I received a file from Rhino containing more than 800 "imported surfaces", I would like to be able to create solid parts from the faces that I can use in another assembly. So I would need the faces to not be linked to the base file that I'm going to clean up by deleting the faces that I replaced.
I used to use a face offset of 0, but if I delete the faces in the assembly I get "rebuild errors".
Is there another way?
Here is a specific case:
http://zupimages.net/up/16/51/vgy8.png
On this "imported surface" I would like to keep only the outer skin and then delete the rest.
It's not the first time I've stuck on this kind of situation so if you have a solution I'm all for it.
In order for you to use these parts in another assembly, you could from your file click on the welded construction icon in order to have a list of welded parts and thus you could right-click and then insert in a new part in order to have all your parts see screen attached.
I also tried to sew the surfaces, but the problem is that these are faces that I would like to sew. The set of what I have selected is only 1 imported surface but which includes the structure inside the keel.
Could you elaborate? I would have to make a weld bead between the faces I want to keep?
My method consisted of separating the assembly from your 800 imported surfaces in order to have parts and to be able to use these parts in another mechanical weld.
Have you tried the "offset surface" function screen attached, with this function you would have your outer skin by specifying an offset on the surface so of 0.
Yes I usually use "offset surface" with an offset of 0, but the problem is that if I delete the original surfaces to "clean up" I get reconstruction errors on the solid that was created.
Otherwise for the mechanically welded method or the thicken function, the problem comes from the fact that my "imported surface" also includes the structure that can be seen inside and I only want to keep the "outer skin", i.e. the faces.
It's true that I could use Rhino, it would take me 5 minutes, unfortunately there is no workstation in the office equipped with it and my version on my personal computer is not really official so it's a bit tricky to use it for professional use.
So I was looking for a solution that would allow me to use only SW
What if your surfaces don't remove them but you hide them?
Otherwise, have you tried with the "offset surface" function in order to get what you want, then, as I showed you above, with my screen, you right-click in your list of welded parts on your obtained surface and you insert it in another part.
There may be sketches, boundaries, or constructions that refer to these surfaces that you can't remove. Try right-clicking on your part in the tree, list the external references, and delete them, and then there won't be any links that prevent you from deleting these surfaces. On the other hand, check that all your sketches are constrained after that, normally he should replace the broken references with fixing constraints with the anchor.
Ah, on the other hand, if it is delimitation functions (cutting with surface) or constructions that refer to these surfaces in your part, you would have to redefine their reference elements (points, tangency,...) outside the part concerned.
So I don't really know how it works exactly, but I shifted the faces with an ofset of 0, made a "filled surface" to "plug" the top and sewed the faces to make a volume body that I "inserted into a new part" (empty in this case).
a priori it works because when I delete the faces on the original file, SW does not display an error on the new part.
Conclusion: this is what I wanted to get =D
thank you very much =)
EDIT
Indeed a.leblanc when I look at the linked files, there was still a link to a piece in the temporary documents. I have broken the links with this reference. Everything still works after emptying the temporary document folder: C:\Users\designer1\AppData\Local\TempFileBackupSW\swxauto\Automatic Backup of Part3.SLDPRT