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Andrew_41012-Amethyst
12-Amethyst
October 8, 2024
Solved

Wrap command in assembly model?

  • October 8, 2024
  • 1 reply
  • 2036 views

Does the wrap command work in assembly mode? Specifically, I'd like to wrap a cosmetic sketch around a part's cylinder of an assembly model. Is this an option? For me, working in Creo 2.0 M250 currently, this seems impossible since while wrap is visible in the model>modifiers overflow tab, it's always greyed out.

 

I can do it in the part file, so will result to that if all else fails.

Best answer by kdirth

It is not available in assembly in Creo 7.0.

 

I would suggest putting it in the part and suppressing it.  Then use flexibility to resume that feature in the assembly.

1 reply

kdirth
21-Topaz I
kdirth21-Topaz IAnswer
21-Topaz I
October 8, 2024

It is not available in assembly in Creo 7.0.

 

I would suggest putting it in the part and suppressing it.  Then use flexibility to resume that feature in the assembly.

There is always more to learn.
    A
    Andrew_41012-AmethystAuthor
    12-Amethyst
    October 10, 2024

    I've no experience with flexibility, but have decided to add the cosmetic sketch to the base level part and then hide it with layers on the assembly level.

     

    Thanks for the suggestion and help!

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

    Here is that section of our tips file.

     

    FLEXIBILITY 

    Predefine flexibility in a component or assembly 

    1. Go to File / Prepare / Model Properties. Select “change” for Flexible under Tools section. 
    2. When part or assembly is assembled into an assembly you will be prompted to use predefined flexibility. 
    3. Select the tap for the type of flexibility needed 
    4. Select a feature or part to flex, select dimension to vary, if needed, and select OK. 
    5. Repeat for additional features or part flexibilities. 
    6. Select OK. 

    Add flexibility when adding part with predefined flexibility. 

    1. Select Yes to prompt “Would you like to use it for flexible component definition?” 
    2. Add new value for flexibility as needed and select OK. 
    3. Add flexibility to part w/o predefined flexibility. 
    4. Right click on part in model tree and select Make Flexible / Make Flexible from menu. 
    5. Select the tab for the type of flexibility needed. 
    6. Select a feature or part to flex, select dimension to vary, if needed, and select OK. 
    7. Repeat for additional feature or part flexibilities. 
    8. Change values as needed for flexible items. 
    9. Select OK. 

    Change flexibility values. 

    1. Edit Definition of component, select Varied Items from Flexibility tab and change values. 
    2. Or right click on part, select Make Flexible / Varied Items from menu and change values. 
    There is always more to learn.
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