a surface model by an industrial designer using a different CAD program, such as Solidworks. The Solidworks geometry is translated (imported) into Autodesk Inventor as a Reference Model into an assembly file. Importing the file as Reference Model establishes direct associativity between the Solidworks file and the Inventor file. Additional design enhancements are made to the original Inventor geometry using Autodesk Inventor modeling commands: A new part is placed into the assembly and constrained to the imported geometry.

Meanwhile, the industrial designer continues to modify the Solidworks design into a more organic, ergonomic shape. The Update icon on the Quick Access toolbar indicates that the original imported file was edited since it was initially imported into Inventor. Now the Autodesk Inventor part file is no longer in sync. Clicking the Update icon loads the revised imported file and incorporates the changes.

Important: When you import geometry as Reference model no additional files are created on disk.

Depending on whether you import into a part or assembly file determines what type of modeling edits you can make:

Import into a Part file
  • Supported:
    • The imported geometry can be edited and parameter features can be added.
    • All "Copy to" workflows.
  • Not supported:
    • Solid Edit is disabled.
    • Repair Environment is disabled.
Import into an Assembly file
  • Supported:
    • Add additional parts or make changes to original Inventor geometry: For example, create constraints to the imported geometry.
    • Reposition and make other cosmetic type changes to the imported geometry.
    • Add top level assembly features.
    • Design View workflows.
    • Management of BOM Structure.
  • Not supported:
    • You cannot modify the imported geometry.
    • You cannot create a BOM or parts list from items excluded from Import.
    • You cannot modify the imported geometry or change the structure of the imported components.
    • You cannot mirror the imported components.

Selective import into Part and Assembly files (CATIA, Solidworks, Pro-E/Creo, NX, Alias, Step, Iges, and Rhino only)

If you do not need to import an entire model, you can specify which bodies (into a part file) or which parts (into an assembly file) to include. Import only the components you need to improve performance.

Importing as Convert Model (CATIA, Solidworks, Pro-E/Creo, NX, JT, Alias, Rhino, IGES, Parasolid, and SAT files)

The Convert Model option creates new Inventor files which are not linked to the original. Use this option if you plan modify the model for a new design.

The import operation does not maintain associativity with the original file. As a result, changes to the original file after the import operation do not affect the imported part or assembly. Likewise, changes to the imported part or assembly do not affect the original file.

When assemblies are imported, Inventor attempts to preserve the assembly and subassembly structure of the original file.

The import process creates base features in Inventor representative of the geometry and topology in the source file. You can use Inventor commands to adjust the base features and add new features to the Inventor feature tree. You cannot modify the original definition of the base features.

Importing DWG files

The following workflows are available for importing

You can import an AutoCAD or Mechanical Desktop DWG file using the DWG/DXF File Wizard. Similar to the Reference Model described above,

To open an AutoCAD file directly as an Associative DWG , click Open in the Import dialog box.

Importing DXF, STL, Revit, DWF Markup, and IDF files

Similar to the Convert Model option described above, the import operation for these file types does not maintain associativity with the original file. Additional import options are available for these file types.

For example, a translation report is generated that includes information pertinent to the import process. You can save the report to disk, in HTML format, and embed the report in your new part or assembly document.

Supported File Import Formats

The following are the supported direct translators and import file formats.

Translator Import Export
Alias V10 or later  
CATIA V4 All Revisions  
CATIA V5 R6 - V5-6R2014 R10 - V5-6R2014
Creo Parametric 1.0; 2.0; 3.0  
IGES All Revisions 5.3
JT 7.0 – 10.0 7.0 – 10.0
NX Unigraphics V13 - NX 9  
Parasolid Up to 27.0 9.0 - 27.0
Pro/ENGINEER Up to Wildfire 5.0  
Pro/ENGINEER Granite Up to 9.0 1.0 - 9.0
Pro/ENGINEER Neutral N/A N/A
Rhino Up to 5.0  
SAT Up to 7.0 7.0
SolidWorks 2001 Plus – 2015  
STEP AP214, AP203E2, AP242 AP214, AP203E2, AP242
STL N/A N/A
XGL/ZGL   N/A

The following table lists those file formats supporting Selective and Associative updates and which is supported.

Format Version Selective Import Associative Update
CATIA V5 V5-6R2014
CATIA V4 All  
PTC Creo Up to 3.0
PTC Wildfire Up to 5.0
SolidWorks Up to 2015
Siemens NX v3 - v9
Alias v11 - 2016
AutoCAD 2d Up to 2016  
Rhino All  
STEP All  
IGES All  
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