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

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

'---------------------------------------------------------------------------
' Preconditions:
' 1. Verify that the part exists.
' 2. Open an Immediate window.
'
' Postconditions:
' 1. Opens the part.
' 2. Selects an edge on the part.
' 3. Creates a cut-sweep feature using a circular profile.
' 4. Accesses the cut-sweep feature.
' 5. Changes the diameter of the circular profile.
' 6. Examine the Immediate window, FeatureManager
'    design tree, and graphics area.
'
' NOTE: Because the part is used elsewhere, do not save changes.
'---------------------------------------------------------------------------
Option Explicit

Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swPathFeat As SldWorks.Feature
Dim swFeatureManager As SldWorks.FeatureManager
Dim swSweep As SldWorks.SweepFeatureData
Dim status As Boolean
Dim errors As Long
Dim warnings As Long

Sub main()

    Set swApp = Application.SldWorks
    Set swModel = swApp.OpenDoc6("C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2018\samples\tutorial\api\block20.sldprt", 1, 0, "", errors, warnings)
    Set swModelDocExt = swModel.Extension    

    'Select an edge for the circular profile
    status = swModelDocExt.SelectByID2("", "EDGE", -3.72983839416747E-02, 3.93904284381961E-02, 4.95042874504179E-02, True, 4, Nothing, 0)
    Set swFeatureManager = swModel.FeatureManager    

    Set swSweep = swModel.FeatureManager.CreateDefinition(swFmSweepCut)

    swSweep.TangentPropagation = False
    swSweep.AlignWithEndFaces = True
    swSweep.TwistControlType = 0
    swSweep.MaintainTangency = False
    swSweep.AdvancedSmoothing = False
    swSweep.StartTangencyType = 0
    swSweep.EndTangencyType = 0
    swSweep.PathAlignmentType = 0
    swSweep.FeatureScope = True
    swSweep.AutoSelect = True
    swSweep.MergeSmoothFaces = True
    swSweep.CircularProfile = True
    swSweep.CircularProfileDiameter = 0.008

    Set swPathFeat = swModel.FeatureManager.CreateFeature(swSweep)
 
    Set swSweep = swPathFeat.GetDefinition
    status = swSweep.AccessSelections(swModel, Nothing)
    Debug.Print "Using a circular profile? " & swSweep.CircularProfile
    Debug.Print "Original size of circular profile = " & swSweep.CircularProfileDiameter
    swSweep.CircularProfileDiameter = 0.003
    Debug.Print "Modified size of circular profile = " & swSweep.CircularProfileDiameter  
    swPathFeat.ModifyDefinition swSweep, swModel, Nothing   

End Sub