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Pro/ENGINEER / Creo Elements>> SolidWorks

The following settings are recommended up to Pro/ENGINEER Wildfire 5.0 Elements Creo Parametric 3.0 and SolidWorks 2016.

Pro/ENGINEER – System

  • From the view of data exchange it is recommended to create models in Pro/ENGINEER with absolute accuracy from the beginning. The values should be 0.01mm or smaller.
  • The setting enable_absolute_accuracy yes needs to be included in configuration file
  • There should be no layer named "255".
  • Components of an assembly should have names no longer than 16 characters.
  • To export mixed model structures, each model type should be saved as one part and transferred in assembly mode.
  • To reduce the neutral file size (save time at import) use "Shrinkwrap functionality" or "Simplified Representation".
  • Before export, check for highlighted menu option Info -> Geometry Checks for design problems. In Creo Parametric use File -> Prepare -> ModelCheck Geometry Check. Indicated features are likely to cause problems in the target system.
  • Delete all non-referenced geometry and external reference. Do not use any suppressed construction geometry (activate all layers).
  • If the model was created with relative accuracy, a conversion to its corresponding absolute accuracy might point out design problems.
  • Force regeneration by selecting: Set Up -> Accuracy -> Absolute -> Enter value or, in Creo Parametric, File -> Prepare -> Model Properties.
  • It is recommended to define therefore a specific start model.

Pro/ENGINEER / Creo Elements - STEP Preprocessor

  • Some STEP specific settings can be added to the configuration file
  • With File -> Options -> Configuration Editor you can add the below mentioned settings in CREO Elements
  • With Tools -> Options... you can add the below mentioned settings in Pro/ENGINEER Wildfire 1.0, 2.0 and 3.0.
  • With Utilities -> Options... you can add the below mentioned settings in Pro/ENGINEER 2001.
  • With Utilities -> Preferences... you can add the below mentioned settings in Pro/ENGINEER 2000i².
  • The default setting for STEP export is AP203. For AP214 export the following setting needs to be added to the Pro/ENGINEER configuration file
  • Other recommended options are:
    • intf3d_out_default_option solid
    • intf3d_out_extend_surface yes
    • intfd_out_blanked_entities no
  • To export a STEP File:
  • In Pro/ENGINEER 2001 and Pro/ENGINEER Wildfire and CREO Elements first select File -> Save a Copy... and then as Type choose STEP (*.stp). If not added in the yet, please select then Solid or Shell (for surface models) depending on the model type. The options Surface (default) and Wireframe should not be used.
  • In Pro/ENGINEER 2000i² first select File -> Export -> ExportOpts and then choose STEP. If not added in the yet, please select then Solid or Shell (for surface models) depending on the model type. The options Surface (default) and Wireframe should not be used.
  • If exporting an Assembly, choose Single File as File structure.
  • In the Options for Pro/ENGINEER STEP Export choose "Solids" and "Shells". The Single Option "Solids" exports only exact Pro/ENGINEER solids, shells and surface will not be exported.
  • To reduce file size (large STEP files cause often conversion problems because of memory limitations) export as multi STEP files with external references if post-processor supports this technology (very good results exporting to CATIA V5).


  • No adjustment is necessary.

SolidWorks - STEP Postprocessor

  • To import a STEP file go to File -> Open… and select the file.
  • Click on Options and the Import Options dialog box appears. Under General options following can be selected:
  • Surface/solid entities: import surface and solid entities.
  • B-Rep mapping: import the model using boundary representation. If not selected, SolidWorks attempts to knit surfaces into solids.
  • Knit surfaces: imports as surfaces and tries to knit imported surfaces.
  • Do not knit: imports as surfaces without knitting them.
  • Free point/curve entities: imports free points and curve entities.
  • Import as sketches
  • Import as 3D curves
  • Import multiple bodies as parts: Imports a multibody part as an assembly document. The multiple bodies are imported as part documents contained in the assembly. With this option cleared the multibody part imports as a part document that contains multiple imported bodies.
  • Perform full entity check and repair errors: default is selected
  • Customize curve tolerance: needed tolerance for the import can be entered here.
  • Map configuration data (for STEP only): Imports STEP file configuration data plus geometric data. To import only the geometry this option must be left unchecked.
  • The other available options are not applicable for the STEP import.
  • Recommended options are to check Surface/solid entities, Try forming solids and Perform full entity check and repair errors.

SolidWorks – System

  • Import errors are indicated in the history tree. By mouse right click over the model and choosing What’s wrong?, a detailed information will be displayed.
  • Doing a Geometry check, the errors will be indicated in the model.



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