in my company we quite regularly use copy and paste of surfaces in assembles to reuse surfaces. We usually create an assembly containing both the part with the surfaces we need (A) and the part we want the surfaces in (B). Activate the part the surfaces need to go into. Then select the surfaces we want to copy, (using CTRL) then do Ctrl C and Ctrl V to paste them. But when I then go into part A and change the surface, the copied surfaces in B fail.
But I am confused by the dependencies of this feature and cant find them specified anywhere. I looked in the help menu but there doesn't seem to be anything there. I would expect either to have no link at all, so modifying A wont affect B. Or to have a updated link so modifying A changes B, possibly also giving a warning when the part is first opened.
To save me doing a lot of trial and error to try to find this out does anyone know what they are? Also can I change them in my settings or by how i perform the function?
We are using Creo 3.0 if that makes a difference to any one with no database management system.
Thanks for any input.
You can find dependencies by looking at the global reference viewer. It'll show you parents and children, internal and external.
A more robust means of copying surfaces would be to use top down design with a skeleton, assuming that you have the advanced assembly extension (AAX). You'd put all your shared geometry (surfaces, datums, curves,etc.) into the skeleton and use copy geometry or external copy geometry features to pass them down to the parts that need it. It's a very powerful and robust technique designed for exactly what you are trying to do.
If you do not have AAX, you can accomplish the same thing with a master model and using a merge feature to bring the master model into the individual parts. It's a bit less flexible, but it will work
Thanks for the information, I hadn't seen the Global Reference Viewer before.
I cant use the methods you suggest, but i am really after a way of creating a copy of the surfaces which wont be linked to the original. In a trial part I created it tells me the link is "<missing model>" but the part created from the copied surfaces seems quite stable.
How stable is this likely to be?
I really like to understand fully with my models and assemblies exactly if and how they are linked and also if I am doing things which is likely to make parts or assemblies unstable later on. To me, it seems less obvious in Creo when things are linked or referenced.
If the source part is not extraodinarily large, as far as the number of surfaces is concerned, then don't copy individual surfaces one by one. That approach is always bound to fail, because of created geometry dependencies for each and every entity separately.
Use all solid surfaces selection type during the copy instead, that one never fails as long, as the source part is solid. On the other hand it takes all unnecessary surfaces to the copy feature as well. Then just perform whatever boolean type of operations you need.
Problem with this approach James62 is I get a load of surfaces then I don't want, which makes navigating the model really difficult. I have been experimenting with copying the surfaces as I mentioned in my original post, Then exporting as a STEP file, then opening the STEP file to create a new part. This appears to give me a dumb model with no links, which is what I wanted. File size so far seems quite reasonable too and it doesn't appear to lose any accuracy. Apart from being a bit of a work around can anyone see any problems with this?
Thanks for any help.
The beauty of Creo is the Power of Parametrics and the ability to link one model to the next. With this, I have to start by saying Doug Schaefer suggestion above with External Copy Geometry and the ability to make it "Independent", or "Dependent" as necessary is my preferred method.
However, if "Dumb" geometry is what you are looking for, and you will never have a reason to update that geometry, then the export/import method will work fine. I will only add that whenever I have done this (or simply want to send export geometry to suppliers who don't have Creo) and I want to export a "solid", I have the best luck with quality imports using STEP. However, when I want to export a surface quilt I have the best luck with quality imports using IGES.
Owner / Designer / Builder
Try to search for some read on about Collapse Geometry feature and how to create and Independent Geometry feature. That's the way to make surfaces/features "dumb" without STEP file or any kind of middle man.