Manufacturing DevBlog

Set a line type for a specific part in the drawing view

By Xiaodong Liang

Issue
I would like to change the way a linetype appears for a specific part, globally throughout my drawing package. I am currently selecting the part in the model tree in the browser and changing it that way, but I have to do it on multiple views, for multiple pages and am wondering if there is a quicker way.

Solution
When you select a part of the drawing, it actually gets the corresponding drawing curves appearing in the drawing view and set their line type. So with code, you need to get the curves firstly. Following is a code demo:

Sub changeLT()

    Dim oDoc As DrawingDocument
    Set oDoc = ThisApplication.ActiveDocument
   
    Dim oEachSheet As Sheet
    Dim oEachView As DrawingView
   
    For Each oEachSheet In oDoc.Sheets
      For Each oEachView In oEachSheet.DrawingViews
       
    ' if you want to change all drawing curves
    ' *****************
    '       Dim oDrwCs As DrawingCurvesEnumerator
    '       Set oDrwCs = oEachView.DrawingCurves()
    '
    '       Dim oEachDrwC As DrawingCurve
    '       For Each oEachDrwC In oDrwCs
    '
    '        'change the line type
    '        oEachDrwC.LineType = kDashedHiddenLineType
    '        ' change the line weight
    '        oEachDrwC.LineWeight = oEachDrwC.LineWeight * 2
    '  
    ' ***********************
           
    ' if you want to change the curves from specific part, assume the referenced document of
    ' the drawing view is from an assembly.
       
        'get the referenced document
        Dim oRefDoc As Document
        Set oRefDoc = oEachView.ReferencedDocumentDescriptor.ReferencedDocument
       
        If TypeOf oRefDoc Is AssemblyDocument Then
            ' this is an assemly
           
            Dim oEachOcc As ComponentOccurrence
           
            For Each oEachOcc In oRefDoc.ComponentDefinition.Occurrences
               If TypeOf oEachOcc.Definition.Document Is PartDocument Then
                ' if this is the part you want to change
                 If oEachOcc.Name = "Part1:1" Then
                
                  'get the drawing cruves the part generates
                   Dim oDrwCs_part As DrawingCurvesEnumerator
                   Set oDrwCs_part = oEachView.DrawingCurves(oEachOcc)
                   
                    Dim oDrwC_part As DrawingCurve
                    For Each oDrwC_part In oDrwCs_part
                   
                     'change the line type
                     oDrwC_part.LineType = kDashedHiddenLineType
                     ' change the line weight
                     oDrwC_part.LineWeight = oDrwC_part.LineWeight * 2
                     Next
                     End If
               End If
            Next
         End If
       
      Next
    Next
End Sub

Add a node to the Model Browser using a ClientFeature

By Wayne Brill

Inventor allows you to create a custom browser pane and you can add browser nodes on the custom pane, even add all nodes of Model Browser Pane. However you can't add any node directly to the node tree of Model Browser pane and the new browser node can only be added as the top node of the custom pane.

One way to add a node to the Model Browser Pane is to use a Client Feature to add the node. Below is a VB.NET example. After this code runs there will be another node added to the Model browser:

 

Sub addClientFeatureToModelBrowserPane()

    Dim m_inventorApp As  _

                Inventor.Application = Nothing

    ' Try to get an active instance of Inventor

    Try

        m_inventorApp = System.Runtime. _

               InteropServices.Marshal. _

         GetActiveObject("Inventor.Application")

    Catch ex As Exception

        System.Windows.Forms.MessageBox. _

        Show("Start an Inventor session")

        Exit Sub

    End Try

 

    Dim oDef As PartComponentDefinition

    oDef = m_inventorApp.ActiveDocument. _

                         ComponentDefinition

 

    Dim oClientDef As ClientFeatureDefinition

    oClientDef = oDef.Features.ClientFeatures. _

                              CreateDefinition()

 

    Dim oClientFeature As ClientFeature

    oClientFeature = oDef.Features. _

      ClientFeatures.Add(oClientDef, "My node")

 

    oClientFeature.Name = "Testing"

End Sub

Setting UserInteractionDisabled to True can improve performance

By Wayne Brill

Performance of out-of-process clients making multiple calls to the API will be slower than running in process like an Add-In does. One way to improve performance is to set the UserInterfaceManager.UserInteractionDisabled property to true.

Setting this property to True before a batch of changes can dramatically improve performance of out-of-process clients.

Note: Be certain to set the UserInteractionDisabled property to false after your process is complete, otherwise the Inventor user interface will remain in a disabled state.

Vault API - Yes/No in the "Restrictions Found" dialog

By Marat Mirgaleev

Issue

I’ve created a very simple code that shall block all attempts to add files to Vault:

    public void OnLoad()

    {

      DocumentService.AddFileEvents.GetRestrictions +=

            new EventHandler<AddFileCommandEventArgs>(

                          AddFileEvents_GetRestrictions);

    }

 

    void AddFileEvents_GetRestrictions(object sender,

                                       AddFileCommandEventArgs e)

    {

      e.AddRestriction(

               new ExtensionRestriction(e.FileName, "Error..."));

    }

  }

It works as expected - it shows this dialog:

and doesn't add the file.

But could you describe the difference between the Yes and No buttons here, please?

Solution

In Vault a number of files can be added at once and, when some restriction is raised, this dialog is shown with a “Do you want to continue?” question. So, this prompt is whether or not you want to cancel any remaining work or to continue execution. I.e. if you’ve selected multiple files to add, choosing “Yes” will continue to attempt to add any remaining files.

Inventor API: Check Visibility of Components in Drawing View

by Vladimir Ananyev

Q: I'm trying to check if a given component occurrence is visible in a drawing view. How can I do it?

A: You can use the DrawingView.GetVisibility function for this. Here is some sample code. First select a drawing view which is referencing an assembly document and then run the code.

 

Sub checkVisibility()

 

  Dim invDV As DrawingView

  Set invDV = ThisApplication.ActiveDocument.SelectSet(1)

 

  Dim invD As Document

  Set invD = invDV.ReferencedDocumentDescriptor.ReferencedDocument

     

  Dim invAD As AssemblyDocument

  If TypeOf invD Is AssemblyDocument Then

    Set invAD = invD

    Call checkVisibilityRecursive( _

        invAD.ComponentDefinition.Occurrences, invDV)

    MsgBox "Result is in the Immediate window"

  Else

    MsgBox "No assembly document is used"

  End If

End Sub

 

Sub checkVisibilityRecursive( _

              invCOs As ComponentOccurrences, _

              invDV As DrawingView)

  Dim iTab As Integer

  iTab = 1 + invCOs(1).OccurrencePath.Count * 3

 

  Dim invCO As ComponentOccurrence

  For Each invCO In invCOs

    If Not invCO.IsSubstituteOccurrence Then

      If invCO.SubOccurrences.Count > 0 Then _

        Call checkVisibilityRecursive( _

              invCO.SubOccurrences, invDV)

      If invCO.Definition.Type = kVirtualComponentDefinitionObject Then

        Debug.Print Space(iTab) & invCO.Name & "  is virtual"

      Else

        Debug.Print Space(iTab) & invCO.Name & _

            " is visible = " & invDV.GetVisibility(invCO)

      End If

    End If

  Next

End Sub

Inventor API: Create constraints for 3D Sketch

by Vladimir Ananyev

Q: I need an example of creating constraints for Sketch3D entities, and I also need to control these entities through parameters. How can this be done using the API?

A: Constraints and dimensions of Sketch3D are similar to those of Sketch 2D. Here is a VBA example. The code will add a new Sketch3D object to an existing Part, then create two lines, add a parallel constraint between them and finally add a length constraint to one of the lines. You can then use the parameter of the length constraint to drive programmatically the dimension of the constrained line.

Note: a part document needs to be the active.

 

Sub AddSketch3DConstraints()

 

  Dim oDoc As PartDocument

  Set oDoc = ThisApplication.ActiveDocument

 

  Dim oCompDef As PartComponentDefinition

  Set oCompDef = oDoc.ComponentDefinition

 

  'Add a new Sketch3D

  Dim oSketch3d As Sketch3D

  Set oSketch3d = oCompDef.Sketches3D.Add

 

  Dim oTG As TransientGeometry

  Set oTG = ThisApplication.TransientGeometry

 

  'Add two lines to the sketch

  Dim oLine1 As SketchLine3D

  Dim oLine2 As SketchLine3D

 

  Set oLine1 = oSketch3d.SketchLines3D _

    .AddByTwoPoints(oTG.CreatePoint(0, 0, 0), _

                    oTG.CreatePoint(10, 10, 10))

  Set oLine2 = oSketch3d.SketchLines3D _

    .AddByTwoPoints(oTG.CreatePoint(0, 10, 0), _

                    oTG.CreatePoint(10, 15, 15))

  

  ' Create a parallel constraint between the lines

  Dim oParallelConstr3D   As ParallelConstraint3D

  Set oParallelConstr3D = oSketch3d _

    .GeometricConstraints3D.AddParallel(oLine1, oLine2)

 

  ' Create length constraint for line 1

  Dim oLineLengthConstr3D As LineLengthDimConstraint3D

  Set oLineLengthConstr3D = oSketch3d _

    .DimensionConstraints3D.AddLineLength(oLine1)

 

  ' Set Driven Property to False so we are sure

  ' Parameter is a ModelParameter

  oLineLengthConstr3D.Driven = False

 

  Dim oModelParam As ModelParameter

  Set oModelParam = oLineLengthConstr3D.Parameter

 

  'set new value in base units (cm)

  oModelParam.value = 15#

   

End Sub

Inventor API: Change the mirrored state of a derived part

by Vladimir Ananyev

Q: I need to change a derived part from "not mirrored" to "mirrored". Is there an example showing how to do this?

A: Here is a VBA example that mirrors a derived part.

Sub testMirrorDerivedPart()

  Dim oPartDoc As Document

  Set oPartDoc = ThisApplication.ActiveDocument

  If oPartDoc.DocumentType <> kPartDocumentObject Then Exit Sub

 

  Dim oRefComps As ReferenceComponents

  Set oRefComps = oPartDoc.ComponentDefinition.ReferenceComponents

 

  Dim oDerPartC As DerivedPartComponent

  Set oDerPartC = oRefComps.DerivedPartComponents(1)

 

  Dim oDerPartDef As DerivedPartDefinition

  Set oDerPartDef = oDerPartC.Definition

 

  If (TypeOf oDerPartDef Is DerivedPartUniformScaleDef) Then

      Dim oDerPartUScaleDef As DerivedPartUniformScaleDef

    Set oDerPartUScaleDef = oDerPartDef

  

    If (oDerPartUScaleDef.MirrorPlane = kDerivedPartNoMirrorPlane) Then

      Debug.Print "not mirrored - mirroring now"

      oDerPartUScaleDef.MirrorPlane = kDerivedPartMirrorPlaneXY

      oDerPartC.Definition = oDerPartUScaleDef

    Else

      Debug.Print "mirrored un-mirrowing now"

      oDerPartUScaleDef.MirrorPlane = kDerivedPartNoMirrorPlane

      oDerPartC.Definition = oDerPartUScaleDef

    End If

  End If

  

End Sub

Inventor API: Alpha Sort Occurrences in Assembly browser

by Vladimir Ananyev

Q: Is it possible to sort the occurrences alphabetically in an assembly browser?

A: The following VBA code illustrates the solution.

Public Sub AlphaSortComponents()

  Dim oDoc As AssemblyDocument

  Set oDoc = ThisApplication.ActiveDocument

 

  Dim odef As AssemblyComponentDefinition

  Set odef = oDoc.ComponentDefinition

 

  Dim strOccs() As String

  ReDim strOccs(odef.Occurrences.Count - 1)

 

  ' Get names of all occurrences in the assembly.

  Dim i As Long

  For i = 1 To odef.Occurrences.Count

    strOccs(i - 1) = odef.Occurrences(i).Name

  Next

     

  ' Sort the names alphabetically.

  QuickSort strOccs, LBound(strOccs), UBound(strOccs)

 

  On Error Resume Next

  Dim oTransaction As Transaction

  Set oTransaction = ThisApplication.TransactionManager _

    .StartTransaction(oDoc, "Sort Components")

 

  ' Get the "model" browser pane

  Dim oPane As BrowserPane

  Set oPane = oDoc.BrowserPanes.Item("AmBrowserArrangement")

 

  Dim oPreviousOcc As ComponentOccurrence

  Set oPreviousOcc = Nothing

 

  Dim j As Long

  For j = 1 To odef.Occurrences.Count

 

    Dim oThisOcc As ComponentOccurrence

    Set oThisOcc = odef.Occurrences.ItemByName(strOccs(j - 1))

   

    'Ignore pattern elements

    If oThisOcc.PatternElement Is Nothing Then

       

      Dim oThisNodeDef As BrowserNodeDefinition

      Set oThisNodeDef = oDoc.BrowserPanes _

          .GetNativeBrowserNodeDefinition(oThisOcc)

         

      Dim oThisBrowserNode As BrowserNode

      Set oThisBrowserNode = oPane.TopNode _

          .AllReferencedNodes(oThisNodeDef).Item(1)

         

      If Not oPreviousOcc Is Nothing Then

        Dim oPreviousNodeDef As BrowserNodeDefinition

        Set oPreviousNodeDef = oDoc.BrowserPanes _

            .GetNativeBrowserNodeDefinition(oPreviousOcc)

        Dim oPreviousBrowserNode As BrowserNode

        Set oPreviousBrowserNode = oPane.TopNode _

            .AllReferencedNodes(oPreviousNodeDef).Item(1)

        Call oPane.Reorder(oPreviousBrowserNode, _

                False, oThisBrowserNode)

        If Err.Number Then

            oTransaction.Abort

            MsgBox "Sorting failed.", vbExclamation

            Exit Sub

        End If

      Else

        'Move the first node below origin folder

        Dim oFirstBrowserNode As BrowserNode

        Dim oTempNode As BrowserNode

 

        For Each oTempNode In oPane.TopNode.BrowserNodes

          Dim oNativeObject As Object

          Set oNativeObject = oTempNode _

              .BrowserNodeDefinition.NativeObject

          If Not oNativeObject Is Nothing Then

            If TypeOf oNativeObject Is ComponentOccurrence Or _

               TypeOf oNativeObject Is OccurrencePattern Then

              Set oFirstBrowserNode = oTempNode

              Exit For

            End If

          End If

         Next

        Call oPane.Reorder(oFirstBrowserNode, True, oThisBrowserNode)

        Err.Clear

      End If

      Set oPreviousOcc = oThisOcc

    End If

  Next

 

  oTransaction.End

 

End Sub

 

Private Sub QuickSort( _

              strArray() As String, _

              intBottom As Integer, _

              intTop As Integer)

  Dim strPivot As String, strTemp As String

  Dim intBottomTemp As Integer, intTopTemp As Integer

  intBottomTemp = intBottom

  intTopTemp = intTop

  strPivot = strArray((intBottom + intTop) \ 2)

  While (intBottomTemp <= intTopTemp)

    While (UCase$(strArray(intBottomTemp)) < UCase$(strPivot) _

            And intBottomTemp < intTop)

      intBottomTemp = intBottomTemp + 1

    Wend

    While (UCase$(strPivot) < UCase$(strArray(intTopTemp)) _

             And intTopTemp > intBottom)

      intTopTemp = intTopTemp - 1

    Wend

    If intBottomTemp < intTopTemp Then

      strTemp = strArray(intBottomTemp)

      strArray(intBottomTemp) = strArray(intTopTemp)

      strArray(intTopTemp) = strTemp

    End If

    If intBottomTemp <= intTopTemp Then

      intBottomTemp = intBottomTemp + 1

      intTopTemp = intTopTemp - 1

    End If

  Wend 

  'the function calls itself until everything is in good order

  If (intBottom < intTopTemp) Then _

        QuickSort strArray, intBottom, intTopTemp

  If (intBottomTemp < intTop) Then _

        QuickSort strArray, intBottomTemp, intTop

End Sub

 

Thanks to Nathaniel for help!

Inventor 2014 API: Set Part material

by Vladimir Ananyev

With Inventor 2014 new API functionality has been introduced that fully supports consistent materials. The primary object in consistent materials is an Asset object, where Asset objects represent materials, physical properties, and colors (which are now referred to as appearances). An asset is essentially a collection of values. You may consider a material as a combination of its physical properties (density, yield strength, etc.) and how it looks or its appearance.

A material property has some basic information that identifies it – name, description, type, etc., and it references a physical properties asset and an appearance asset.

Assets exist within libraries. Inventor API Help contains several code samples that write out all of the information associated with the material, appearance, and physical property assets.

The following VBA sample set desired material from the Autodesk Material Library to the active part.

 

Private Sub SetMaterialToPart() 

  Dim oDoc As PartDocument

  Set oDoc = ThisApplication.ActiveDocument

 

  Dim Name As String

  Name = "Copper"

'    Name = "Steel"

 

  Dim localAsset As Asset

  On Error Resume Next

  Set localAsset = oDoc.Assets.Item(Name)

  If Err Then

    On Error GoTo 0

    ' Failed to get the appearance

    ' in the document, so import it.

   

    ' Get an asset library by name.

    ' Either the displayed name (which

    ' can changed based on the current language)

    ' or the internal name

    ' (which is always the same) can be used.

    Dim assetLib As AssetLibrary

    Set assetLib = ThisApplication.AssetLibraries _

        .Item("Autodesk Material Library")

'    Set assetLib = ThisApplication.AssetLibraries _

       '.Item("AD121259-C03E-4A1D-92D8-59A22B4807AD")

   

    ' Get an asset in the library

    Dim libAsset As Asset

    Set libAsset = assetLib.MaterialAssets.Item(Name)

    ' Copy the asset locally.

    Set localAsset = libAsset.CopyTo(oDoc)

  End If

  On Error GoTo 0

 

  'set material to the part

  oDoc.ActiveMaterial = localAsset

 

  ' Select the top browser node of the model pane.

  ' This is a workaround to refresh materials info in the UI.

  Call oDoc.BrowserPanes.ActivePane.TopNode.DoSelect

 

End Sub

Recursively accessing parameters from an Inventor assembly document

By Wayne Brill

This VB.NET example shows how to recursively access parameters from an assembly document containing multiple levels of parts and sub-assemblies.

    Private Sub AccessParametersFromAssembly()

        Dim oApp As Inventor.Application =

     System.Runtime.InteropServices.Marshal.

      GetActiveObject("Inventor.Application")

 

        Dim oDoc As Document

        oDoc = oApp.ActiveDocument

 

        If (oDoc.DocumentType = _

  DocumentTypeEnum.kAssemblyDocumentObject) Then

          

            Debug.Print(oDoc.DisplayName)

 

            Dim oDef As AssemblyComponentDefinition

            oDef = oDoc.ComponentDefinition

            Call PrintParameters(oDef.Occurrences)

        Else

            MsgBox("Need an assembly document.")

        End If

    End Sub

 

    Private Sub PrintParameters _

                  (oOccs As ComponentOccurrences)

        Dim oOcc As ComponentOccurrence

        For Each oOcc In oOccs

            If (oOcc.DefinitionDocumentType = _

      DocumentTypeEnum.kPartDocumentObject) Then

 

            Dim oPartDef As  _

                         PartComponentDefinition

                oPartDef = oOcc.Definition

                Dim i As Integer

 

                For i = 1 To oPartDef.Parameters.Count

                    Debug.Print(oOcc.Name & "," _

                  & oPartDef.Parameters.Item(i).Name _

            & "=" & oPartDef.Parameters.Item(i).Value)

                Next i

 

            ElseIf (oOcc.DefinitionDocumentType = _

        DocumentTypeEnum.kAssemblyDocumentObject) Then

                Debug.Print(UCase(oOcc.Name))

            Call PrintParameters _

                            (oOcc.SubOccurrences)

            End If

        Next

    End Sub