Import DXF File into Part Sketch Example (VBA)
This example shows how to import a DXF file to a part sketch.
'--------------------------------------
'
' Preconditions: The specified DXF file exists.
'
' Postconditions: The specified file is imported into
SolidWorks.
'
'---------------------------------------
Option Explicit
Sub main()
Dim
swApp As SldWorks.SldWorks
Dim
filename As String
Dim
longerrors As Long
Dim
retVal As Boolean
filename
= "e:\samples\importdxfdwgdata\Draw3.DXF"
Set
swApp = Application.SldWorks
Dim
importData As SldWorks.ImportDxfDwgData
Set
importData = swApp.GetImportFileData(filename)
' Import method
importData.ImportMethod("") = SwConst.swImportDxfDwg_ImportMethod_e.swImportDxfDwg_ImportToPartSketch
' Load the specified DXF/DWG file
Dim
newDoc As SldWorks.ModelDoc2
Set
newDoc = swApp.LoadFile4(filename,
"", importData, longerrors)
' Gets
Debug.Print
"Part Sketch Gets:"
Debug.Print
" Add
constraints: "
& importData.AddSketchConstraints("")
Debug.Print
" Merge
points: "
& importData.GetMergePoints("")
Debug.Print
" Merge
distance: "
& (importData.GetMergeDistance("")
* 1000#) & " mm"
Debug.Print
" Import
dimensions: " & importData.ImportDimensions("")
Debug.Print
" Import
hatch: "
& importData.ImportHatch("")
'Sets
Debug.Print
"Part Sketch Sets:"
importData.AddSketchConstraints("") =
True
Debug.Print
" Add
constraints: "
& importData.AddSketchConstraints("")
retVal
= importData.SetMergePoints("",
True, 0.000002)
Debug.Print
" Merge
points: "
& retVal
Debug.Print
" Merge
distance: "
& (importData.GetMergeDistance("")
* 1000#) & " mm"
importData.ImportDimensions("")
= True
Debug.Print
" Import
dimensions: " & importData.ImportDimensions("")
importData.ImportHatch("")
= False
Debug.Print
" Import
hatch: "
& importData.ImportHatch("")
End Sub