Hide Table of Contents

Insert Sweep Cut Feature Example (VBA)

This example shows how to create a sweep cut feature and get its properties.

'-----------------------------------------------------------------------------
' Preconditions:

' 1. Ensure that the specified document exists.
' 2. Open an Immediate Window.
'
' Postconditions:
' 1. Cut-Sweep1 is in the FeatureManager design tree.
' 2. Inspect the Immediate Window for sweep feature data.
'
' NOTE: Because this part document is used by other macros,
'       do not save any changes when closing the document.
'------------------------------------

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

Public Enum swTangencyType_e
    swTangencyNone = 0
    swTangencyNormalToProfile = 1
    swTangencyDirectionVector = 2
    swTangencyAllFaces = 3
End Enum

Public Enum swThinWallType_e
    swThinWallOneDirection = 0
    swThinWallOppDirection = 1
    swThinWallMidPlane = 2
    swThinWallTwoDirection = 3
End Enum

Public Enum swTwistControlType_e
    swTwistControlFollowPath = 0
    swTwistControlKeepNormalConstant = 1
    swTwistControlFollowPathFirstGuideCurve = 2
    swTwistControlFollowFirstSecondGuideCurves = 3
End Enum

Public Enum swCutSweepOption_e
    swProfileSweep = 1
    swSolidSweep = 2
End Enum

Sub main()

Set swApp = Application.SldWorks

Set Part = swApp.OpenDoc6("C:\program files\SolidWorks Corp\SolidWorks\samples\tutorial\api\sweepcutextrude.SLDPRT", 1, 0, "", longstatus, longwarnings)
swApp.ActivateDoc2 "sweepcutextrude.SLDPRT", False, longstatus
Set Part = swApp.ActiveDoc
Dim myModelView As Object
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) ' profile has Mark = 1
boolstatus = Part.Extension.SelectByID2("Sketch3", "SKETCH", -0.03797488317814, -0.02133214444164, 0, True, 4, Nothing, 0) ' path sweep has Mark = 4
Dim myFeature As SldWorks.Feature
Set myFeature = Part.FeatureManager.InsertCutSwept4(False, True, 0, False, False, 0, 0, False, 0, 0, 0, 0, True, True, 0, True, True, True, False)

Set swSweep = myFeature.GetDefinition
Set swProfFeat = swSweep.Profile: Debug.Assert Not Nothing Is swProfFeat
Set swProfSketch = swProfFeat.GetSpecificFeature: Debug.Assert Not Nothing Is swProfSketch

' Rollback to access selections
bRet = swSweep.AccessSelections(Part, Nothing): Debug.Assert bRet

Set swPathFeat = swSweep.Path: Debug.Assert Not Nothing Is swPathFeat
Set swPathSketch = swPathFeat.GetSpecificFeature: Debug.Assert Not Nothing Is swPathSketch

Debug.Print "File = " & Part.GetPathName
Debug.Print "  " & myFeature.Name
Debug.Print "    Path                      = " & swPathFeat.Name
Debug.Print "    Path alignment type       = " & swSweep.PathAlignmentType 'swTangencyType_e
Debug.Print "    Profile                   = " & swProfFeat.Name
Debug.Print "    AdvancedSmoothing         = " & swSweep.AdvancedSmoothing
Debug.Print "    AlignWithEndFaces         = " & swSweep.AlignWithEndFaces
Debug.Print "    AutoSelect                = " & swSweep.AutoSelect
Debug.Print "    AutoSelectComponents      = " & swSweep.AutoSelectComponents
Debug.Print "    EndTangencyType           = " & swSweep.EndTangencyType   'swTangencyType_e
Debug.Print "    AssemblyFeatureScope      = " & swSweep.AssemblyFeatureScope
Debug.Print "    FeatureScope              = " & swSweep.FeatureScope
Debug.Print "    FeatureScopeBodiesCnt     = " & swSweep.GetFeatureScopeBodiesCount
Debug.Print "    GetPathType               = " & swSweep.GetPathType       'swSelectType_e
Debug.Print "    Wall thickness foward     = " & swSweep.GetWallThickness(True) * 1000# & " mm"
Debug.Print "    Wall thickness reverse    = " & swSweep.GetWallThickness(False) * 1000# & " mm"
Debug.Print "    IsBossFeature             = " & swSweep.IsBossFeature
Debug.Print "    IsThinFeature             = " & swSweep.IsThinFeature
Debug.Print "    MaintainTangency          = " & swSweep.MaintainTangency
Debug.Print "    Merge                     = " & swSweep.Merge
Debug.Print "    MergeSmoothFaces          = " & swSweep.MergeSmoothFaces
Debug.Print "    PropagateFeatureToParts   = " & swSweep.PropagateFeatureToParts
Debug.Print "    StartTangencyType         = " & swSweep.StartTangencyType 'swTangencyType_e
Debug.Print "    TangentPropagation        = " & swSweep.TangentPropagation
Debug.Print "    ThinWallType              = " & swSweep.ThinWallType
Debug.Print "    TwistControlType          = " & swSweep.TwistControlType  'swTwistControlType_e
Debug.Print "    CutSweepOption            = " & swSweep.GetCutSweepOption  'swCutSweepOption_e

' Roll forward
swSweep.ReleaseSelectionAccess

End Sub

 



Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

 
*Email:  
Subject:   Feedback on Help Topics
Page:   Insert Sweep Cut Feature Example (VBA)
*Comment:  
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:



x

We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again
x

Web Help Content Version: API Help (English only) 2014 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.