I do something like this all the time. To link a face(s) from the part into your part, open assy1. Edit 'my part'. Then, Insert, Surface, Offset, select the face, set the offset to 0.00 (notice the title changes from 'Offset Surface' to 'Copy Surface'), and the hit enter. The face will be in 'my part' and will be linked to the original part. For solid bodies, it's not quite as easy. One way to do it is to use the Join feature. Once again, edit 'my part' in assy1. The, Insert, Features, Join, and select the component with the solid that you want. Now the bad part. If there are multiple bodies in the part the solid is from, they will all be brought in and the extras will need to be deleted. Also, if the join isn't the first feature in the tree, the solids will be 'joined' into one solid. Another alternative (the one that I use all the time), is to open 'my part', and then Insert, Part, and insert the part with the solid. You can insert solids, surfaces, sketches, etc. and get to choose which entity type(s) that you want. However, you still will get all of the entity type, so in a multibody part, you get all the solids and have to delete the 'extras'. But at least the solids don't get 'joined'.
Hope that that was somewhat helpful.
Edit: Forgot to mention that when you insert a part, you also get to mate it in 'my part', so there is added flexibiltiy. I attached an assembly showning the techniques.
Thank you Mark,
your comment was spot on and very useful to better understand how SW handles things.
I have tried some of the command you suggested before your comment and it seemed to took a lot of effort to control the whole thing, so I was wondering if I was doing it right. If I understand correctly your explaination, there are not "dedicated" commands to extract external geometry references on the fly and other strategies must be used to import them into the part.
I noticed that a second join command produced a single solid body with a previously imported one.
Is there a way to avoid exporting parasolid and import them to have separate bodies without history?
Also Is there a command to remove parameters and transform surfaces/solids in "dummy bodies"?
Thank you again
PS I cannot see the attachment...
There is no command to remove parameters, unlike NX. Exporting as a parasolid and re-importing is probably about the best you are going to get from SW. As far as the attachment, what do you mean by you can't see it? It is a zipped assembly of SolidWorks parts. Can you download it?
Thank you again Mark.
As for the attachment is probably an issue of my browser.
Sometimes they disappear and I miss the download placeholder.
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