API -- Change dimension in part without opening it?

What I want to do is locate a part file on the system by name, including folder,
save that under a new name, and with that newly saved part, change a dimension
and save it, without opening anything.
Then I want to locate a drawing file on the system by name, save it under a new
name, and assign the newly saved part file to it as the reference.
Is this possible? If so, how do I get started? I can get this to work if the
parts and drawings are opened, and I can open them with API, but I want to go
further and do it without opening them in the first place, to make the process
go faster.
Thank You,
-plh

 

I can tell you why you might not want to do this. If you change the
dimension without rebuilding and saving the drawing will open in
SWViewer with the old dimension even though you have given it a new
filename. I have seen this kind of thing get to mfg. It ain't pretty.

 

I am aware of that limitation, thanks. What I am going to do is bring the
drawing up (in SW) *after* A have done all the "silent" changes, it will rebuild
then (see original post)
Thanx,
-plh

 

You can do all this EXCEPT change the dimension while files are closed.
There might be a somewhat clumsy work-around if you built your parts
to include an externally linked design table, or a macro feature that
would read a dimension from custom properties or other external source
each time the part rebuilds. Short of extraordinary measures like
these, however, a dimensional change would necessitate a file-open on
the part or assembly model (not necessarily the drawing that references
them).

HTH,
BDB

 

If you opened just the drawing and the dimension was imported you just
change it there.

 

True enough. Still requires a file-open, which takes some time.

 

True enough. Still requires a file-open, which takes some time.

 

Of course with SW saying you have the file open is a relative term.
Just how open does it have to be? For example if you write directly to
database or turn off visibility you minimize overhead related to
interactive use while still capturing the important stuff.

 

Hi,
I have not looked at this thread in a while.
The whole point of this project is to programatically clone parts with different
"driver" dimensions with the end result of rapidly produced and consistent
drawings. I am resigned to opening the drawings and parts. I now have the
following sequence pretty good:
Copy "base" drawing to new name. (using FileSystemObject)
Open new drawing (Opendoc6)
Open base part (OpenDoc6)
Save base part under new name. (swModelDocExt.SaveAs)This causes to the drawing
to refer to the correct part.
The problem is that at the save as routine closes the part. I want to leave it
open so that I can go in and programatically change the relevant dimension. I
tried to reopen it (OpenDoc6) but nWarnings is returning 128 (& as of this time
I don't know what that means) and I end up with the Drawing open, referencing
the correct part, but the part closed. So, that is my current problem, can I
prevent swModelDocExt.SaveAs from closing the part.
Thank You,
-plh

PS:
bolRetVal = swApp.SetCurrentWorkingDirectory(strHomeFolder)

Set obFSO = CreateObject("Scripting.FileSystemObject")
With obFSO

If .FileExists(Me.txtFolder.Value & "\" & Me.txtPartNumber.Value & ".SLDPRT") _
Or .FileExists(Me.txtFolder.Value & "\" & Me.txtPartNumber.Value & ".SLDDRW")
Then
'in case of overwrite make sure user wants to do that
If MsgBox("File Exists! Want to Overwrite?", vbYesNo) <> 6 Then
Me.txtFolder.Value = ""
Me.txtPartNumber.Value = ""
Exit Sub
Else
'.CopyFile strBasePart, Me.txtFolder.Value _
'& "\" & Me.txtPartNumber.Value & ".SLDPRT"
'copy the part to that folder

.CopyFile strBaseDrawing, Me.txtFolder.Value _
& "\" & Me.txtPartNumber.Value & ".SLDDRW"
'copy the drawing to that folder

End If
Else
.CopyFile strBaseDrawing, Me.txtFolder.Value _
& "\" & Me.txtPartNumber.Value & ".SLDDRW"
'copy the drawing to that folder
End If
End With



strPartToReference = Me.txtFolder.Value & "\" & Me.txtPartNumber.Value &
".SLDPRT"
'Me.txtFolder.Value & "\" & Me.txtPartNumber.Value & ".SLDPRT"
strDrawingToOpen = Me.txtFolder.Value & "\" & Me.txtPartNumber.Value & ".SLDDRW"

Set swDrawing = swApp.OpenDoc6(strDrawingToOpen, swDocDRAWING, _
swOpenDocOptions_Silent, "", nErrors, nWarnings)
If ReportNErrors(nErrors, nWarnings, strDrawingToOpen) = False Then Exit Sub
'open the New drawing which will still reference the BASE part

Set swPart = swApp.OpenDoc6(strBasePart, swDocPART, _
swOpenDocOptions_Silent, "", nErrors, nWarnings)
If ReportNErrors(nErrors, nWarnings, strBasePart) = False Then Exit Sub
'open the BASE part

bolRetVal = swApp.SetCurrentWorkingDirectory(Me.txtFolder.Value)

Set swModelDocExt = swPart.Extension
bolRetVal = swModelDocExt.SaveAs(strPartToReference, 0, swSaveAsOptions_Silent,
Nothing, nErrors, nWarnings)
If ReportNErrors(nErrors, nWarnings, strPartToReference) = False Then Exit Sub
'do a save as in order to link the new part to th drawing

Set swPart = swApp.OpenDoc6(strPartToReference, swDocPART, _
0, "", nErrors, nWarnings)
If ReportNErrors(nErrors, nWarnings, strPartToReference) = False Then Exit Sub
'open the NEW part

Set swPart = swApp.ActivateDoc2(strPartToReference, False, longstatus)

 

I was able to solve this by opening the part first then the drawing. For some
reason that did it.
-plh