Inventor iLogic "The Parameter is Incorrect" Exception Not Making Sense

justinS3RHN — Tue, 30 Apr 2024 12:22:45 GMT

Looking for input from any Inventor iLogic gurus out there...

INTENT: I've written an external iLogic rule that runs when the user clicks on a macro button within an .ipt environment. The intent is to (in 2 clicks) model the path our routers take when we don't want a radiused inside corner. We have always had to draw this manually but it takes about 30-40 seconds, whereas now it takes 3 with this iLogic rule.

LOGIC: When the user clicks on the macro button, they are prompted to select a model edge (selection filtered only for edges). When selected, the edge length data is collected and a workpoint is added at the midpoint of the edge.
Next, a workplane is added at that workpoint perpendicular to the edge.

Next, a sketch is created on that workplane and the workpoint is projected.

Next, a pre-created sketchblock is added to the sketch and the insert point is constrained to the projected workpoint.
Next, I iterate through the sketch entities to find a circle entity and ground its center point (just to prevent the sketch from rotating).

Then, the user is prompted to select one of the 4 circle profiles in the sketch and once clicked, an extrusion feature is added symmetrically to a distance of the previously collected edge length.

That's basically it, other than a few other fluff/maintenance things like setting a parameter that tracks the number of these features that are added (for feature-naming reasons), checking if that parameter exists and adds if necessary, checking if the sketchblock exists and adding if necessary, etc...

ISSUE: I had it working perfectly yesterday (both when running the rule when working on an .ipt file that was open on its own and when editing a part directly from within an assembly), however today I get an error when trying to run the rule when editing the part within an assembly.

The exception is cast on line 74 when trying to make the workpoint and the error is "The parameter is incorrect". However, I've ensured that I'm passing the correct types into the method and ensured that the parent the rule is seeing is a 'Part Document' (because I know creating the work point doesn't work in an assembly).

I've been pulling my hair out (not literally lol) trying to figure out what's causing the exception.

Again, it used to work both while editing the part in an assembly AND with the part open on its own, but now it only works with the latter. 95% of the time we'll want to use it while editing the part within an assembly, so any help with what's causing the error would be GREATLY appreciated!

Thanks!

(view in My Videos)

Sub Main 'Define Part environment Dim oPartDoc As PartDocument Dim oCompDef As PartComponentDefinition If TypeOf ThisDoc.Document Is PartDocument Then oPartDoc = ThisDoc.Document oCompDef = oPartDoc.ComponentDefinition ElseIf TypeOf ThisDoc.Document Is AssemblyDocument Then MessageBox.Show("This program can only be run on a PART document.", "Incorrect Filetype - Assembly",MessageBoxButtons.OK,MessageBoxIcon.Information) ElseIf TypeOf ThisDoc.Document Is DrawingDocument Then MessageBox.Show("This program can only be run on a PART document.", "Incorrect Filetype - Drawing",MessageBoxButtons.OK,MessageBoxIcon.Information) Else MessageBox.Show("Unable to determine filetype.", "Incorrect Filetype",MessageBoxButtons.OK,MessageBoxIcon.Information) End If ' Prompt selection of the edge to work with Dim selectedEdge As Edge = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartEdgeFilter, "Select an edge") Dim edgeLength As Double 'Holds the length of the model edge that was selected If selectedEdge IsNot Nothing Then edgeLength = ThisApplication.MeasureTools.GetMinimumDistance(selectedEdge.StartVertex, selectedEdge.StopVertex) Else MessageBox.Show("No edge selected.", "Router Path Selection Cancelled", MessageBoxButtons.OK, MessageBoxIcon.Information) Exit Sub End If 'Get access to and update a parameter that tracks the number of these extra planes and points added to create unique feature names Dim oUserParams As UserParameters = oCompDef.Parameters.UserParameters Dim currentRuns As Integer 'This is the value that is managed within this rule Dim newParam As Parameter = Nothing Dim defaultValue As Integer Dim paramName As String paramName = "routerPathRuns" 'First check to see if it exists in this model... For Each p As Parameter In oUserParams If p.Name = paramName Then newParam = p currentRuns = p.Value currentRuns += 1 p.Value = currentRuns RuleParametersOutput() Exit For ' Exit loop once parameter is found and the above has run End If Next 'If the parameter doesn't exist, add it first then continue If newParam Is Nothing Then newParam = oUserParams.AddByExpression(paramName, defaultValue, UnitsTypeEnum.kUnitlessUnits) currentRuns = oUserParams.Item(paramName).Value currentRuns += 1 oUserParams.Item(paramName).Value = currentRuns RuleParametersOutput() End If 'Create a workpoint at the MidPoint of the selected line Dim oWorkPoint As WorkPoint Try oWorkPoint = oCompDef.WorkPoints.AddByMidPoint(selectedEdge, False) Catch ex As Exception MessageBox.Show("Try adding this feature while having the part opened on its own.", "Houston... We have a problem.", MessageBoxButtons.OK, MessageBoxIcon.Information) Exit Sub End Try Dim workPointName As String = "Router Path MidPoint " & currentRuns oWorkPoint.Name = workPointName oWorkPoint.Visible = False 'Create a work plane perpendicular to the selected edge's MidPoint Dim oWorkPlanes = oCompDef.WorkPlanes Dim oWorkPlane As WorkPlane oWorkPlane = oWorkPlanes.AddByNormalToCurve(selectedEdge, oCompDef.WorkPoints(workPointName), False) oWorkPlane.Name = "Router Path Plane " & currentRuns oWorkPlane.Visible = False 'Create the sketch and add it to the new work plane Dim oSketch As PlanarSketch oSketch = oCompDef.Sketches.Add(oWorkPlane) oSketch.Name = "Router Path Sketch " & currentRuns oSketch.Edit Dim centre = oCompDef.WorkPoints.Item(workPointName) Dim existingCentrePoint As SketchEntity = oSketch.AddByProjectingEntity(centre) Dim oTransGeom As TransientGeometry oTransGeom = ThisApplication.TransientGeometry Dim oDef As ControlDefinition oDef = ThisApplication.CommandManager.ControlDefinitions.Item("SketchProjectCutEdgesCmd") oDef.Execute 'Check if the required SketchBlock exists in the model and if not, add it. If oCompDef.SketchBlockDefinitions.Count = 0 Then Dim oSourceDoc As PartDocument 'Referene to the template .ipt Dim oSourceSketchBlock As SketchBlockDefinition oSourceDoc = ThisApplication.Documents.Open("C:\Vault_Work\Templates\Standard.ipt") 'Find the template PART oSourceSketchBlock = oSourceDoc.ComponentDefinition.SketchBlockDefinitions.Item("Router Path") 'Get access to the SKETCH BLOCK in the template oSourceSketchBlock.CopyTo(oPartDoc) oSourceDoc.Close() End If 'Insert the pre-created sketch block and position it Dim routerPathBlock As SketchBlockDefinition routerPathBlock = oCompDef.SketchBlockDefinitions.Item("Router Path") Dim oPosition As Point2d oPosition = ThisApplication.TransientGeometry.CreatePoint2d(centre.Point.X, centre.Point.Z) Call oSketch.SketchBlocks.AddByDefinition(routerPathBlock, oPosition) Dim sketchBlockRef As SketchBlock = oSketch.SketchBlocks.Item(1) Dim insertRef As SketchPoint = sketchBlockRef.Definition.InsertionPoint Dim insertRef2 As SketchPoint = sketchBlockRef.GetObject(insertRef) oSketch.GeometricConstraints.AddCoincident(insertRef2, existingCentrePoint) 'Iterate through the sketch objects to find the first reference to a circle and ground the centre point to prevent SketchBlock rotation. For Each sEntity As SketchEntity In oSketch.SketchEntities If sEntity.Type = ObjectTypeEnum.kSketchCircleObject Then Dim chosenCircle As SketchCircle = sEntity Dim chosenCircleCentre As SketchPoint = chosenCircle.CenterSketchPoint oSketch.GeometricConstraints.AddGround(chosenCircleCentre) Exit For End If Next oSketch.ExitEdit ThisApplication.ActiveView.Update() 'Pass through the distance for the extrude ExtrudeProfile(edgeLength, oCompDef, oWorkPoint, oUserParams, currentRuns) End Sub 'Perform the extrude of the router path Sub ExtrudeProfile(edgeLength As Double, part As PartComponentDefinition, selectedWorkpoint As WorkPoint, forwardedUserParams1 As UserParameters, routerPathCount As Integer) 'Hold the distance for the extrude Dim extrudeLength As Double = edgeLength 'Prompt the user to select the correct profile Dim selectedProfile As Profile = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kSketchProfileFilter, "Select a profile") If selectedProfile IsNot Nothing Then 'Extrude the selected profile to the extent of the selected edge length Dim extrudeDef As ExtrudeDefinition = part.Features.ExtrudeFeatures.CreateExtrudeDefinition(selectedProfile, PartFeatureOperationEnum.kCutOperation) extrudeDef.SetDistanceExtent(extrudeLength, PartFeatureExtentDirectionEnum.kSymmetricExtentDirection) Dim extrudeFeature As ExtrudeFeature = part.Features.ExtrudeFeatures.Add(extrudeDef) extrudeFeature.Name = "Router Path Extrusion " & routerPathCount Else 'No profile selected, remove the features (Workplane, Workpoint and sketch) that were just added. MessageBox.Show("No profile selected.", "Router Path Selection Cancelled", MessageBoxButtons.OK, MessageBoxIcon.Information) DeleteFeatures(part, selectedWorkpoint, forwardedUserParams1) Exit Sub End If End Sub 'If extruding the router path was cancelled before completion, delete the features that were already created during setup. Sub DeleteFeatures(thisPart As PartComponentDefinition, workPointToDelete As WorkPoint, forwardedUserParams2 As UserParameters) 'Iterate through all the model work points to delete the one just added. It also deletes any dependent children (the new sketch plane and sketch) For Each modelWorkPoint As WorkPoint In thisPart.WorkPoints If modelWorkPoint.Name = workPointToDelete.Name Then modelWorkPoint.Delete(False) End If Next 'Backtrack the routerPathRuns variable count so that it doesn't count up for the one that was just cancelled. Dim reverseRunCount As Integer For Each oParameter In forwardedUserParams2 If oParameter.Name = "routerPathRuns" reverseRunCount = oParameter.Value reverseRunCount -= 1 oParameter.Value = reverseRunCount RuleParametersOutput() Exit For End If Next End Sub

Re: Inventor iLogic "The Parameter is Incorrect" Exception Not Making Sense

daltonNYAW9 — Tue, 30 Apr 2024 13:50:24 GMT

I think the problem is when you click the edge in an assembly environment the edge is a proxy; it's not the real part edge.

add this after you select the edge

	If selectedEdge.Type = kEdgeProxyObject
		selectedEdge = selectedEdge.NativeObject
	End If

Re: Inventor iLogic "The Parameter is Incorrect" Exception Not Making Sense

justinS3RHN — Tue, 30 Apr 2024 14:05:26 GMT

Well I'll be... that's fantastic! Thanks for the tip!

Works beautifully now 😄

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Inventor iLogic "The Parameter is Incorrect" Exception Not Making Sense

Re: Inventor iLogic "The Parameter is Incorrect" Exception Not Making Sense

Re: Inventor iLogic "The Parameter is Incorrect" Exception Not Making Sense