Function InsertUntrimSurface2( _
   ByVal FaceUntrimType As System.Integer, _
   ByVal EdgeUntrimType As System.Integer, _
   ByVal Distance As System.Double, _
   ByVal BMerge As System.Boolean, _
   ByVal BTrimOppositeSide As System.Boolean _
) As Feature

Dim instance As IFeatureManager
Dim FaceUntrimType As System.Integer
Dim EdgeUntrimType As System.Integer
Dim Distance As System.Double
Dim BMerge As System.Boolean
Dim BTrimOppositeSide As System.Boolean
Dim value As Feature
 
value = instance.InsertUntrimSurface2(FaceUntrimType, EdgeUntrimType, Distance, BMerge, BTrimOppositeSide)

Feature InsertUntrimSurface2( 
   System.int FaceUntrimType,
   System.int EdgeUntrimType,
   System.double Distance,
   System.bool BMerge,
   System.bool BTrimOppositeSide
)

Feature^ InsertUntrimSurface2( 
&   System.int FaceUntrimType,
&   System.int EdgeUntrimType,
&   System.double Distance,
&   System.bool BMerge,
&   System.bool BTrimOppositeSide
) 

Parameters

FaceUntrimType

Untrim face edge type as defined by swFaceUntrimType_e; valid only if a face is selected

EdgeUntrimType

Connect endpoints or extend edges as defined by swEdgeUntrimType_e; valid only of one or more edges are selected

Distance

Distance by which to untrim the surface

BMerge

True to create a surface extension that merges with the original surface, false to create a new, separate surface body

BTrimOppositeSide

True to remove the surface outside the selected surface edges or interior surface holes, false to not; valid only if BMerge is false

Return Value

'VBA

'This example creates a planar polygonal surface, untrims (extends) the surface outside the selected face edges,
'and trims (removes) the surface inside the selected face edges.
'=======================================================================
'Preconditions: Ensure that the specified template exists.
'
'Postconditions:
'1. Creates Surface-Plane1.
'2. Creates Surface-Untrim1 by untrimming outside all edges of the selected face, not merging with the original part, and trimming inside all edges of the selected face.
'3. Click on Surface-Untrim1. The untrimmed areas are in green.
'========================================================================
Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Dim swPart As SldWorks.PartDoc
Dim skSegment As SldWorks.SketchSegment
Dim boolstatus As Boolean
Dim longstatus As Long, longwarnings As Long

Sub main()

    Set swApp = Application.SldWorks
 
    Dim swSheetWidth As Double
    swSheetWidth = 0
    Dim swSheetHeight As Double
    swSheetHeight = 0
    Set Part = swApp.NewDocument("C:\ProgramData\SolidWorks\SOLIDWORKS 2024\templates\Part.prtdot", 0, swSheetWidth, swSheetHeight)
    Set swPart = Part
    Set Part = swApp.ActiveDoc
    Part.SketchManager.InsertSketch True
    boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", -4.90383108306059E-02, 3.86835343160318E-02, 3.91373764799244E-03, False, 0, Nothing, 0)
    Part.ClearSelection2 True
    Set skSegment = Part.SketchManager.CreateLine(-0.035002, 0.035119, 0#, 0.025668, 0.036519, 0#)
    Set skSegment = Part.SketchManager.CreateLine(0.025663, 0.036519, 0#, 0.025201, -0.016451, 0#)
    Set skSegment = Part.SketchManager.CreateLine(0.025201, -0.016451, 0#, -0.068137, -0.018551, 0#)
    Set skSegment = Part.SketchManager.CreateLine(-0.068137, -0.018551, 0#, -0.067204, 0.026718, 0#)
    Set skSegment = Part.SketchManager.CreateLine(-0.067204, 0.026713, 0#, -0.036169, 0.026251, 0#)
    Set skSegment = Part.SketchManager.CreateLine(-0.036169, 0.026251, 0#, -0.035002, 0.035119, 0#)
    Part.ClearSelection2 True
    Part.SketchManager.InsertSketch True
    Part.SelectionManager.EnableContourSelection = True
    boolstatus = Part.Extension.SelectByID2("Sketch1", "SKETCHREGION", 2.26345552080154E-02, -0.013184045043844, 0, True, 1, Nothing, 0)
    boolstatus = Part.InsertPlanarRefSurface()
    Part.ClearSelection2 True
    boolstatus = Part.Extension.SelectByRay(-4.08355377464196E-02, 1.83176555033939E-02, 0, 0, 0, -1, 7.93376161930438E-04, 2, True, 0, 0)
    Part.FeatureManager.InsertUntrimSurface2 0, 2, 0, False, True
    Part.SelectionManager.EnableContourSelection = False

End Sub

This method:

• is valid only for surface parts.
• requires preselection of the face or edges you want to untrim.

For learn more about Untrim Surfaces, see the SOLIDWORKS Help > Parts and Features > Features > Surfaces > Surface Controls > Untrim Surface topic.