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Pulling data from an Assembly to use on a New Part. Ie curvs


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I am new to Wildfire Pro/E. I want to pull some data (edges, sizes) from an assebly over to a newly created part. What would it be called - references, relations, parent/child??? I am having no luck with PTC's web help.

Thanks, Jeff
Don't know in Wildfire, but in 2001, its insert, shared geometry, copy geometry.

I havn't tried copying geometry from an assembly to a new part, but it works well when copying from a part to a new part.
in response to BobP: Don't know in Wildfire, but in 2001, its insert, shared geometry, copy geometry.

this only works if you have the Advanced Assembly Extension, if you don't have this, you can't use this option.

I do not have AAE, so I do it a different way.

create a new part, assemble it into the assembly. then modify, modify part, (pick the newly assembled part), feature, create, surface, copy. then pick all relevant surfaces. hit done & done return until you get back to the main menu. then go back to the new part, and you will have all the surfaces you just copied from the assembly.
If you don't want the information to be parametric, you can just IGES out the curves from the assembly and then import them into your part.

I have also used shrinkwrap for this type of data transfer.

If you want parametrics external ref copy geom works well as long as all of your curve information is located in one assy or part. If this isn't the case you will just have to make seperate features for each part /assy you are copying from.
In WF right click on the part you want to modify in the model tree.

edit definition>pick the curve then go to the edit menu and select copy.

Use the shift key to select more than one tangent segment.

You can drag the handles on the end of the curve to extend or use points,surfs etc to trim while you are copying the curve.



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