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Solid to surface
You can use "offset surface" with a distance of 0. Just make sure to select all the faces.-
Solid to surface
This is not enough, when I have got more than 1000 non planar and non tangent surfaces...
Any better way?
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Solid to surface
I don;t think SolidWorks has a convert solid to surfaces command so here's what I do:
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.-
Re: Solid to surface
Thank you Kevin!
was looking for similar solution and your post was exactly what worked for me.
Thanks!
Brendan
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Solid to surface
Deleting a single face without healing will result in a surface body. If you do not wish to lose your original solid body, make a copy of it and delete a face from the copy. -
Solid to surface
Can you explain exactly what you want to do, what is the end result you are trying to get?
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Solid to surface
I have got a part, next I need modify it without removing faces, bodies etc.
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.-
Solid to surface
Use Freeform feature, use Replace Face. These are better methods than what it sounds like you are trying to do.
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Solid to surface
A one click function does not exist! And even if it did you would be no further ahead because SW is a history based app', and a feature would be added ... much like the Delete Face and Patch feature.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. -
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Solid to surface
Click on the offset surface tool. Set the offset distance to 0. Click on all the faces that you want to be a single surface body. Then click OK. -
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Solid to surface
pelase select tools->options->display/selection ,check "allow selection in hlr and shade modes"
then click ok,go to model,
press F5, click "filter faces" then select the model . you saw all the face will be selected. -
Re: Solid to surface
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.
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Re: Solid to surface
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>
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Re: Solid to surface
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)
Option Explicit Dim swApp As SldWorks.SldWorks Dim swModel As SldWorks.ModelDoc2 Dim swSelMgr As SldWorks.SelectionMgr Dim swBody As SldWorks.Body2 Dim i As Integer Sub main() Set swApp = Application.SldWorks Set swModel = swApp.ActiveDoc Set swSelMgr = swModel.SelectionManager For i = 1 To swSelMgr.GetSelectedObjectCount2(Mark:=-1) If swSelMgr.GetSelectedObjectType3(index:=i, Mark:=-1) = swSelSOLIDBODIES Then Set swBody = swSelMgr.GetSelectedObject6(index:=i, Mark:=-1) swModel.CreateSurfaceFeatureFromBody swBody, swCreateFeatureBodyOpts_e.swCreateFeatureBodyCheck End If Next i End Sub
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Re: Solid to surface
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.
