Get Sketch Points in Hole Wizard Feature Example (VBA)

This example shows how to get the center-hole sketch points  in a hole wizard feature.

 

'---------------------------------------------------

'

' Preconditions:

'            (1) Part document is open.

'            (2) Part contains an M12x1.75 Tapped Hole1 hole wizard feature.

'

' Postconditions: None

'

'----------------------------------------------------

 

Option Explicit

 

Sub main()

 

    Dim swApp As SldWorks.SldWorks

    Dim swModel As SldWorks.ModelDoc2

    Dim FeatureData As SldWorks.WizardHoleFeatureData2

    Dim Feature As SldWorks.Feature

    Dim swModelDocExt As SldWorks.ModelDocExtension

    Dim swSelMgr As SldWorks.SelectionMgr

    Dim Component As Object

    Dim pt As Variant

    Dim swSketchPoint As SldWorks.SketchPoint

    Dim boolstatus As Boolean

    Dim longstatus As Long

    Dim longwarnings As Long

    Dim vPtArr As Variant

    Dim nCount As Long

 

    Set swApp = Application.SldWorks

    Set swModel = swApp.ActiveDoc

    Set swModelDocExt = swModel.Extension

    Set swSelMgr = swModel.SelectionManager

    swModel.ShowNamedView2 "*Isometric", 7

    swModel.ViewZoomtofit2

    swModel.ClearSelection2 True

    boolstatus = swModelDocExt.SelectByID2("M12x1.75 Tapped Hole1", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, swSelectOptionDefault)

    Set Feature = swSelMgr.GetSelectedObject5(1)

    Set Component = swSelMgr.GetSelectedObjectsComponent2(1)

    swModel.ClearSelection2 True

    Set FeatureData = Feature.GetDefinition

       

    nCount = FeatureData.GetSketchPointCount

    Debug.Print " Sketch Point Count = " & nCount

    

    vPtArr = FeatureData.GetSketchPoints

    For Each pt In vPtArr

        Set swSketchPoint = pt

        pt.Select4 False, Nothing

    Next

    boolstatus = Feature.ModifyDefinition(FeatureData, swModel, Nothing)

    

End Sub