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Translate Sketch Example (VB.NET)

This example shows how to move a sketch.

'----------------------------------------------------------------------------
' Preconditions: Verify that the specified template exists.
'
' Postconditions:
' 1. Creates a sketch.
' 2. Creates a parabola.
' 3. While observing the graphics area, press F5 at Stop
'    to move the sketch.
'----------------------------------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System.Runtime.InteropServices
Imports System

Partial Class SolidWorksMacro

    
Sub main()

        
Dim swModel As ModelDoc2
        swModel = swApp.NewDocument(
"C:\ProgramData\SOLIDWORKS\SOLIDWORKS 2012\templates\Part.prtdot", 0, 0, 0)

        
If swModel Is Nothing Then
            swApp.SendMsgToUser2("A part document must be active.", swMessageBoxIcon_e.swMbWarning, swMessageBoxBtn_e.swMbOk)
            
Exit Sub
        End If

        Dim modelType As Integer
        modelType = swModel.GetType

        
If modelType <> swDocumentTypes_e.swDocPART Then
            swApp.SendMsgToUser2("A part document must be active.", swMessageBoxIcon_e.swMbWarning, swMessageBoxBtn_e.swMbOk)
            
Exit Sub
        End If

        'Select a plane on which to sketch
        If SelectPlane(swModel) = False Then
            MsgBox("Could not select plane.")
            
Exit Sub
        End If

        'Get point data
        Dim pFocal As SketchPoint
        
Dim pApex As SketchPoint
        
Dim pStart As SketchPoint
        
Dim pEnd As SketchPoint
        
Dim swSkMgr As SketchManager
        swSkMgr = swModel.SketchManager

        
Dim swSelMgr As SelectionMgr
        swSelMgr = swModel.SelectionManager

        
Dim swSketch As Sketch
        swSkMgr.InsertSketch(
True)
        swSketch = swSkMgr.ActiveSketch

        
' Focal point
        pFocal = swSkMgr.CreatePoint(0, -0.025930732990048, 0)
        
' Apex point
        pApex = swSkMgr.CreatePoint(0.0110754938634727, -0.0485199777778575, 0)
        
' Start point
        pStart = swSkMgr.CreatePoint(0.057136404168939, 0.0869770346454566, 0)
        
' End point
        pEnd = swSkMgr.CreatePoint(-0.120690397734139, -0.00465528735997846, 0)

        
Dim vPoint As Object

        ' Make sure a sketch is active
        If swSketch Is Nothing Then
            MsgBox("Please sketch a focal point, apex point, start point, and end point.")
            
Exit Sub
        End If

        vPoint = swSketch.GetSketchPoints2

        
Dim SkParabola As SketchParabola
        SkParabola = swModel.SketchManager.CreateParabola(pFocal.X, pFocal.Y, 0, pApex.X, pApex.Y, 0, pStart.X, pStart.Y, 0, pEnd.X, pEnd.Y, 0)

        swModel.ViewZoomtofit2()
        swSkMgr.InsertSketch(
True)

        
Stop

        swModel.SketchModifyTranslate(pApex.X, pApex.Y, 0.06, -0.01)

    
End Sub

    Public Function SelectPlane(ByVal Plane As ModelDoc2) As Boolean

        Dim featureTemp As Feature
        featureTemp = Plane.FirstFeature

        
While Not featureTemp Is Nothing
            Dim sFeatureName As String
            sFeatureName = featureTemp.GetTypeName2


            
If sFeatureName = "RefPlane" Then
                featureTemp.Select2(True, 0)
                SelectPlane =
True
                Exit Function
            End If


            featureTemp = featureTemp.GetNextFeature

        
End While

    End Function


    Public swApp As SldWorks


End Class

 

 



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