Hi @STECORO. Maybe this similar example will work better for you. It includes the use of a 'List(Of String)' type variable, to hold the names of the colors/appearances that you do not want to include as painted area. Alternately, you could use the same strategy to only find faces that are set to specific colors, using 'ColorsToInclude' type list, instead of 'ColorsToExclude' list. It iterates all bodies, and all faces of each body. But this example uses newer properties / objects / methods. The 'render style' objects have been obsolete since around 2013 (see link below for more details about that).
Consistent Materials (Materials and Appearances)
Sub Main
Dim oPDoc As PartDocument = TryCast(ThisDoc.Document, Inventor.PartDocument)
If oPDoc Is Nothing Then Return
Dim oColorsToExclude As New List(Of String)
oColorsToExclude.Add("Steel")
oColorsToExclude.Add("Polished Steel")
' Dim oColorsToInclude As New List(Of String)
' oColorsToInclude.Add("Orange")
Dim dPaintedArea As Double = 0.0
For Each oBody As SurfaceBody In oPDoc.ComponentDefinition.SurfaceBodies
For Each oFace As Face In oBody.Faces
Dim sFaceAppearanceName As String = oFace.Appearance.DisplayName
If oColorsToExclude.Contains(sFaceAppearanceName) Then Continue For
Dim dArea As Double = oFace.Evaluator.Area
dPaintedArea += dArea
Next oFace
Next oBody
Parameter.Value("PAINTED_AREA") = CStr(dPaintedArea * 100)
oPDoc.Update2(True)
End SubIf this solved your problem, or answered your question, please click ACCEPT SOLUTION .
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Wesley Crihfield
(Not an Autodesk Employee)
Hi @STECORO. Sure. Here is a modified version of the first code I posted here, which includes the requested TransientBRep manipulations. If the part only has one body, it will process that one body without this extra process, but if it has multiple bodies, it will create a new transient body that is a combined union of all bodies, then process that transient body instead. I just finished typing this up for you, so I have not tested it yet. Let me know how it works for you.
Sub Main
Dim oPDoc As PartDocument = TryCast(ThisDoc.Document, Inventor.PartDocument)
If oPDoc Is Nothing Then Return
Dim oPDef As PartComponentDefinition = oPDoc.ComponentDefinition
Dim oBodies As SurfaceBodies = oPDef.SurfaceBodies
If oBodies.Count = 0 Then Return
Dim oColorsToExclude As New List(Of String)
oColorsToExclude.Add("Steel")
oColorsToExclude.Add("Polished Steel")
Dim oTBody As SurfaceBody = Nothing
If Not oPDef.HasMultipleSolidBodies Then
oTBody = oBodies.Item(1)
Else
Dim oTBRep As TransientBRep = ThisApplication.TransientBRep
Dim oFirstBody, oBodyToBeModified, oToolBody As SurfaceBody
oFirstBody = oBodies.Item(1)
oBodyToBeModified = oTBRep.Copy(oFirstBody)
For i As Integer = 1 To oBodies.Count
oBody = oBodies.Item(i)
If oBody Is oFirstBody Then Continue For
oToolBody = oTBRep.Copy(oBody)
oTBRep.DoBoolean(oBodyToBeModified, oToolBody, BooleanTypeEnum.kBooleanTypeUnion)
Next i
oTBody = oBodyToBeModified
End If
Dim dPaintedArea As Double = 0.0
For Each oFace As Face In oTBody.Faces
Dim sFaceAppearanceName As String = oFace.Appearance.DisplayName
If oColorsToExclude.Contains(sFaceAppearanceName) Then Continue For
Dim dArea As Double = oFace.Evaluator.Area
dPaintedArea += dArea
Next oFace
Parameter.Value("PAINTED_AREA") = CStr(dPaintedArea * 100)
oPDoc.Update2(True)
End SubIf this solved your problem, or answered your question, please click ACCEPT SOLUTION .
Or, if this helped you, please click (LIKE or KUDOS) 👍.
Wesley Crihfield
(Not an Autodesk Employee)
Hi @STECORO. It seems as though the faces of copied 'transient' bodies do not retain the 'appearances' of the original, real bodies, and attempting to access them causes an error. So, the next alternative is to use 'real' geometry techniques similar to the BRep Boolean operation to combine all bodies into one (temporarily), then check face appearances and areas, then 'UNDO' the feature that combined all the bodies again. Below is an example iLogic code doing it that way, utilizing an Inventor.Transaction so that we can 'UNDO' the actions it is doing, and also utilizing a CombineFeature to join all bodies together.
Sub Main
Dim oInvApp As Inventor.Application = ThisApplication
Dim oPDoc As PartDocument = TryCast(ThisDoc.Document, Inventor.PartDocument)
If oPDoc Is Nothing Then Return
Dim oPDef As PartComponentDefinition = oPDoc.ComponentDefinition
Dim oBodies As SurfaceBodies = oPDef.SurfaceBodies
If oBodies.Count = 0 Then Return
Dim oColorsToExclude As New List(Of String)
oColorsToExclude.Add("Steel")
oColorsToExclude.Add("Polished Steel")
Dim oTBody As SurfaceBody = oBodies.Item(1)
Dim dPaintedArea As Double = 0.0
If Not oPDef.HasMultipleSolidBodies Then
dPaintedArea = GetPaintedArea(oTBody, oColorsToExclude)
ElseIf oPDef.HasMultipleSolidBodies Then
Dim oTrans As Inventor.Transaction = oInvApp.TransactionManager.StartTransaction(oPDoc, "Combine Bodies - iLogic")
Dim oCFs As CombineFeatures = oPDef.Features.CombineFeatures
Dim oToolBodies As ObjectCollection = oInvApp.TransientObjects.CreateObjectCollection
For i As Integer = 1 To oBodies.Count
oBody = oBodies.Item(i)
If oBody Is oTBody Then Continue For
oToolBodies.Add(oBody)
Next i
Dim oCF As CombineFeature = oCFs.Add(oTBody, oToolBodies, PartFeatureOperationEnum.kJoinOperation, False)
dPaintedArea = GetPaintedArea(oTBody, oColorsToExclude)
oTrans.Abort
End If
iLogicVb.Automation.ParamValue(oPDoc, "PAINTED_AREA") = CStr(dPaintedArea * 100)
oPDoc.Update2(True)
End Sub
Function GetPaintedArea(oBody As SurfaceBody, oAppearancesToExclude As List(Of String)) As Double
If oBody Is Nothing OrElse oAppearancesToExclude Is Nothing OrElse oAppearancesToExclude.Count = 0 Then Exit Function
Dim dPaintedArea As Double = 0.0
For Each oFace As Face In oBody.Faces
Dim sFaceAppearanceName As String = oFace.Appearance.DisplayName
If oAppearancesToExclude.Contains(sFaceAppearanceName) Then Continue For
Dim dArea As Double = oFace.Evaluator.Area
dPaintedArea += dArea
Next oFace
Return dPaintedArea
End FunctionIf this solved your problem, or answered your question, please click ACCEPT SOLUTION .
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Wesley Crihfield
(Not an Autodesk Employee)
