AnsweredAssumed Answered

Solid to surface

Question asked by Pawel Keska on Mar 10, 2008
Latest reply on Feb 1, 2018 by Sergio Monti

Like • Show 0 Likes0
Comment • 18

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?

1 person has this question

Outcomes

18 Replies

Charles Culp Mar 10, 2008 11:29 AM
Mark Correct
Correct Answer
You can use "offset surface" with a distance of 0. Just make sure to select all the faces.
Like • Show 0 Likes0
Actions
- Pawel Keska @ Charles Culp on Mar 11, 2008 6:23 AM
  Mark Correct
  Correct Answer
  This is not enough, when I have got more than 1000 non planar and non tangent surfaces...
  Any better way?
  Like • Show 0 Likes0
  Actions
Kevin Quigley Mar 11, 2008 9:24 AM
Mark Correct
Correct Answer
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.
Like • Show 0 Likes0
Actions
- Brendan Zarechian @ Kevin Quigley on May 11, 2010 10:30 AM
  Mark Correct
  Correct Answer
  Thank you Kevin!
  was looking for similar solution and your post was exactly what worked for me.
  Thanks!
  Brendan
  Like • Show 0 Likes0
  Actions
Roland Schwarz Mar 11, 2008 12:29 PM
Mark Correct
Correct Answer
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.
Like • Show 0 Likes0
Actions
Brian Hoerner Mar 11, 2008 3:12 PM
Mark Correct
Correct Answer
Can you explain exactly what you want to do, what is the end result you are trying to get?
Like • Show 0 Likes0
Actions
- Pawel Keska @ Brian Hoerner on Mar 17, 2008 9:08 AM
  Mark Correct
  Correct Answer
  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.
  Like • Show 0 Likes0
  Actions
  - Matt Lombard @ Pawel Keska on Jul 28, 2008 2:05 PM
    Mark Correct
    Correct Answer
    Use Freeform feature, use Replace Face. These are better methods than what it sounds like you are trying to do.
    Like • Show 0 Likes0
    Actions
Kelvin Lamport Mar 17, 2008 11:03 AM
Mark Correct
Correct Answer

I expect features: create surface from solid, one click - thats all.

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.

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.
Like • Show 0 Likes0
Actions
1-7KHSPD Jul 24, 2008 7:10 PM
Mark Correct
Correct Answer
How I convert solid to "multiple" surfaces?
Like • Show 0 Likes0
Actions
Charles Culp Jul 24, 2008 8:16 PM
Mark Correct
Correct Answer
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.
Like • Show 0 Likes0
Actions
1-7KHSPD Jul 28, 2008 10:06 AM
Mark Correct
Correct Answer
"offset surface tool" create a single surface. I need multiple surfaces.
Like • Show 0 Likes0
Actions
Charles Culp Jul 28, 2008 1:43 PM
Mark Correct
Correct Answer
Offset surface will create multiple bodies.
Attachments
- OffsetMultipleBodies.png92.3 KB
Like • Show 0 Likes0
Actions
1-DFUOJQ Jul 29, 2008 6:40 AM
Mark Correct
Correct Answer
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.
Like • Show 0 Likes0
Actions
Kevin De Smet May 12, 2010 8:32 AM
Mark Correct
Correct Answer
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.
Like • Show 0 Likes0
Actions
- Ryan Laplante @ Kevin De Smet on May 12, 2010 6:30 PM
  Mark Correct
  Correct Answer
  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>
  Like • Show 0 Likes0
  Actions

Rob Edwards Feb 1, 2018 7:29 AM

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

Actions

Sergio Monti Feb 1, 2018 8:53 AM
Mark Correct
Correct Answer
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.
Like • Show 0 Likes0
Actions

Solid to surface

Outcomes

Attachments

Related Content

Recommended Content