creating a solid assembly in SolidWorks

[rudragoo]

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.

 

[handleman]

Two ways. In the File->Open dialog, when you change the file type to IGES/SAT/Parasolid, etc, the "References" button changes to an "Options" button. One of the options in there is "Import multiple solid bodies as parts." Un-check that option.

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)

 

[rudragoo]

Thanks for your note. I just tried the FILE OPTIONS suggestion and clicked the import as parts - that is what it did - imported them as separate parts rather than merging them all into one solid.

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

 

[MikeHalloran]

How about, in the SaveAs dialog, you drag down the filetype selection to SldPrt instead of SldAsm? I think that's how it works. I'd try it myself now, but I have a monster part loaded and I don't want to get SW confused any more than it is.



Mike Halloran
Pembroke Pines, FL, USA

 

[Gupta65]

Try recording a macro and then edit it accordingly. I tried one and it saves the assembly into a part with with exterior faces. Please modify the codes.

'--------------------
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

 

[Gupta65]

Try this:

'--------------------
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

 

[Gupta65]

Works on any assembly to save as part (exterior faces)
'------------------
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

 

[rudragoo]

Thanks to everyone for the help.

 

[GRF]

Another option would be to edit one of the parts then use a join (I believe it is under insert feature but I am running a simulation at the moment). Then you can open the part outside of the assembly and save it off as the name your company uses for the full assembly.

 

[rudragoo]

Thanks for the help from everyone. Here is the technique that worked for us.......

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.