Manufacturing DevBlog

AnyCAD structure with original file names

By Adam Nagy

Inside Inventor 2016 you can reference other CAD file formats directly from an assembly. In this case you can also see the structure of the referenced assembly in the model tree. If you'd also need to get back the structure using the original file names - i.e. going from Occurrence to the original file - that is currently not exposed in the API: no direct access from "SubOccurrence1" to "AnyCAD Part1" in the blow picture.

One workaround could be finding the original files based on the Occurrence.Name, since both that and the Inventor document names created from the foreign file are based on the name of the original file. You can find the list of the original file names through Document.File.AllReferencedFiles:

Function GetFileName(filePath As String) As String
  Dim i1 As Integer
  i1 = InStrRev(filePath, "\")
   
  Dim i2 As Integer
  i2 = InStrRev(filePath, ".")
  
  ' Check for occurrence name as well
  If i2 < 1 Then i2 = InStrRev(filePath, ":")
  
  GetFileName = Mid(filePath, i1 + 1, i2 - i1 - 1)
End Function

Function GetFullPath(fileName As String) As String
  Dim asm As AssemblyDocument
  Set asm = ThisApplication.ActiveDocument
  
  Dim f As File
  For Each f In asm.File.AllReferencedFiles
    If GetFileName(f.FullFileName) = fileName Then
      GetFullPath = f.FullFileName
      Exit Function
    End If
  Next
End Function

Sub PrintOccurrences( _
occs As ComponentOccurrences, _
i As Integer)
  Dim occ As ComponentOccurrence
  For Each occ In occs
    Debug.Print Space(i); occ.name
    
    Dim doc As Document
    Set doc = occ.Definition.Document
    
    Dim fullPath As String
    
    If doc.IsEmbeddedDocument Then
      Dim fileName As String
      fileName = GetFileName(occ.name)
      fullPath = GetFullPath(fileName)
    Else
      fullPath = doc.FullFileName
    End If
    
    Debug.Print Space(i); " - " + fullPath
    
    Call PrintOccurrences( _
      occ.SubOccurrences, _
      i + 2)
  Next
End Sub

Sub PrintStructure()
  Dim doc As AssemblyDocument
  Set doc = ThisApplication.ActiveDocument
  
  Dim acd As AssemblyComponentDefinition
  Set acd = doc.ComponentDefinition
  
  Call PrintOccurrences(acd.Occurrences, 1)
End Sub

I get this output in case of my assembly that is referencing a SolidWorks assembly file called gears.SLDASM:

 gears:1
  - C:\SolidWorks\Gears\gears.SLDASM
   frame:1
    - C:\SolidWorks\Gears\frame.SLDPRT
   Internal Spur Gear:1
    - C:\SolidWorks\Gears\Internal Spur Gear.sldprt
   Spur Gear:1
    - C:\SolidWorks\Gears\Spur Gear.sldprt
   Spur Gear:2
    - C:\SolidWorks\Gears\Spur Gear.sldprt
   Spur Gear:3
    - C:\SolidWorks\Gears\Spur Gear.sldprt
   Spur Gear:4
    - C:\SolidWorks\Gears\Spur Gear.sldprt
   shaft1:1
    - C:\SolidWorks\Gears\shaft1.SLDPRT
   shaft2:1
    - C:\SolidWorks\Gears\shaft2.SLDPRT
   shaft2:2
    - C:\SolidWorks\Gears\shaft2.SLDPRT
   shaft2:3
    - C:\SolidWorks\Gears\shaft2.SLDPRT

Endless loop when using IsFileInActiveProject inside OnFileResolution

By Adam Nagy

It seems that in Inventor 2016 the behaviour of IsFileInActiveProject has been modified in a way that now it triggers the OnFileResolution event. Which of course means that if you are calling IsFileInActiveProject from inside OnFileResolution then you are creating an endless loop that will bring Inventor down.

I'm not sure yet if this change in behaviour is by-design or not, but it could be. I can imagine that now we allow add-ins to chip in when finding files even in case of using IsFileInActiveProject.

In order to avoid the endless loop, you just need to use a flag variable to signal if OnFileResolution has been called as a result of IsFileInActiveProject or not. Here is my VBA clsEvents class that shows what I mean:

Dim WithEvents faEvents As FileAccessEvents

' To avoid recursion
Private inside As Boolean

Private Sub Class_Initialize()
  Set faEvents = ThisApplication.FileAccessEvents
  inside = False
End Sub

Private Sub faEvents_OnFileResolution( _
ByVal RelativeFileName As String, _
ByVal LibraryName As String, _
CustomLogicalName() As Byte, _
ByVal BeforeOrAfter As EventTimingEnum, _
ByVal Context As NameValueMap, _
FullFileName As String, _
HandlingCode As HandlingCodeEnum)
    Dim str As String
    Dim loc As LocationTypeEnum
    
    ' To avoid recursion we use a flag variable
    ' called "inside"
    If Not inside Then
        inside = True
        
        Dim dpm As DesignProjectManager
        Set dpm = ThisApplication.DesignProjectManager
        
        Call dpm.IsFileInActiveProject( _
            "1.ipt", _
            loc, _
            str)
            
        inside = False

        HandlingCode = HandlingCodeEnum.kEventHandled
    End If
End Sub

Autodesk Cloud Accelerator Extension in Prague

By Adam Nagy

We had two very successful Autodesk Cloud Accelerators already in the US by now. We thought it's time for one in Europe too :)

It will be held in beautiful Prague 13 - 18 September, 2015.

 

Autodesk Exchange Apps Store surpasses 1 million downloads

By Adam Nagy

We reached a great milestone in the success of the Exchange Apps Store: one million downloads. 

Here is a nice overview of the store and why you should seriously consider publishing an app on it if you have not done it yet :)
http://inthefold.autodesk.com/in_the_fold/2015/06/autodesk-exchange-apps-store-reaches-1-million-downloads.html 

 

Getting points of tangency to a circle

By Balaji Ramamoorthy

In a recent query, a developer wanted to retrieve the points of tangency of sketch lines with circles. The way to do get that information is to set up the sketch constraints right just as you would with the Inventor UI. The geometry can then be retrieved from the tangent lines using SketchLine.Geometry. Here is a sample code snippet and the screenshot of sketch that it generates.

     Dim  partDoc As  PartDocument = _

         TryCast (_invApp.ActiveDocument, PartDocument)

     Dim  oCompDef As  PartComponentDefinition _

         = partDoc.ComponentDefinition

     Dim  oSketch As  PlanarSketch = _

         oCompDef.Sketches.Add(oCompDef.WorkPlanes(3))

     oSketch.Name = "MySketch" 

     Dim  oTG As  TransientGeometry = _

         _invApp.TransientGeometry

     Dim  geomConstraints As  GeometricConstraints _

         = oSketch.GeometricConstraints

     Dim  points As  SketchPoints = oSketch.SketchPoints

     Dim  skp0 As  SketchPoint = points.Add( _

         oTG.CreatePoint2d(0, 0), False )

     Dim  skp1 As  SketchPoint = points.Add( _

         oTG.CreatePoint2d(10, 0), False )

     Dim  oCenLine As  SketchLine = _

         oSketch.SketchLines.AddByTwoPoints(skp0, skp1)

     oCenLine.Construction = True 

     geomConstraints.AddHorizontal(oCenLine)

     Dim  oCircle1 As  SketchCircle = _

         oSketch.SketchCircles.AddByCenterRadius( _

             oCenLine.StartSketchPoint, 4)

     Dim  oCircle2 As  SketchCircle = _

         oSketch.SketchCircles.AddByCenterRadius( _

             oCenLine.EndSketchPoint, 2)

     geomConstraints.AddGround(oCircle1.CenterSketchPoint)

     geomConstraints.AddGround(oCircle2.CenterSketchPoint)

     Dim  skp2 As  SketchPoint = _

         points.Add(oTG.CreatePoint2d(0, 4), False )

     Dim  skp3 As  SketchPoint = _

         points.Add(oTG.CreatePoint2d(10, 2), False )

     Dim  oTanLine1 As  SketchLine = _

         oSketch.SketchLines.AddByTwoPoints(skp2, skp3)

     Dim  skp4 As  SketchPoint = points.Add( _

         oTG.CreatePoint2d(0, -4), False )

     Dim  skp5 As  SketchPoint = points.Add( _

         oTG.CreatePoint2d(10, -2), False )

     Dim  oTanLine2 As  SketchLine = _

         oSketch.SketchLines.AddByTwoPoints(skp4, skp5)

     geomConstraints.AddTangent(oCircle1, oTanLine1)

     geomConstraints.AddTangent(oCircle2, oTanLine1)

     geomConstraints.AddTangent(oCircle1, oTanLine2)

     geomConstraints.AddTangent(oCircle2, oTanLine2)

     geomConstraints.AddCoincident( _

         oTanLine1.StartSketchPoint, oCircle1)

     geomConstraints.AddCoincident( _

         oTanLine1.EndSketchPoint, oCircle2)

     geomConstraints.AddCoincident( _

         oTanLine2.StartSketchPoint, oCircle1)

     geomConstraints.AddCoincident( _

         oTanLine2.EndSketchPoint, oCircle2)

     Dim  oTanLine1Geom As  LineSegment2d _

         = oTanLine1.Geometry

     Dim  oTanLine2Geom As  LineSegment2d _

         = oTanLine2.Geometry

     Dim  sp1 As  Point2d = oTanLine1Geom.StartPoint

     Dim  ep1 As  Point2d = oTanLine1Geom.EndPoint

     MessageBox.Show(String .Format( _

         "Tangent 1 SP : {0} {1} EP : {2} {3}" , _

         sp1.X, sp1.Y, ep1.X, ep1.Y))

GetIsoCurve

By Adam Nagy

The SurfaceEvaluator object has a GetIsoCurve function that can return a curve on the surface running in the U or V parametric direction.

The function's UDirection parameter could be confusing. It tells the function if the curve should be along the U or V parametric direction, and not what the passed in parameter should be: i.e. in case of UDirection = True you get back a curve that runs in the U parametric direction, but the parameter you pass to the function should be a V parametric value.

Here is a function that goes along the U direction of a Face and creates WorkPoints there plus creates a circle based on what GetIsoCurve(UDirection = False) returns:

Sub GetIsoCurveTest()
  Dim doc As PartDocument
  Set doc = ThisApplication.ActiveDocument
  
  Dim cd As PartComponentDefinition
  Set cd = doc.ComponentDefinition
  
  Dim f As Face
  For Each f In cd.SurfaceBodies(1).Faces
    ' We only deal with the cylindrical side face now
    If TypeOf f.Geometry Is Cylinder Then
      Dim s As SurfaceEvaluator
      Set s = f.Evaluator
    
      Dim paramRange As Box2d
      Set paramRange = s.ParamRangeRect

      ' Create points along U direction
      Dim uDif As Double
      uDif = (paramRange.MaxPoint.x - paramRange.MinPoint.x) / 5
    
      Dim tr As TransientGeometry
      Set tr = ThisApplication.TransientGeometry
    
      Dim wps As WorkPoints
      Set wps = cd.WorkPoints
    
      Dim i As Integer
      For i = 0 To 5
        Dim pt() As Double
        Dim params(1) As Double
        params(0) = paramRange.MinPoint.x + (uDif * i)
        params(1) = paramRange.MinPoint.y
        Call s.GetPointAtParam(params, pt)
        Call wps.AddFixed(tr.CreatePoint(pt(0), pt(1), pt(2)))
      Next
        
      ' Get IsoCurve in the V direction (UDirection = False) 
      ' at the mid U parametric position
      ' In case of our model this should provide a Circle
      Dim midU As Double
      midU = (paramRange.MinPoint.x + paramRange.MaxPoint.x) / 2#
      
      Dim oc As ObjectCollection
      Set oc = s.GetIsoCurve(midU, False)

      Dim circ As Inventor.Circle
      Set circ = oc(1)
    
      Dim s3d As Sketch3D
      Set s3d = cd.Sketches3D.Add()
    
      ' Show it in the UI by adding it to a 3d sketch
      Call s3d.SketchCircles3D.AddByCenterRadius( _
        circ.Center, circ.Normal, circ.Radius)
    End If
  Next
End Sub

The result is:

In case of the above cylinder's side Face if you call the GetIsoCurve with UDirection = True then you'll get back a straight LineSegment (and the passed in parameter should be along the V direction, Point2d.Y), but if pass in UDirection = False then the returned curve will be a Circle (and the passed in parameter should be along the U direction, Point2d.X) - this is highlighted in blue in the above picture.    

Flipping direction of a Hem feature

By Balaji Ramamoorthy

The Hem feature relies on an edge to decide its direction. When editing the hem feature to flip its direction, Inventor identifies another edge and uses it for the hem feature. To do this programmatically, the HemDefinition.Edges collection is to be set. Currently the HemDefinition.Edges displays a "NotImplemented" error when trying to set it.

A workaround is to create a new Hem feature using the HemDefinition from the existing feature and use another edge in the process. The existing feature can be deleted after the new one is created. Also, it is important to set the end of part for retrieving the Edges collection from a Hem feature.

Here is a sample iLogic and C# code to flip the direction :

iLogic code snipet :

 Dim  oPartDoc As  PartDocument

 oPartDoc = ThisApplication.ActiveDocument

 Dim  oSheetMetalCompDef As  SheetMetalComponentDefinition

 oSheetMetalCompDef = oPartDoc.ComponentDefinition

 Dim  smFeatures As  SheetMetalFeatures

 smFeatures = oSheetMetalCompDef.Features

 Dim  oHems As  HemFeatures

 oHems = smFeatures.HemFeatures

 Dim  oHemFeature As  HemFeature

 oHemFeature = oHems.Item(1)

 Dim  oHemDef As  HemDefinition

 oHemDef = oHemFeature.Definition

 oHemFeature.SetEndOfPart(True)

 Dim  currentHemEdge As  Edge

 Dim  oHemEdgeColl As  EdgeCollection

 oHemEdgeColl = oHemDef.Edges

 currentHemEdge = oHemDef.Edges.Item(1)

 Dim  oStartVertex As  Vertex

 oStartVertex = currentHemEdge.StartVertex

 Dim  oStopVertex As  Vertex

 oStopVertex = currentHemEdge.StopVertex

 Dim  edge1 As  Edge

 edge1 = oSheetMetalCompDef.SurfaceBodies(1).Edges(1)

 Dim  edge2 As  Edge

 edge2 = oSheetMetalCompDef.SurfaceBodies(1).Edges(3)

 Dim  oEdgeColl As  EdgeCollection

 = ThisApplication.TransientObjects.CreateEdgeCollection

 If  edge1.StartVertex Is  oStartVertex  

 And  edge1.StopVertex Is  oStopVertex Then 

 	oEdgeColl.Add(edge2)

 Else  If  edge2.StartVertex Is  oStartVertex  

 And  edge2.StopVertex Is  oStopVertex Then 

 	oEdgeColl.Add(edge1)

 Else 

 	MessageBox.Show("Sorry, could not  flip direction. 

 	The hem Feature does Not  use a known edge", 

 	"iLogic HemFeature Flip direction")

 	oHemFeature.SetEndOfPart(False)

 	Return 

 End  If 

 Dim  oHemDefNew As  HemDefinition

 oHemDefNew = oHemDef.Copy

 oHemDefNew.Edges = oEdgeColl

 Dim  hemFeatureName As  String 

 hemFeatureName = oHemFeature.Name

 oHemFeature.Delete 

 Dim  oHemFeatureNew As  HemFeature

 oHemFeatureNew = oHems.Add(oHemDefNew)

 oHemFeatureNew.Name = hemFeatureName

C# code snipet :

 PartDocument oPartDoc 

 	= (PartDocument)_invApp.ActiveDocument;

 SheetMetalComponentDefinition oSheetMetalCompDef 

 	= oPartDoc.ComponentDefinition 

 	as SheetMetalComponentDefinition;

 SheetMetalFeatures smFeatures 

 	= oSheetMetalCompDef.Features as SheetMetalFeatures;

 HemFeatures oHems = smFeatures.HemFeatures;

 HemFeature oHemFeature = oHems[1];

 HemDefinition oHemDef = oHemFeature.Definition;

 // Important to get the right edge from the HemDefinition 

 oHemFeature.SetEndOfPart(true );

 EdgeCollection oHemEdgeColl = oHemDef.Edges;

 Edge currentHemEdge = oHemDef.Edges[1];

 Vertex oStartVertex = currentHemEdge.StartVertex;

 Vertex oStopVertex = currentHemEdge.StopVertex;

 Edge edge1 

 	= oSheetMetalCompDef.SurfaceBodies[1].Edges[1];

 Edge edge2 

 	= oSheetMetalCompDef.SurfaceBodies[1].Edges[3];

 EdgeCollection oEdgeColl = 

 	_invApp.TransientObjects.CreateEdgeCollection();

 if  (object.ReferenceEquals(edge1.StartVertex, oStartVertex) && 

     object.ReferenceEquals(edge1.StopVertex, oStopVertex))

 {

     // edge1 is the hem edge.  

 	//'s use another edge to flip the hem feature 

     oEdgeColl.Add(edge2);

 }

 else  if  (object.ReferenceEquals(edge2.StartVertex, oStartVertex) &&

     object.ReferenceEquals(edge2.StopVertex, oStopVertex))

 {

     // edge2 is the hem edge.  

 	//'s use another edge to flip the hem feature 

     oEdgeColl.Add(edge1);

 }

 else 

 {

     MessageBox.Show(@"Sorry, could not flip direction.  

 		The hem feature does not use a known edge",  

 		"HemFeature Flip direction" );

     oHemFeature.SetEndOfPart(false );

     return ;

 }

 HemDefinition oHemDefNew = oHemDef.Copy();

 oHemDefNew.Edges = oEdgeColl;

 string hemFeatureName = null;

 hemFeatureName = oHemFeature.Name;

 // Delete the existing hem feature 

 oHemFeature.Delete();

 HemFeature oHemFeatureNew = default (HemFeature);

 oHemFeatureNew = oHems.Add(oHemDefNew);

 oHemFeatureNew.Name = hemFeatureName;

Get COM object type name programmatically

By Adam Nagy

In different programming languages you can get the name of the object's type in different ways.

VBA, VB, VB.NET

Here you can use the TypeName built-in function and just pass in the object whose type name you want to know

C#

The object.GetType().Name property only return __ComObject for COM objects, and not the underlying type, so it is not that useful.
In C# you can either declare the ITypeInfo object and use that like in this article, or just take advantage of the VB.NET functionality by adding a reference to Microsoft.VisualBasic assembly and use Microsoft.VisualBasic.Information.TypeName() function.

C++

Here you do need to use ITypeInfo interface as shown in this article.

Note: most Inventor object types also have a Type property that returns an ObjectTypeEnum which can also be useful when identifying object type.

What object am I getting?

By Adam Nagy

The easiest way to check is by debugging into the code and see what object type the Watches window  shows. 

E.g. the following code ...

Sub TestObjects()
  Dim f As Face
  Set f = ThisApplication.ActiveDocument.SelectSet(1)

  Dim paramRange As Box2d
  Set paramRange = f.Evaluator.ParamRangeRect
  
  Dim oc As ObjectCollection
  Set oc = f.Evaluator.GetIsoCurve(paramRange.MinPoint.X, True)
End Sub

... would show this in the Watches window when I select the side face of a cylinder:

In case of VB and VB.NET you can also use the TypeName function to find out the type name of an object:

Sub TestObjects()
  Dim f As Face
  Set f = ThisApplication.ActiveDocument.SelectSet(1)

  Dim paramRange As Box2d
  Set paramRange = f.Evaluator.ParamRangeRect
  
  Dim oc As ObjectCollection
  Set oc = f.Evaluator.GetIsoCurve(paramRange.MinPoint.X, True)
  
  Dim item As Object
  Set item = oc(1)
  
  Call MsgBox(TypeName(item))
End Sub

Vault Browser control – icon column incorrect – call .Library.Initialize()

By Wayne Brill

This Login method used to log in to the Vault does not support a read-only login. 

Autodesk.DataManagement.Client.Framework.Vault.Forms Namespace > Library  Login Method

To log in read only you could use:

Autodesk.DataManagement.Client.Framework.Vault.Services Namespace > IVaultConnectionManagerService Interface > LogIn Method

Logging in this way adversely effects the Vault Browser control. Instead of the getting the icons in the icon column you get text with the ImageInfo type. (this behavior has been reported to Vault engineering).

The solution is to Initialize the library before logging in by making this call:

Autodesk.DataManagement.Client.Framework.Vault.Forms.Library.Initialize()