How using one feature convert solid to surface?
I know, it is possible - after removed face I can fill and next knit result. You got any better (faster) idea?
I know, it is possible - after removed face I can fill and next knit result. You got any better (faster) idea?
Any better way?
Export the part to IGES - in the options in the Solids/Surfaces section choose Trimmed surfaces type 144
Open the IGES file but in the options dialogue for Surface/solid entities turn off Try forming solid(s) and select Do not knit if you want mutiple surfaces or Knit surfaces if you want joined surfaces.
Of course you lose all associativity using this method abd the surfaces are just dumb surfaces.
Thank you Kevin!
was looking for similar solution and your post was exactly what worked for me.
Thanks!
Brendan
I only try to deform any faces.
I know, it is possible (export as surface, delete face but after that I must add new feature (fill, loft, delete edge). I expect features: create surface from solid, one click - thats all.
You should be able to deform or modify the solid without needing to convert to surfaces.
If you explain in more detail what shapes you are trying to form, maybe someone can offer a detailed solution.
Attachments
then click ok,go to model,
press F5, click "filter faces" then select the model . you saw all the face will be selected.
I would go Offset Surface Copy a single face somewhere, then hide that surface, and use Delete Face to remove it on the solid. Since the Offset came before the Delete, the surface body will still remain. All you need to do now, is Knit the offset surface to the main surface body.
if you remove just one face the entire part becomes a surface, you can then knit the face back on but not "try to make body solid" and you should have a crazy complex surface
you got it right>
Just found this old post because I had the exact same question..
The frustrating thing is in the PartDoc Interface there is a method that does this exact thing
2016 SOLIDWORKS API Help - CreateSurfaceFeatureFromBody Method (IPartDoc)
Hi Pawel,
if it is an assembly model, have you tried to save as part using the option "Exterior faces"
If it is a part, create an assembly and save as faces.
Sometimes doesn't keep all surfaces but you can have a go and see.
I usually use this function in layout drawings to reduce sizes of complex sub-assemblies.
Hope it will help.