Hide Table of Contents

Import DXF File into Part Sketch Example (VBA)

This example shows how to import a DXF file to a part sketch.

'-------------------------------------------------
' Preconditions:
' 1. Verify that the specified DXF file exists.
' 2. Open the Immediate window.
'
' Postconditions:
' 1. Imports the specified file into SOLIDWORKS.
' 2. Examine the Immediate window and graphics area.
'-------------------------------------------------
Option Explicit
Sub main()
    Dim swApp As SldWorks.SldWorks
    Dim filename As String
    Dim longerrors As Long
    Dim retVal As Boolean
    filename = "C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2018\samples\tutorial\importexport\rainbow.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


Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

 
*Email:  
Subject:   Feedback on Help Topics
Page:   Import DXF File into Part Sketch Example (VBA)
*Comment:  
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:



x

We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again
x

Web Help Content Version: API Help (English only) 2018 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.