topic Re: Determine thickness in Ilogic in Inventor Programming Forum

Determine thickness in Ilogic

mjplaatwerk — Thu, 17 Apr 2025 07:26:46 GMT

Hello forum members,

I'm trying to determine the thickness of imported (step-file) parts in Ilogic but my knowledge is unsufficient.

After determining the thickness the corresponding "Sheet Metal Rule" an "Unfold Rule" must be selected.

In the parameters the "Export Parameter" box must be checked.

Your help would be much appreciated

Re: Determine thickness in Ilogic

a.brusamolino — Thu, 17 Apr 2025 12:34:18 GMT

Hi! You can try using this code.
You just need to select the edge that represents the thickness, and the code will do the rest.
It checks if a sheet metal rule matching that thickness exists and applies it if found.
Then, it verifies that the parameter you're looking for exists and enables the export option.
Finally, it unfolds the model.

Dim oPartDoc As PartDocument = ThisApplication.ActiveDocument ' Prompt user to select an edge Dim oSelectedEdge As Edge = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartEdgeFilter, "Select the thickness edge. Press ESC to cancel.") If oSelectedEdge Is Nothing Then Exit Sub ' Get edge length Dim minParam, maxParam, oOutputLength As Double Dim oCurveEval As CurveEvaluator = oSelectedEdge.Evaluator oCurveEval.GetParamExtents(minParam, maxParam) oCurveEval.GetLengthAtParam(minParam, maxParam, oOutputLength) Dim oThickness As Double = Math.Round(oOutputLength * 10, 1) ' Convert to mm ' Build sheet metal rule name based on thickness Dim oStyleName As String = "Sp_" + CStr(oThickness) + "_mm" ' This depends on your defined sheet metal rules ' Convert to sheet metal if it isn’t already If Not oPartDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then oPartDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" End If ' Assign the matching sheet metal rule Dim oSheetMetalCompDef As SheetMetalComponentDefinition = oPartDoc.ComponentDefinition Try Dim oStyle As SheetMetalStyle = oSheetMetalCompDef.SheetMetalStyles(oStyleName) oStyle.Activate() Catch MessageBox.Show("Failed to apply a sheet metal rule." & vbNewLine & "Detected thickness: " & CStr(oThickness), "WARNING", MessageBoxButtons.OK) Exit Sub End Try ' check flag to export Dim ParamName As String = "Thickness" ' This also depends on the parameter you're lookin for Try Dim ThicknessParam As Parameter = oPartDoc.ComponentDefinition.Parameters(ParamName) ThicknessParam.ExposedAsProperty = True Catch MessageBox.Show("Failed to find the parameter: " & CStr(ParamName), "WARNING", MessageBoxButtons.OK) Exit Sub End Try ' Unfold oSheetMetalCompDef.Unfold

Hope it helps!

Re: Determine thickness in Ilogic

mjplaatwerk — Thu, 17 Apr 2025 15:04:07 GMT

Thanks for your help

I'm not sure when I will be able to test this because I'm terribly busy but
I'll let you know the result

Re: Determine thickness in Ilogic

Andrii_Humeniuk — Thu, 17 Apr 2025 18:04:42 GMT

Hi @mjplaatwerk . To make my rule work, you don't need anything except to run it. It calculates the distance between the largest face and its opposite.

Public Sub Main() oInvApp = ThisApplication Dim oPDoc As PartDocument = TryCast(oInvApp.ActiveDocument, PartDocument) If oPDoc Is Nothing Then Exit Sub If oPDoc.SubType = "{4D29B490-49B2-11D0-93C3-7E0706000000}" Then oPDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" End If Dim oCompDef As SheetMetalComponentDefinition = oPDoc.ComponentDefinition If oCompDef.SurfaceBodies.Count = 0 Then Exit Sub Dim dThickness As Double = GetThickFromMaxFace(oCompDef.SurfaceBodies(1)) oCompDef.UseSheetMetalStyleThickness = False oCompDef.Thickness.Value = dThickness If Not oCompDef.HasFlatPattern Then : oCompDef.Unfold Else : oCompDef.FlatPattern.Edit : End If End Sub Property oInvApp As Inventor.Application Private Function GetThickFromMaxFace(ByVal oBody As SurfaceBody) As Double Dim oMaxFace As Face = GetMaxFace(oBody.Faces) If oMaxFace Is Nothing Then Return Nothing Dim origin As Inventor.Point = oMaxFace.PointOnFace Dim pt(2) As Double pt(0) = origin.X : pt(1) = origin.Y : pt(2) = origin.Z Dim n(2) As Double Call oMaxFace.Evaluator.GetNormalAtPoint(pt, n) Dim normal As Inventor.UnitVector = oInvApp.TransientGeometry.CreateUnitVector(-n(0), -n(1), -n(2)) Dim objects As ObjectsEnumerator Dim pts As ObjectsEnumerator Call oBody.FindUsingRay(origin, normal, 0.001, objects, pts, True) If objects.Count = 1 Then Return Nothing Return oInvApp.MeasureTools.GetMinimumDistance(origin, objects.Item(2)) End Function Private Function GetMaxFace(ByVal oFaces As Faces) As Face Dim dArea(oFaces.Count) As Double For i As Integer = 1 To oFaces.Count dArea(i-1) = oFaces(i).Evaluator.Area Next i For i As Integer = 1 To oFaces.Count If oFaces(i).Evaluator.Area = dArea.Max Then Return oFaces(i) Next i Return Nothing End Function

Re: Determine thickness in Ilogic

mjplaatwerk — Fri, 18 Apr 2025 11:11:33 GMT

Hi Andrii,

Your code works super. Thanks a lot.

it helps me (as a beginner) to learn and understand Ilogic.

Would you be so kind to make some extra code

After determining the thickness the corresponding "Sheet Metal Rule" an "Unfold Rule" must be selected. (see the attached files)

The name for the "Sheet Metal Rule" will be "Staal-" followed by the thickness

The name for the "Unfold Rule" will be "Staal-" followed by the thickess and "_Kfactor"

After doing this the "Use Thickness from Rule" box must be checked.

And finaly in the parameters the "Export Parameter" box must be checked.

Many thanks in advance

Re: Determine thickness in Ilogic

Andrii_Humeniuk — Fri, 18 Apr 2025 13:41:47 GMT

Hi @mjplaatwerk . I'm glad to hear that everything is working well. Try the new code that selects the Sheet Metal Rule and Unfold Rule according to the metal thickness in case there are any in the list.

Public Sub Main() oInvApp = ThisApplication Dim oPDoc As PartDocument = TryCast(oInvApp.ActiveDocument, PartDocument) If oPDoc Is Nothing Then Exit Sub If oPDoc.SubType = "{4D29B490-49B2-11D0-93C3-7E0706000000}" Then oPDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" End If Dim oCompDef As SheetMetalComponentDefinition = oPDoc.ComponentDefinition Dim dThickness As Double With oCompDef.SurfaceBodies If .Count = 0 Then Exit Sub If Not .Item(1).IsSolid Then Exit Sub dThickness = GetThickFromMaxFace(.Item(1)) End With Dim sSMRule As String = sMetalRule & (dThickness * 10) Dim sURule As String = sSMRule & sKfactor With oCompDef Try If Not .UseSheetMetalStyleThickness Then .UseSheetMetalStyleThickness = True .SheetMetalStyles(sSMRule).Activate() .UnfoldMethod = oCompDef.UnfoldMethods(sURule) Catch If .UseSheetMetalStyleThickness Then .UseSheetMetalStyleThickness = False If Not .Thickness.Value = dThickness Then .Thickness.Value = dThickness End Try If Not .HasFlatPattern Then : .Unfold() Else : .FlatPattern.Edit() : End If ' Else : .FlatPattern.Delete() : .Unfold() : End If End With End Sub Property oInvApp As Inventor.Application Property sMetalRule As String = "Staal-" Property sKfactor As String = "_Kfactor" Private Function GetThickFromMaxFace(ByVal oBody As SurfaceBody) As Double With oBody.Faces.Cast(Of Face).OrderBy(Function(f) f.Evaluator.Area).Last() Dim pt(2), n(2) As Double Call.Evaluator.GetNormalAtPoint(pt, n) Dim normal As Inventor.UnitVector = oInvApp.TransientGeometry.CreateUnitVector(-n(0), -n(1), -n(2)) Dim objects, pts As ObjectsEnumerator Call oBody.FindUsingRay(.PointOnFace, normal, 0.001, objects, pts, True) If objects.Count = 1 Then Return Nothing Return oInvApp.MeasureTools.GetMinimumDistance(.PointOnFace, objects(2)) End With End Function

Line 33 is the prefix for the Sheet Metal Rule.
Line 34 is the suffix for the Unfold Rule.

Re: Determine thickness in Ilogic

mjplaatwerk — Sat, 19 Apr 2025 06:52:57 GMT

Hello Andrii,

It works flawless. Thank you very much

I have one last request

How do I check the box in the Export parameters? (see the attached file)

Re: Determine thickness in Ilogic

Andrii_Humeniuk — Sat, 19 Apr 2025 07:19:40 GMT

Hi @mjplaatwerk . Line 26 makes the thickness parameter exportable.

Public Sub Main() oInvApp = ThisApplication Dim oPDoc As PartDocument = TryCast(oInvApp.ActiveDocument, PartDocument) If oPDoc Is Nothing Then Exit Sub If oPDoc.SubType = "{4D29B490-49B2-11D0-93C3-7E0706000000}" Then oPDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" End If Dim oCompDef As SheetMetalComponentDefinition = oPDoc.ComponentDefinition Dim dThickness As Double With oCompDef.SurfaceBodies If .Count = 0 Then Exit Sub If Not .Item(1).IsSolid Then Exit Sub dThickness = GetThickFromMaxFace(.Item(1)) End With Dim sSMRule As String = sMetalRule & (dThickness * 10) Dim sURule As String = sSMRule & sKfactor Dim oThick As Inventor.Parameter = oCompDef.Thickness Try If Not oCompDef.UseSheetMetalStyleThickness Then oCompDef.UseSheetMetalStyleThickness = True oCompDef.SheetMetalStyles(sSMRule).Activate() oCompDef.UnfoldMethod = oCompDef.UnfoldMethods(sURule) Catch If oCompDef.UseSheetMetalStyleThickness Then oCompDef.UseSheetMetalStyleThickness = False If Not oThick.Value = dThickness Then oThick.Value = dThickness End Try oThick.ExposedAsProperty = True If Not oCompDef.HasFlatPattern Then : oCompDef.Unfold() Else : oCompDef.FlatPattern.Edit() : End If ' Else : oCompDef.FlatPattern.Delete() : oCompDef.Unfold() : End If End Sub Property oInvApp As Inventor.Application Property sMetalRule As String = "Staal-" Property sKfactor As String = "_Kfactor" Private Function GetThickFromMaxFace(ByVal oBody As SurfaceBody) As Double With oBody.Faces.Cast(Of Face).OrderBy(Function(f) f.Evaluator.Area).Last() Dim pt(2), n(2) As Double Call.Evaluator.GetNormalAtPoint(pt, n) Dim normal As Inventor.UnitVector = oInvApp.TransientGeometry.CreateUnitVector(-n(0), -n(1), -n(2)) Dim objects, pts As ObjectsEnumerator Call oBody.FindUsingRay(.PointOnFace, normal, 0.001, objects, pts, True) If objects.Count = 1 Then Return Nothing Return oInvApp.MeasureTools.GetMinimumDistance(.PointOnFace, objects(2)) End With End Function