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Insert and Position DXF/DWG File in Drawing Example (VB.NET)

This example shows how to insert and position a DXF/DWG file in a drawing.

'---------------------------------------------------------------------------
' Preconditions:
' 1. Open a drawing.
' 2.
Replace DXF_file_path with the pathname of an existing DXF/DWG file.
'
' Postconditions:
' 1. Inspect the Immediate window.
' 2. The DXF/DWG file is inserted as per the specified import data.
' 3. The drawing is moved to the right.
'---------------------------------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System
Imports System.Diagnostics

Partial Class SolidWorksMacro

    
Sub main()

        
Const sDwgFileName As String = "DXF_file_path"

        Dim swModel As ModelDoc2
        
Dim swModelView As ModelView
        
Dim swDraw As DrawingDoc
        
Dim swFeatMgr As FeatureManager
        
Dim swFeat As Feature
        
Dim swSketch As Sketch
        
Dim swView As View
        
Dim vPos As Object
        Dim bRet As Boolean
        Dim importData As ImportDxfDwgData

        swModel = swApp.ActiveDoc
        swModelView = swModel.ActiveView

        bRet = swModel.Extension.SelectByID2(
"Sheet1", "SHEET", 0.0#, 0.0#, 0, False, 0, Nothing, 0)

        swDraw = swModel
        swFeatMgr = swModel.FeatureManager
        importData = swApp.GetImportFileData(sDwgFileName)

        
'Unit
        importData.LengthUnit("") = swLengthUnit_e.swINCHES

        
'Position
        bRet = importData.SetPosition("", swDwgImportEntitiesPositioning_e.swDwgEntitiesCentered, 0, 0)

        
'Sheet scale
        bRet = importData.SetSheetScale("", 1.0#, 2.0#)

        
'Paper size
        bRet = importData.SetPaperSize("", swDwgPaperSizes_e.swDwgPaperAsize, 0.0#, 0.0#)

        
'Import method
        importData.ImportMethod("") = swImportDxfDwg_ImportMethod_e.swImportDxfDwg_ImportToExistingDrawing

        
'Import file with importData
        swFeat = swFeatMgr.InsertDwgOrDxfFile2(sDwgFileName, importData)
        swSketch = swFeat.GetSpecificFeature2

        swView = swDraw.GetFirstView

        
Do While Not swView Is Nothing
            If swSketch Is swView.GetSketch Then
                Exit Do
            End If
            swView = swView.GetNextView
        
Loop

        vPos = swView.Position

        Debug.Print(
"File = " & swModel.GetPathName)
        Debug.Print(
"  Sketch       = " & swFeat.Name)
        Debug.Print(
"  View         = " & swView.Name)
        Debug.Print(
"    Old Pos    = (" & vPos(0) * 1000.0# & ", " & vPos(1) * 1000.0# & ") mm")

        
' Move to right
        vPos(0) = vPos(0) + 0.01
        swView.Position = vPos

        vPos = swView.Position
        Debug.Print(
"    New Pos    = (" & vPos(0) * 1000.0# & ", " & vPos(1) * 1000.0# & ") mm")

        
' Redraw
        Dim rect() As Double
        rect = Nothing
        swModelView.GraphicsRedraw(rect)

    
End Sub


    Public swApp As SldWorks


End Class
 



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