Offset a WorkPlane that is not Driven by an Offset Parameter

By Barbara Han

Issue

I need to offset a WorkPlane in a Part Document that is not driven by a model parameter. How can I do it so other work features based on it are offset as well?

Solution

The following example offsets a selected WorkPlane. After the WorkPlane has been offset it will be driven by a model parameter.

 VBA sample:
Public Function OffsetPartWorkPlane(oWorkPlane As WorkPlane, Offset As Double)
    Dim oPartDoc As PartDocument
    Set oPartDoc = ThisApplication.ActiveDocument
   
    Dim oWorkPlanes As WorkPlanes
    Set oWorkPlanes = oPartDoc.ComponentDefinition.WorkPlanes
   
    Dim oConstrucWorkPoint As WorkPoint
    Set oConstrucWorkPoint = oPartDoc.ComponentDefinition.WorkPoints.AddFixed(oWorkPlane.Plane.RootPoint)
   
    Dim oConstrucWorkAxis As WorkAxis
    Set oConstrucWorkAxis = oPartDoc.ComponentDefinition.WorkAxes.AddFixed(oWorkPlane.Plane.RootPoint, oWorkPlane.Plane.Normal)
   
    Dim oConstrucWorkPlane As WorkPlane
    Set oConstrucWorkPlane = oWorkPlanes.AddByNormalToCurve(oConstrucWorkAxis, oConstrucWorkPoint)
   
    Call oWorkPlane.SetByPlaneAndOffset(oConstrucWorkPlane, Offset)
   
    oConstrucWorkPoint.Visible = False
    oConstrucWorkAxis.Visible = False
    oConstrucWorkPlane.Visible = False
End Function

'Select a WorkPlane and offset it
Public Sub TestOffsetPlane()
    Dim oPartDoc As PartDocument
    Set oPartDoc = ThisApplication.ActiveDocument
    Dim oWorkPlane As WorkPlane
    Set oWorkPlane = oPartDoc.SelectSet.Item(1)
    Call OffsetPartWorkPlane(oWorkPlane, 5)
End Sub
VB.NET sample:
Public Sub OffsetPartWorkPlane()
  Dim m_inventorApp As Inventor.Application = Nothing
  Dim m_quitInventor As Boolean = False
  ' Try to get an active instance of Inventor
  Try
    m_inventorApp = System.Runtime.InteropServices.Marshal.GetActiveObject("Inventor.Application")
  Catch ex As Exception
  End Try
  ' If not active, create a new Inventor session
  If m_inventorApp Is Nothing Then
    Dim inventorAppType As Type = System.Type.GetTypeFromProgID("Inventor.Application")
    m_inventorApp = System.Activator.CreateInstance(inventorAppType)
    m_quitInventor = True
  End If
  Dim oPartDoc As PartDocument
  oPartDoc = m_inventorApp.ActiveDocument
  Dim oWorkPlane As WorkPlane
  oWorkPlane = oPartDoc.SelectSet.Item(1)
  Dim oWorkPlanes As WorkPlanes
  oWorkPlanes = oPartDoc.ComponentDefinition.WorkPlanes
  Dim oConstrucWorkPoint As WorkPoint
  oConstrucWorkPoint = oPartDoc.ComponentDefinition.WorkPoints.AddFixed(oWorkPlane.Plane.RootPoint)
  Dim oConstrucWorkAxis As WorkAxis
  oConstrucWorkAxis = oPartDoc.ComponentDefinition.WorkAxes.AddFixed(oWorkPlane.Plane.RootPoint, oWorkPlane.Plane.Normal)
  Dim oConstrucWorkPlane As WorkPlane
  oConstrucWorkPlane = oWorkPlanes.AddByNormalToCurve(oConstrucWorkAxis, oConstrucWorkPoint)
  oWorkPlane.SetByPlaneAndOffset(oConstrucWorkPlane, 5)
  oConstrucWorkPoint.Visible = False
  oConstrucWorkAxis.Visible = False
  oConstrucWorkPlane.Visible = False
End Sub