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