SplitFeature is also a type of feature. But if you do not want to split a feature without SplitFeature, you could calcuate the new profiles and create the new splitting features. The following is a small code which converts an extrude feature to two extrude features with a middle line, and also creates a surface of the middle line to represent the split plane.
Assume the orignal extrude feature is based on a profile of a rectangle lines.
Sub test()
Dim oPartDoc As PartDocument
Set oPartDoc = ThisApplication.ActiveDocument
Dim oDef As PartComponentDefinition
Set oDef = oPartDoc.ComponentDefinition
Dim oOldF As ExtrudeFeature
Set oOldF = oDef.Features.ExtrudeFeatures(1)
Dim oOldFDef As ExtrudeDefinition
Set oOldFDef = oOldF.Definition
Dim oPath As ProfilePath
Set oPath = oOldFDef.Profile(1)
Dim oSketchEnt As SketchEntity
Dim oSketch As PlanarSketch
Dim oSketchLine1 As SketchLine
Set oSketchLine1 = oPath(1).SketchEntity
Dim oSketchLine2 As SketchLine
Set oSketchLine2 = oPath(2).SketchEntity
Dim oSketchLine3 As SketchLine
Set oSketchLine3 = oPath(3).SketchEntity
Dim oSketchLine4 As SketchLine
Set oSketchLine4 = oPath(4).SketchEntity
'get sketch
Set oSketch = oSketchLine1.Parent
'get mid pt of line 1
Dim oMidPtOfLine1 As Point2d
Set oMidPtOfLine1 = oSketchLine1.Geometry.MidPoint
'add sketch mid pt
Dim oMidSketchPtLine1 As SketchPoint
Set oMidSketchPtLine1 = oSketch.SketchPoints.Add(oMidPtOfLine1)
Call oSketch.GeometricConstraints.AddCoincident(oMidSketchPtLine1, oSketchLine1)
'get mid pt of line3 which is parallel to line 1
Dim oMidPtOfLine3 As Point2d
Set oMidPtOfLine3 = oSketchLine3.Geometry.MidPoint
'add sketch mid pt
Dim oMidSketchPtLine3 As SketchPoint
Set oMidSketchPtLine3 = oSketch.SketchPoints.Add(oMidPtOfLine3)
Call oSketch.GeometricConstraints.AddCoincident(oMidSketchPtLine3, oSketchLine3)
' create mid line
Dim oMiddleLine As SketchLine
Set oMiddleLine = oSketch.SketchLines.AddByTwoPoints(oMidPtOfLine1, oMidPtOfLine3)
Call oMiddleLine.StartSketchPoint.Merge(oMidSketchPtLine1)
Call oMiddleLine.EndSketchPoint.Merge(oMidSketchPtLine3)
' create new extrude 1: just change the old feature's profile
Dim oNewPaths1 As ObjectCollection
Set oNewPaths1 = ThisApplication.TransientObjects.CreateObjectCollection
oNewPaths1.Add oSketchLine1
oNewPaths1.Add oSketchLine2
oNewPaths1.Add oSketchLine3
oNewPaths1.Add oMiddleLine
Dim oNewProfile1 As Profile
Set oNewProfile1 = oSketch.Profiles.AddForSolid(False, oNewPaths1)
oOldFDef.Profile = oNewProfile1
'create the other extrude feature
Dim oNewPaths2 As ObjectCollection
Set oNewPaths2 = ThisApplication.TransientObjects.CreateObjectCollection
oNewPaths2.Add oSketchLine1
oNewPaths2.Add oSketchLine4
oNewPaths2.Add oSketchLine3
oNewPaths2.Add oMiddleLine
Dim oNewProfile2 As Profile
Set oNewProfile2 = oSketch.Profiles.AddForSolid(False, oNewPaths2)
Dim oNewExtrudeDef As ExtrudeDefinition
Set oNewExtrudeDef = oDef.Features.ExtrudeFeatures.CreateExtrudeDefinition(oNewProfile2, kJoinOperation)
Call oNewExtrudeDef.SetDistanceExtent(1, kNegativeExtentDirection)
Dim oNewExtrude As ExtrudeFeature
Set oNewExtrude = oDef.Features.ExtrudeFeatures.Add(oNewExtrudeDef)
'create surface on
Dim oNewPaths3 As ObjectCollection
Set oNewPaths3 = ThisApplication.TransientObjects.CreateObjectCollection
oNewPaths3.Add oMiddleLine
Dim oNewProfile3 As Profile
Set oNewProfile3 = oSketch.Profiles.AddForSurface(oMiddleLine)
Dim oSurfaceDef As ExtrudeDefinition
Set oSurfaceDef = oDef.Features.ExtrudeFeatures.CreateExtrudeDefinition(oNewProfile3, kSurfaceOperation)
Call oSurfaceDef.SetDistanceExtent(10, kSymmetricExtentDirection)
Dim oSurface As ExtrudeFeature
Set oSurface = oDef.Features.ExtrudeFeatures.Add(oSurfaceDef)
End Sub
After the code, the feature becomes:
