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Importing Pro/ENGINEER and Creo Parametric Part Files
Importing Pro/Engineer and Creo Parametric Assembly Files
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Importing Pro/Engineer and Creo Parametric Assembly Files

To import a Pro/ENGINEER or Creo Parametric assembly file into SolidWorks:

  1. Click Open (Standard toolbar) or File > Open.
  2. In the dialog box, set Files of type to ProE/Creo Assembly (*.asm;*.asm.*;*.xas).
  3. Browse to a file, and click Open.
  4. In the Pro/E & Creo to SolidWorks Converter dialog box, set these options:
    Option Description
    Component Import Options Select one of the following:

    Use feature import for all parts

    Imports all component parts as features.

    Use body import for all parts

    Imports all component parts as bodies.

    • BREP. Imports the model as a solid using Boundary Representation data. In general, BREP mode is faster than Knitting, especially for complex models.
    • Knitting.
    • Do not knit.

    Prompt for each part

    Prompts you to import each individual component as a feature or a body.

    If same name SolidWorks file is found:
    • Use Existing. Does not import the new file.
    • Overwrite.
    • Save with new name.
    Import material properties  
    Import sketch/curve entities  
    Import component constraints (Mates) Pro/E and Creo constraints are translated into SolidWorks assembly mates. All the basic types, plus Pro/ENGINEER Point on Surface, Point on Edge, and Edge on Surface constraints are supported. Only Pro/E and Creo high level motion constraints such as Gear mates are not supported.
  5. Click Import.

    SolidWorks converts and imports the file.

    If you selected Prompt for each part in the Component Import Options section, SolidWorks redisplays the Pro/E &Creo to SolidWorks Converter dialog box.

  6. Set these options:
    Option Description
    Import geometry directly Imports a model without features, either as a solid or as surfaces.
    • BREP. Imports the model using Boundary Representation data. In general, BREP mode is faster than Knitting, especially for complex models. BREP attempts to import the model as a solid.
    • Knitting. Attempts to knit surfaces during import. Select Try forming solid model(s) to try to form solids using Knitting mode. Otherwise, the models are imported as surface bodies.
    • Do not knit.
    Analyze the model completely Determines the number of features that SolidWorks can recognize and import.
    Import material properties  
    Import sketch/curve entities  
  7. Click OK.

    If you select Import geometry directly, SolidWorks imports the model. If you select Analyze the model completely, SolidWorks parses the imported file and redisplays the Pro/E & Creo to SolidWorks Converter dialog box with the following options:


    Imports the model and attempts to recognize features. Attempt to correct invalid features attempts to correct problems such as reversed extrusions.


    Attempts to import the model as a solid using Knitting. Attempt to correct invalid feature has no effect.

    Generate translation report

    If you select Features, generates a report that includes the features plus the recognition and import status.

  8. Click Features or Body to import the model component.
  9. In the Translation Report:
    • Print
    • Copy
  10. Close the dialog box.

    SolidWorks imports the component. The Pro/E & Creo to SolidWorks Converter dialog box prompts you to import the next component.

  11. Continue importing components until you have imported the entire assembly.

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