Assign Layer to part sketch in a drawing using iLogic

They_Call_Me_Jake · ‎07-01-2016

I am trying to assign a part sketch in a drawing to a specific layer but have been unable to find anything on how to do this. I have been able to turn the visibility of a part sketch on and off using a proxy. The problem is that you can't assign the sketch itself to a layer you have to select as edges first to assign the sketch to a specific layer. Is what I am trying to do possible? My thought was if there is anyway to, with iLogic, either select the sketch I want and then select its edges and assign it to a layer or create a drawing sketch based off of the part sketch and then assign the drawing sketch to a specific layer. Any help would be greatly appreciated.

petestrycharske · ‎07-01-2016

mrsmithTYTMZ,

I've got a start here, but am having a little trouble with one of my lines (which I've underlined). I'm baffled as to why this won't work, so am hoping that someone smarter and wiser than I can shed some light on this. Anyway, it at least tells me when the drawing sketch is named the same as a layer, so I feel like I am on the right track. Hope this helps and have a most blessed day!

' Set a reference to the drawing document.
' This assumes a drawing document is active.
Dim oDrawDoc As DrawingDocument
oDrawDoc = ThisApplication.ActiveDocument

' Set a reference to the active sheet.
Dim oActiveSheet As Sheet
oActiveSheet = oDrawDoc.ActiveSheet

' Create a Drawing View Object
Dim oDrawingView As DrawingView
Dim oDrawingSketch As DrawingSketch
Dim oSketchEntity As SketchEntity
Dim oLayer As Layer

For Each oDrawingView In oActiveSheet.DrawingViews
   For Each oDrawingSketch In oDrawingView.Sketches
       For Each oLayer In oDrawDoc.StylesManager.Layers
           If oDrawingSketch.Name = oLayer.Name Then
               MessageBox.Show(oDrawingSketch.Name & " sketch should be on the " & oLayer.Name & " layer", "Title")
               For Each oSketchEntity In oDrawingSketch.SketchEntities
                   oSketchEntity.Layer = oLayer
               Next
           End If

       Next
   Next
Next

iLogicVb.UpdateWhenDone = True

Peace,

Pete

Just a guy on a couch...

Please give a kudos if helpful and mark as a solution if somehow I got it right.

Anonymous · ‎07-04-2016

@petestrycharske

Yes you are on a right track but since you where in drawing document you need to activate the sketch environment to change the layer of sketch. So I've added a simple code which was underlined that might help you most.

' Set a reference to the drawing document.
' This assumes a drawing document is active.
Dim oDrawDoc As DrawingDocument
oDrawDoc = ThisApplication.ActiveDocument

' Set a reference to the active sheet.
Dim oActiveSheet As Sheet
oActiveSheet = oDrawDoc.ActiveSheet

' Create a Drawing View Object
Dim oDrawingView As DrawingView
Dim oDrawingSketch As DrawingSketch
Dim oSketchEntity As SketchEntity
Dim oLayer As Layer

For Each oDrawingView In oActiveSheet.DrawingViews
For Each oDrawingSketch In oDrawingView.Sketches
For Each oLayer In oDrawDoc.StylesManager.Layers
If oDrawingSketch.Name = oLayer.Name Then
MessageBox.Show(oDrawingSketch.Name & " sketch should be on the " & oLayer.Name & " layer", "Title")
For Each oSketchEntity In oDrawingSketch.SketchEntities
oDrawingSketch.Edit
oSketchEntity.Layer = oLayer
oDrawingSketch.ExitEdit
Next
End If

Next
Next
Next

iLogicVb.UpdateWhenDone = True

If you find this was helpful for your query please accept it as solution / give a kudos

Cheers,

SK.

petestrycharske · ‎07-05-2016

SK,

Brilliant! That was definitely the missing piece to my puzzle. I rewrote it slightly, so that the sketch wouldn't edit as often, but that is what I was missing. Here is the revised code below with SK's missing pieces. Hope this helps and have a most blessed day!

Peace,

Pete

' Set a reference to the drawing document.
' This assumes a drawing document is active.
Dim oDrawDoc As DrawingDocument
oDrawDoc = ThisApplication.ActiveDocument

' Set a reference to the active sheet.
Dim oActiveSheet As Sheet
oActiveSheet = oDrawDoc.ActiveSheet

' Create a Drawing View Object
Dim oDrawingView As DrawingView
Dim oDrawingSketch As DrawingSketch
Dim oSketchEntity As SketchEntity
Dim oLayer As Layer

For Each oDrawingView In oActiveSheet.DrawingViews
   For Each oDrawingSketch In oDrawingView.Sketches
       For Each oLayer In oDrawDoc.StylesManager.Layers
           If oDrawingSketch.Name = oLayer.Name Then
               MessageBox.Show(oDrawingSketch.Name & " sketch should be on the " & oLayer.Name & " layer", "Title")
               oDrawingSketch.Edit
               For Each oSketchEntity In oDrawingSketch.SketchEntities
                   oSketchEntity.Layer = oLayer
               Next
               oDrawingSketch.ExitEdit

           End If

       Next
   Next
Next

iLogicVb.UpdateWhenDone = True

Just a guy on a couch...

Please give a kudos if helpful and mark as a solution if somehow I got it right.

They_Call_Me_Jake · ‎07-06-2016

Thanks petestrycharske and srinivas.kasilingam for the quick replies. Question tho and correct me if I am wrong but won't this code only change a sketch that has been created in the drawing itself? What I am trying to accomplish is this....I have sketches that were created in the part or assembly itself and then after I have created the Base view from the part/Assembly I then right click on the part in the model tree in that view and select "Get Part Sketches" after which I select the part sketches I want to include. It is these said sketches that I am wanting to assign a layer to. I know that you can't even just click on the sketch in the model tree and then click a layer....you have to right click on the sketch in the model tree and then click "Select as Edges" before you can assign a layer to the entire sketch.

They_Call_Me_Jake · ‎07-06-2016

Just as an example this is what I have to do to change the visibility of a model sketch....

Dim oDoc As DrawingDocument
	oDoc = ThisApplication.ActiveDocument

Dim oActiveSheet As Sheet
	oActiveSheet = oDoc.ActiveSheet

Dim oDrawingView As DrawingView
	oDrawingView = oActiveSheet.DrawingViews(3)
    
Dim oRefDoc As AssemblyDocument
	oRefDoc = oDrawingView.ReferencedDocumentDescriptor.ReferencedDocument
	
Dim oAssDef As AssemblyComponentDefinition
	oAssDef = oRefDoc.ComponentDefinition
    
Dim oOcc As ComponentOccurrence
	oOcc = oAssDef.Occurrences(1)
    
Dim oPart As PartDocument
	oPart = oOcc.Definition.Document

Dim oDef As PartComponentDefinition
	oDef = oPart.ComponentDefinition

Dim oSketch As PlanarSketch
	For Each oSketch In oDef.Sketches
		Dim oSketchProxy As PlanarSketchProxy
		oOcc.CreateGeometryProxy(oSketch, oSketchProxy)
			If oSketch.Name = "SK Back MTG Holes With Cutouts" Then
				oDrawingView.SetVisibility(oSketchProxy, True)
			End If
	Next

Anonymous · ‎07-06-2016

Hi @They_Call_Me_Jake

I have modified the code as per your requirement. Hope this will help you.

' Set a reference to the drawing document.
' This assumes a drawing document is active.
Dim oDrawDoc As DrawingDocument
oDrawDoc = ThisApplication.ActiveDocument

' Set a reference to the active sheet.
Dim oActiveSheet As Sheet
oActiveSheet = oDrawDoc.ActiveSheet

' Create a Drawing View Object
Dim oDrawingView As DrawingView
Dim oDrawingSketch As PlanarSketch
Dim oSketchEntity As SketchEntity
Dim oLayer As Layer
Dim oPartDoc As DocumentDescriptor
Dim oCd As ComponentDefinition
For Each oDrawingView In oActiveSheet.DrawingViews
    Dim oReferencedDocument As DocumentDescriptorsEnumerator
    oReferencedDocument = oActiveSheet.Parent.ReferencedDocumentDescriptors
        For Each oPartDoc In oReferencedDocument
            For Each oCd In oPartDoc.ReferencedDocument.ComponentDefinitions
                 For Each oDrawingSketch In oCd.Sketches
                    For Each oLayer In oDrawDoc.StylesManager.layers
                        If oDrawingSketch.name = oLayer.name Then
                            MsgBox oDrawingSketch.name & " sketch should be on the " & oLayer.name & " layer", "Title"
                            oDrawingSketch.Edit
                            For Each oSketchEntity In oDrawingSketch.SketchEntities
                                oSketchEntity.Layer = oLayer
                            Next
                            oDrawingSketch.ExitEdit
            
                        End If
                    Next
                Next
            Next
        Next
Next

iLogicVb.UpdateWhenDone = True

If you find this was helpful please accept this as solution /Press the kudos button

Cheers,

SK.

They_Call_Me_Jake · ‎07-06-2016

@Anonymous Thank you for you help on this. We're close but I'm getting an error right after I close the message box:

Unspecified error (Exception from HRESULT: 0x80004005 (E_FAIL))

and this in the More Info tab:

System.Runtime.InteropServices.COMException (0x80004005): Unspecified error (Exception from HRESULT: 0x80004005 (E_FAIL))
at System.RuntimeType.ForwardCallToInvokeMember(String memberName, BindingFlags flags, Object target, Int32[] aWrapperTypes, MessageData& msgData)
at Inventor.SketchEntity.set_Layer(Layer )
at LmiRuleScript.Main()
at Autodesk.iLogic.Exec.AppDomExec.ExecRuleInAssembly(Assembly assem)
at iLogic.RuleEvalContainer.ExecRuleEval(String execRule)

it looks like the error is in the last For Loop.....I think...... If I comment out the line "oSketchEntity.Layer = oLayer" then the rule continues on and I get the message box that pops up about 15 times.

I hope I'm not being to much of a pain but could I ask for a slight change? 99 percent of my drawing views have Assemblies in them and the Sketches that I want to assign to a layer are in a part in said assembly. Also I would like to specify the name of the sketch (If oSketch.Name = "Skatch Name" and the name of the layer (oLayer.Name = "Layer Name") as the sketches are not named the same as the layers.....is this possible?

Thanks again....you don't realize how much easier this will make my job. 🙂

They_Call_Me_Jake · ‎07-15-2016

Can anyone explain why I would be getting this error when I use the code that @Anonymous posted. I have tried it on a few different parts and I get the same thing so I'm not sure what is wrong. Any help would be very much appreciated.

They_Call_Me_Jake · ‎07-28-2016

I talked with someone that said for what I'm trying to do the code that @Anonymous posted would not work as it is for drawing sketches only and I am trying to change the layer of a sketch imported from a part. They told me to look at the ChangeLayer method however I get nothing we I search for this method. Does anyone have any insight on this and willing to help me out. Many thanks.....

They_Call_Me_Jake · ‎08-15-2016

Just a bump to see if there is anyone that could help me with this problem.

Anonymous · ‎05-02-2017

Maybe this helps, if still needed...

Dim oDoc As DrawingDocument
    oDoc = ThisApplication.ActiveDocument

Dim oActiveSheet As Sheet
    oActiveSheet = oDoc.ActiveSheet

Dim oDrawingView As DrawingView
    oDrawingView = oActiveSheet.DrawingViews(1) 'View of Sheet
    
Dim oRefDoc As AssemblyDocument
    oRefDoc = oDrawingView.ReferencedDocumentDescriptor.ReferencedDocument
    
Dim oAssDef As AssemblyComponentDefinition
    oAssDef = oRefDoc.ComponentDefinition
    
Dim oOcc As ComponentOccurrence
    oOcc = oAssDef.Occurrences(2) 'Assembly in sheet
    
Dim oPart As PartDocument
    oPart = oOcc.Definition.Document

Dim oDef As PartComponentDefinition
    oDef = oPart.ComponentDefinition

Dim oSketch As PlanarSketch
    For Each oSketch In oDef.Sketches
        Dim oSketchProxy As PlanarSketchProxy
            If oSketch.Name = "SK Back MTG Holes With Cutouts" Then
                oOcc.CreateGeometryProxy(oSketch, oSketchProxy)
                oDrawingView.SetVisibility(oSketchProxy, True)
######### Set Lines As DrawingCurves And Set Layer #############

         Dim oNewLayer As Layer
         oNewLayer = oDoc.StylesManager.Layers.Item("MyLayer Change Me")

          ' Get the TransientsObjects object to use later.
         Dim transObjs As TransientObjects
          transObjs = ThisApplication.TransientObjects

         Dim drawcurves As DrawingCurvesEnumerator
         drawcurves = oDrawingView.DrawingCurves(oSketchProxy)
         If Err.Number = 0 Then
            On Error GoTo 0
            ' Create an empty collection.
            Dim objColl As ObjectCollection
            objColl = transObjs.CreateObjectCollection()

            ' 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
                  objColl.Add segment
               Next
            Next

            ' Change the layer of all of the segments.
            oDrawingView.Parent.ChangeLayer(objColl, oNewLayer)

         End If
         
##################         
         


            End If
    Next

If want it for more than a special view or part, I would recoment to change it to an "for each" code.

Anonymous · ‎06-28-2017

Hi Pete,

Your code works really well and is what I am after (altering a sketch in a drawing document).

I was wondering if you where able to tweak it a little...?

Firstly I should give you a little bit more info about my drawing...

My .idw drawing has multiple sheets

On each sheet, within the first view, I have a sketch called "Workpiece size" which contains geometry on a layer called "Workpiece size"

tweaks...

1) I want to loop your code through all sheets within the drawing

2) I want to move all geometry within the sketch "Workpiece size" to a new layer

3) I want the new layer name to be set per sheet based on a Prompted Entry within each sheet.

For example...

On sheet 1 the Prompted Entry '{Item.Thickness}' = 18. I want to move the geometry within the sketch "Workpiece size" to a new layer called 'XLYP1H18'

On sheet 2 the Prompted Entry '{Item.Thickness}' = 13. I want to move the geometry within the sketch "Workpiece size" to a new layer called 'XLYP1H13' ('XLYP1H' will always be the same. the numer at the end will come from the 'Prompted Entry')

I have found some code that extracts the 'Prompted Entry' thanks to cadlinecommunity below.

Thanks in advance to any help you can give to either or all of the 3 questions

Regards

Mike

On Error Resume Next

Dim oDoc As DrawingDocument

oDoc = ThisApplication.ActiveDocument

Dim oSheet As Sheet

Dim oPromptEntry

Dim oCurrentSheet

oCurrentSheet = oDoc.ActiveSheet.Name

i = 1

For Each oSheet In oDoc.Sheets

'i = i+1

ThisApplication.ActiveDocument.Sheets.Item(i).Activate

oTitleBlock=oSheet.TitleBlock

oTextBoxes=oTitleBlock.Definition.Sketch.TextBoxes

For Each oTextBox In oTitleBlock.Definition.Sketch.TextBoxes

Select oTextBox.Text

Case "{Item.Thickness}"

oPromptEntry = oTitleBlock.GetResultText(oTextBox)

iProperties.Value("Custom", "layer name")=oPromptEntry

End Select

Next

******Your original code*********

' Set a reference to the drawing document.
' This assumes a drawing document is active.
Dim oDrawDoc As DrawingDocument
oDrawDoc = ThisApplication.ActiveDocument

' Set a reference to the active sheet.
Dim oActiveSheet As Sheet
oActiveSheet = oDrawDoc.ActiveSheet

' Create a Drawing View Object
Dim oDrawingView As DrawingView
Dim oDrawingSketch As DrawingSketch
Dim oSketchEntity As SketchEntity
Dim oLayer As Layer

For Each oDrawingView In oActiveSheet.DrawingViews
   For Each oDrawingSketch In oDrawingView.Sketches
       For Each oLayer In oDrawDoc.StylesManager.Layers
           If oDrawingSketch.Name = oLayer.Name Then
               MessageBox.Show(oDrawingSketch.Name & " sketch should be on the " & oLayer.Name & " layer", "Title")
               oDrawingSketch.Edit
               For Each oSketchEntity In oDrawingSketch.SketchEntities
                   oSketchEntity.Layer = oLayer
               Next
               oDrawingSketch.ExitEdit

           End If

       Next
   Next
Next

iLogicVb.UpdateWhenDone = True

Assign Layer to part sketch in a drawing using iLogic

Assign Layer to part sketch in a drawing using iLogic

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