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hugou (Automotive)
14 Jan 10 6:13
If I have a surface in a part, copied from another part (just by going Edit>Copy and Edtit>Paste). Is it possible to break the dependency/reference to the parent part either from within the reference viewer (as the tutorial would suggest) or by any other means? I have gone into the reference viewer and right clicked on the link but it does not give me the option for 'break dependencies'.
aafuni (Mechanical)
15 Jan 10 9:15
hugou,

The break dependency option in the reference viewer is only available if the dependency is no longer needed, so it wouldn't work for what you're doing.  

Normally your best option it to go through your part and redefine your references to reference a coordinate system or independent feature.  With a copy of a face this option will not work.  You would have had more options if you copied whatever features defined the face initially (copy the boundary blend for instance, rather than copying the geometry of the resulting surface).

Is the face you are trying to copy from an imported feature that isn't in Pro/E format?  You could try importing the geometry that you are trying to copy into your working model, then use the import data doctor (IDD) to remove all of the surfaces except for the one you are trying to copy.  This would give you the same effect as importing a model then copying a surface and then deleting the original.

-Funi
hugou (Automotive)
15 Jan 10 18:27
thank you aafuni, I have found that using a copy geometry gives you the otion of making the feture non-dependant you it still shows the parent in reference viewer. I does seepp to pass a model check done this way.
Basically I wanted to take a surface from another part in an assembly and use it to either merge or just extrude up to. The surface sits at a compund angle to my part. and I want no links between the part and the assembly so the part can be used anywhere and checked into team centre without causing issue.
I have come up with a way of defining a plane by creating a centre line where one of my part datums intersects the surface. I can then sketch a curve on this, delete the references and centerline and use the curve to define a new datum at a measured angle from the existing plane - IYSWIM. A bit long winded but got the job done.
hugou (Automotive)
15 Jan 10 18:31
Again apologies for all the typos, I can't type for toffee, particularly not at 11:30pm!

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