topic Re: Calling Workaxes from a drawing to get automated ordinate dimensions. in Inventor Programming Forum

Calling Workaxes from a drawing to get automated ordinate dimensions.

krishnaprasad.veedu — Tue, 06 Feb 2024 14:31:15 GMT

Dears,

I was able to automate Ordinate dimensions for a subassembly as shown in the pic using ilogic. I have taken tips from here and there and used ChatGPT+copilot to get something working. I was able to achieve the dimensions shown above. Now I'm trying to get dimensions as shown below. Basically, I need to get axis from the parts and get ordinate dimensions starting from the left most side of the drawing view. Kindly let me know if anyone can help me to get this done. Thanks. Im posting the code for getting ordinate dimensions as shown above.

Sub Main() Dim oDrawDoc As DrawingDocument oDrawDoc = ThisApplication.ActiveDocument Dim oSheet As Sheet oSheet = oDrawDoc.ActiveSheet Dim oView As DrawingView oView = oSheet.DrawingViews(1) Dim oMainAsmDoc As AssemblyDocument oMainAsmDoc = oView.ReferencedDocumentDescriptor.ReferencedDocument ' Assuming the subassembly is the first occurrence in the main assembly Dim oSubAsmOcc As ComponentOccurrence oSubAsmOcc = oMainAsmDoc.ComponentDefinition.Occurrences.Item(2) Dim FPColl As ObjectCollection Dim OverallColl As ObjectCollection Dim oText As Point2d FPColl = ThisServer.TransientObjects.CreateObjectCollection OverallColl = ThisServer.TransientObjects.CreateObjectCollection ' Loop through all occurrences in the subassembly For Each occurrence As ComponentOccurrence In oSubAsmOcc.SubOccurrences ' Get the named entities for the occurrence's document Dim namedEntities = iLogicVb.Automation.GetNamedEntities(occurrence.Definition.Document) ' Find the entity named "zx" within the named entities Dim entity As Face Try entity = namedEntities.FindEntity("zx") Catch ex As Exception ' Skip the occurrence if named entity "zx" is not found Continue For End Try ' Create geometry proxy for the entity Dim oSketchProxy As Object Call occurrence.CreateGeometryProxy(entity, oSketchProxy) ' Get the drawing curves for the sketch proxy Dim curves = oView.DrawingCurves(oSketchProxy) ' Create geometry intent for the first curve Dim oIntent = oSheet.CreateGeometryIntent(curves.Item(1)) ' Add the geometry intent to the overall collection Call OverallColl.Add(oIntent) Next ' Create a point at the top-left corner of the view Dim topLeftPoint As Point2d topLeftPoint = ThisServer.TransientGeometry.CreatePoint2d(oView.Left, oView.Top) ' Create a point slightly to the right of the top-left corner to leave space for the dimension text Dim offset As Double offset = 0.1 ' Adjust this value as needed Dim oText1 As Point2d oText1 = ThisServer.TransientGeometry.CreatePoint2d(topLeftPoint.X + offset, topLeftPoint.Y) ' Create Ordinate Dimension Dim geomIntents As ObjectCollection geomIntents = ThisApplication.TransientObjects.CreateObjectCollection For i As Integer = 1 To OverallColl.Count ' Loop from 1 to count Call geomIntents.Add(OverallColl.Item(i)) ' Add intents in the order they are retrieved Next ' Create Ordinate Dimension Call oSheet.DrawingDimensions.OrdinateDimensionSets.Add(geomIntents, oText1, kHorizontalDimensionType) End Sub

Re: Calling Workaxes from a drawing to get automated ordinate dimensions.

A.Acheson — Tue, 06 Feb 2024 20:42:28 GMT

Hi @krishnaprasad.veedu

Here is an article that does just that to include a workplane in a part and or assembly occurrence.

The workaxis is just a similar object in the collection so it's an easy change. Hopefully that gets you moving in the right direction.

Re: Calling Workaxes from a drawing to get automated ordinate dimensions.

krishnaprasad.veedu — Wed, 07 Feb 2024 12:22:39 GMT

Hi @A.Acheson , thanks for your input. I have been able to call the axes and make them visible in the drawing view using this code, tried adding ordinate set dimensions but with no luck. Any idea how can i do it?

Re: Calling Workaxes from a drawing to get automated ordinate dimensions.

krishnaprasad.veedu — Wed, 07 Feb 2024 13:36:00 GMT

Hi @A.Acheson, Here is what I have tried doing, would you have a look please. I'm getting unspecified error running this. I'm kinda new to codes.

Sub Main() Dim oDrawDoc As DrawingDocument oDrawDoc = ThisApplication.ActiveDocument Dim oSheet As Sheet oSheet = oDrawDoc.ActiveSheet Dim oView As DrawingView oView = oSheet.DrawingViews(1) Dim oAsmDoc As AssemblyDocument oAsmDoc = oView.ReferencedDocumentDescriptor.ReferencedDocument Dim oCompDef As AssemblyComponentDefinition oCompDef = oAsmDoc.ComponentDefinition Dim FPColl As ObjectCollection Dim OverallColl As ObjectCollection Dim oText As Point2d FPColl = ThisServer.TransientObjects.CreateObjectCollection OverallColl = ThisServer.TransientObjects.CreateObjectCollection ' Loop through all occurrences in the assembly For Each occurrence As ComponentOccurrence In oCompDef.Occurrences ' Get the named entities for the occurrence's document Dim namedEntities = iLogicVb.Automation.GetNamedEntities(occurrence.Definition.Document) ' Find the entity named "zx" within the named entities Dim entity As WorkAxis Try entity = namedEntities.FindEntity("axs") Catch ex As Exception ' Skip the occurrence if named entity "axs" is not found Continue For End Try ' Create geometry proxy for the entity Dim oSketchProxy As Object Call occurrence.CreateGeometryProxy(entity, oSketchProxy) ' Get the drawing curves for the sketch proxy Dim curves = oView.DrawingCurves(oSketchProxy) ' Create geometry intent for the first curve Dim oIntent = oSheet.CreateGeometryIntent(curves.Item(1)) ' Add the geometry intent to the overall collection Call OverallColl.Add(oIntent) Next ' Create a point at the bottom-left corner of the view Dim bottomLeftPoint As Point2d bottomLeftPoint = ThisServer.TransientGeometry.CreatePoint2d(oView.Left, oView.Top - oView.Height-1) ' Create a point slightly above the bottom-left corner to leave space for the dimension text Dim offset As Double offset = 0.1 ' Adjust this value as needed Dim oText1 As Point2d oText1 = ThisServer.TransientGeometry.CreatePoint2d(bottomLeftPoint.X, bottomLeftPoint.Y) ' Create Ordinate Dimension Dim geomIntents As ObjectCollection geomIntents = ThisApplication.TransientObjects.CreateObjectCollection For i As Integer = 1 To OverallColl.Count Call geomIntents.Add(OverallColl.Item(i)) Next ' Create Ordinate Dimension Call oSheet.DrawingDimensions.OrdinateDimensionSets.Add(geomIntents, oText1, kHorizontalDimensionType) End Sub

Re: Calling Workaxes from a drawing to get automated ordinate dimensions.

A.Acheson — Wed, 07 Feb 2024 15:15:46 GMT

I am not sure what your design intent is for the ordination dimension. Are you trying to dimension between the now included axis?

If so I think you would need to supply the

work axis proxy at this location in your first code to get the drawing curve associated with the axis.

' Get the drawing curves for the sketch proxy Dim curves = oView.DrawingCurves(oSketchProxy)

Your last post does not included the axis visibility you had working in post 2. So go back and combine post 1 & 2 with this in mind. Hopefully that is all that is needed.

For the error checking the more info tab can give you more insight so please share that, it might indicate what object the code is failing on. If you don’t have the latest version showing the line number where the error message occurs, step through the code with a message box or logger statement until the error message occurs this way you can narrow down what line it fails on.

Re: Calling Workaxes from a drawing to get automated ordinate dimensions.

J-Camper — Thu, 08 Feb 2024 05:29:02 GMT

@krishnaprasad.veedu,

Give this a try:

Sub Main() Dim oDrawDoc As DrawingDocument = TryCast(ThisApplication.ActiveDocument, DrawingDocument) If IsNothing(oDrawDoc) Then Logger.Debug("Not Run In Drawing Document") : Exit Sub Dim oSheet As Sheet = oDrawDoc.ActiveSheet If oSheet.DrawingViews.Count < 1 Then Logger.Debug("No Views on active sheet") : Exit Sub Dim oView As DrawingView = oSheet.DrawingViews(1) Dim oAsmDoc As AssemblyDocument = TryCast(oView.ReferencedDocumentDescriptor.ReferencedDocument, AssemblyDocument) If IsNothing(oAsmDoc) Then Logger.Debug("View(1) of the active drawing is not an assembly document") : Exit Sub Dim oCompDef As AssemblyComponentDefinition = oAsmDoc.ComponentDefinition Dim CenterlineGeometryIntentList As New List(Of GeometryIntent) ' Loop through all occurrences in the assembly For Each occurrence As ComponentOccurrence In oCompDef.Occurrences ' Get the named entities for the occurrence's document Dim namedEntities = iLogicVb.Automation.GetNamedEntities(occurrence.Definition.Document) If Not namedEntities.NameExists("axs") Then Continue For Dim entity As WorkAxis = namedEntities.FindEntity("axs") ' Create geometry proxy for the entity Dim oGeometryProxy As Object occurrence.CreateGeometryProxy(entity, oGeometryProxy) 'Get Drawing Reference of the axis oView.SetIncludeStatus(oGeometryProxy, True) Dim axisCenterline As Centerline Try axisCenterline = oSheet.Centerlines.AddByWorkFeature(oGeometryProxy, oView) Catch Logger.Debug("Work Axis ""axs"" in component ""{0}"" does not produce a centerline object", occurrence.Name) Continue For End Try CenterlineGeometryIntentList.Add(oSheet.CreateGeometryIntent(axisCenterline)) Next If CenterlineGeometryIntentList.Count < 1 Then Logger.Debug("Did not collect any Geometry Intents") : Exit Sub CenterlineGeometryIntentList.Sort(Function(x, y) x.Geometry.EndPoint.X.CompareTo(y.Geometry.EndPoint.X)) ' Add the geometry intent to the object collection Dim geomIntents As ObjectCollection = ThisServer.TransientObjects.CreateObjectCollection() For Each Item In CenterlineGeometryIntentList geomIntents.Add(Item) Next Dim oPlacementPoint As Point2d = oView.Position oPlacementPoint.Y -= 1 ' Create Ordinate Dimension Call oSheet.DrawingDimensions.OrdinateDimensionSets.Add(geomIntents, oPlacementPoint, DimensionTypeEnum.kHorizontalDimensionType) End Sub

The drawing reference object of an axis, which is not perpendicular to the view, is a Centerline, not a drawing curve. I collected the GeometryIntent with a list so i could sort it before putting the objects into a collection.

Let me know if you have any questions, or if this is not working as intended

Re: Calling Workaxes from a drawing to get automated ordinate dimensions.

krishnaprasad.veedu — Thu, 08 Feb 2024 13:00:15 GMT

@J-Camper

Thank you so much. Really appreciated. It does work for the axes. One question is how do I get the starting of ordinate dimension as the left most end of the view (highlighted below)

Also, this works when I have the drawing view referring to an assembly and there are parts which contain axes named axs in the parts. Now, lets say I have subassemblies named "abc" inside the main assembly and it has parts containing axes named axs. I need to include them as well. please help.

Thank you.

Re: Calling Workaxes from a drawing to get automated ordinate dimensions.

krishnaprasad.veedu — Thu, 08 Feb 2024 13:08:13 GMT

@A.Acheson, thank you for the input but as @J-Camper mentioned we should consider the drawing reference of axes as centrelines instead of curves, I guess. It did not work when I combined those two codes probably because it wasn't creating curves and geometry intents.

Re: Calling Workaxes from a drawing to get automated ordinate dimensions.

J-Camper — Thu, 08 Feb 2024 13:59:40 GMT

@krishnaprasad.veedu,

We can find an entity on the left most part of the view for the first intent.

When you have parts in sub-assemblies are we only pulling axes from part files or will the intended axes exist in a mix of part and assembly files?

Re: Calling Workaxes from a drawing to get automated ordinate dimensions.

krishnaprasad.veedu — Thu, 08 Feb 2024 14:34:28 GMT

hi @J-Camper, I have situations where it is a mix of parts and parts inside subassemblies. Axes are not there in assemblies as it is. To be more specific I have the main assembly named 'a' inside that i have parts named 'b' and subassemblies named 'c'. The subassembly named 'c' contains another part named 'd' and the parts 'b' and 'd' has axes named 'axs'. I need to get all the 'axs' in my drawing.

Re: Calling Workaxes from a drawing to get automated ordinate dimensions.

krishnaprasad.veedu — Thu, 08 Feb 2024 14:25:14 GMT

@J-Camper : Also, for the first intent, I have this frame assembly and the web(face) of these frames are named entity(zx). I have the code in this first post. Will that work?

Re: Calling Workaxes from a drawing to get automated ordinate dimensions.

J-Camper — Thu, 08 Feb 2024 15:46:36 GMT

@krishnaprasad.veedu,

I think this should do it:

Sub Main() Dim oDrawDoc As DrawingDocument = TryCast(ThisApplication.ActiveDocument, DrawingDocument) If IsNothing(oDrawDoc) Then Logger.Debug("Not Run In Drawing Document") : Exit Sub Dim oSheet As Sheet = oDrawDoc.ActiveSheet If oSheet.DrawingViews.Count < 1 Then Logger.Debug("No Views on active sheet") : Exit Sub Dim oView As DrawingView = oSheet.DrawingViews(1) Dim oAsmDoc As AssemblyDocument = TryCast(oView.ReferencedDocumentDescriptor.ReferencedDocument, AssemblyDocument) If IsNothing(oAsmDoc) Then Logger.Debug("View(1) of the active drawing is not an assembly document") : Exit Sub Dim oCompDef As AssemblyComponentDefinition = oAsmDoc.ComponentDefinition Dim CenterlineGeometryIntentList As New List(Of GeometryIntent) Dim FirstGeometryProxy As Object Dim FirstGeoFound As Boolean = False ' Loop through all occurrences in the assembly For Each occurrence As ComponentOccurrence In oCompDef.Occurrences.AllLeafOccurrences 'Only looking at occurrences from part files ' Get the named entities for the occurrence's document Dim namedEntities = iLogicVb.Automation.GetNamedEntities(occurrence.Definition.Document) If namedEntities.NameExists("zx") Then occurrence.CreateGeometryProxy(namedEntities.FindEntity("zx"), FirstGeometryProxy) : FirstGeoFound = True If Not namedEntities.NameExists("axs") Then Continue For Dim entity As WorkAxis = namedEntities.FindEntity("axs") ' Create geometry proxy for the entity Dim oGeometryProxy As Object occurrence.CreateGeometryProxy(entity, oGeometryProxy) 'Get Drawing Reference of the axis oView.SetIncludeStatus(oGeometryProxy, True) Dim axisCenterline As Centerline Try axisCenterline = oSheet.Centerlines.AddByWorkFeature(oGeometryProxy, oView) Catch Logger.Debug("Work Axis ""axs"" in component ""{0}"" does not produce a centerline object", occurrence.Name) Continue For End Try CenterlineGeometryIntentList.Add(oSheet.CreateGeometryIntent(axisCenterline)) Next If CenterlineGeometryIntentList.Count < 1 Then Logger.Debug("Did not collect any Geometry Intents") : Exit Sub CenterlineGeometryIntentList.Sort(Function(x, y) x.Geometry.EndPoint.X.CompareTo(y.Geometry.EndPoint.X)) If Not FirstGeoFound Then Logger.Debug("Did find named face ""zx"" in any part component in the assembly. Will build the dimension set without it.") ' Add the geometry intent to the object collection Dim geomIntents As ObjectCollection = ThisServer.TransientObjects.CreateObjectCollection() Dim FirstIntent As GeometryIntent If FirstGeoFound Then geomIntents.Add(oSheet.CreateGeometryIntent(oView.DrawingCurves(FirstGeometryProxy).Item(1))) For Each Item In CenterlineGeometryIntentList geomIntents.Add(Item) Next Dim oPlacementPoint As Point2d = oView.Center oPlacementPoint.Y -= oView.Height*.55 ' Create Ordinate Dimension Call oSheet.DrawingDimensions.OrdinateDimensionSets.Add(geomIntents, oPlacementPoint, DimensionTypeEnum.kHorizontalDimensionType) End Sub

Let me know if you have any questions

Re: Calling Workaxes from a drawing to get automated ordinate dimensions.

krishnaprasad.veedu — Fri, 09 Feb 2024 06:00:56 GMT

@J-Camper,

Thats awesome. just works perfectly. One more request I would like to ask is, lets say if none of the parts in main assembly contains axes named axs and only the parts inside the subassembly contains it, it should still work, currently if i dont have parts with axs inside the main assembly, it returns me an unspecified error. More info on the error is "System.Runtime.InteropServices.COMException (0x80004005): Unspecified error (Exception from HRESULT: 0x80004005 (E_FAIL))
at System.RuntimeType.ForwardCallToInvokeMember(String memberName, BindingFlags flags, Object target, Int32[] aWrapperTypes, MessageData& msgData)
at Inventor.ComponentOccurrence.get_Definition()
at ThisRule.Main() in rule: Rule16, in document Ordim_asm.idw:line 21
at Autodesk.iLogic.Exec.AppDomExec.ExecRuleInAssembly(Assembly assem)
at iLogic.RuleEvalContainer.ExecRuleEval(String execRule)"

The line 21 is "

Dim namedEntities = iLogicVb.Automation.GetNamedEntities(occurrence.Definition.Document)"

Re: Calling Workaxes from a drawing to get automated ordinate dimensions.

krishnaprasad.veedu — Fri, 09 Feb 2024 06:26:11 GMT

@J-Camper

So the issue is not parts and subassemblies, it works fine. The problem happens when there are suppressed components in the assembly, if I suppress a component, it returns the error.
Initially I suppressed the parts to check if it works only with subassemblies. It gave me the error but when I deleted the parts and checked, it worked fine. So the problem is with suppression. Any idea how to solve this?? thanks

Re: Calling Workaxes from a drawing to get automated ordinate dimensions.

krishnaprasad.veedu — Fri, 09 Feb 2024 06:50:25 GMT

@J-Camper,

So I added an extra line for skipping suppressed components and it works fine now. Thanks a lot

    ' Loop through all occurrences in the assembly
    For Each occurrence As ComponentOccurrence In oCompDef.Occurrences.AllLeafOccurrences 'Only looking at occurrences from part files
        ' Skip suppressed components
        If occurrence.Suppressed Then Continue For

        ' Get the named entities for the occurrence's document
        Dim namedEntities = iLogicVb.Automation.GetNamedEntities(occurrence.Definition.Document)