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NESCFFR3-Newcomer
3-Newcomer
November 11, 2024
Question

Is there a way to import STEP files so that they can be modified?

  • November 11, 2024
  • 3 replies
  • 2978 views

Hello, recently I am using CREO parametric 11 for a project, and I have found useful STEP files online that I need. However, when importing they seem to lose many features and even the ability to edit them in basic ways. Is there a way to import STEP files so that they can be edited?

3 replies

kdirth
21-Topaz I
kdirth21-Topaz I
21-Topaz I
November 11, 2024

There are many settings in the import Details that can help.  The one that seems to make the most difference is Model Accuracy.  Setting Model Accuracy to External helps ensure the math behind the step works.  I have also been told to change the part accuracy to that of the import, if known, before importing it.

 

Not all step files can be imported fully intact and some repair with IDD will be needed.

 

As far as editing, the import is "dumb" and cannot be edited like a native file.  Flexible modeling can allow you to make some changes to the imported model.

There is always more to learn.
    B
    Blue_Oranges4-Participant
    4-Participant
    November 14, 2024

    I've had luck with this parameter setting in my config.pro file: 

     

    intf3d_in_as_part yes

     

    Why STEP file import to .prt file functionality doesn't already work out of the box, we'll never know... one of the many complaints myself and my coworkers have with this cluster of a CAD package. Just typical Creo. 

     

    Anyways, hope this helps!

    K
    KenFarley21-Topaz II
    21-Topaz II
    November 15, 2024

    The setting intf3d_in_as_part is a hidden option. It tells Creo to import any STEP file you read in as a part file, even if it is an assembly. This can cause crashes, and will often result in models that are just surfaces, not solid bodies. This is because an assembly STEP file will contain geometric data for parts that overlap each other, etc. Interfering surfaces and such will prevent Creo from making a manifold solid.

    If you're importing a file and it is an assembly, you always have the option of specifying that it be read in as a part on a case by case basis, if that's the source of the troubles.

      J
      JavierL12-Amethyst
      12-Amethyst
      May 30, 2025

      To Echo what Ken is suggesting, forcing a neutral format file to import as a part can cause a really unstable assembly that uses the imported step part. What I have found to be best practice is to import the step as an assembly, then use the inseparable assembly workflow to keep the imported step as a single line item on your assembly, but still retain all the parts inside. This keeps your BOM clean, but also retains the original part structure to an extent, you never know what manufacturing is going to want to see inside the imported step.

      Otherwise an option if you are really deadset on importing as a single prt is to import as an assembly, then use Component operations to merge all the bodies with no associativity and you end up with a single prt step file, little bit more of a slog, but way better than ending up with a bad top level assembly due to some file import shenanigans 

       

      B
      BR_140829071-Visitor
      1-Visitor
      June 2, 2025
      • STEP files are dummy geometries, designed for sharing data, in your case, your vendor's 3d models - its principal 
        • If I want to edit it, use flexible modeling 
        • There is a feature recognition
        • You can modify, add, or remove geometry 
        • It is not the easiest, but it can get the job done

      cheers!

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