Insert Sheet Metal Hem Example (VBA)

This example shows how to insert a hem into a sheet metal part.

'----------------------------------------------------------------------------
' Preconditions:
' 1. Open a sheet metal part.
' 2. Specify the coordinates of the edge to which to add a hem in SelectByID2.
'
' Postconditions: Hem1 is added to the FeatureManager design tree
' with a custom relief of type Obround and a relief ratio of 1.0.
'
' NOTE: Because the model is used elsewhere,
' do not save changes when closing it.
' ---------------------------------------------------------------------------

Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Dim CBAObject As SldWorks.CustomBendAllowance
Dim myFeature As SldWorks.Feature
Dim boolstatus As Boolean

Option Explicit
Sub main()
    Set swApp = Application.SldWorks
    Set Part = swApp.ActiveDoc

    boolstatus = Part.Extension.SelectByID2("", "EDGE", -0.07026043643646, 0.06501174209842, 0.04893806198987, False, 0, Nothing, 0)

    Set CBAObject = Part.FeatureManager.CreateCustomBendAllowance()
    CBAObject.Type = 2
    CBAObject.KFactor = 0.5
   

    ' Insert an open hem of custom relief type Obround and relief ratio 1.0
    Set myFeature = Part.FeatureManager.InsertSheetMetalHem2(swHemTypes_e.swHemTypeOpen, swHemPositionTypes_e.swHemPositionTypeOutside, False, 0.01, 0.01, 0, 0.005, 0.0011, CBAObject, False, swSheetMetalReliefTypes_e.swSheetMetalReliefObround, 0, True, 1#, 0, 0)
    Part.ClearSelection2 True
End Sub