Two planar faces which are coplanar are not always overlapped. To know if they are overlapped and the touching area, one workaround could be extrude the sketches based on the faces with a tiny distance, and use TransientBRep.DoBoolean to check if the bodies of the two extrude features are intersected.
The following is demo code. It assumes two planar faces are selected. One material named “Magenta” is available.
Note: in UI, if the two planar faces are within one surface body and are overlapped, they cannot be selected independently. So to make a demo, it assumes the two planar faces are from different bodies. Of course, you can distinguish two faces from one surface body in the workflow of code.
Private Sub Test()
Try
‘get application
oApp =
System.Runtime.InteropServices.
Marshal.GetActiveObject("Inventor.Application")
Catch
End Try
Dim oPartDoc As PartDocument = oApp.ActiveDocument
Dim oPartDef = oPartDoc.ComponentDefinition
‘get face1
Dim oFace1 As Face
oFace1 = oPartDoc.SelectSet(1)
‘get face2
Dim oFace2 As Face
oFace2 = oPartDoc.SelectSet(2)
‘if two faces are planar and coplanar
If oFace1.SurfaceType =
SurfaceTypeEnum.kPlaneSurface _
And oFace2.SurfaceType =
SurfaceTypeEnum.kPlaneSurface Then
Dim oPlane1 As Plane
oPlane1 = oFace1.Geometry
Dim oPlane2 As Plane
oPlane2 = oFace2.Geometry
‘ if normal of two faces are same
If oPlane1.Normal.IsEqualTo(oPlane2.Normal) Then
Dim extrudeDis As Double = 0.001
‘create the extrude feature from face1
Dim oSketch1 As PlanarSketch =
oPartDef.Sketches.Add(oFace1)
Dim oEdgeInFace1 As Edge
For Each oEdgeInFace1 In oFace1.Edges
oSketch1.AddByProjectingEntity(oEdgeInFace1)
Next
Dim oProfile1 As Profile
oProfile1 = oSketch1.Profiles.AddForSolid()
Dim oExtrudeF1Def As ExtrudeDefinition
oExtrudeF1Def =
oPartDef.Features.ExtrudeFeatures.
CreateExtrudeDefinition(oProfile1,
PartFeatureOperationEnum.kNewBodyOperation)
oExtrudeF1Def.SetDistanceExtent(extrudeDis,
PartFeatureExtentDirectionEnum.kPositiveExtentDirection)
Dim oExtrudeF1 As ExtrudeFeature
oExtrudeF1 =
oPartDef.Features.ExtrudeFeatures.Add(oExtrudeF1Def)
Dim oSB1 As SurfaceBody
oSB1 = oExtrudeF1.SurfaceBodies(1)
‘create the extrude feature from face2
Dim oSketch2 As PlanarSketch =
oPartDef.Sketches.Add(oFace2)
Dim oEdgeInFace2 As Edge
For Each oEdgeInFace2 In oFace2.Edges
oSketch2.AddByProjectingEntity(oEdgeInFace2)
Next
Dim oProfile2 As Profile
oProfile2 =
oSketch2.Profiles.AddForSolid()
Dim oExtrudeF2Def As ExtrudeDefinition
oExtrudeF2Def =
oPartDef.Features.ExtrudeFeatures.
CreateExtrudeDefinition(oProfile2,
PartFeatureOperationEnum.kNewBodyOperation)
oExtrudeF2Def.SetDistanceExtent(extrudeDis,
PartFeatureExtentDirectionEnum.
kPositiveExtentDirection)
Dim oExtrudeF2 As ExtrudeFeature
oExtrudeF2 =
oPartDef.Features.ExtrudeFeatures.Add(oExtrudeF2Def)
Dim oSB2 As SurfaceBody
oSB2 = oExtrudeF2.SurfaceBodies(1)
Dim oTransientB1 As SurfaceBody =
oApp.TransientBRep.Copy(oSB1)
Dim oTransientB2 As SurfaceBody =
 
; oApp.TransientBRep.Copy(oSB2)
‘check if bodies of the two extrude features are intersected
oApp.TransientBRep.DoBoolean(oTransientB1,
oTransientB2,
BooleanTypeEnum.kBooleanTypeIntersect)
If oTransientB1.Volume(0.01) > 0 Then
MsgBox("The two faces are overlapped!")
‘create a client graphics to show the intersect area
Dim oClientGraphics As ClientGraphics
Try
oClientGraphics =
oPartDef.ClientGraphicsCollection.Item("overlap")
oClientGraphics.Delete()
Catch ex As Exception
End Try
oApp.ActiveView.Update()
oClientGraphics =
oPartDef.ClientGraphicsCollection.Add("overlap")
‘add graphics node
Dim oSurfacesNode As GraphicsNode
oSurfacesNode =
oClientGraphics.AddNode(1)
‘add the face of WeldBead.BeadFaces
Dim oSurfaceGraphics As SurfaceGraphics
oSurfaceGraphics =
oSurfacesNode.AddSurfaceGraphics(oTransientB1)
‘set graphics’ color. assume “Magenta” exists in the document
oSurfacesNode.Appearance =
oPartDoc.Assets("Magenta")
‘transform the client graphics to a location
Dim oTransGeom As TransientGeometry
oTransGeom =
oApp.TransientGeometry
Dim oV As Vector
oV = oTransGeom.CreateVector(1, 1, 1)
Dim oM As Matrix
oM = oTransGeom.CreateMatrix()
Call oM.SetTranslation(oV)
oSurfacesNode.Transformation = oM
‘update the view
oApp.ActiveView.Update()
Else
MsgBox("The two faces are NOT overlapped!")
End If
oExtrudeF1.Delete()
oExtrudeF2.Delete()
Else
MsgBox("the faces are NOT coplanar!")
End If
Else
MsgBox("one of the faces are NOT planar!")
End If
End Sub
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