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Insert Swept-cut Feature Using Sketch Profile Example (VBA)

This example shows how to create a swept-cut feature using a sketch profile and get its properties.

'----------------------------------------------------------------------------
' Preconditions:
' 1. Verify that the part to open exists.
' 2. Open an Immediate window.
'
' Postconditions:
' 1. Creates Cut-Sweep1.
' 2. Inspect the FeatureManager design tree, graphics area,
'    and Immediate window.
'
' NOTE: Because this part document is used elsewhere, do not save changes.
'---------------------------------------------------------------------------
Option Explicit

Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Dim boolstatus As Boolean
Dim longstatus As Long, longwarnings As Long
Dim swSweep As SldWorks.SweepFeatureData
Dim swProfFeat As SldWorks.Feature
Dim swProfSketch As SldWorks.Sketch
Dim swPathFeat As SldWorks.Feature
Dim swPathSketch As SldWorks.Sketch
Dim bRet As Boolean
Dim myModelView As Object
Dim myFeature As SldWorks.Feature

Sub main()

Set swApp = Application.SldWorks

Set Part = swApp.OpenDoc6("C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2018\samples\tutorial\api\sweepcutextrude.SLDPRT", 1, 0, "", longstatus, longwarnings)
swApp.ActivateDoc2 "sweepcutextrude.SLDPRT", False, longstatus
Set Part = swApp.ActiveDoc

Set myModelView = Part.ActiveView
myModelView.FrameLeft = 0
myModelView.FrameTop = 0

myModelView.FrameState = swWindowState_e.swWindowMaximized
Part.ShowNamedView2 "*Isometric", 7

boolstatus = Part.Extension.SelectByID2("Sketch2", "SKETCH", 0.01948983274156, -0.02564816935317, 0, False, 1, Nothing, 0)
boolstatus = Part.Extension.SelectByID2("Sketch3", "SKETCH", -0.03797488317814, -0.02133214444164, 0, True, 4, Nothing, 0)
 

Set swSweep = Part.FeatureManager.CreateDefinition(swFmSweepCut)


swSweep.TwistControlType = 0

swSweep.PathAlignmentType = 0

swSweep.CircularProfile = False


Set myFeature = Part.FeatureManager.CreateFeature(swSweep)

Set swSweep = myFeature.GetDefinition
Set swProfFeat = swSweep.Profile
Set swProfSketch = swProfFeat.GetSpecificFeature


bRet = swSweep.AccessSelections(Part, Nothing)

Set swPathFeat = swSweep.Path
Set swPathSketch = swPathFeat.GetSpecificFeature

Debug.Print "File = " & Part.GetPathName
Debug.Print "  " & myFeature.Name
Debug.Print "    Sweep path  = " & swPathFeat.Name
Debug.Print "    Path type as defined in swSelectType_e  = " & swSweep.GetPathType      
Debug.Print "    Path alignment type as defined in swTangencyType_e  = " & swSweep.PathAlignmentType
Debug.Print "    Sweep Profile  = " & swProfFeat.Name
Debug.Print "    Profile type as defined in swSelectType_e  = " & swSweep.GetProfileType
Debug.Print "    Profile orientation/twist type as defined in swTwistControlType_e  = " & swSweep.TwistControlType 
Debug.Print "    Cut sweep type as defined in swCutSweepOption_e    = " & swSweep.GetCutSweepOption
Debug.Print "    Align sweep with end faces? " & swSweep.AlignWithEndFaces
Debug.Print "    Automatically select all bodies to be affected if a multibody part? " & swSweep.AutoSelect
Debug.Print "    Start of sweep tangency type as defined in swTangencyType_e   = " & swSweep.StartTangencyType  
Debug.Print "    End of sweep tangency type as defined in swTangencyType_e   = " & swSweep.EndTangencyType  
Debug.Print "    Only specific bodies affected by this sweep feature? " & swSweep.FeatureScope
Debug.Print "    Feature scope bodies count = " & swSweep.GetFeatureScopeBodiesCount
Debug.Print "    Is a boss feature? " & swSweep.IsBossFeature
Debug.Print "    Is a thin-walled feature? " & swSweep.IsThinFeature
Debug.Print "    Thin-walled type (0=1D, 1=1DReverse, 2=MidPlane, 3=2D)  = " & swSweep.ThinWallType
Debug.Print "    Wall thickness Direction 1  = " & swSweep.GetWallThickness(True) * 1000# & " mm"
Debug.Print "    Wall thickness Direction 2  = " & swSweep.GetWallThickness(False) * 1000# & " mm"
Debug.Print "    Merge tangent faces? " & swSweep.MaintainTangency
Debug.Print "    Merge results if a multibody part? " & swSweep.Merge
Debug.Print "    Merge smooth faces if using guide curves? " & swSweep.MergeSmoothFaces

swSweep.ReleaseSelectionAccess

End Sub

 



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