Wrap command in assembly model?

[Andrew_410]

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.

[kdirth · Accepted solution]

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.

[Andrew_410]

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]

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. 

[BH_13569156]

Your work-around will not work for me. Because an extrude cut will not work for engraving on a round surface, I use wrap. While that does not actually cut, it gives the appearance of the engravement. So, I want to wrap the assembly part number on the round surface of a part. The sketch text is driven by the PARTNUMBER parameter, I cannot add the wrap to the part because the part has different PARTNUMBER text.

[StephenV]

I didn't get involved in your whole inquiry, but I did see you say, "an extrude cut will not work for engraving on a round surface".  I believe that is untrue as a whole but maybe in your path or expectation it could be true. Or, maybe you have a very limited Creo license. Otherwise, if you have a cylindrical (or other shape) surface or a solid you can offset such surface from a solid (or surface) to the engraving depth. Then above that, on a plane or on your wrap that contains the characters (or entities) you want engraved to do the following depending on surface or solid. Surface: Extrude characters to or thru as a surface to the offset surface and merge them to solidify for final command. Solid: Do an extrude cut from the characters to the offset surface (depth= up to surface). You should have a physical engravement. If I'm on another planet here, then sorry and lotsa luck.

[Andrew_410]

I believe you can use a part parameter at an assembly level with relations. You just need to know the the session ID for the part and then can create a dummy parameter in the assembly equating it to that of the part, or you could use the part parameter directly at the assembly level with the code PARTNUMBER:XX, where XX is the session ID. Both items would have to be in session.