Create Circular Pattern Example (VBA)

This example shows how to create a circular-pattern feature using a preselected axis, a preselected feature, and a specified angle between instances.

'--------------------------------------------------------------
' Preconditions: Make sure that the specified file exists.
'
' Postconditions: A circular-pattern feature is created.
'
' NOTE: Because the model is used elsewhere, do not
' save any changes when closing it.
'--------------------------------------------------------------
Option Explicit

Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swFeatureMgr As SldWorks.FeatureManager
Dim swFeature As SldWorks.Feature
Dim status As Boolean
Dim warnings As Long
Dim errors As Long

Sub main()

Set swApp = Application.SldWorks

Set swModel = swApp.OpenDoc6("C:\Program Files\SolidWorks Corp\SolidWorks\samples\tutorial\api\FeatureCircularPattern.SLDPRT", swDocPART, swOpenDocOptions_Silent, "", errors, warnings)
Set swModelDocExt = swModel.Extension
Set swFeatureMgr = swModel.FeatureManager

' Select boss feature to use for circular pattern; selection mark is 4
status = swModelDocExt.SelectByID2("Boss-Extrude2", "BODYFEATURE", 0, 0, 0, False, 4, Nothing, 0)
' Select axis around which to create circular pattern; selection mark is 1
status = swModelDocExt.SelectByID2("Axis1", "AXIS", 0, 0, 0, True, 1, Nothing, 0)

' Create circular-pattern feature
Set swFeature = swFeatureMgr.FeatureCircularPattern2(6, 1.047197551197, False, "NULL", False)

End Sub