Sub AddSMNormalCutType( _
   ByVal AutoPropagation As System.Boolean, _
   ByVal Optimize As System.Boolean, _
   ByVal BExtent As System.Boolean _
) 

Dim instance As IFeatureManager
Dim AutoPropagation As System.Boolean
Dim Optimize As System.Boolean
Dim BExtent As System.Boolean
 
instance.AddSMNormalCutType(AutoPropagation, Optimize, BExtent)

void AddSMNormalCutType( 
   System.bool AutoPropagation,
   System.bool Optimize,
   System.bool BExtent
)

void AddSMNormalCutType( 
&   System.bool AutoPropagation,
&   System.bool Optimize,
&   System.bool BExtent
) 

Parameters

AutoPropagation

True to automatically propagate the Normal Cut, false to not

Optimize

True to optimize geometry, false to not

BExtent

True to maximize the cutout using the top and bottom intersection profiles, false to use an offset plane

'VBA

'1. Open a sheet metal part that has two cut extrudes.
'2. Modify the macro below as needed.

Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Dim myFeature As SldWorks.Feature
Dim myNormalCutFeatData As SldWorks.SMNormalCutFeatureData
Dim boolstatus As Boolean

Option Explicit
Sub main()

    Set swApp = Application.SldWorks
    Set Part = swApp.ActiveDoc

    'Select a cut-extrude face for which to create a Normal Cut
    boolstatus = Part.Extension.SelectByRay(-6.38655841527864E-02, -1.56055561574817E-02, 3.58410081097382E-03, -9.80322952634684E-02, -0.994744620924993, -2.95433279467378E-02, 2.7317052985792E-04, 2, False, 1, 0)
    Dim OneFaceGroup As Long
    OneFaceGroup = Part.FeatureManager.AddSMNormalCut()
    Part.ClearSelection2 True

    
    'Use an offset plane to create the Normal Cut feature
    boolstatus = Part.Extension.SelectByRay(-6.00249578326526E-02, -1.83129588701831E-02, 1.70249820822459E-02, -9.80322952634684E-02, -0.994744620924993, -2.95433279467378E-02, 2.69645748827495E-04, 2, False, 4, 0)

    Part.FeatureManager.AddSMNormalCutType True, True, False
    
    'Create a Normal Cut feature using the previously selected cut-extrude faces
    Set myFeature = Part.FeatureManager.FinishSMNormalCut()

    Set swFeatData = myFeature.GetDefinition
    Dim Number As Long
    Number = swFeatData.GetNumberOfFaceGroups()

    'Select another cut-extrude face for which to create a second Normal Cut
    boolstatus = swFeatData.AccessSelections(Part, Nothing)
        
    boolstatus = Part.Extension.SelectByRay(-6.24756020285346E-02, -1.97848124440725E-02, 1.18685503457829E-02, -9.80322952634684E-02, -0.994744620924993, -2.95433279467378E-02, 2.7317052985792E-04, 2, False, 1, 0)
    Dim instance As ISelectionMgr
    Set face = Part.SelectionManager.GetSelectedObject6(1, -1)
    Dim faces As Variant
    Dim aFaces() As SldWorks.face
    ReDim aFaces(0)
    Set aFaces(0) = face
    faces = aFaces
    longwarnings = swFeatData.AddAGroupOfFaces(faces, longwarnings)

    Number = swFeatData.GetNumberOfFaceGroups()

    'Change the profile of the Normal Cut by adjusting the offset of the offset plane
    myNormalCutFeatData.Offset = 1.0

    Dim bStatus As Boolean
    bStatus = myFeature.ModifyDefinition(swFeatData, Part, Nothing)
    Part.ClearSelection2 True

End Sub

To create a Normal Cut feature in a sheet metal part, call:

1. IFeatureManager::AddSMNormalCut.
2. IFeatureManager::AddSMNormalCutType.
3. IModelDocExtension::SelectByID2 with Mark = 1 to select the cut-extrude faces that you wish to make Normal Cuts.
4. IModelDocExtension::SelectByID2 with Mark = 2 to select the group of cut-extrude faces.
5. IModelDocExtension::SelectByID2 with Mark = 4 to select the offset plane, if BExtent is false.
6. (Optional) IModelDocExtension::SelectByID2 with Mark = 8 to select the direction of normal cut, if BExtent is true.
7. IFeatureManager::FinishSMNormalCut.
8. ISMNormalCutFeatureData::Offset to change the profile of the Normal Cut.