Manufacturing DevBlog

Set drawing's view back to normal

By Adam Nagy

Just like the Camera of the View of a part or an assembly, a drawing view's camera can be modified as well. However, this is not possible through the UI. Using an ISO view can give an insight into the iternals of Inventor: what seems to be just a bunch of 2d lines are actually 3d:

Sub DrawingIsoView()
  Dim v As View
  Set v = ThisApplication.ActiveView
  
  Dim c As Camera
  Set c = v.Camera
  
  c.ViewOrientationType = kIsoTopRightViewOrientation
  c.ApplyWithoutTransition
End Sub

If you ended up with such a view by accident - it happened to someone somehow - then you can easily set things back to normal:

Sub DrawingNormalView()
  Dim v As View
  Set v = ThisApplication.ActiveView
  
  Dim c As Camera
  Set c = v.Camera
  
  c.ViewOrientationType = kFrontViewOrientation
  c.ApplyWithoutTransition
End Sub

More info on Camera manipulation: http://modthemachine.typepad.com/my_weblog/2013/09/working-with-cameras-part-1.html

Set Drawing View Width

By Adam Nagy

You cannot set the Width or Height of a DrawingView directly. However, you can calculate the Scale necessary to achieve the width or height you need. Here is a VBA code demonstrating it. First you need to select the drawing view in question through the UI then run the code:

Sub SetDrawingViewWidth()
  Dim dv As DrawingView
  Set dv = ThisApplication.ActiveDocument.SelectSet(1)
  
  ' Current width
  Dim cw As Double
  cw = dv.Width
  
  ' New width we want
  ' Set in 'cm' (internal length unit)
  Dim nw As Double
  nw = 10
  
  ' New scale
  Dim ns As Double
  ns = nw / cw * dv.Scale
  
  dv.[Scale] = ns
  
  Call MsgBox("Width = " + Str(dv.Width))
End Sub

 

Drawing coordinate systems and camera

By Adam Nagy

There are 3 coordinate systems being used inside a drawing: Sheet, DrawingView and Model.

The Sheet and DrawingView coordinate systems are almost identical apart from their origin: they have the same axes and same scaling. The Model coordinate system is the coordinate system of the document that is being shown inside the drawing view.

The API makes it really easy to jump between the coordinate systems. There are functions like ModelToSheetSpace(), to transform a point from one coordinate system to the other. If you want to transform a direction then it's easier to use the transformation matrix, which is also provided, e.g. ModelToSheetTransform matrix, and use that to transform a vector using Vector.TransformBy(Matrix).

We can write a simple function which transforms the origin of the various coordinate systems and the model workpoint into sheet coordinate system, and draws a circle at each position. This might make it easier to see the relationship between them.

Sub DrawCircle(pt As Point2d, s As Sheet)
  Dim sk As DrawingSketch
  
  ' Sheet sketches are in Sheet coordinate system
  ' and DrawingView sketches are in DrawingView
  ' coordinate system
  If s.Sketches.count > 0 Then
    Set sk = s.Sketches(1)
  Else
    Set sk = s.Sketches.Add()
  End If
  
  If Not s.Parent.ActivatedObject Is sk Then
    sk.Edit
  End If
  
  Call sk.SketchCircles.AddByCenterRadius(pt, 1)
End Sub

Sub DrawCircles()
  Dim doc As DrawingDocument
  Set doc = ThisApplication.ActiveDocument
  
  Dim s As Sheet
  Set s = doc.ActiveSheet
  
  Dim tg As TransientGeometry
  Set tg = ThisApplication.TransientGeometry
  
  Dim v As DrawingView
  Set v = s.DrawingViews(1)
  
  ' (1) Show the origin of the sheet
  Call DrawCircle(tg.CreatePoint2d(), s)
  
  ' (2) Show origin of the DrawingView
  Call DrawCircle(v.DrawingViewToSheetSpace(tg.CreatePoint2d()), s)
  ' Same as
  'Call DrawCircle(v.Position, s)
  
  ' (3) Show origin of Model coordinate system
  Call DrawCircle(v.ModelToSheetSpace(tg.CreatePoint()), s)
  
  ' (4) Show WorkPoint of model
  ' transformed to Sheet coordinate system
  Dim prt As PartDocument
  Set prt = v.ReferencedDocumentDescriptor.ReferencedDocument
  
  Dim wp As WorkPoint
  Set wp = prt.ComponentDefinition.WorkPoints("MyPoint")
  
  Call DrawCircle(v.ModelToSheetSpace(wp.Point), s)
End Sub

There is also the Camera of the drawing view which is described with Model coordinates. In our case the Target is the middle of the box and Eye (the position of our eye looking at the model, described with Model coordinates) is in front of it along the (1, 1, 1) vector. Though the UpVector looks as if it's the same as the Model's Y axis, it points behind that axis and equals to (-1, 2, -1). The view direction, which points from the Eye to the Target, and the UpVector are always perpendicular. 

Here is a nice post on Cameras: http://modthemachine.typepad.com/my_weblog/2013/09/working-with-cameras-part-1.html

Rotate camera around any axis any angle

By Adam Nagy

This is a generalization of this post: 
http://adndevblog.typepad.com/manufacturing/2014/11/rotate-drawing-view-around-x-axis-of-sheet.html

Here we'll use the Matrix class to help us create a matrix that can transform any point or vector around any vector/axis and an angle: Matrix.SetToRotation(Angle As Double, Axis As Vector, Center As Point) 

To make sure we have a precise radian value for 90 degrees I'm using 2 * Atn(1) inside VBA. In languages like .NET there is a constant for PI, so you could use that instead.

We just need to get the vector we want to rotate around inside the Model space. If the vector we want to use is in the Sheet space then we need to transform it using SheetToModelTransform matrix. 

Once we have both the rotation centre (Camera.Target in our case) and the rotation axis (Sheet X inside the model space in our case) then we can create the transformation matrix and use it to get the new Eye position and UpVector direction.

Sub RotateBaseView()
  Dim baseView As DrawingView
  Set baseView = ThisApplication.ActiveDocument.SelectSet(1)
  
  Dim tr As TransientGeometry
  Set tr = ThisApplication.TransientGeometry
  
  Dim c As Camera
  Set c = baseView.Camera
  
  Dim oldEye As Point
  Set oldEye = c.eye.Copy
  
  Dim oldTarget As Point
  Set oldTarget = c.Target.Copy
  
  Dim oldUpVector As UnitVector
  Set oldUpVector = c.UpVector.Copy
  
  ' Get the Sheet's X axis into the model space
  Dim sheetXInModel As Vector
  Set sheetXInModel = tr.CreateVector(1, 0, 0)
  Call sheetXInModel.TransformBy(baseView.SheetToModelTransform)
  
  ' Calculate rotation in the model
  ' around the Target and the Sheet X
  ' in model space
  Dim m As Matrix
  Set m = tr.CreateMatrix()
  
  ' Set the rotation angle to 90 degrees
  ' Atn(1) = 45 degrees in radian
  Dim Rad90 As Double
  Rad90 = 2 * Math.Atn(1)
  Call m.SetToRotation(Rad90, sheetXInModel, oldTarget)

  ' Now we just have to transform the points and
  ' vectors
  Call oldEye.TransformBy(m)
  c.eye = oldEye
  Call oldUpVector.TransformBy(m)
  c.UpVector = oldUpVector
  
  Call c.ApplyWithoutTransition
End Sub

Get ready for the Autodesk Cloud Accelerator Program

By Stephen Preston

• Have a great idea for a new product that leverages an Autodesk web service?
  
  
• Want up close and personal help from Autodesk to turn your idea into a working prototype?  
  
  
• Interested in getting face to face with Autodesk Cloud Engineers to both learn and make sure they know what you want?

 

If yes, the 2015 Autodesk Cloud Accelerator may be for you.

Autodesk will be hosting a Cloud Accelerator in our San Francisco office for up to 14 creative software developers for two weeks – March 9 to March 20, 2015. During the Accelerator, participants will work intensively on their chosen project  with the help, support, and training of the Autodesk Cloud engineering teams.  This includes daily classes by industry experts on important aspects of Cloud development – and 1 on 1 help from these experts in real time. At the end of the Accelerator, you will also have the opportunity to present your prototype to senior Autodesk Executives.

To pursue a place in the Accelerator, send us a proposal (in English) of not more than 1000 words explaining why you should be one of participants and graduates in the “first class”. Proposals should be emailed to [email protected] no later than January 10, 2015. Successful candidates will be notified on or around January 17, 2015.

How will Autodesk choose who participates in this first Cloud Accelerator class?

To get a position in the Accelerator, Autodesk will be looking for the following in your proposal:

• Use of an Autodesk Web Service API to fill a compelling customer need. (View & Data, AutoCAD® I/O, Autodesk® Fusion 360™, Autodesk® BIM 360™ or Autodesk® ReCap 360™)
• Likelihood of having a demonstrable prototype by the end of the Accelerator.
• Strong development skills.
• High motivation.
  
  

Too costly for you?  

Autodesk recognizes two weeks of time out of the office, as well as travel and living costs, is a large investment.  To partially offset these costs, Autodesk will pay lodging costs for all the developers in this first class (14 nights in a hotel).  Up to 2 people from a single company will be accepted so be clear in your proposal if this is for 1 or 2 people (maybe you want both a product designer and developer to participate?). All other expenses are the responsibility of the participants including airfare and food (though you can be confident Autodesk will be buying a number of lunches and dinners for the class).

Questions?

Don’t be shy to ask us if you need more information to decide whether to apply.  We are happy to talk with you about what you are considering developing as part of the Accelerator – or about details you may want to know on Accelerator logistics.

We want to help you make progress developing your own products that use Cloud technologies – whether or not you end up participating in the 2015 Accelerator.  So we strongly encourage you to be quick to ask us any questions you may have on the Accelerator.  Send your questions to
[email protected].

Rotate drawing view around X axis of sheet

By Adam Nagy

In order to rotate a drawing view, you need to modify the paraneters of its Camera: UpVector (shown in below picture), the Eye (from where you are looking at the model) and the Target (the point in the model you are looking at)

If you want to rotate the view around the X axis of the sheet, so that if the drawing view currently shows Front then it will switch to Top, then you can just swap the UpVector for the current view direction (i.e. Eye to Target direction) and calculate the new Eye position. The Target position remains the same.

Sub RotateBaseView()
  Dim baseView As DrawingView
  Set baseView = ThisApplication.ActiveDocument.SelectSet(1)
   
  ' Rotate by setting the UpVector
  ' as the current view direction
  ' (i.e. Eye to Target) and then
  ' calculate the new eye
  ' which should be in the same
  ' direction as the old UpVector
  
  Dim c As Camera
  Set c = baseView.Camera
  
  Dim oldEye As Point
  Set oldEye = c.eye.Copy
  
  Dim oldTarget As Point
  Set oldTarget = c.Target.Copy
  
  Dim oldViewDir As Vector
  Set oldViewDir = oldEye.VectorTo(oldTarget)
  
  Dim viewDist As Double
  viewDist = oldViewDir.Length
  
  Dim newTargetToEye As Vector
  Set newTargetToEye = c.UpVector.AsVector().Copy
  Call newTargetToEye.ScaleBy(viewDist)
  
  Call oldTarget.TranslateBy(newTargetToEye)

  c.eye = oldTarget
  c.UpVector = oldViewDir.AsUnitVector()
  
  Call c.ApplyWithoutTransition
End Sub

And this is what you get when running the above VBA code:

 

Highlight Assembly Interference Body

By Xiaodong Liang

Question
I want to highlight the Assembly Interference result in Inventor Assembly. I get Assembly Interference Result but want the highlighting behavior same as Inventor 'Analyze Interference' result. I don't want to highlight complete component occurrences only their interference area.

Solution
You could either insert the interference body as an non-parametric body and highlight the body by HighlightSet, or add the interference body as the client graphics. The following code demo shows the workflows with the two ways.

You can even check interference yourself without 'Analyze Interference' result. The other blog tells the workflow.

http://adndevblog.typepad.com/manufacturing/2013/07/inventor-api-intersection-of-two-bodies.html

'main function

Public Sub Interference()

 

    Dim oAssDoc As AssemblyDocument

    Set oAssDoc = ThisApplication.ActiveDocument

   

    Dim oAssDef As AssemblyComponentDefinition

    Set oAssDef = oAssDoc.ComponentDefinition

    

    Dim oResults As InterferenceResults

    Dim oCheckSet As ObjectCollection

    Set oCheckSet = _

        ThisApplication.TransientObjects.CreateObjectCollection

 

    ' Add all occurrences to the object collection

    Dim oOcc As ComponentOccurrence

    For Each oOcc In oAssDef.Occurrences

        oCheckSet.Add oOcc

    Next

   

    ' Get the interference between everything.

    Set oResults = _

        oAssDef.AnalyzeInterference(oCheckSet)

   

    If oResults.Count > 0 Then

        MsgBox "There are " & _

            oResults.Count & " interferences."

       

        'Call way_HighlightSet(oResults, oAssDoc)

       

        Call way_ClientGraphics(oResults, oAssDoc)

    Else

        MsgBox "There is no interference."

    End If

End Sub

 

Sub way_HighlightSet(oResults As InterferenceResults, _

        oAssDoc As AssemblyDocument)

 

 'get the transparent appearance

  Dim localAsset As Asset

    On Error Resume Next

    Set localAsset = _

        oAssDoc.Assets.Item("Clear")

    If Err Then

        On Error GoTo 0

       

        Dim assetLib As AssetLibrary

        Set assetLib = _

          ThisApplication.AssetLibraries. _

            Item("Autodesk Appearance Library")

      

        Dim libAsset As Asset

        Set libAsset = _

            assetLib.AppearanceAssets.Item("Clear")

      

        Set localAsset = _

            libAsset.CopyTo(oAssDoc)

    End If

   

    Dim oHS As HighlightSet

    Set oHS = oAssDoc.HighlightSets.Add

    Call oHS.Color.SetColor(255, 0, 0)

       

   For i = 1 To oResults.Count

     

      'create a new part file

       Dim oPartDoc As PartDocument

       Set oPartDoc = ThisApplication.Documents _

           .Add(kPartDocumentObject, _

           ThisApplication.FileManager _

               .GetTemplateFile(kPartDocumentObject), _

           False)

 

        'insert the interfererence body to the new file

        Call oPartDoc.ComponentDefinition.Features _

             .NonParametricBaseFeatures. _

                Add(oResults.Item(i).InterferenceBody)

 

        'save the temp file

        Call oPartDoc.SaveAs( _

            "c:\temp\DifferencePart" & i & ".ipt", False)

   

       'add the new part to the assembly

       Dim oTempOcc As ComponentOccurrence

       Set oTempOcc = oAssDoc.ComponentDefinition _

           .Occurrences.AddByComponentDefinition( _

           oPartDoc.ComponentDefinition, _

           ThisApplication.TransientGeometry.CreateMatrix())

          

           'record the old appearance of occurrence one and two

           Dim oOccOne_Old_Appearance

            Dim oOccTwo_Old_Appearance

           Set oOccOne_Old_Appearance = _

            oResults.Item(i).OccurrenceOne.Appearance

           Set oOccTwo_Old_Appearance = _

            oResults.Item(i).OccurrenceTwo.Appearance

          

          

           'apply the transparent appearance to

           'occurrence one and two

            oResults.Item(i).OccurrenceOne.Appearance = _

                localAsset

           oResults.Item(i).OccurrenceTwo.Appearance = _

             localAsset

     

           ' highlight the temp occurrence

           oHS.Clear

           oHS.AddItem oTempOcc

 

 

        'pause to see the result

         MsgBox "Occurrences are highlighted from interference " & i

      

        'restore all status

       

         oTempOcc.Delete

         oPartDoc.Close

        Set oOccOne_Old_Appearance = oOccOne_Old_Appearance

        Set oOccTwo_Old_Appearance = oOccTwo_Old_Appearance

          

   Next

 

End Sub

 

Public Sub way_ClientGraphics(oResults As InterferenceResults, _

        oAssDoc As AssemblyDocument)

 

 

  'get the transparent appearance

 

   Dim localAsset As Asset

    On Error Resume Next

    Set localAsset = oAssDoc.Assets.Item("Clear")

    If Err Then

        On Error GoTo 0

       

        Dim assetLib As AssetLibrary

        Set assetLib = ThisApplication.AssetLibraries.Item("Autodesk Appearance Library")

      

        Dim libAsset As Asset

        Set libAsset = assetLib.AppearanceAssets.Item("Clear")

      

        Set localAsset = libAsset.CopyTo(oAssDoc)

    End If

   

 

   For i = 1 To oResults.Count

          

               

     Dim oClientGraphics As ClientGraphics

     Set oClientGraphics = _

        oAssDoc.ComponentDefinition.ClientGraphicsCollection.Add("InterferenceBody")

                                       

    ' Create a new graphics node within the client graphics objects.

    Dim oSurfacesNode As GraphicsNode

    Set oSurfacesNode = _

        oClientGraphics.AddNode(1)

 

    Dim oTransientBRep As TransientBRep

    Set oTransientBRep = _

        ThisApplication.TransientBRep

 

    ' Create a copy of the solid body in the part

    Dim oBody As SurfaceBody

    Set oBody = _

        oTransientBRep.Copy(oResults.Item(i).InterferenceBody)

   

        ' Create client graphics based on the transient body

        Dim oSurfaceGraphics As SurfaceGraphics

        Set oSurfaceGraphics = _

            oSurfacesNode.AddSurfaceGraphics(oBody)

   

        ' Color it red

        oSurfacesNode.RenderStyle = _

        oAssDoc.RenderStyles.Item("Red")

     

     

       'record the old appearance of occurrence one and two

        Dim oOccOne_Old_Appearance

         Dim oOccTwo_Old_Appearance

        Set oOccOne_Old_Appearance = _

            oResults.Item(i).OccurrenceOne.Appearance

        Set oOccTwo_Old_Appearance = _

            oResults.Item(i).OccurrenceTwo.Appearance

           

         'apply the transparent appearance to

          'occurrence one and two

        oResults.Item(i).OccurrenceOne.Appearance = _

            localAsset

        oResults.Item(i).OccurrenceTwo.Appearance = _

            localAsset

       

       

        ' Update the view to see the result

         ThisApplication.ActiveView.Update

   

               

        'pause to see the result

       MsgBox "Occurrences are highlighted from interference " & i

    

    

      'restore all status

       oClientGraphics.Delete

   

      Set oOccOne_Old_Appearance = oOccOne_Old_Appearance

      Set oOccTwo_Old_Appearance = oOccTwo_Old_Appearance

        

      ThisApplication.ActiveView.Update

       

    Next

       

 

  

End Sub

 

Get notified about parameter change

By Adam Nagy

You can use either the Inventor API to achieve this (from an AddIn, external application or VBA), but can also use iLogic.

If you have a Rule that is using directly the parameter you are interested in then that rule will be run when that parameter changes. If I have a model that has an extrusion with d0 height and d1 angle and create the below rules then they will be fired when those are changed:

s = d0
MsgBox("HeightChanged")

You can do the same with a Multi-Value parameter as well:

s = MultiValue

MsgBox("MultiValue changed to " + s)

In case of using the Inventor API you can listen to the ModelingEvents.OnParameterChange event.

Use UpdateAndCommitItem()to change the Category of an Item

By Wayne Brill

The function to change the category of an item may not be easy to find. To change the category of a file you can use  UpdateFileCategories(). To change the category of a folder you use UpdateFolderCategories(). To change the category of an Item you change the ItemTypId field of the item and then use UpdateAndCommitItem().

You can test this using the code below by adding a button to the ItemEditor example.

C:\Program Files (x86)\Autodesk\Autodesk Vault 2014 SDK\VS10\VB\ItemEditor

 

Private Sub Button1_Click _

(sender As System.Object, e As System.EventArgs) _

                 Handles Button1.Click

 

    Dim myItem As Item = Nothing

 

    Try

        ' Using this to get the category to change

        ' the Item to. On the form select the

        ' dropdown for the Type (category).

        ' Not using the Title so just leave

        ' it blank and hit ok

        Dim form As New CreateItemForm(m_connection)

        form.ShowDialog()

 

        If form.DialogResult <> DialogResult.OK Then

            Return

        End If

        ' Get the latest item

        Dim itemRev As Item =

            m_connection.WebServiceManager.ItemService. _

        GetLatestItemByItemNumber(m_selectedItem.ItemNum)

        'Edit the item

        myItem = m_connection.WebServiceManager. _

                     ItemService.EditItem(itemRev.RevId)

        'Change the category of the item

        myItem.ItemTypId = form.Category.Id '3

        'commit

        m_connection.WebServiceManager.ItemService. _

            UpdateAndCommitItem(myItem, _

               0, False, Nothing, Nothing, _

               Nothing, Nothing, Nothing, _

               Nothing, 2)

 

    Catch ex As Exception

        If Not myItem Is Nothing Then

            m_connection.WebServiceManager. _

ItemService.UndoEditItems(New Long() {myItem.Id})

        End If

 

        MessageBox.Show _

            ("Error occurred " + ex.ToString())

 

    End Try

End Sub

GDI Exception converting IPictureDisp to System.Drawing.Image & Image stretched

By Wayne Brill

You can get the thumbnail of a document using the ThumbNail property of a Document. This property returns an IPictureDisp. To show the Thumbnail you may need to convert it to a System.Drawing.Image. When using GetPictureFromIPicture to do this you may get GDI Exceptions. This issue is discussed on this post:

AxHost.GetPictureFromIPicture does not work correctly on x64 systems

Here is the workaround from that page. (Resolved the error in my tests)

>> >>>

Posted by Stefan Cuypers on 5/15/2009 at 4:34 AM

Here's code that does work correctly all the time (you'll need to set a reference to stdole):

using System.Drawing.Imaging;

...

public static Image GetPictureFromIPicture

                    (stdole.IPictureDisp picture)

{

    if (picture == null)

        return null;

    IntPtr hpal = IntPtr.Zero;

    if (picture.Type == 1) // bitmap

    {

        try

        {

            hpal = new IntPtr(picture.hPal);

        }

        catch (COMException)

        {

        }

    }

 

    Image retval = GetPictureFromParams

        (new IntPtr(picture.Handle), picture.Type,

        hpal, picture.Width, picture.Height);

    GC.KeepAlive(picture); // Be sure we keep this   picture alive

      // until we copied it safely into our image.

    return retval;

}

 

private static Image GetPictureFromParams

    (IntPtr handle, int type, IntPtr paletteHandle,

                             int width, int height)

{

    switch (type)

    {

        case -1:

            return null;

 

        case 0:

            return null;

 

        case 1:

            return Image.FromHbitmap(handle,

                                   paletteHandle);

 

        case 2:

            {

                WmfPlaceableFileHeader wmfHeader =

                      new WmfPlaceableFileHeader();

                wmfHeader.BboxRight = (short)width;

                wmfHeader.BboxBottom = (short)height;

                return (Image)new Metafile

                  (handle, wmfHeader, false).Clone();

            }

        case 3:

            return (Image)Icon.FromHandle(handle).Clone();

 

        case 4:

            return (Image)new Metafile(handle, false).Clone();

    }

    throw new ArgumentException("AXUnknownImage", "type");

}

<< <<<

PictureBox – Thumbnail stretched
When using the Thumbnail of a drawing converted from iPictureDisp to Drawing.System.Image in a PictureBox, it may look stretched. A solution is to set the SizeMode property to StretchImage. This forces the image to be the size of the picture box. The picture box should be square and then the image will look correct.