Automatic Sheet Metal Thickness Detection

[p_kompier]

I've been struggling to find an easy way to automatically detect whether the geometry in a part qualifies as a sheet metal part, and if so, what the sheet metal thickness is. I couldn't find anything satisfactory so I wrote the following rule which in our situation seems to work 100% of the time for 2 years now. I hope this can be useful to someone now that it seemed to have proved itself.

What the rule does is:

-Check if a part is a standard or sheet metal part, and convert if neccesary.

-Determine the sheet metal thickness within the accepted thickness values

-Else, it will be regarded it as a standard part regardsless

Those willing to use it will undoubtedly have to modify the rule to work for their use-case, but I hope this may prove as a good starting point. I'm very eager to recieve improvements on the rule to make it even more robust.

Sub Main()

Dim oPartDoc As PartDocument = ThisDoc.Document  ' <-- fixed
Dim oCompDef As PartComponentDefinition = oPartDoc.ComponentDefinition

'Declaring Public Variables
Dim acceptableValues() As Double = {0.5, 1, 1.25, 1.5, 2, 2.5, 3, 4, 5, 6, 8, 10 }
Dim largestFace As Face = Nothing
Dim largestFlatFace As Face = Nothing
Dim largestArea As Double = 0
Dim outerLoopPoints As New List(Of Point)
Dim outerLoopEdge As Edge = Nothing
Dim planeDistance As Double = 0

If oCompDef.SurfaceBodies(1).Faces.Count < 2 Then
	oPartDoc.SubType = "{4D29B490-49B2-11D0-93C3-7E0706000000}"
	Return
End If

'Get the largest face
For Each oFace As Face In oCompDef.SurfaceBodies(1).Faces
	Dim area As Double = oFace.Evaluator.Area
	If area > largestArea Then
		largestArea = area
		largestFace = oFace
	End If
Next

If Not largestFace Is Nothing Then

	'Store Outer Loop Vertex Points
	For Each oEdgeLoop As EdgeLoop In largestFace.EdgeLoops
		If oEdgeLoop.IsOuterEdgeLoop Then
			outerLoopEdge = oEdgeLoop.Edges.Item(1)
			For Each oEdge As Edge In oEdgeLoop.Edges
				outerLoopPoints.Add(oEdge.StartVertex.Point)
				outerLoopPoints.Add(oEdge.StopVertex.Point)
			Next
		End If
	Next

	'Check if there's a straight edge connected to the outer edge and aligned with the largestFace normal
	For Each oEdge As Edge In oCompDef.SurfaceBodies(1).Edges
		If oEdge.GeometryType = kLineSegmentCurve Then
			Dim sharedVertex As Point = OnlyPointConnectingEdgeToLoop(oEdge, outerLoopPoints)
			If Not sharedVertex Is Nothing Then
				If AlignedEdgeAndFaceNormalAtPoint(oEdge, largestFace, sharedVertex) Then
					Dim edgeLength As Double = Math.Round(EgdeLength(oEdge) * 10, 4)
					If acceptableValues.Contains(edgeLength) Then
						SetThickness(edgeLength, oPartDoc)  ' <-- pass oPartDoc
						Return
					End If
				End If
			End If
		End If
	Next

	largestArea = 0

	For Each oFace As Face In oCompDef.SurfaceBodies.Item(1).Faces
		If oFace.SurfaceType = SurfaceTypeEnum.kPlaneSurface Then
			Dim area As Double = oFace.Evaluator.Area
			If area > largestArea Then
				largestArea = area
				largestFlatFace = oFace
			End If
		End If
	Next

	For Each oFace As Face In oCompDef.SurfaceBodies.Item(1).Faces
		If oFace IsNot largestFlatFace And oFace.SurfaceType = SurfaceTypeEnum.kPlaneSurface Then
			Dim oPlane As Plane = oFace.Geometry
			Dim largestPlane As Plane = largestFlatFace.Geometry
			Dim Distance As Double = Double.MinValue
			If largestPlane.IsParallelTo(oPlane) Then
				Distance = Math.Abs(Math.Round(largestPlane.DistanceTo(oPlane.RootPoint) * 10, 4))
			End If
			If Distance > 0 And Distance > planeDistance Then
				planeDistance = Distance
			End If
		End If
	Next

	If acceptableValues.Contains(planeDistance) Then
		SetThickness(planeDistance, oPartDoc)  ' <-- pass oPartDoc
		Return
	Else
		For Each oFace As Face In oCompDef.SurfaceBodies.Item(1).Faces
			If oFace IsNot largestFlatFace And oFace.SurfaceType = SurfaceTypeEnum.kPlaneSurface Then
				Dim oPlane As Plane = oFace.Geometry
				Dim largestPlane As Plane = largestFlatFace.Geometry
				Dim Distance As Double = Double.MaxValue
				If largestPlane.IsParallelTo(oPlane) Then
					Distance = Math.Abs(Math.Round(largestPlane.DistanceTo(oPlane.RootPoint) * 10, 4))
				End If
				If Distance > 0 And Distance < planeDistance Then
					planeDistance = Distance
				End If
			End If
		Next

		If acceptableValues.Contains(planeDistance) Then
			SetThickness(planeDistance, oPartDoc)  ' <-- pass oPartDoc
			Return
		Else
			Dim connectedFaces As Faces = outerLoopEdge.Faces
			Dim otherFace As Face = Nothing
			For Each oFace As Face In connectedFaces
				If oFace IsNot largestFace Then
					otherFace = oFace
					Exit For
				End If
			Next

			Dim otherFaceArea As Double = otherFace.Evaluator.Area
			Dim totalLoopLenght As Double = 0
			For Each oEdge In otherFace.Edges
				totalLoopLenght += EgdeLength(oEdge)
			Next

			Dim ratio As Double = Math.Abs(Math.Round(otherFaceArea / (totalLoopLenght / 2) * 10, 4))

			If acceptableValues.Contains(ratio) Then
				SetThickness(ratio, oPartDoc)  ' <-- pass oPartDoc
				Return
			Else
				oPartDoc.SubType = "{4D29B490-49B2-11D0-93C3-7E0706000000}"
			End If
		End If
	End If
End If

End Sub

Function OnlyPointConnectingEdgeToLoop(E As Edge, VA As List(Of Point)) As Point
	Dim startVertex As Point = E.StartVertex.Point
	Dim stopVertex As Point = E.StopVertex.Point
	For Each oLoopVertex As Point In VA
		If startVertex.IsEqualTo(oLoopVertex) Xor stopVertex.IsEqualTo(oLoopVertex) Then
			Return oLoopVertex
		End If
	Next
End Function

Function AlignedEdgeAndFaceNormalAtPoint(E As Edge, F As Face, P As Point) As Boolean
	Dim oPoint As Double() = {P.X, P.Y, P.Z }
	Dim oNormal As Double() = New Double(2) {}
	F.Evaluator.GetNormalAtPoint(oPoint, oNormal)
	Dim oParam As Double() = {0, 0, 0 }
	Dim oTangent As Double() = New Double(2) {}
	E.Evaluator.GetTangent(oParam, oTangent)
	Dim DotProduct As Double = oNormal(0) * oTangent(0) + oNormal(1) * oTangent(1) + oNormal(2) * oTangent(2)
	Dim Tolerance As Double = 0.001
	If Math.Abs(DotProduct) >= (1 - Tolerance) Then
		Return True
	End If
End Function

Function EgdeLength(oEdge As Edge) As Double
	Dim curveEval As CurveEvaluator = oEdge.Evaluator
	Dim MinParam As Double
	Dim MaxParam As Double
	Dim Length As Double
	curveEval.GetParamExtents(MinParam, MaxParam)
	curveEval.GetLengthAtParam(MinParam, MaxParam, Length)
	Return Length
End Function

Function SetThickness(T As Double, oPartDoc As PartDocument)  ' <-- accepts oPartDoc as argument
	Dim new_smcd As SheetMetalComponentDefinition = oPartDoc.ComponentDefinition  ' <-- fixed
	new_smcd.ActiveSheetMetalStyle.Thickness = T
	new_smcd.UseSheetMetalStyleThickness = True
End Function

[Yijiang.Cai]

@p_kompier many thanks for posting the feedback to us, and now it only supports to select the specific face to detect thickness when converting part to sheet metal. There is a similar idea in idea station, and please vote it.

https://forums.autodesk.com/t5/inventor-ideas/auto-detect-sheet-metal-thickness/idi-p/6285970

[p_kompier]

@Yijiang.Cai  thank you for sharing this workflow, which should work in most cases, I've never noticed that option.

Unfortunately we import a lot of external STEP-files, this way we can easily convert and modify the parts.

We also create sheet metal solids in our multi bodied parts using standard features, allowing more flexibility. (e.g. draw sheet parts in a sketch, use 2 workplanes at either end of the drawn edge to extrude a face from another sketch between), useful for when thickness is variable, and keeps number of sketches and projected geometry low.

This is not how Inventor was meant to be used but it keeps thinks clean.

Ayway, thanks for your reply, and let me know what you think.

[Yijiang.Cai]

@p_kompier understanding your idea, and you prefer to detect the thickness of part automatically as to batch conversion on 3rd party dataset to Inventor sheet metal. Anyway, please vote the idea, and we could prioritize it later. Many thanks!