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cadbart1-Visitor
1-Visitor
January 8, 2021
Question

How to move `copy` feature from one part to another

  • January 8, 2021
  • 2 replies
  • 8711 views

Hi, I'm using Creo Parametric 3.0 in which Copy Geometry, Shrinkwrap and Copy From features are blocked (grayed out). I'd like to copy geometry (complicated hole) from one part in order to use it (make shaft based on that hole's geometry) in another part. The only way I can imagine is to make copy in basic model and move it to the other part. The problem is that I don't know how to do it. Could you please tell me if it's possible in Creo 3.0 and if so - how can I achieve this? 

Thank you in advance for all answers!

2 replies

KenFarley
KenFarley21-Topaz II
21-Topaz II
January 8, 2021

Probably the way I'd do this, given your situation, is

* edit the sketch that generates the feature in your original part

* save that sketch as a separate file

* read that sketch into the section definition for your new part (shaft)

 

The better way to do this type of thing in the future is to build your assembly in a top-down fashion, where there is a "higher level" assembly used to generate the two parts, which defines the complex geometry. That way you have a parametric link between the two models so if you change the feature (larger diameter, keyway, etc.) the change is automatically reflected in both parts. It's more complicated to set up but speaking from experience it will save you time and more importantly prevent forgetting to change things so the two parts are compatible.

    C
    cadbart1-VisitorAuthor
    1-Visitor
    January 11, 2021

    Thank you for your answer, Ken! Your way seems to be a good practice but can you explain what exactly did you mean? Let's say I need to create an injection mold and in order to create a seat I have to copy geometry from final product (which comes out from mold) model. There's many of various features in that part. How would you make this by following your way? 

    KenFarley
    KenFarley21-Topaz II
    21-Topaz II
    January 11, 2021

    Oh, what you're describing is much more complicated. When you said "feature" I thought you meant a single protrusion, revolve, etc. Feature is the term we use to refer to a single entry in the model tree.

    To do what you're talking about I might have to (painfully) go through the creation of the sequence of features needed to define the matching geometry. It might be a case of doing what I suggested for each feature (save the sketch defining the feature, import it into the new model, use it for a feature in the new model).

    Something I've seen done by co-workers, but that I find is dangerous is to export the surfaces of the geometry region, then import them into the new model. Then use solidify or to add the geometry into the new model. I hate this because (a) It's not parametric. If you change the original model (change a round radius, etc.) it doesn't automatically update the new model. You have to re-do the geometry import and solidification. (b) Surface export and import can introduce inaccuracy into the model, particularly it can mess up the tangency between surfaces. You might also see surface edges that almost but not quite intersect the surfaces of the part you are trying to add to with the solidify, which will cause features to fail.

    tbraxton
    22-Sapphire II
    tbraxton22-Sapphire II
    22-Sapphire II
    January 8, 2021

    The options may be "greyed out" due to licensing. You need to have the advanced assembly extension or equivalent to use the top down functions (copy geom etc.),

     

    You can copy and paste features from one model to another. This would save you the time of recreating the hole geometry. The key to doing this is to understand the parent references of the features you will copy to another model as you will need to map those 1:1 to get the copied features to regenerate in the target model. Ideally the features should be contiguous or grouped. It will likely  help if your new target model uses the same start part template as the source part.

     

    Without seeing your models I would suggest copying the hole feature(s) to a new model (target) and change them to surface from solid if possible (this should be easy if it is a revolve feature or the like and not actually a hole feature). You can then use the surface geometry as a reference to create the shaft.

     

    In the source model select the feature(s) you you want to copy and use CTRL+C or UI selection to copy them.

    Activate the target model and then use the paste special option where you will be prompted for scaling options.

    The advanced reference configuration menu will be presented with a list of references to map between the models. The references will be highlighted in the target model window to help you select the reference to map in the target model. Map the references and then complete the copy operation and you will have a copy of the features in the new model.

     

    http://support.ptc.com/help/creo/creo_pma/usascii/index.html#page/part_modeling/part_modeling/part_four_sub/To_Copy_a_Feature_Across_Models.html 

     

     

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      cadbart1-VisitorAuthor
      1-Visitor
      January 11, 2021

      Thank you very much, tbraxton, for your answer and tips! I tried your way and copying features to new part works properly but I need to have at least one feature (inside target) in which that copy (by paste special) could resist. Also I don't know how could I change solid to surface because almost all surface-editing options are greyed out.

      tbraxton
      22-Sapphire II
      tbraxton22-Sapphire II
      22-Sapphire II
      January 11, 2021

      If you are using a commercial license of Creo then post a sample of your hole feature. I would need to see the feature/geometry to comment on the copy/paste approach further.

       

      In some features you can change them from solid to surface by editing the definition of the feature. 

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