Get and Add Sketch Points in Hole Wizard Feature Example (VBA)
This example shows how to get and add the sketch points in
a Hole Wizard feature.
'------------------------------------------------------------------------------
' Preconditions:
' 1. Verify that the specified part document template exists.
' 2. Open the Immediate window.
'
' Postconditions:
' 1. Creates a new part document.
' 2. Creates Boss-Extrude1 and #0-80 Tapped Hole1 features.
' 3. Selects #8-80 Tapped Hole1; i.e., the Hole Wizard feature.
' 4. Gets the number of sketch points in the Hole Wizard feature.
' 5. Adds two sketch points to the Hole Wizard feature; thus, adds two more
' holes to the Hole Wizard feature.
' 6. Examine the Immediate window and graphics area.
'-----------------------------------------------------------------------------
Option Explicit
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swSketchMgr As SldWorks.SketchManager
Dim swFeatureMgr As SldWorks.FeatureManager
Dim swFeature As SldWorks.Feature
Dim swSelectionMgr As SldWorks.SelectionMgr
Dim swWizardHoleFeatureData As SldWorks.WizardHoleFeatureData2
Dim swSketchPoint As SldWorks.SketchPoint
Dim sketchLines As Variant
Dim status As Boolean
Dim count As Long
Dim points As Variant
Dim point As Variant
Sub main()
Set swApp = Application.SldWorks
'Create part with Hole Wizard feature
Set swModel = swApp.NewDocument("C:\ProgramData\SolidWorks\SolidWorks 2015\templates\Part.prtdot", 0, 0, 0)
Set swModelDocExt = swModel.Extension
status = swModelDocExt.SetUserPreferenceToggle(swUserPreferenceToggle_e.swSketchAddConstToRectEntity, swUserPreferenceOption_e.swDetailingNoOptionSpecified, False)
status = swModelDocExt.SetUserPreferenceToggle(swUserPreferenceToggle_e.swSketchAddConstLineDiagonalType, swUserPreferenceOption_e.swDetailingNoOptionSpecified, True)
Set swSketchMgr = swModel.SketchManager
sketchLines = swSketchMgr.CreateCornerRectangle(0, 0, 0, 9.68848174375125E-02, -7.08129015764598E-02, 0)
swModel.ClearSelection2 True
status = swModelDocExt.SelectByID2("Line2", "SKETCHSEGMENT", 0, 0, 0, False, 0, Nothing, 0)
status = swModelDocExt.SelectByID2("Line1", "SKETCHSEGMENT", 0, 0, 0, True, 0, Nothing, 0)
status = swModelDocExt.SelectByID2("Line4", "SKETCHSEGMENT", 0, 0, 0, True, 0, Nothing, 0)
status = swModelDocExt.SelectByID2("Line3", "SKETCHSEGMENT", 0, 0, 0, True, 0, Nothing, 0)
Set swFeatureMgr = swModel.FeatureManager
Set swFeature = swFeatureMgr.FeatureExtrusion2(True, False, False, 0, 0, 0.0254, 0.00254, False, False, False, False, 1.74532925199433E-02, 1.74532925199433E-02, False, False, False, False, True, True, True, 0, 0, False)
Set swSelectionMgr = swModel.SelectionManager
swSelectionMgr.EnableContourSelection = False
status = swModelDocExt.SelectByID2("", "FACE", 4.71052662929878E-02, -3.36338467782298E-02, 2.53999999998769E-02, False, 0, Nothing, 0)
Set swFeature = swFeatureMgr.HoleWizard5(4, 0, 27, "#0-80", 1, 0.00119126, 0.0254, 0.020066, 0, 0, 0, 0, 0, 0, 1, 0, 0, -1, -1, -1, "2B", False, True, True, True, True, False)
swModel.ViewZoomtofit2
status = swModelDocExt.SelectByID2("#0-80 Tapped Hole1", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
Set swFeature = swSelectionMgr.GetSelectedObject6(1, -1)
swModel.ClearSelection2 True
Set swWizardHoleFeatureData = swFeature.GetDefinition
count = swWizardHoleFeatureData.GetSketchPointCount
Debug.Print " Number of sketch points in original Hole Wizard Feature = " & count
points = swWizardHoleFeatureData.GetSketchPoints
For Each point In points
Set swSketchPoint = point
swSketchPoint.Select4 False, Nothing
Next
status = swFeature.ModifyDefinition(swWizardHoleFeatureData, swModel, Nothing)
swModel.ClearSelection2 True
'Select sketch point of Hole Wizard feature
'and add two sketch points to Hole Wizard feature
status = swModelDocExt.SelectByID2("Sketch3", "SKETCH", 0, 0, 0, False, 0, Nothing, 0)
swSketchMgr.AddToDB = True
swModel.EditSketch
Set swSketchPoint = swSketchMgr.CreatePoint(0.01, -0.04, 0)
Set swSketchPoint = swSketchMgr.CreatePoint(0.01, -0.02, 0)
swSketchMgr.InsertSketch True
swSketchMgr.AddToDB = False
swModel.ForceRebuild3 True
'Get number of sketch points in modified Hole Wizard feature
status = swModelDocExt.SelectByID2("#0-80 Tapped Hole1", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
Set swFeature = swSelectionMgr.GetSelectedObject6(1, -1)
swModel.ClearSelection2 True
Set swWizardHoleFeatureData = swFeature.GetDefinition
count = swWizardHoleFeatureData.GetSketchPointCount
Debug.Print " Number of sketch points in modified Hole Wizard Feature = " & count
points = swWizardHoleFeatureData.GetSketchPoints
For Each point In points
Set swSketchPoint = point
swSketchPoint.Select4 False, Nothing
Next
status = swFeature.ModifyDefinition(swWizardHoleFeatureData, swModel, Nothing)
swModel.ClearSelection2 True
End Sub