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Constrain Sketch Example (VB.NET)

This example shows how to fully constrain a sketch.

 

Before constraining the sketch

After constraining the sketch

 

 

 

'----------------------------------------------------------------------------
' Preconditions: Before constraining the sketch sketch exists.
'
' Postconditions: Fully constrains the sketch, which looks like
' After constraining the sketch.
'----------------------------------------------------------------------------


Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System.Runtime.InteropServices
Imports System

Partial Class SolidWorksMacro

    
Dim swModel As ModelDoc2
    
Dim swSketchMgr As SketchManager
    
Dim swSketch As Sketch
    
Dim swSelMgr As SelectionMgr
    
Dim swFeat As Feature
    
Dim nSketchStatus As Long
    Dim boolstatus As Boolean


    Sub main()

        swModel = swApp.ActiveDoc

        
' Is a model document active?
        If swModel Is Nothing Then

            swApp.SendMsgToUser2("A part document must be open and the active document.", swMessageBoxIcon_e.swMbWarning, swMessageBoxBtn_e.swMbOk)
            
Exit Sub

        End If

        ' Is it a part document?
        Dim modelType As Long
        modelType = swModel.GetType

        
If modelType <> swDocumentTypes_e.swDocPART Then

            swApp.SendMsgToUser2("A part document must be open and the active document.", swMessageBoxIcon_e.swMbWarning, swMessageBoxBtn_e.swMbOk)
            
Exit Sub

        End If


        swSketchMgr = swModel.SketchManager
        swSketch = swSketchMgr.ActiveSketch

        
If swSketch Is Nothing Then

            swApp.SendMsgToUser2("No active sketch; thus, a sketch could not be selected.", swMessageBoxIcon_e.swMbWarning, swMessageBoxBtn_e.swMbOk)
            
Exit Sub

        End If

        ' Select the lines and make them colinear and vertical
        boolstatus = swModel.Extension.SelectByID2("Line2", "SKETCHSEGMENT", 0.02116924482339, 0.04904427527406, 0, False, 0, Nothing, 0)
        boolstatus = swModel.Extension.SelectByID2(
"Line3", "SKETCHSEGMENT", 0.06508556638246, 0.02563976857491, 0, True, 0, Nothing, 0)

        swModel.SketchAddConstraints(
"sgCOLINEAR")
        swModel.SketchAddConstraints(
"sgVERTICAL2D")

        MsgBox(
"The lines have been selected, made colinear, and vertically constrained.")
        swModel.ClearSelection2(
True)

        
'Select the center of the circles and constrain them to the origin
        boolstatus = swModel.Extension.SelectByID2("Point7", "SKETCHPOINT", 0.1074240560292, 0.006179841656516, 0, False, 0, Nothing, 0)
        boolstatus = swModel.Extension.SelectByID2(
"Point1@Origin", "EXTSKETCHPOINT", 0, 0, 0, True, 0, Nothing, 0)

        swModel.SketchAddConstraints(
"sgCOINCIDENT")
        MsgBox(
"The center of the circles and the origin were selected and made coincident")
        swModel.ClearSelection2(
True)

        
' Select a line and the circle and make them tangent
        boolstatus = swModel.Extension.SelectByID2("Line2", "SKETCHSEGMENT", 0.005390925700365, 0.009861449451888, 0, False, 0, Nothing, 0)
        boolstatus = swModel.Extension.SelectByID2(
"Arc1", "SKETCHSEGMENT", -0.01222819732034, 0.04720347137637, 0, True, 0, Nothing, 0)

        swModel.SketchAddConstraints(
"sgTANGENT")
        MsgBox(
"One line and a cirle were selected; both lines are now tangent with the circle.")
        swModel.ClearSelection2(
True)

        
'Select the circles and make them concentric
        boolstatus = swModel.Extension.SelectByID2("Arc2", "SKETCHSEGMENT", -0.0290584043849, 0.03116218026797, 0, False, 0, Nothing, 0)
        boolstatus = swModel.Extension.SelectByID2(
"Arc1", "SKETCHSEGMENT", -0.01222819732034, 0.04720347137637, 0, True, 0, Nothing, 0)

        swModel.SketchAddConstraints(
"sgCONCENTRIC")
        MsgBox(
"The circles have been selected and made concentric.")
        swModel.ClearSelection2(
True)

        
'Select all the sketch entities and fix their positions
        MsgBox("All  sketch entities will be selected and made fixed to fully constrain the sketch.")
        boolstatus = swModel.Extension.SelectByID2(
"Line2", "SKETCHSEGMENT", 0.02116924482339, 0.04904427527406, 0, False, 0, Nothing, 0)
        boolstatus = swModel.Extension.SelectByID2(
"Line3", "SKETCHSEGMENT", 0.06508556638246, 0.02563976857491, 0, True, 0, Nothing, 0)
        boolstatus = swModel.Extension.SelectByID2(
"Arc2", "SKETCHSEGMENT", -0.0290584043849, 0.03116218026797, 0, False, 0, Nothing, 0)
        boolstatus = swModel.Extension.SelectByID2(
"Arc1", "SKETCHSEGMENT", -0.01222819732034, 0.04720347137637, 0, True, 0, Nothing, 0)

        swModel.SketchAddConstraints(
"sgFIXED")
        swModel.ClearSelection2(
True)

    
End Sub


    Public swApp As SldWorks


End Class

 

 



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