Getting a sketch segment's underlying curve and using CreateTrimmedSheet4

Ok, So I have made some headway. I the curves need to be trimmed, so i took care of by making a wire body, getting its edge, getting the start and end point vertexes and used ICurve::CreateTrimmedCurve2 to trim them. But CreateTrimmedSheet4 is still not giving me any objects...

Function CreateCutBody(sketch As SldWorks.sketch, SurFace As SldWorks.Face2) As SldWorks.Body2()
Dim swSurf As SldWorks.SurFace
Dim SktXForm As SldWorks.MathTransform

Dim swSktSeg As SldWorks.SketchSegment
Dim swCurve() As SldWorks.Curve
Dim WrieBody As SldWorks.Body2

Dim swEdge As SldWorks.Edge
Dim swVrtx As SldWorks.Vertex

Dim vSeg As Variant
Dim vEdges As Variant
Dim vRetBods As Variant

Dim vSrt() As Double
Dim vEnd() As Double

Dim dSrt(2) As Double
Dim dEnd(2) As Double

Dim i As Integer
Dim DisBod() As SldWorks.Body2  'Remove after working
On Error GoTo errH
    Set swSurf = SurFace.GetSurface
    Set SktXForm = sketch.ModelToSketchTransform
    vSeg = sketch.GetSketchSegments
    ReDim swCurve(UBound(vSeg))
    ReDim DisBod(UBound(vSeg))
       
    For i = 0 To (UBound(vSeg))
        Set swSktSeg = vSeg(i)
        Set WrieBody = swSktSeg.CreateWireBody
        WrieBody.ApplyTransform SktXForm
       
        'Get edge points to trim the curve
            vEdges = WrieBody.GetEdges
            Set swEdge = vEdges(0)
            'Get Start Points
                Set swVrtx = swEdge.GetStartVertex
                vSrt = swVrtx.GetPoint
                For n = 0 To 2
                    dSrt(n) = Round(vSrt(n), 5)
                Next n
            'Get End Points
                Set swVrtx = swEdge.GetEndVertex
                vEnd = swVrtx.GetPoint
                For n = 0 To 2
                    dEnd(n) = Round(vEnd(n), 5)
                Next n
           
        'Get Curve and Trim
            Set swCurve(i) = swSktSeg.GetCurve
            swCurve(i).ApplyTransform SktXForm
            Set swCurve(i) = swCurve(i).CreateTrimmedCurve2(dSrt(0), dSrt(1), dSrt(2), dEnd(0), dEnd(1), dEnd(2))
       
        'Sanity Check
            Set DisBod(i) = swCurve(i).CreateWireBody
            DisBod(i).Display3 swPart, 255, 1
            Debug.Print "Curve(" & i; ") (" & dSrt(0) & ", " & dSrt(1) & ", " & dSrt(2) & ", " _
                                            & dEnd(0) & ", " & dEnd(1) & ", " & dEnd(2) & ")"
       
    Next i
   
    Set vRetBods = swSurf.CreateTrimmedSheet4((swCurve), False)
    CreateCutBody = vRetBods

Exit Function
errH: Debug.Print "CreateCutBody Error: " & Err.Description
End Function

100% Working!

CutSktFeat is the feature holding the sketch, SelFace is the selected face, and EditBody is the body the cut extrude is being applied to.

The trick to this one is lines 71 and 72. The Extrude depth is an arbitrary 6 meters.

Function CreateCutBody(CutSktFeat As Feature, SelFace As Face2, EditBody As Body2) As SldWorks.Body2
Dim SktXForm As SldWorks.MathTransform
Dim swCurveParams As SldWorks.CurveParamData
Dim dirVector As SldWorks.MathVector
Dim swMath As SldWorks.MathUtility


Dim swRetBods As SldWorks.Body2
Dim TempBody As SldWorks.Body2
Dim swTrimBody As SldWorks.Body2
Dim swWorkBody As SldWorks.Body2
Dim swToolBody As SldWorks.Body2


Dim TmpSurf As SldWorks.SurFace


Dim swSketch As SldWorks.Sketch
Dim swSktContour As SldWorks.SketchContour


Dim swSktCurve As SldWorks.Curve
Dim swCurve() As SldWorks.Curve


Dim swSktSeg As SldWorks.SketchSegment
Dim swEdge As SldWorks.Edge


Dim RootPoint(2) As Double
Dim Normal() As Double
Dim InvNorm(2) As Double


Dim vContours As Variant
Dim vRetBody As Variant
Dim vFacePt As Variant
Dim vStrPt As Variant
Dim vEndPt As Variant
Dim vEdges As Variant


Dim lngErr As Long
Dim i As Integer
Dim n As Integer


On Error GoTo errH


    Set swModeler = swApp.GetModeler
    Set swMath = swApp.GetMathUtility
    
    Set swWorkBody = EditBody
    Set swSketch = CutSktFeat.GetSpecificFeature2
    Set SktXForm = swSketch.ModelToSketchTransform
    
    Normal = SelFace.Normal
    InvNorm(0) = -Normal(0)
    InvNorm(1) = -Normal(1)
    InvNorm(2) = -Normal(2)
    
    vFacePt = SelFace.GetClosestPointOn(0, 0, 0)
    vContours = swSketch.GetSketchContours
    
    RootPoint(0) = vFacePt(0) 'X
    RootPoint(1) = vFacePt(1) 'Y
    RootPoint(2) = vFacePt(2) 'Z


    Set TempBody = swPart.CreateNewBody
    Set TmpSurf = TempBody.CreatePlanarSurface(RootPoint, Normal)
    
    For i = 0 To (UBound(vContours))
        Set swSktContour = vContours(i)
        
        vEdges = swSktContour.GetEdges
        
        ReDim DisBod(UBound(vEdges))
        ReDim swCurve(UBound(vEdges))
        
        For n = 0 To UBound(vEdges)
            Set swEdge = vEdges(n)
            
            Set swCurveParams = swEdge.GetCurveParams3
            Set swSktCurve = swEdge.GetCurve
            
            vStrPt = swCurveParams.StartPoint
            vEndPt = swCurveParams.EndPoint
            
            Set swSktCurve = swSktCurve.CreateTrimmedCurve2(vStrPt(0), vStrPt(1), vStrPt(2), vEndPt(0), vEndPt(1), vEndPt(2))
            Set swCurve(n) = swSktCurve
        Next n
        Set swTrimBody = TmpSurf.CreateTrimmedSheet((swCurve))
        
        Set dirVector = swMath.CreateVector((InvNorm))
        Set swToolBody = swModeler.CreateExtrudedBody(swTrimBody, dirVector, 6 * m)
        swToolBody.Display3 swModel, RGB(1, 0, 0), 0
        
        vRetBody = swWorkBody.Operations2(SWBODYCUT, swToolBody, lngErr)
        Set swWorkBody = vRetBody(0)
        
    Next i
    
    Set CreateCutBody = swWorkBody


Exit Function
errH: Debug.Print "CreateCutBody Error: " & Err.Description
End Function