add Occurrences to the Selection (in drawing mode)

[Anonymous]

Hello all,

since a long time I'm dreaming of a Macro to automate the following process that we use every day. We use it to highlight connectors so people can build our product easier.

We manually do the following:

In a drawing view we select a whole set of components (the connectors). Afterwards we change the color to green (using properties) & press hidden lines. This way you can clearly see where you need to place the connectors.

-> see .pdf attached with some pictures making it all clear

I'm being busy to create the code for this but I'm stuck over adding occurrences to a selection set so I can then apply the hidden line command

This is my code so far:

Sub AutoColor()

'Step 1 Select a drawing view
   ' Get the active drawing document.
   Dim drawDoc As DrawingDocument
   Set drawDoc = ThisApplication.ActiveDocument

   ' Have the user select a drawing view.
   Dim drawView As DrawingView
   Set drawView = ThisApplication.CommandManager.Pick(kDrawingViewFilter, "Select a drawing view.")

   Dim docDesc As DocumentDescriptor
   Set docDesc = drawView.ReferencedDocumentDescriptor

   ' Verify that the selected drawing view is of an assembly.
   If docDesc.ReferencedDocumentType <> kAssemblyDocumentObject Then
      MsgBox "The selected view must be of an assembly."
      Exit Sub
   End If

   ' Get the component definition for the assembly.
   Dim asmDef As AssemblyComponentDefinition
   Set asmDef = docDesc.ReferencedDocument.ComponentDefinition
   
'Step 2 Call the function that selects the correct occurrences
    Call SelectOcc(drawView, asmDef.Occurrences)

'Step 3 change to hidden lines
    Dim oControlDef As ControlDefinition
    Set oControlDef = ThisApplication.CommandManager.ControlDefinitions.Item("DrawingBodyHiddenLinesCtxCmd")
    oControlDef.Execute
    
'Step 4 for all components in selection, select all lines of them
'Step 5 place all lines on new layer with green color
End Sub


Private Sub SelectOcc(drawView As DrawingView, Occurrences As ComponentOccurrences)
   ' Iterate through the current collection of occurrences.
   Dim occ As ComponentOccurrence
      For Each occ In Occurrences
        'check if the occurence is the folder "03 PARTS", if it is then proces, else ignore
        ' the file location should be adjusted so it suits your files
        Dim OccFullLocation As String
        OccFullLocation = occ.ReferencedDocumentDescriptor.FullDocumentName
        If Left(OccFullLocation, 33) = "O:\04 R&D\08 beCAD 2013\03 PARTS\" Then
            'MsgBox ("It is a part")
        
            '
            '
            '<<<<<HERE SHOULD BE THE CODE TO ADD THE OCC TO THE SELECTIONSET>>>>
            '
        End If
   Next
End Sub

Step 1 works

Step 3 works

Step 4 & 5 are for a later moment

Step 2 calls the sub "SelectOCC". this sub cycles true the occurrences, I can filter them on file location so I only get the components needed (the connectors). In theory it should be possible to add the given occurrences to the selection set so I can run Step 3 afterwards on it.

But I don't succeed in doing this, I've tried countless of methods and went to this forum and the help but without success 😞

for the man (woman) helping me: Thanks!

[Anonymous]

I went a little bit further on this and I notice that I am working in the wrong environment with my code.

I am messing with the occurences in the assembly environment and not in the drawing environment.

so new question's:

1) can you address the occurrences of an assembly IN the drawing environment using the API? just like the model tree in the drawing env.

2) if not would a possible method be:

• go to the assembly environment
• making 2 new view's (A)
• setting the connectors in this first view visible, the frames invisible (B)
• setting the connectors in the second view invisble, frames visible
• add a overlay view so everything pops out correctly (C)

-> will (A) (B) (C) be possible true the API?

thx!

C

[Vladimir.Ananyev]

You may consider the following workflow. 

Initial state: 
Active document is your drawing document. 

Task:
You want to select all graphics that is associated with connectors.  Their part files are saved in the subfolder "O:\04 R&D\08 beCAD 2013\03 PARTS\".  Then you want to change color and line style for all connectors.

Possible workflow: 

1. Get the reference to the main assembly from the base view.(oAssyDoc)

2. Get the reference to the collection of all documents referenced by main assembly (oAssyDoc.AllReferencedDocuments).

3. Filter references to documents that are from given folder (e.g., "O:\04 R&D\08 beCAD 2013\03 PARTS\").  This also can be done using iProperties, parameters, attributes, etc.

4. For each document we can get all dependent components in main assembly (ComponentOccurrences.AllReferencedOccurrences(Document))

4. For each found occurrence we are able to find its graphics in our base view  (if any exists) and if DrawingCurveSegments are found add them to SelectSet.

5. Change color and line style of all DrawingCurveSegments in SelectSet.

[Anonymous]

Hello,

I've looked into this but in the 4th step you will add lines to an selection set and not parts. By doing this you cannot emulate the button "hidden lines" in the RB menu. because online the visible lines of the parts will be colourd, not the invisble.

I see 2 options:

A) selecting the parts left in the browser and run the command of hidden lines (oControlDef ...)

B)

• set the drawingview to hidden lines
• select all DrawingCurveSegements =  hidenlines from NOT parts (= frames)
• make them invisble
• select all DrawingCurve Segments from parts
• change color of the parts to Green

Option A) looks simple to me, but I have no idea how to get them using VBA

Option B) is more programming but see below my try, I can't get it to work but maybe it will work with some help

Public Sub AutoColor()

'step 1. select a drawingview
   ' Get the active drawing document.
   Dim oDrawDoc As DrawingDocument
   Set oDrawDoc = ThisApplication.ActiveDocument

   ' Have the user select a drawing view.
   Dim oDrawView As DrawingView
   Set oDrawView = ThisApplication.CommandManager.Pick(kDrawingViewFilter, "Select a drawing view.")

   Dim oDocDesc As DocumentDescriptor
   Set oDocDesc = oDrawView.ReferencedDocumentDescriptor

   ' Verify that the selected drawing view is of an assembly.
   If oDocDesc.ReferencedDocumentType <> kAssemblyDocumentObject Then
      MsgBox "The selected view must be of an assembly."
      Exit Sub
   End If

'step 2. set it to hiddenlines
    'Call oDrawView.SetDesignViewRepresentation(kHiddenLineDrawingViewStyle, True)
       '>>> error <<<<
   
'step 3. fill al drawingcurves in a ObjectCollection
    ' Get the TransientsObjects object
    Dim transObjs As TransientObjects
    Set transObjs = ThisApplication.TransientObjects
    
    ' create an Collection for Parts
    Dim objCollParts As ObjectCollection
    Set objCollParts = transObjs.CreateObjectCollection()
    
    'get the assembly
    Dim oAssyDoc As AssemblyComponentDefinition
    Set oAssyDoc = oDocDesc.ReferencedDocument.ComponentDefinition
       
    'call the function that adds the Part segments to the Collection
    Call SelectOccParts(oDrawView, oAssyDoc.Occurrences)
   
'step 4. Change the layer of the curves in the Collection
    'Call oDrawView.Parent.ChangeLayer(objCollParts, <<<< a layer schould be here but I can't get it to work>>>>>)
   
End Sub


Private Sub SelectOccParts(drawView As DrawingView, Occurrences As ComponentOccurrences)
 
   ' Iterate through the current collection of occurrences.
    Dim occ As ComponentOccurrence
    For Each occ In Occurrences
        ' Check to see if this occurrence is a part or assembly.
        If occ.DefinitionDocumentType = kPartDocumentObject Then
            ' It's a part
            ' check if the occurence is the folder "03 PARTS", if it is then proces, else ignore
            ' the file location should be adjusted so it suits your files
            Dim OccFullLocation As String
            OccFullLocation = occ.ReferencedDocumentDescriptor.FullDocumentName
            If Left(OccFullLocation, 33) = "O:\04 R&D\08 beCAD 2013\03 PARTS\" Then
                MsgBox OccFullLocation
                'add the segments to a collection
                     On Error Resume Next
                     Dim drawcurves As DrawingCurvesEnumerator
                     Set drawcurves = drawView.DrawingCurves(occ)
                     If Err.Number = 0 Then
                        On Error GoTo 0
                        ' Add the curve segments to the collection.
                        Dim drawCurve As DrawingCurve
                        For Each drawCurve In drawcurves
                           Dim segment As DrawingCurveSegment
                           For Each segment In drawCurve.Segments
                              'objCollParts.Add segment
                              '>>> error<<<
                           Next
                        Next
                     End If
            On Error GoTo 0
            End If
        Else
             ' It's an assembly so process its contents.
             Call SelectOccParts(drawView, occ.SubOccurrences)
        End If
    Next
End Sub

The errors that I get and can't solve:

• I don't succed in getting the drawingview to hidden lines (see code step 2. >>>> <<<<<)
• I can't add segments to my collection (see the sub code)
• I can't change the layer of the collection  (see step 4)

 Thanks for the help!

[Vladimir.Ananyev · Accepted solution]

Let's consider the follownig procedure. It finds all drawing curve segments projected from all occurrences of Cylinder.ipt part in all drawing views on the active sheet. Found graphics is moved to the new red colored layer "AAA".

 

Public Sub AutoColor_VA()

'step 1. select a drawingview
  Dim oDrawDoc As DrawingDocument
  Set oDrawDoc = ThisApplication.ActiveDocument
  
  Dim oSheet As Sheet
  Set oSheet = oDrawDoc.ActiveSheet
  
  'for objects to be moved to specified layer
  Dim oColl As ObjectCollection
  Set oColl = ThisApplication.TransientObjects.CreateObjectCollection
  
  
  '%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
  ' select drawing views on active sheet
  '%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
  Dim oDrawView As DrawingView
  
' Option 1: Have the user select a drawing view.
' Set oDrawView = ThisApplication.CommandManager _
        .Pick(kDrawingViewFilter, "Select a drawing view.")

' Option 2: we may process all drawing views on active sheet
For Each oDrawView In oSheet.DrawingViews

  'adjust drawing view style
  oDrawView.ViewStyle = DrawingViewStyleEnum.kHiddenLineDrawingViewStyle
  
'step 2.
  'Get the active drawing document.
  Dim oDocDesc As DocumentDescriptor
  Set oDocDesc = oDrawView.ReferencedDocumentDescriptor
  ' Verify that the selected drawing view is of an assembly.
  If oDocDesc.ReferencedDocumentType <> kAssemblyDocumentObject Then
     MsgBox "The selected view must be of an assembly."
     Exit Sub
  End If
  Dim oAssyDoc As AssemblyDocument
  Set oAssyDoc = oDocDesc.ReferencedDocument
   
'step 3
  'filter required docs
  Dim oRefDocs As DocumentsEnumerator
  Set oRefDocs = oAssyDoc.AllReferencedDocuments

  Dim oDoc As Inventor.Document
  For Each oDoc In oRefDocs
  
    'Criteria depends on your requirements:
    'substring from filename, custom iProperty value, parameter value, etc.
    
    If InStr(oDoc.FullFileName, "Cylinder") > 0 Then
      'this is required document
      Debug.Print oDoc.FullFileName  'debug print only
      
      'find all occurrences for every part found
      Dim oOccEnum As ComponentOccurrencesEnumerator
      Set oOccEnum = oAssyDoc.ComponentDefinition.Occurrences _
          .AllReferencedOccurrences(oDoc)
      
      Dim oOcc As ComponentOccurrence
      
      For Each oOcc In oOccEnum
      
        Dim oCurveUnum As DrawingCurvesEnumerator
        Set oCurveUnum = oDrawView.DrawingCurves(oOcc)
        
        Dim oCurve As DrawingCurve
        Dim oSegment As DrawingCurveSegment
        
        'add segments to collection to be moved to required layer
        For Each oCurve In oCurveUnum
          For Each oSegment In oCurve.Segments
            Call oColl.Add(oSegment)
          Next
        Next
        
      Next 'oOcc
    End If
    
  Next  'oDoc
Next  'oDrawView


'step 4.
  'move found curves to desired layer

  'create layer (if it doesn't exist), set color and styles
  Dim oLayer As Layer
  On Error Resume Next
  Set oLayer = oDrawDoc.StylesManager.Layers.Item("AAA")
  If Err Then
    Set oLayer = oDrawDoc.StylesManager.Layers _
          .Item("Sketch Geometry (ANSI)").Copy("AAA")
          
    'define color
    Dim oColor As Color
    Set oColor = ThisApplication.TransientObjects.CreateColor(255, 0, 0)
    oLayer.Color = oColor
    
    'define style
    'oLayer.LineType = kDashedLineType
  End If
  
  'change layer for curves collection
  Call oSheet.ChangeLayer(oColl, oLayer)

  oSheet.Update

End Sub 'AutoColor_VA

 I didn't test it much but hope this code can help you to solve your problem.

Cheers,

[Anonymous]

Hi VLadmir,

your code seems to do the trick on a efficiënt method!

really really thanks for this.

I'm now tweaking it to integrate into or processes. I'm now still searching for a method to get rid of the hidden lines of the frames. I can do this by making the hiddenlines invisible inside the layers and storing this inside the template.

Do you think there are other methods to do this? Maybe using VBA?

Thx,

Chris

[Vladimir.Ananyev]

Nice to get good new from you. 
Please mark this case as solved.

With regard to hidden lines see Layer object functionality. 
You can adjust its properties via Inventor API.

Have a good weekend 🙂

Cheers,

[KenVaessen]

I can't put this code in the ilogic part of the idw. Is it possible to adjust this code so it works in ilogic?

[KenVaessen]

Is it possible to get a text window where you can type in the partname you need, or it would be better if I could chose it out of a multi value list? And is it possible to chose the layer out of a multi value list?

And is it also possible to chose the discription instead of the filename?

[j.van.dodewaard]

copy pasting it in a new rule doesnt work.

[lauri_link]

Hi is it possible to make similar macro but  for multisolid.ipt drawings where user can make only certain solid lines red  (filtered by SOLID name)?

[_dscholtes_]

---

@Anonymous wrote:

I'm now still searching for a method to get rid of the hidden lines of the frames. I can do this by making the hiddenlines invisible inside the layers and storing this inside the template.

Do you think there are other methods to do this? Maybe using VBA?

---

Not sure if this will help, but drawing curve segments have a 'hidden line' property. If this property is true, it means the curve segment is drawn using the hidden drawing / line style.  Here's a snippet from a VBA macro of mine:

'Add only the visible drawing curve segments to the collection.
If oDrawCurveSegment.HiddenLine = False Then
    colSegmentsToColor.Add oDrawCurveSegment
End If

/Oops, didn't see the date on the specific post. Way too late.

[raja]

instead of 
oDrawView.ViewStyle = DrawingViewStyleEnum.kHiddenLineDrawingViewStyle

use

 oDrawView.ViewStyle = DrawingViewStyleEnum.kHiddenLineRemovedDrawingViewStyle