Manufacturing DevBlog

File vs Document

By Adam Nagy

Note: this information is from https://github.com/ADN-DevTech/Inventor-Training-Material/tree/master/Module%2014%20-%20Assembly%20Advanced

The File object represents a file on disk and a File can contain multiple Documents. Each Level of Detail corresponds to a specific Document within the same File. All files have a default document so treating a Document as a file on disk will work in most cases.
Document.FullFilename property returns the filename of the file the document is contained within. Document.FullDocumentName property returns a document name which is the filename concatenated with the level of detail name, e.g.

C:\Temp\Assembly1.iam<MyLevelOfDetail>

A special case is the Master level of detail. Supplying or getting back a full document name that consists of only the filename implies the “Master” level of detail:

oAsmDoc = oDocuments.Open("C:\Temp\Assembly1.iam")
'Is equivalent to:
oAsmDoc = oDocuments.Open("C:\Temp\Assembly1.iam<Master>")

This also explains the difference between Document.ReferencedDocumentDescriptors and Document.File.ReferencedFileDescriptors.
Note: Document.ReferencedFileDescriptors is deprecated/hidden and should not be used, instead use Document.File.ReferencedFileDescriptors. 

A Document may reference multiple Documents from the same File. So e.g. in case of this Derived Part the following code would provide this result:

VBA code:

Sub FilesAndDocs()
  Dim d As Document
  Set d = ThisApplication.ActiveDocument

  Debug.Print "ReferencedDocumentDescriptors = " + _
    str(d.ReferencedDocumentDescriptors.count)
  
  Debug.Print "File.ReferencedFileDescriptors = " + _
    str(d.File.ReferencedFileDescriptors.count)
End Sub

Output:

ReferencedDocumentDescriptors =  2
File.ReferencedFileDescriptors =  1

iLogic search path for custom references

By Philippe Leefsma

It is possible to use functionalities from custom dlls in your iLogic rules, you just need to declare the AddReference “adn.dll” (replaced by the name of your dll obviously) at the top of your rule.

iLogic will look in the following places to find your dll:

1) The folder of the document running the rule
2) The workspace path of the current project
3) The library paths of the current project
4) The external rule directories set in Tools >> Options >> iLogic Configuration >> External Rule Directories
5) The reference path set in Tools >> Options >> iLogic Configuration >> iLogic Addin DLLs Directory

In all these locations, it only looks in the directory itself. It doesn’t go into subdirectories.

Sketch extents

By Adam Nagy

Though the sketch object itself has no RangeBox that could be used to tell its extents, you can iterate through its entities and combine their extents into a single Box2d object that will provide that information:

Sub GetSketchExtents()
  ' Select the sketch in the UI before running the code
  Dim oSketch As PlanarSketch
  Set oSketch = ThisApplication.ActiveDocument.SelectSet(1)
  
  Dim oRB As Box2d
  Set oRB = ThisApplication.TransientGeometry.CreateBox2d
  
  Dim oEnt As SketchEntity
  For Each oEnt In oSketch.SketchEntities
      Call oRB.Extend(oEnt.RangeBox.MinPoint)
      Call oRB.Extend(oEnt.RangeBox.MaxPoint)
  Next
  
  Call MsgBox( _
    "(Value in internal length unit (cm))" + vbCrLf + _
    "Min = " + _
    str(oRB.MinPoint.x) + _
    str(oRB.MinPoint.y) + vbCrLf + _
    "Max = " + _
    str(oRB.MaxPoint.x) + _
    str(oRB.MaxPoint.y))
End Sub

 

 

Reorder browser pane nodes

By Adam Nagy

In the UI you can drag&drop some of the nodes in the Browser Pane to reorder them. You can do the same through the API. This sample swaps the order of the first two relationships in the assembly:

Sub ReorderConstraints()
  Dim doc As Document
  Set doc = ThisApplication.ActiveDocument
  
  Dim bp As BrowserPane
  Set bp = doc.BrowserPanes("AmBrowserArrangement")
  
  ' "Relationships" node
  Dim rs As BrowserNode
  Set rs = bp.TopNode.BrowserNodes(1)
  
  Dim bn1 As BrowserNode
  Set bn1 = rs.BrowserNodes(1)
  
  Dim bn2 As BrowserNode
  Set bn2 = rs.BrowserNodes(2)
  
  Dim bn2d As BrowserNodeDefinition
  Set bn2d = bn2.BrowserNodeDefinition
  
  Call bp.Reorder(bn1, True, bn2)
  
  Call bp.Update
End Sub

 

Make Components command implemented via API

By Adam Nagy

If you want to customize the behaviour of Manage >> Layout >> Make Components command then doing the whole thing via the API might be a good alternative. Here is the code which seems to be doing the same - as far as I can tell. This VBA code also sets the Project >> Description iProperty of each created part to the name of the Solid Body that it is referencing from the original part:

' Run this inside a Multi-Solid part
Sub MakeComponentsProgrammatically()
  ' Folder to place the new components:
  ' assembly and subcomponents
  Dim f As String: f = "C:\temp\test1\"
  
  ' Make sure the folder exists
  Dim fso As Object
  Set fso = ThisApplication.FileManager.FileSystemObject
  If Not fso.FolderExists(f) Then Call fso.CreateFolder(f)
  
  Dim doc As PartDocument
  Set doc = ThisApplication.ActiveDocument
  
  ' Create the assembly
  Dim asm As AssemblyDocument
  Set asm = ThisApplication.Documents.Add(kAssemblyDocumentObject)
  
  Dim sb As SurfaceBody
  For Each sb In doc.ComponentDefinition.SurfaceBodies
    ' Create part for each body
    Dim prt As PartDocument
    Set prt = ThisApplication.Documents.Add(kPartDocumentObject)
    
    ' Set iProperties >> Project >> Description
    ' It's inside "Design Tracking Properties"
    Dim p As Property
    Set p = prt.PropertySets( _
      "{32853F0F-3444-11D1-9E93-0060B03C1CA6}")("Description")
    p.Expression = sb.name
    
    Dim dpcs As DerivedPartComponents
    Set dpcs = prt.ComponentDefinition.ReferenceComponents. _
      DerivedPartComponents
    
    Dim dpd As DerivedPartUniformScaleDef
    Set dpd = dpcs.CreateUniformScaleDef(doc.FullDocumentName)
       
    ' Exclude the other solid bodies
    Dim dpe As DerivedPartEntity
    For Each dpe In dpd.Solids
      ' Have to set it for all entities as the default value
      ' can differ in various cases 
      dpe.IncludeEntity = dpe.ReferencedEntity Is sb
    Next
    
    Call dpcs.Add(dpd)
    
    ' Could have any name but we use the solid body's name
    Call prt.SaveAs(f + sb.name + ".ipt", False)
        
    ' Place an instance of it inside the assembly
    Dim mx As Matrix
    Set mx = ThisApplication.TransientGeometry.CreateMatrix()
    Call asm.ComponentDefinition.Occurrences. _
      AddByComponentDefinition(prt.ComponentDefinition, mx)
    
    ' Don't need it anymore
    Call prt.Close
  Next
  
  Call asm.SaveAs( _
    f + Left(doc.DisplayName, Len(doc.DisplayName) - 4) + _
    ".iam", False)
  Call asm.Close
End Sub

This is what we start off with:

And this is what we get after running the code:

 

 

Track End Of Part change in part document

By Adam Nagy

If you want to track how the 'End Of Part' symbol is moved around the part then you could listen to the DocumentEvents.OnChange event and store it's current position.

clsEndOfPart:

Dim WithEvents de As DocumentEvents
Dim wasAt As String

Private Sub Class_Initialize()
    Set de = ThisApplication.ActiveDocument.DocumentEvents
End Sub

Private Sub de_OnChange( _
ByVal ReasonsForChange As CommandTypesEnum, _
ByVal BeforeOrAfter As EventTimingEnum, _
ByVal Context As NameValueMap, _
HandlingCode As HandlingCodeEnum)

    If Context.Value("InternalName") = "Reorder Feature" Then
        Dim doc As PartDocument
        Set doc = ThisApplication.ActiveDocument
        
        Dim a As Object, b As Object
        Call doc.ComponentDefinition.GetEndOfPartPosition(a, b)
        
        Dim nowAt As String
        If b Is Nothing Then
            nowAt = "at the very end"
        Else
            nowAt = "before " + b.Name
        End If
        
        If BeforeOrAfter = kBefore Then
            wasAt = nowAt
        Else
            MsgBox ("'End Of Part' was " + wasAt + _
                ", but now it's " + nowAt + ".")
        End If
    End If
End Sub

Then call it like this:

Dim eop As clsEndOfPart

Sub TestEndOfPart()
    Set eop = New clsEndOfPart
End Sub

This is how it works:

 

Region Properties for Section View

By Adam Nagy

The code which is getting Region Properties information from a given sketch can be extended for Section Views as well. You just need to create a sketch on the Section View and project the curves from that view into the region:

Sub CreateSketchForSectionView()
  ' Select the section view in the UI first
  Dim oView As SectionDrawingView
  Set oView = ThisApplication.ActiveDocument.SelectSet(1)
 
  ' Create the sketch
  Dim oDSketch As DrawingSketch
  Set oDSketch = oView.sketches.Add()
 
  ' Fill it with the curves from the section view
  Call oDSketch.Edit
 
  Dim oCurve As DrawingCurve
  For Each oCurve In oView.DrawingCurves
    Dim oEntity As SketchEntity
    Set oEntity = oDSketch.AddByProjectingEntity(oCurve)
  Next
 
  Call oDSketch.ExitEdit
 
  ' Create a profile from the entities
  Dim oProfile As Profile
  Set oProfile = oDSketch.Profiles.AddForSolid()
 
  ' Get region properties
  Dim oRegionProps As RegionProperties
  Set oRegionProps = oProfile.RegionProperties
 
  ' Set the accuracy to medium.
  oRegionProps.Accuracy = AccuracyEnum.kMedium
 
  ' Display the region properties of the profile.
  Call MsgBox("Area: " & oRegionProps.Area)

  Call MsgBox("Perimeter: " & oRegionProps.Perimeter)

  Call MsgBox("Centroid: " & _
    oRegionProps.Centroid.X & ", " & _
    oRegionProps.Centroid.Y)
                
  Dim adPrincipalMoments(2) As Double
  Call oRegionProps.PrincipalMomentsOfInertia( _
    adPrincipalMoments(0), _
    adPrincipalMoments(1), _
    adPrincipalMoments(2))
 
  Call MsgBox("Principal Moments of Inertia: " & _
    adPrincipalMoments(0) & ", " & _
    adPrincipalMoments(1))

  Dim adRadiusOfGyration(2) As Double
  Call oRegionProps.RadiusOfGyration( _
    adRadiusOfGyration(0), _
    adRadiusOfGyration(1), _
    adRadiusOfGyration(2))
   
  Call MsgBox("Radius of Gyration: " & _
    adRadiusOfGyration(0) & ", " & _
    adRadiusOfGyration(1))

  Dim Ixx As Double
  Dim Iyy As Double
  Dim Izz As Double
  Dim Ixy As Double
  Dim Iyz As Double
  Dim Ixz As Double
  Call oRegionProps.MomentsOfInertia(Ixx, Iyy, Izz, Ixy, Iyz, Ixz)
 
  Call MsgBox(" Ixx: " & Ixx)
  Call MsgBox(" Iyy: " & Iyy)
  Call MsgBox(" Ixy: " & Ixy)

  Call MsgBox("Rotation Angle from projected Sketch " & _
    "Origin to Principal Axes: " & _
    Str(oRegionProps.RotationAngle))
End Sub

 

Parameter dependency in iLogic form

By Adam Nagy

You may want to show the possible parameter values of a part in an iLogic form where the parameters depend on each other, like in case of a Content Center part: if x is 2, then y can ony be 3 or 4, etc

Let's say this is the table that contains the possible values:

Width	Depth	Height
1	1	1
1	1	2
1	2	1
1	2	2
2	2	2
2	2	3
2	3	3
2	3	4

We can create multi-value parameters for each parameter to store their possible values: WidthValues, DepthValues, HeightValues

We can now place these parameters on a form and then create a rule that is using those parameters, e.g. "Update":

' Need this for List(Of Double) which has a Contains function
Imports System.Collections.Generic

'MsgBox(Str(WidthValues) + "; " + 
'  Str(DepthValues) + "; " + 
'  Str(HeightValues))

' Let's say these are the possible values (pv) for the parameters
' that we got from the Content Center
' Width, Depth, Height
Dim pv = New List(Of Double)
pv.AddRange(New Double(){
  1, 1, 1,
  1, 1, 2,
  1, 2, 1,
  1, 2, 2,
  2, 2, 2,
  2, 2, 3,
  2, 3, 3,
  2, 3, 4})

' WIDTH -------------------------------------------------------------- 
' Width is the main param so all its possible values are listed
Dim widths = New List(Of Double) 
widths.AddRange(New Double(){1, 2})
MultiValue.List("WidthValues") = widths

' If the current width value is not in the list then use the first one
If Not widths.Contains(WidthValues) Then WidthValues = widths(0)

' DEPTH -------------------------------------------------------------- 
' Depending on the width value we set the DepthValues
Dim depths = New List(Of Double)
For i As Integer = 0 To pv.Count - 1 Step 3
  If pv(i) = WidthValues Then
    If Not depths.Contains(pv(i + 1)) Then depths.Add(pv(i + 1))
  End If
Next

MultiValue.List("DepthValues") = depths

' If the current depth value is not in the list then use the first one
If Not depths.Contains(DepthValues) Then DepthValues = depths(0)

' HEIGHT ------------------------------------------------------------- 
' Depending on the width and depth value we set the HeightValues
Dim heights = New List(Of Double)
For i As Integer = 0 To pv.Count - 1 Step 3
  If pv(i) = WidthValues And pv(i + 1) = DepthValues Then
    If Not heights.Contains(pv(i + 2)) Then heights.Add(pv(i + 2))
  End If
Next

MultiValue.List("HeightValues") = heights

' If the current height value is not in the list then use the first one
If Not heights.Contains(HeightValues) Then HeightValues = heights(0)

' Let's change the model based on the values
Width = WidthValues
Depth = DepthValues
Height = HeightValues

InventorVb.DocumentUpdate()

Inventor 2015 sample part file: Download ILogicTest

Change Row Order of item in a BOM - Vault 2015 example

By Wayne Brill

Below is a Vault 2015 API example that changes the Row Order of an item in an Item BOM. (In the API this is BOMOrder of the ItemAssoc).

Details about Editing Items

When you call EditItems() the returned object(s) supersede all former representations of that item. You may notice that the returned item has a different ID than the item whose revID was passed in.

The association IDs for a given item’s rows are different between item iterations. Therefore, the association IDs of the rows of the item whose revID was passed to EditItems are different from the association IDs of the rows of the item returned by EditItems.

So in short:
1) Use EditItems() before manipulating an item’s rows.
2) Call GetItemBOMAssociationsByItemIds() with the id of the item returned from the call to EditItems() to get the rows for the uncommitted item.
3) Call UpdateItemBOMAssociations() with the id of the item returned from the call to EditItems() to update the rows for the uncommitted item. You can also use the ParItemID of the ItemAssoc object if its more convenient.

Note: You don’t have to call EditItems() if the item you are working with is already uncommitted and reserved to your session.  For example the item returned from AddItemRevision() is uncommitted and reserved to the calling session and you do not need to call EditItems().

 

C# example

To use this example add a button to the main form in this SDK sample:

C:\Program Files (x86)\Autodesk\Autodesk Vault 2015 SDK\vs12\CSharp\ItemEditor

 

private void button1_Click(object sender, EventArgs e)

{

    if (m_selectedItem == null)

    {

        MessageBox.Show("Select an Item first");

        return;

    }

 

    ItemService itemSvc =

         m_connection.WebServiceManager.ItemService;

    //Need to use the RevId of the item

    long[] itemRevIds = new long[]

                           { m_selectedItem.RevId };

    // Lock the item

    Item[] itemsArray_Editing =

                      itemSvc.EditItems(itemRevIds);

    //Get the id of the Item being edited

    long[] itemIds_Editing = new long[]

                       { itemsArray_Editing[0].Id };

 

    try

    {

        //Get the BOM items

        ItemAssoc[] itemAssocArray =

         itemSvc.GetItemBOMAssociationsByItemIds

                          (itemIds_Editing, false);

      //Another way to get the array of longs

      //for the Id of Items returned from EditItems

      //ItemAssoc[] itemAssocArray =

      //    itemSvc.GetItemBOMAssociationsByItemIds(

    //itemsArray_Editing.Select(i => i.Id).ToArray(),

        //  recurse: false

        //  );

 

        //Get arrays to use

        // for UpdateItemBOMAssociations()

        int numberOfItems = itemAssocArray.Length;

        long[] childIds = new long[numberOfItems];

        long[] itemAssocIds = new long[numberOfItems];

        double[] quantities =

                            new double[numberOfItems];

        bool[] isStatic = new bool[numberOfItems];

        bool[] isIncluded = new bool[numberOfItems];

        int[] bomOrder = new int[numberOfItems];

        string[] positionNums =

                          new string[numberOfItems];

        BOMEditAction[] actions =

                   new BOMEditAction[numberOfItems];

 

        //Set the values - only changing the BOMOrder

        for (int i = 0; i < numberOfItems; i++)

        {

            // add the Id of the existing

            //items to the array

            itemAssocIds[i] = itemAssocArray[i].Id;

            childIds[i] = itemAssocArray[i].CldItemID;

            quantities[i] = itemAssocArray[i].Quant;

            isStatic[i] = itemAssocArray[i].IsStatic;

            isIncluded[i] =

                        itemAssocArray[i].IsIncluded;

            // bomOrder[i] =

            //        itemAssocArray[i].BOMOrder + 1;

            bomOrder[i] = i + 2;

            positionNums[i] =

                        itemAssocArray[i].PositionNum;

            actions[i] = BOMEditAction.Update;

        }

 

        //Update using the values set above

        ItemBOM itemBOM =

            itemSvc.UpdateItemBOMAssociations

                       (itemAssocArray[0].ParItemID,

                 itemAssocIds, childIds, quantities,

                     isStatic, isIncluded, bomOrder,

                              positionNums, actions,

                       BOMViewEditOptions.Defaults);

 

        //Need to commit the items - removes the lock

        itemSvc.UpdateAndCommitItems

                                (itemsArray_Editing);

    }

    catch (Exception ex)

    {

        //Undo the edit items when a problem occurs

        itemSvc.UndoEditItems(itemIds_Editing);

    }

 

}

Exchange Apps Webinar Recording and Resources

By Adam Nagy

The easiest way to distribute/sell your Autodesk application AddIn's is to use the Autodesk Exchange Apps Store. This is what the webinar of Jim Quanci and Stephen Preston on May 22nd was about. More info can be found on Jeremy's blog: http://thebuildingcoder.typepad.com/blog/2014/05/exchange-apps-webinar-recording-and-resources.html