To Import Files from Other CAD systems - Options Tab

Import CATIA, Solidworks, Pro-E/Creo, NX, JT, Alias, STEP, Iges, Rhino, SAT, Parasolid Binary files.

Translate files into Autodesk Inventor data

You can open or import part and assembly files from other CAD systems. You can also place part and assembly files as components into new or existing Autodesk Inventor assemblies (not available in Inventor LT).

1. To selectively import into file, do one of the following:
   • To import to a new file select:
     • File Open Import CAD Formats
     • Get Started tab Launch panel Import CAD Formats

     When you import a file, Inventor automatically detects whether the imported file is a part or assembly and creates the new document accordingly. For example, 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.

   • To import into a part file select:
     • Manage tab Insert panel Import
     • 3D Model tab Create panel Import
   • To import into an assembly, select Assemble tab Component panel Place Imported CAD (not available in Inventor LT).
2. In the applicable dialog box, set the Files of type to view the available files.
3. Select the file to import and click Open.

To edit the import options after importing, right-click on the file in the browser, and select Edit Import from the context menu.

Options tab

1. Specify the Import Type. Select one of the following:
   • Reference Model ( CATIA, Solidworks, Pro-E/Creo, NX, STEP, and Alias only): to maintain a link to the selected file which enables you to monitor and update as the model changes. Use this option if the design is evolving and you are not required to edit the referenced model (not available in Inventor LT).
   • Convert Model (CATIA, Solidworks, Pro-E/Creo, NX, JT, Alias, Rhino, IGES, STEP, Parasolid, and SAT files): to create a new Inventor file which is not linked to the original. Use this option if you plan modify the model for a new design.
2. The Object Filters section allows you to specify the type of geometry to import. Specify the type of geometry to import:
   Model Geometry

   • Solids imports solid bodies and water tight stitched shells as individual solid bodies.
   • Surfaces imports surface bodies.
   • Meshes imports meshes. Mesh data is for visualization purposes only.
   • Wires import wires.

   Work Geometry: imports the desired work geometry.

3. Inventor Length Units: In the Inventor Length Units field, specify the type of Inventor length units to use for the imported geometry and parameter values. The unit value selected only changes the length units for the new document. The length and other units for the document can be viewed in the Document Settings dialog box on the Units tab.
4. Reduced Memory Mode: Select Reduced Memory Mode only if you are translating a large data set and expect additional memory will be required to complete the operation. This setting increases memory capacity and decreases performance. Reduced Memory Mode minimizes memory consumption by saving each component to disk during the import process.
The following options are only available if Convert Model is selected as the Import Type. Specify how to import solids into the file:
• Assembly Options (not available in Inventor LT):
  • Assembly preserves the source structure.
  • Multi-body part imports an assembly as solid bodies in a single part.
  • Composite PartThe composites are created from the levels, layer, or groups. Each level, layer, or group is created as an individual composite feature that has the same name as the level, layer, or group it originates from. Each composite feature has its own browser node that is a child of the root node.
• Part Options
  • Composite imports the assembly as a single composite feature in the part environment.
  • Individual imports the assembly as a single composite feature in the part environment.
  • Stitch (IGES and STEP files only) stitches several edge-matched surfaces or faces together.
5. If applicable, provide a file name:
   • Provide a file name to avoid name duplication issues.
   • Specify a prefix or suffix to add to the file name.
6. Browse to specify where to save the file.
7. Click OK to import the file.

Import Alias files

The geometry is created in Inventor using the same colors as assigned in Alias. However, texture maps included in the Alias definition are not translated to the Inventor file.

Import CATIA V4 files

Open and change models created in CATIA V4 (all versions). Autodesk Inventor translates assembly and part files, solids, multi-solids, surfaces, and more. After the import operation is complete, you have a base feature or features which match the geometry and topology of the original file. Use Autodesk Inventor commands to adjust the base features and add new features to the feature tree.

These types of CATIA V4 files can be imported:

• *.model
• *.session
• *.dlv3
• *.exp
  Note: When you open a .exp file, Inventor displays the models it contains in the CATIA V4 Model Selection dialog box. Select the appropriate .model file to import and click OK.

If you select to import mesh data, Inventor creates mesh features and groups them under mesh folders in the browser. The mesh features are for visualization purposes only and cannot be modified. You can right-click the mesh features or folders to access the context menu and select to show mesh edges, change visibility, and more.

After changing the file, you can continue to open it in Autodesk Inventor.

Import CATIA V5 files

Open and change models created in CATIA V5 (R6 - V5-6R2015) Autodesk Inventor translates assembly and part files, solids, multi-solids, surfaces, and more. After the import operation is complete, you have a base feature or features which match the geometry and topology of the original file. Use Autodesk Inventor commands to adjust the base features and add new features to the feature tree.

These types of CATIA V5 files can be imported:

• *.CATPart (part)
• *.CATProduct (assembly)
  Note: Inventor automatically translates CATIA V4 files referenced by *.CATProduct files.
• *.cgr
  Note: Mesh data from .cgr files are for visualization purposes only.

If you select to import mesh data, Inventor creates mesh features and groups them under mesh folders in the browser. The mesh features are for visualization purposes only and cannot be modified. You can right-click the mesh features or folders to access the context menu and select to show mesh edges, change visibility, and more.

After changing the file, you can continue to open it in Autodesk Inventor.

Import JT files

Open and change models created in JT (*.jt) (versions 7.0, 8.0, 8.1, 8.2, 9.0, 9.1, 9.2, 9.3, 9.4, 9.5,and 10.0). Autodesk Inventor translates assembly and part files, solids, multi-solids, surfaces, and more. After the import operation is complete, you have a base feature or features which match the geometry and topology of the original file. Use Autodesk Inventor commands to adjust the base features and add new features to the feature tree.

Import Pro/ENGINEER and Creo Parametric files

Open and change models created in Pro/ENGINEER and Creo Parametric. Autodesk Inventor translates assembly and part files, solids, multi-solids, surfaces, and more. After the import operation is complete, you have a base feature or features which match the geometry and topology of the original file. Use Autodesk Inventor commands to adjust the base features and add new features to the feature tree.

These types of Pro/ENGINEER files can be imported:

• *.prt* (part) (up to version Wildfire 5.0 or Creo Parametric 1.0 - 3.0)
• *.asm* (assembly) (up to version Wildfire 5.0 or Creo Parametric 3.0)
• *.g (Granite) (up to version 9.0)
• *.neu* (Neutral)

Note: To import part or assembly files that contain family table instances, load your model into Pro/ENGINEER and save the accelerator files (.xpr or .xas) along with the Pro/ENGINEER part or assembly files. The accelerator files contain the specific instances referred to by the family table.

Import Parasolid files

Open and change models created in Parasolid (up to version 28.0). Autodesk Inventor translates assembly and part files, solids, multi-solids, surfaces, and more. After the import operation is complete, you have a base feature or features which match the geometry and topology of the original file. Use Autodesk Inventor commands to adjust the base features and add new features to the feature tree.

These types of Parasolid files can be imported:

• *.x_t (text)
• *.x_b (binary)

Import Rhino files

The import process supports up to version 5.0 and 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.

Import SolidWorks files

Open and change models created in SolidWorks (up to version 2016). Autodesk Inventor translates assembly and part files, solids, multi-solids, surfaces, and more. After the import operation is complete, you have a base feature or features which match the geometry and topology of the original file. Use Autodesk Inventor commands to adjust the base features and add new features to the feature tree.

These types of SolidWorks files can be imported:

• *.prt, *.sldprt (part)
• *.asm, *.sldasm (assembly)

Import NX files

Open and change models created in NX (formerly UGS NX) (versions Unigraphics 13 - NX 10.0). Autodesk Inventor translates assembly and part files, solids, multi-solids, surfaces, and more. After the import operation is complete, you have a base feature or features which match the geometry and topology of the original file. Use Autodesk Inventor commands to adjust the base features and add new features to the feature tree.

These types of NX files can be imported:

• *.prt (part)
• *.prt (assembly)

Import STEP or IGES files

You can import a STEP (versions AP214, AP203E2, and AP242) or IGES (all versions) file. The solid body is saved in an Autodesk Inventor file, and no links are maintained to the original file.

If an imported STEP or IGES file contains one part, it produces an Autodesk Inventor part file. If it contains assembly, it produces an assembly with multiple part files.

Note: By default, Autodesk Inventor applies the part name (file name of the inserted part) to browser file nodes. Other CAD systems might apply the part number property. When a STEP or IGES file is imported into Autodesk Inventor, its name might differ from that of the CAD system which generated the STEP or IGES file. To avoid confusion, use the Rename Browser Nodes command to specify the browser node naming scheme.

Note: STEP file part numbers translate to the Part Number field in the iProperties Project tab of an Autodesk Inventor Part document.

See Assembly Tools for more information about the Rename Browser Nodes command.

Import SAT files

You can import an SAT file (versions 4.0 - 7.0). The curves, surfaces, and solids are saved in an Autodesk Inventor file, and no links are maintained to the original file.

If an imported SAT file contains a single body, it produces an Autodesk Inventor part file with a single part. If it contains multiple bodies, it produces an assembly with multiple part files.

Import SMT files

You can import an SMT file type extension from Autodesk Shape Manager (ASM) that can be used for interoperability operations among Autodesk products.