Macro: Retrieving custom props from Part while in a Drawing?

[JamesMcD]

I have a macro which I pieced together from another one found on the web. It saves a drawing as a pdf and names the file with a concatenated list of properties. My problem is that the properties I want it to look at are in the part file, not the drawing, and I don't know how to get the macro to look in the part as opposed to the current/active document (the drawing) which it is printing.

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Here is part of the code:

Set swCustPrpMgr = swModel.Extension.CustomPropertyManager("")

'Get Custom Property

swCustPrpMgr.Get3 "Part Number", False, "", vPartNumber
swCustPrpMgr.Get3 "Description", False, "", vDescription
swCustPrpMgr.Get3 "Revision", False, "", vRevision
swCustPrpMgr.Get3 "Date", False, "", vDate

filename = vPartNumber & "_" & vDescription & "_" & vRevision & "_" & vDate & ".PDF"

boolstatus = swExportData.SetSheets(swExportData_ExportAllSheets, 1)

boolstatus = swModelDocExt.SaveAs(filename, 0, 0, swExportData, lErrors, lWarnings)

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Thanks for any help,
James

 

[DesignerGuy16]

This is a snippet from my macro to export a SW drawing to pdf, dwg, and/or parasolid. It exports to PDF always, dwg when the model contains a "sheet metal" part, and parasolid otherwise except for our actual assemblies based on our part numbering scheme.

Sub CheckDrawing()

Set swDraw = swModel

InitialDocName = swModel.GetPathName
Set swInitialSheet = swDraw.GetCurrentSheet
InitialSheet = swInitialSheet.GetName

ToggleShtMtl = 0
ToggleModel = 0
ToggleShtSize = 0
SheetNumber = 1

'Check all Sheet Views for Sheet Metal Flat Pattern
SheetCount = swDraw.GetSheetCount
vSheetName = swDraw.GetSheetNames

For i = 0 To SheetCount - 1
SheetName = vSheetName(i)
boolstatus = swDraw.ActivateSheet(SheetName)
Set swSheet = swDraw.Sheet(SheetName)

If ToggleShtMtl = 0 Then
Call FindShtMtlFlat
End If
Next i

Call GetModelProps

If ToggleShtSize = 0 And ToggleShtMtl = 0 Then
Call SaveParasolid
Call SavePDF
ElseIf ToggleShtSize = 0 And ToggleShtMtl = 1 Then
Call SaveDWG
Call SavePDF
ElseIf ToggleShtSize = 1 And ToggleShtMtl = 0 Then
Call SavePDF
ElseIf ToggleShtSize = 1 And ToggleShtMtl = 1 Then
MsgBox "Drawing has a Sheet Metal flat pattern view, but the PartShtSize is not 01, 02, 03, or 04." & vbNewLine & "Please correct PartShtSize or remove view/configuration."
ElseIf ToggleShtSize = 2 Then
MsgBox "PartShtSize in model is not recognized." & vbNewLine & "PartShtSize must be 01, 02, 03, or 04 to export as a parasolid with this macro."
End If

End Sub

Sub FindShtMtlFlat()

Set swView = swDraw.GetFirstView

Do Until (Right(ViewConfigName, 15) = "SM-FLAT-PATTERN") Or swView Is Nothing
ViewConfigName = swView.ReferencedConfiguration

If Right(ViewConfigName, 15) = "SM-FLAT-PATTERN" And (ToggleShtMtl = 0) Then
Set swModel = swView.ReferencedDocument
ToggleShtMtl = 1
SheetNumber = SheetNumber + i
ShtMtlSheet = swSheet.GetName()
Exit Do
ElseIf (ViewConfigName <> "") And (ToggleShtMtl = 0) Then
Set swModel = swView.ReferencedDocument
End If

Set swView = swView.GetNextView

Do Until (Right(ViewConfigName, 15) = "SM-FLAT-PATTERN") Or swView Is Nothing
ViewConfigName = swView.ReferencedConfiguration

If (Right(ViewConfigName, 15) = "SM-FLAT-PATTERN") And (ToggleShtMtl = 0) Then
Set swModel = swView.ReferencedDocument
ToggleShtMtl = 1
SheetNumber = SheetNumber + i
ShtMtlSheet = swSheet.GetName()
Exit Do
ElseIf (ViewConfigName <> "") And (ToggleShtMtl = 0) Then
Set swModel = swView.ReferencedDocument
End If

Set swView = swView.GetNextView

Loop
Loop

End Sub

Sub GetModelProps()

CheckPartShtSize = swModel.GetCustomInfoValue(ViewConfigName, "PartShtSize")
CheckPartBase = swModel.GetCustomInfoValue(ViewConfigName, "PartBase")
CheckRevision = swModel.GetCustomInfoValue(ViewConfigName, "Revision")

If CheckRevision = "-" Then
CheckRevision = "0"
End If

If Len(CheckPartShtSize) = 2 And Left(CheckPartShtSize, 1) = "0" And 0 < Right(CheckPartShtSize, 1) And Right(CheckPartShtSize, 1) < 5 Then
ElseIf Len(CheckPartShtSize) = 2 And Left(CheckPartShtSize, 1) = "0" And 4 < Right(CheckPartShtSize, 1) And Right(CheckPartShtSize, 1) < 10 Then
ToggleShtSize = 1
Else
ToggleShtSize = 2
End If

End Sub

Sub SaveParasolid()

boolstatus = swModel.Extension.SelectByID2(ViewConfigName, "CONFIGURATIONS", 0, 0, 0, False, 0, Nothing, 0)
boolstatus = swModel.ShowConfiguration2(ViewConfigName)

If Len(SheetNumber) = 1 And IsNumeric(CheckPartBase) And Len(CheckPartBase) = 6 And Len(CheckRevision) = 1 Then
longstatus = swModel.SaveAs3(PreReleasePath & CheckPartBase & SheetNumber & CheckRevision & ".X_T", 0, 0)
End If

End Sub

Sub SaveDWG()

Set swDraw = swApp.ActivateDoc2(InitialDocName, True, 2)
swDraw.ActivateSheet (ShtMtlSheet)
Set swSheet = swDraw.Sheet(ShtMtlSheet)

swModel.ViewZoomtofit2
swModel.ClearSelection2 True

If Len(CheckPartShtSize) = 2 And Left(CheckPartShtSize, 1) = "0" And 0 < Right(CheckPartShtSize, 1) And Right(CheckPartShtSize, 1) < 5 And Len(SheetNumber) = 1 And IsNumeric(CheckPartBase) And Len(CheckPartBase) = 6 And Len(CheckRevision) = 1 Then
longstatus = swDraw.SaveAs3(PreReleasePath & CheckPartBase & SheetNumber & CheckRevision & ".DWG", 0, 0)
End If

End Sub

Sub SavePDF()

Set swDraw = swApp.ActivateDoc2(InitialDocName, True, 2)
swDraw.ActivateSheet (InitialSheet)
Set swSheet = swDraw.Sheet(InitialSheet)

swModel.ViewZoomtofit2
swModel.ClearSelection2 True

If ToggleShtSize = 0 And IsNumeric(CheckPartBase) And Len(CheckPartBase) = 6 And Len(CheckRevision) = 1 Then
longstatus = swDraw.SaveAs3(PreReleasePath & CheckPartBase & "1" & CheckRevision & ".PDF", 0, 0)
ElseIf ToggleShtSize = 1 And IsNumeric(CheckPartBase) And Len(CheckPartBase) = 6 And Len(CheckRevision) = 1 Then
longstatus = swDraw.SaveAs3(PreReleasePath & CheckPartBase & "1" & CheckRevision & ".PDF", 0, 0)
End If

End Sub

Sub SaveECNNumber()

If IsNumeric(ECNNumber) And Len(ECNNumber) = 5 Then
Set fs = CreateObject("Scripting.FileSystemObject")
Set MyFile = fs.OpenTextFile(ECNTextPath, 2, True)
MyFile.Write ECNNumber
MyFile.Close
End If

End Sub

James Spisich
Design Engineer, CSWP

 

[SolidWorksEngineer]

Hello,

What version of Solidworks this macro runs ?

Best Regard, SolidWorks Engineer

http://solidworksengineer.com

http://sketchupengineer.com

 

[TheTick]

What you need to do is get access to the part (or assembly) that is in the drawing.

For 99% of drawings, the model of interest is in the default view of the first sheet. So, from a drawing, get the first sheet, then the default view, then the model associated with the default view.

Take note of the differences between ModelDoc, DrawingDoc, PartDoc, and AssemblyDoc objects. Your drawing needs to be in accessed vie DrawingDoc object to get hold of the views.