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. Select the edge to which you can add a hem.
' 3. Open the Immediate window.
'
' Postconditions:
' 1. Adds an open hem with a custom relief of type Obround and
'    a relief ratio of 1.0.
' 2. Gets the hem type.
' 3. Examine the Immediate window and graphics area.
' -----------------------------------------------------------------

Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Dim CBAObject As SldWorks.CustomBendAllowance
Dim myFeature As SldWorks.Feature
Dim myHem As SldWorks.HemFeatureData
 

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

    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
   

    Set myHem = myFeature.GetDefinition
    Debug.Print "Hem type as defined in swHemTypes_e: " & myHem.Type
End Sub