creating a solid assembly in SolidWorks
creating a solid assembly in SolidWorks
(OP)
Hi
I have an IGES file from a vendor that is an assembly of several parts. I opened it in SW and have an assembly with several dumbsolid models. This is a part we purchase and add to the top assembly just like a bolt or nut so I don't need the many small parts that all have part numbers different then ours.
I thought there was a way I could take this SW assembly or IGES assembly and save it as one dumb solid rather than as a multi-part assembly but none of the SAVE AS PART functions work for this.
I don't want to have to track all the many small parts to this buy-and-use assembly.
Does anyone know how to turn an assembly into a single part solid?
Thank you.
I have an IGES file from a vendor that is an assembly of several parts. I opened it in SW and have an assembly with several dumbsolid models. This is a part we purchase and add to the top assembly just like a bolt or nut so I don't need the many small parts that all have part numbers different then ours.
I thought there was a way I could take this SW assembly or IGES assembly and save it as one dumb solid rather than as a multi-part assembly but none of the SAVE AS PART functions work for this.
I don't want to have to track all the many small parts to this buy-and-use assembly.
Does anyone know how to turn an assembly into a single part solid?
Thank you.






RE: creating a solid assembly in SolidWorks
The other way is to do File->Save As from the assembly and change the file type to "Part".
-handleman, CSWP (The new, easy test)
RE: creating a solid assembly in SolidWorks
I have also tried the save as part and the ASSEMBLY GEOMETRY TO SAVE IN PART FILE: options -
clicking the exterior faces crashed me out of SW and did the same to my VAR and the other two buttons just didn't work to create a merged, solid file.
Thanks
RE: creating a solid assembly in SolidWorks
Mike Halloran
Pembroke Pines, FL, USA
RE: creating a solid assembly in SolidWorks
'--------------------
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swDraw As SldWorks.DrawingDoc
Dim swSheet As SldWorks.Sheet
Dim boolstatus As Boolean
Dim longstatus As Long, longwarnings As Long
Public Const sTemplatePath As String = "\TEMPLATES\Part.prtdot" ' Change the path to your part template file
Sub main()
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
Set swModel = swApp.NewDocument(sTemplatePath, 0, 0, 0)
swApp.ActivateDoc2 "Part1", False, longstatus
swApp.ActivateDoc2 "3 in Clamp Assy", False, longstatus
Set swModel = swApp.ActiveDoc
longstatus = swModel.SaveAs3("\\Documents and Settings\Desktop\Part.SLDPRT", 0, 0) ' Change the path to your part file name and path
End Sub
'--------------------
Deepak Gupta
SW2009 SP3.0
SW2007 SP5.0
MathCAD 14.0
RE: creating a solid assembly in SolidWorks
'--------------------
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim boolstatus As Boolean
Dim longstatus As Long, longwarnings As Long
Sub main()
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
longstatus = swModel.SaveAs3("\\Documents and Settings\Desktop\Part.SLDPRT", 0, 0) ' Change the path to your part file name and path
End Sub
'--------------------
Deepak Gupta
SW2009 SP3.0
SW2007 SP5.0
MathCAD 14.0
RE: creating a solid assembly in SolidWorks
'------------------
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim boolstatus As Boolean
Sub main()
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
Dim FilePath As String
Dim PathSize As Long
Dim PathNoExtension As String
Dim NewFilePath As String
FilePath = swModel.GetPathName
PathSize = Strings.Len(FilePath)
PathNoExtension = Strings.Left(FilePath, PathSize - 6)
NewFilePath = PathNoExtension & "SLDPRT"
boolstatus = swModel.SaveAs3(NewFilePath, 0, 0)
End Sub
'------------------
Deepak Gupta
SW2009 SP3.0
SW2007 SP5.0
MathCAD 14.0
RE: creating a solid assembly in SolidWorks
RE: creating a solid assembly in SolidWorks
RE: creating a solid assembly in SolidWorks
When you go to File->Open and change the file type to IGES or Parasolid... etc there is a button there for "Options". Click that button. In the import options there is a checkbox for "Import solid bodies as parts". Un-check that box, then open the IGES file.
Also, you said that saving the assembly as a part also saves all the components as individual parts. Actually, all those components were saved as parts when you opened the IGES file in the first place. When you have the "Import solid bodies as parts" option checked during open, SW automatically creates all those component files.
Thanks again.