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Create Corner Relief Feature Example (VBA)

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.
'----------------------------------------------------------------------------

Option Explicit

Sub main()

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

    ' Connect to SOLIDWORKS
    Set swApp = Application.SldWorks

    ' Get active document
    Set swModel = swApp.ActiveDoc

    ' Flange parameters

    ' Set the angle
    dAngle = (90# / 180#) * 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", 3.72105002552985E-02, 0.052846642716446, -9.93711211094706E-06, False, 0, Nothing, 0)

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

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

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

    ' Start sketch editing
    swModel.EditSketch

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

    ' Add the edge to the sketch

    ' Cast edge to entity
    Set 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

    Set swSketchLine = vSketchSegments(0)

    ' Get start and end point
    Set swStartPoint = swSketchLine.GetStartPoint2
    Set 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#, swStartPoint.X, swStartPoint.Y + dLength, 0#
    swModel.SketchManager.CreateLine swStartPoint.X, swStartPoint.Y + dLength, 0#, swStartPoint.X + dFactor1 * dSize, swStartPoint.Y + dFactor2 * dLength, 0#
    swModel.SketchManager.CreateLine swStartPoint.X + dFactor1 * dSize, swStartPoint.Y + dFactor2 * dLength, 0#, swEndPoint.X - dFactor1 * dSize, swStartPoint.Y + dFactor2 * dLength, 0#
    swModel.SketchManager.CreateLine swEndPoint.X - dFactor1 * dSize, swStartPoint.Y + dFactor2 * dLength, 0#, swEndPoint.X, swEndPoint.Y + dLength, 0#
    swModel.SketchManager.CreateLine swEndPoint.X, swEndPoint.Y, 0#, swEndPoint.X, swEndPoint.Y + dLength, 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

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

    vFlangeEdges = aFlangeEdges
    vSketchFeats = aSketchFeats

    Set swFeature = swModel.FeatureManager.InsertSheetMetalEdgeFlange2((vFlangeEdges), (vSketchFeats), nOptions, dAngle, 0#, swFlangePositionTypes_e.swFlangePositionTypeBendOutside, dLength, swSheetMetalReliefTypes_e.swSheetMetalReliefNone, 0#, 0#, 0#, swFlangeDimTypes_e.swFlangeDimTypeInnerVirtualSharp, Nothing)

    ' Rotate view so that IModelDocExtension::SelectByID2 coordinates can be found
    Dim myModelView As SldWorks.ModelView
    Set myModelView = swModel.ActiveView
    myModelView.RotateAboutCenter 45, 9.11235438195936E-03

    ' 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", 5.49242492243928E-02, 0.053073918098565, 2.42634000000049E-02, True, 4, Nothing, 0)
    bValue = swModel.Extension.SelectByID2("", "FACE", 2.76778697571744E-02, 5.30739180985651E-02, -1.04170971004399E-03, 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, 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", 2.76778697571744E-02, 5.30739180985651E-02, -1.04170971004399E-03, True, 4, Nothing, 0)
    bValue = swModel.Extension.SelectByID2("", "FACE", 4.31490289955978E-04, 0.053073918098565, 2.42634000000049E-02, 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, swCornerObroundRelief, 0.0001, 0.0029464, 0.0007366, False, False, False, False, False)

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

End Sub

 



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