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Create Corner Relief Feature Example (VB.NET)

This example shows how to create a corner relief feature.

'----------------------------------------------------------------------------
' Preconditions:
' Open install_dir\samples\tutorial\sheetmetal\formtools\cover.sldprt.
'
' Postconditions:
' 1. The model is rotated to the back view.
' 2. An edge flange is created.
' 3. The model is rotated slightly about the x-axis.
' 4. A corner relief feature is created:
'    * A rectangular corner relief is added to one corner of the edge flange.
'    * An obround corner relief is added to another corner of the edge flange.
'----------------------------------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System.Runtime.InteropServices
Imports System

Partial Class SolidWorksMacro

    
Sub main()

        
Dim swModel As ModelDoc2
        
Dim bValue As Boolean
        Dim swEdge As Edge
        
Dim dAngle As Double
        Dim dLength As Double
        Dim swFeature As Feature
        
Dim swEntity As Entity
        
Dim swSketch As Sketch
        
Dim vSketchSegments As Object
        Dim swSketchLine As SketchLine
        
Dim swStartPoint As SketchPoint
        
Dim swEndPoint As SketchPoint
        
Dim nOptions As swInsertEdgeFlangeOptions_e
        
Dim dSize As Double
        Dim dFactor1 As Double
        Dim dFactor2 As Double
        Dim aFlangeEdges(0) As Edge
        
Dim vFlangeEdges As Object
        Dim aSketchFeats(0) As Sketch
        
Dim vSketchFeats As Object

        ' Get active document
        swModel = swApp.ActiveDoc

        
' Flange parameters

        ' Set the angle
        dAngle = (90.0# / 180.0#) * 3.1415926535897

        dLength = 0.01

        
' Rotate model so that IModelDocExtension::SelectByID2 coordinates can be found
        swModel.ShowNamedView2("*Back", -1)
        swModel.ViewZoomtofit2()

        
' Select edge for flange
        bValue = swModel.Extension.SelectByID2("", "EDGE", 0.0372105002552985, 0.052846642716446, -0.00000993711211094706, False, 0, Nothing, 0)

        
' Get edge
        swEdge = swModel.SelectionManager.GetSelectedObject6(1, -1)

        
' Insert a sketch for an edge flange
        swFeature = swModel.InsertSketchForEdgeFlange(swEdge, dAngle, False)

        
' Select
        bValue = swFeature.Select2(False, 0)

        
' Start sketch editing
        swModel.EditSketch()

        
' Get the active sketch
        swSketch = swModel.SketchManager.ActiveSketch

        
' Add the edge to the sketch

        ' Cast edge to entity
        swEntity = swEdge

        
' Select edge
        bValue = swEntity.Select4(False, Nothing)

        
' Use the edge in the sketch
        bValue = swModel.SketchManager.SketchUseEdge(False)

        
' Get the created sketch line
        vSketchSegments = swSketch.GetSketchSegments

        swSketchLine = vSketchSegments(0)

        
' Get start and end point
        swStartPoint = swSketchLine.GetStartPoint2
        swEndPoint = swSketchLine.GetEndPoint2

        
' Create additional lines to define sketch
        ' Set parameters defining the sketch geometry
        dSize = swEndPoint.X - swStartPoint.X
        dFactor1 = 0.1
        dFactor2 = 1.25

        swModel.SetAddToDB(
True)
        swModel.SetDisplayWhenAdded(
False)

        swModel.SketchManager.CreateLine(swStartPoint.X, swStartPoint.Y, 0.0#, swStartPoint.X, swStartPoint.Y + dLength, 0.0#)
        swModel.SketchManager.CreateLine(swStartPoint.X, swStartPoint.Y + dLength, 0.0#, swStartPoint.X + dFactor1 * dSize, swStartPoint.Y + dFactor2 * dLength, 0.0#)
        swModel.SketchManager.CreateLine(swStartPoint.X + dFactor1 * dSize, swStartPoint.Y + dFactor2 * dLength, 0.0#, swEndPoint.X - dFactor1 * dSize, swStartPoint.Y + dFactor2 * dLength, 0.0#)
        swModel.SketchManager.CreateLine(swEndPoint.X - dFactor1 * dSize, swStartPoint.Y + dFactor2 * dLength, 0.0#, swEndPoint.X, swEndPoint.Y + dLength, 0.0#)
        swModel.SketchManager.CreateLine(swEndPoint.X, swEndPoint.Y, 0.0#, swEndPoint.X, swEndPoint.Y + dLength, 0.0#)

        
' Reset
        swModel.SetDisplayWhenAdded(True)
        swModel.SetAddToDB(
False)

        
' Commit changes made to the sketch
        swModel.SketchManager.InsertSketch(True)

        
' Set options
        nOptions = swInsertEdgeFlangeOptions_e.swInsertEdgeFlangeUseDefaultRadius + swInsertEdgeFlangeOptions_e.swInsertEdgeFlangeUseDefaultRelief

        aFlangeEdges(0) = swEdge
        aSketchFeats(0) = swSketch

        vFlangeEdges = aFlangeEdges
        vSketchFeats = aSketchFeats

        swFeature = swModel.FeatureManager.InsertSheetMetalEdgeFlange2((vFlangeEdges), (vSketchFeats), nOptions, dAngle, 0.0#, swFlangePositionTypes_e.swFlangePositionTypeBendOutside, dLength, swSheetMetalReliefTypes_e.swSheetMetalReliefNone, 0.0#, 0.0#, 0.0#, swFlangeDimTypes_e.swFlangeDimTypeInnerVirtualSharp,
Nothing)

        
' Rotate view so that IModelDocExtension::SelectByID2 coordinates can be found
        Dim myModelView As ModelView
        myModelView = swModel.ActiveView
        myModelView.RotateAboutCenter(45, 0.00911235438195936)

        
' Select the sheet metal body to which to apply a corner relief
        bValue = swModel.Extension.SelectByID2("Edge-Flange1", "SOLIDBODY", 0, 0, 0, True, 0, Nothing, 0)
        swModel.ClearSelection2(
True)

        
' Specify two corners of the edge flange for which to create a corner relief

        ' Select faces that define the first corner
        bValue = swModel.Extension.SelectByID2("", "FACE", 0.0549242492243928, 0.053073918098565, 0.0242634000000049, True, 4, Nothing, 0)
        bValue = swModel.Extension.SelectByID2(
"", "FACE", 0.0276778697571744, 0.0530739180985651, -0.00104170971004399, True, 4, Nothing, 0)
        
Dim myCorner As Long
        myCorner = swModel.FeatureManager.AddCornerReliefCorner()

        
' Specify the type of corner relief to apply to the first corner
        Dim myReliefType As Boolean
        myReliefType = swModel.FeatureManager.AddCornerReliefType(-1, swCornerReliefType_e.swCornerSquareRelief, 0.0001, 0.0007366, 0.00018415, False, False, False, True, False)
        swModel.ClearSelection2(
True)

        
' Select faces that define the second corner
        bValue = swModel.Extension.SelectByID2("", "FACE", 0.0276778697571744, 0.0530739180985651, -0.00104170971004399, True, 4, Nothing, 0)
        bValue = swModel.Extension.SelectByID2(
"", "FACE", 0.000431490289955978, 0.053073918098565, 0.0242634000000049, True, 4, Nothing, 0)
        myCorner = swModel.FeatureManager.AddCornerReliefCorner()

        
' Specify the type of corner relief to apply to the second corner
        myReliefType = swModel.FeatureManager.AddCornerReliefType(-1, swCornerReliefType_e.swCornerObroundRelief, 0.0001, 0.0029464, 0.0007366, False, False, False, False, False)

        
' Create the corner relief feature
        Dim myFeature As Feature
        myFeature = swModel.FeatureManager.FinishCornerRelief()

    
End Sub


    Public swApp As SldWorks


End Class

 



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