how to change appearance of part or assambly with Ilogic

[Darkforce_the_ilogic_guy]

How do I change appearance  with use of Ilogic?   I need a code for both IPT file and Iam file

[Sergio.D.Suárez]

Hi, here I send you two codes, the first changes the appearance of each part from assembly, at the level of the part (as if you open the part and change the color)

Dim oAsset As Asset
Dim oAsset_Array As New ArrayList
For Each oAsset_Array_X In ThisApplication.ActiveAppearanceLibrary.AppearanceAssets
oAsset_Array.Add(oAsset_Array_X.DisplayName)
oAsset_Array.Sort()
Next
'present the user with the list to choose from
100:
oAsset_Array_Selected = InputListBox("CHOOSE TEXTURE FROM ABOVE LIST", oAsset_Array, oAsset_Array.Item(0), "TEXTURE SELECTION", "LIST OF TEXTURES")
If oAsset_Array_Selected = "" Then GoTo 100 :

Dim comps As ObjectCollection
Dim comp As Object
comps = ThisApplication.TransientObjects.CreateObjectCollection

While True
	comp = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAssemblyLeafOccurrenceFilter, "Select a component")
		
	' If nothing gets selected then we're done	
	If IsNothing(comp) Then Exit While
	comps.Add(comp) 
End While

' If there are selected components we can do something
For Each comp In comps
	Dim oDef As PartDocument
    oDef = comp.Definition.Document
    Dim oRenderStyle As RenderStyle
    oRenderStyle = oDef.RenderStyles.Item(oAsset_Array_Selected)
    oDef.ActiveRenderStyle = oRenderStyle
    iLogicVb.UpdateWhenDone = True		
Next

the second changes the appearance of the part or assembly at the level of assembly (the part maintains the color of origin)

Dim oAsset As Asset
Dim oAsset_Array As New ArrayList
For Each oAsset_Array_X In ThisApplication.ActiveAppearanceLibrary.AppearanceAssets
oAsset_Array.Add(oAsset_Array_X.DisplayName)
oAsset_Array.Sort()
Next
'present the user with the list to choose from
100:
oAsset_Array_Selected = InputListBox("CHOOSE TEXTURE FROM ABOVE LIST", oAsset_Array, oAsset_Array.Item(0), "TEXTURE SELECTION", "LIST OF TEXTURES")
If oAsset_Array_Selected = "" Then GoTo 100 :

Dim comps As ObjectCollection
Dim comp As Object
comps = ThisApplication.TransientObjects.CreateObjectCollection

While True
comp = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAssemblyOccurrenceFilter, "Select a component")  'kAssemblyOccurrenceFilter. kAssemblyLeafOccurrenceFilter

' If nothing gets selected then we're done 
If IsNothing(comp) Then Exit While
comps.Add(comp) 
End While

' If there are selected components we can do something
For Each comp In comps

	Component.Color(comp.name)=oAsset_Array_Selected
	iLogicVb.UpdateWhenDone = True 
Next

[Darkforce_the_ilogic_guy]

Thanks for the code... it is not what I needed 

I need a code that I can add to I if stement that I already have ... 

when I force the user to select betwine Colour 1 and Colour 2 and Galz

in the if statment 

If you selece Colour 1

Change appearance of this part or assambly to "Ral 7035"

If you selece Colour 2

Change appearance of this part or assambly to "Ral 7037"

If you selece Galz.

Change appearance of this part or assambly to "Galvanized"

I only want to change the top level ... not the assambly or part in the assambly

I use this in a before save ilogic code

[Sergio.D.Suárez]

This is a code that just probes and works for me, it is by way of example. Need to add select an occurrence and then create a list of the two colors

Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = ThisApplication.ActiveDocument.ComponentDefinition
Dim oPart As ComponentOccurrence

'Pick part occurrence
oPart = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAssemblyLeafOccurrenceFilter, "Seleccione Pieza")
	If oPart Is Nothing Then
		Exit Sub
	Else




		Dim oValueList As New ArrayList
			oValueList.Add("Colour 1")
			oValueList.Add("Colour 2")

		Dim oValue As String
			'get user input
			oValue = InputListBox("Select colour", oValueList, "Colour 1", "Customizar Plantilla", "Selecciones Disponibles")




		If oValue = "Colour 1" Then
			Component.Color(oPart.Name)="Magenta"
			iLogicVb.UpdateWhenDone = True 
		End If

		If oValue = "Colour 2" Then
			Component.Color(oPart.Name)="Negro"
			iLogicVb.UpdateWhenDone = True 
		End If
	
	
	
	
end if

 ,you do not need to copy all this code, you should copy a line like this inside the "If then end if"

Component.Color("Occurrence")="chosen colour"

iLogicVb.UpdateWhenDone = True

You must make sure that the chosen color belongs to the current appearance library, otherwise you must specify it

[Darkforce_the_ilogic_guy]

Can´t get it to work .. how can it be so hard just to change color of a part

and for the same when it goes for assembly.

both at top level...

no seletect ingen ,... no list ...

just change change the appearance on the part  or Assambl that you are saving right now .. it may need 2 illogic code .. one for part and one for assembly ... it is just 2 click with the mouse .. so it most be simple but I do not know the code for it

[chandra.shekar.g]

@Darkforce_the_ilogic_guy ,

Try below iLogic code for assembly document.

        Dim oAssyDoc As AssemblyDocument
	oAssyDoc = ThisApplication.ActiveDocument

	'define the appearance library
	Dim oLib As AssetLibrary
	oLib = ThisApplication.AssetLibraries("Autodesk Appearance Library")

	'make sure colors are in assembly doc
	Dim libAsset As Asset
	libAsset = oLib.AppearanceAssets.Item("Steel") 

	Dim localAsset As Asset 
	Try  
		localAsset = oAssyDoc.Assets.Item("Steel") 
	Catch 
		localAsset = libAsset.CopyTo(oAssyDoc)
	End Try 
	oAssyDoc.ActiveAppearance = localAsset 

For Part Document

Dim oPartDoc As PartDocument 
	oPartDoc = ThisApplication.ActiveDocument 

	'define the appearance library
	Dim oLib As AssetLibrary
	oLib = ThisApplication.AssetLibraries("Autodesk Appearance Library")

	'make sure colors are in assembly doc
	Dim libAsset As Asset
	libAsset = oLib.AppearanceAssets.Item("Steel") 

	Dim localAsset As Asset 
	Try  
		localAsset = oPartDoc.Assets.Item("Steel") 
	Catch 
		localAsset = libAsset.CopyTo(oPartDoc)
	End Try 
	
	oPartDoc.ActiveAppearance = localAsset

Thanks and regards,

[Darkforce_the_ilogic_guy]

I have only test the part function so far ... it is working as i want it to... have not have time to test the assambly jet 

[chandra.shekar.g]

@Darkforce_the_ilogic_guy ,

if it is working for PartDocument, it should work for Assembly as well.

Please let me know if it is not working.

Thanks and regards,

[Darkforce_the_ilogic_guy]

I can´t get it to work.. it seems that you have to change colour on en asammebly componemt(hope it is the right word)  not on some the hole assembly as you can with the part.. think it might have to you a while loop to go throungt all of them one by one... hope it can be not on only the toplevel.. not all the way down in the sub assembly.

You know how to do that ?

[chandra.shekar.g]

@Darkforce_the_ilogic_guy ,

It seems that appearance of assembly is not allowed to change through UI. Can you please confirm the same?

Thanks and regards,

[RoyWickrama_RWEI]

Hi.

I also found it is not working. I moved steel from library to favorites. then it worked. Only for the part, anyway.

[ice_sid]

Thank you so much for your work.

[_KarlH]

@Sergio.D.Suárez- I can't thank you enough. I've searched far and wide to find a method to update a parts appearance from within an assembly based iLogic rule - and you've given the perfect example of how to do so.

ActiveRenderStyle 

ActiveRenderStyle! Not Color, or PartColor, or Appearance, or iProperty.Color.Appearance. ... no, it was "ActiveRenderStyle" all along!!! No wonder I'm losing my hair...

Thank you kindly again! :hot_beverage:

[Darkforce_the_ilogic_guy · Accepted solution]

This is a very old tread .. but I have develope  something like I wanted  today . I will try add some of the code seens I have add a lot more to the code today .. hope you can use it ... If need more of help to use it for your project .. write here again and I will try to make a code that work for you

Sub AddsurfaceAssembly()
	
	Dim NameList As New ArrayList()
	
NameList.Add("Raw")
'NameList.Add("------------------------------------------------------------------------------")
NameList.Add("Colour 1		Basic colour for chassis, etc.")'Colour Ral 7035 OR RAL 9010
NameList.Add("Colour 2 		Basic colour for moving parts.")'Colour Ral 7037 OR RAL 5003
NameList.Add("RAL 1028	Melon yellow")
NameList.Add("RAL 5003 	Sapphire blue")
NameList.Add("RAL 9005	Jet black")
NameList.Add("RAL 9010 	Pure white")
'NameList.Add("------------------------------------------------------------------------------")
NameList.Add("Electro galvanized	Preferable/Cheapest")'Eletro Galvanizes
NameList.Add("Hot dip galvanized 	Outdoor Use")'Hot Dip galvanized
'NameList.Add("------------------------------------------------------------------------------")
NameList.Add("Hardened	Set specifications on Drawing")
NameList.Add("Glassblasted")
NameList.Add("Sandblasted")
'NameList.Add("Shot blasted")
'NameList.Add("Pickled")


'NameList.Add("------------------------------------------------------------------------------")
'NameList.Add("Do not select")




Dim msg As String
	msg = ("Surface needed - Select Surface " & vbLf & "Part Numner: "+iProperties.Value("Project", "Part Number")& vbLf & "Description: "+iProperties.Value("Project", "Description")& vbLf & "Title: "+ iProperties.Value("Summary", "Title")& vbLf).ToString






	d0 = InputListBox(msg, NameList, d0, Title := "Info - Surface needed", ListName := "Surface")
	
	' iProperties.Value("Custom", "Surface") = d0
	'Tilføj farve 
	 If d0 = "Do not select" Then
	
	  
	 Else
	

	TextToSurface(d0)
	
	 'iProperties.Value("Custom", "Surface") = d0
	 End If 
	
	'find Document type
	Dim doc = ThisDoc.Document
	Dim sDocumentSubType As String = doc.SubType
	If sDocumentSubType <> "{4D29B490-49B2-11D0-93C3-7E0706000000}"  And  sDocumentSubType <>"{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then '  = "Part"
	'------------------
	debug("Colour Assambly")
	Try
	Dim oAsmCompDef 'As AssemblyComponentDefinition
	debug("Loading Variable Finish 0,5")
	
oAsmCompDef = ThisApplication.ActiveDocument.ComponentDefinition 

	
	



debug("Loading Variable Finish 1")
'define view rep collection
Dim oViewReps As DesignViewRepresentations
oViewReps = oAsmCompDef.RepresentationsManager.DesignViewRepresentations

debug("Loading Variable Finish 2")
'define view rep 
Dim oViewRep As DesignViewRepresentation
debug("Loading Variable Finish 3")

Dim NumberOfView = oViewReps.Count
' get Manager of Representations
debug("Loading Variable Finish 4")
 Dim dViewRepMgr As RepresentationsManager
 dViewRepMgr = oAsmCompDef.RepresentationsManager
 debug("Loading Variable Finish 5")
 'Get active Representation View
 Dim dViewRep As DesignViewRepresentation
 dViewRep = dViewRepMgr.ActiveDesignViewRepresentation
 debug("Loading Variable Finish 6")
 debug("Loading Variable Finish")
 Try
	

For i = 1 To NumberOfView 
	If iProperties.Value("Custom", "Surface") = "Raw" Or iProperties.Value("Custom", "Surface") = "Galv." Or iProperties.Value("Custom", "Surface") = "Colour 1" Or iProperties.Value("Custom", "Surface") = "Colour 2" Or iProperties.Value("Custom", "Surface") = "RAL 5003" Or iProperties.Value("Custom", "Surface") = "RAL 9010" Or iProperties.Value("Custom", "Surface") = "RAL 1028" Or iProperties.Value("Custom", "Surface") = "RAL 9005"  Or iProperties.Value("Custom", "Surface") = "EG-Galv" Or iProperties.Value("Custom", "Surface") = "HDG-Galv"  Then
debug("chance view")
oViewReps.Item(i).Activate
End if
iLogicVb.RunExternalRule("SurfaceColour")
iLogicVb.UpdateWhenDone = True

Next



If iProperties.Value("Custom", "Surface") = "RAL 9010"


End If 

If iProperties.Value("Custom", "Surface") = "RAL 5003"


End If 

Catch
	debug("Run Error Code 7")
	dViewRepMgr.DesignViewRepresentations.Item(1).Activate
	 
	
	End Try
	Try
dViewRep.Activate
'Home View
ThisApplication.CommandManager.ControlDefinitions.Item _
("AppViewCubeHomeCmd").Execute

'Home View
Catch
	debug("Run Error Code 8")
	iLogicVb.RunExternalRule("SurfaceColour")
iLogicVb.UpdateWhenDone = True
End Try

Catch
	debug("Run Error Code 9")
	debug("Add Colour to Assambly")
	
	
	iLogicVb.RunExternalRule("SurfaceColour") 
End Try
	
	'---------------
	'iLogicVb.RunExternalRule("SurfaceColour") 
	
	
	End If 
	
	
If sDocumentSubType = "{4D29B490-49B2-11D0-93C3-7E0706000000}" Or sDocumentSubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then '  = "Part"
	debug("Colour Part")
	

	If d0 = "Colour 1		Basic colour for chassis, etc." Then
		debug("Colour 1 ")
		'iProperties.Value("Custom", "Surface") = d0
ChangeView
End If 

If d0 = "Colour 2 		Basic colour for moving parts." Then
	'iProperties.Value("Custom", "Surface") = d0
	ChangeView
	End If
 	

If d0 = "Galv." Or d0 = "Electro galvanized	Preferable/Cheapest" Or d0 = "Hot dip galvanized 	Outdoor Use" Then
	'iProperties.Value("Custom", "Surface") = d0
ChangeView
End If



If d0 = "RAL 1028	Melon yellow" Or d0 = "RAL 9005	Jet black" Or d0 = "RAL 9010 	Pure white"  Or d0 = "RAL 5003 	Sapphire blue" Then
	'iProperties.Value("Custom", "Surface") = d0
ChangeView
End If

If d0 = "RAL 5003 Sapphire blue" Then
	'iProperties.Value("Custom", "Surface") = d0
ChangeView
End If



'gør intet
	


End If
End Sub
Sub Colour1
	
	debug("Loading Colour 1")
Dim oPartDoc As PartDocument 
	Try
	oPartDoc = ThisApplication.ActiveDocument 
	Catch
	oPartDoc =	ThisDoc.Document
	End Try

	'define the appearance library
	Dim oLib As AssetLibrary
	oLib = ThisApplication.AssetLibraries("KallesoeMaterialLibrary")

	'make sure colors are in assembly doc
	Dim libAsset As Asset
	

	
	'libAsset = oLib.AppearanceAssets.Item("RAL 9010 Pure white") 
	libAsset = oLib.AppearanceAssets.Item("RAL 7035 Light grey") 
	Dim localAsset As Asset 
	
	Try  
		
		localAsset = oPartDoc.Assets.Item("RAL 7035 Light grey") 
		
	Catch 
		debug("Run Error Code 10")
		localAsset = libAsset.CopyTo(oPartDoc)
	End Try 
	
	oPartDoc.ActiveAppearance = localAsset
	Debug("Loading Colour 1 END")
	End Sub

Surfacecolour(ilogic code)

Farvelægge samlinger
Sub Main()		
	Debug("Starting Surfacecolour")
If iProperties.Value("Custom", "Surface")="Colour 1" Then


	
Dim oAsmDoc As AssemblyDocument
oAsmDoc = ThisDoc.Document
Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = oAsmDoc.ComponentDefinition

Dim oOccurrence As ComponentOccurrence
For Each oOccurrence In oAsmCompDef.Occurrences

	Component.Color(oOccurrence.name)="RAL 7035 Light grey"
	iLogicVb.UpdateWhenDone = True 

Next

End If

If iProperties.Value("Custom", "Surface")="Colour 2" Then


	
Dim oAsmDoc As AssemblyDocument
oAsmDoc = ThisDoc.Document
Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = oAsmDoc.ComponentDefinition

Dim oOccurrence As ComponentOccurrence
For Each oOccurrence In oAsmCompDef.Occurrences

	Component.Color(oOccurrence.name)="RAL 7037 Dusty grey"
	iLogicVb.UpdateWhenDone = True 

Next

End If

If iProperties.Value("Custom", "Surface")="HDG-Galv"  Then


	
Dim oAsmDoc As AssemblyDocument
oAsmDoc = ThisDoc.Document
Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = oAsmDoc.ComponentDefinition

Dim oOccurrence As ComponentOccurrence
For Each oOccurrence In oAsmCompDef.Occurrences

	Component.Color(oOccurrence.name)="Galvanized (texture)"
	iLogicVb.UpdateWhenDone = True 

Next

End If

If iProperties.Value("Custom", "Surface")="Galv." Or iProperties.Value("Custom", "Surface")="EG-Galv"   Then


	
Dim oAsmDoc As AssemblyDocument
oAsmDoc = ThisDoc.Document
Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = oAsmDoc.ComponentDefinition

Dim oOccurrence As ComponentOccurrence
For Each oOccurrence In oAsmCompDef.Occurrences

	Component.Color(oOccurrence.name)="Galvanized"
	iLogicVb.UpdateWhenDone = True 

Next

End If

If iProperties.Value("Custom", "Surface")="RAL 1028" Then


	
Dim oAsmDoc As AssemblyDocument
oAsmDoc = ThisDoc.Document
Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = oAsmDoc.ComponentDefinition

Dim oOccurrence As ComponentOccurrence
For Each oOccurrence In oAsmCompDef.Occurrences

	Component.Color(oOccurrence.name)="RAL 1028 Melon yellow"
	iLogicVb.UpdateWhenDone = True 

Next

End If

If iProperties.Value("Custom", "Surface")="RAL 9005" Then
debug("Colour 1")

	
Dim oAsmDoc As AssemblyDocument
oAsmDoc = ThisDoc.Document
Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = oAsmDoc.ComponentDefinition

Dim oOccurrence As ComponentOccurrence
For Each oOccurrence In oAsmCompDef.Occurrences

	Component.Color(oOccurrence.name)="RAL 9005 Jet black"
	iLogicVb.UpdateWhenDone = True 

Next

End If

If iProperties.Value("Custom", "Surface")="RAL 9010" Then


	
Dim oAsmDoc As AssemblyDocument
oAsmDoc = ThisDoc.Document
Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = oAsmDoc.ComponentDefinition

Dim oOccurrence As ComponentOccurrence
For Each oOccurrence In oAsmCompDef.Occurrences

	Component.Color(oOccurrence.name)="RAL 9010 Pure white"
	iLogicVb.UpdateWhenDone = True 

Next

End If

If iProperties.Value("Custom", "Surface")="RAL 5003" Then


	
Dim oAsmDoc As AssemblyDocument
oAsmDoc = ThisDoc.Document
Dim oAsmCompDef As AssemblyComponentDefinition
oAsmCompDef = oAsmDoc.ComponentDefinition

Dim oOccurrence As ComponentOccurrence
For Each oOccurrence In oAsmCompDef.Occurrences

	Component.Color(oOccurrence.name)="RAL 5003 Sapphire blue"
	iLogicVb.UpdateWhenDone = True 

Next

End If







End Sub




Public Sub debug(txt As String)
	Trace.WriteLine("NTI : Colour" & txt)
End Sub

[gordon.bowe]

Thank you everyone for the examples in this post.
I would like to do something slightly different than I have seen elsewhere, but I figure there is a good start in this thread, so I decided to post it here.

Occasionally we will append "REF" or "MOCK" or some other descriptors to the file name of a part.  The part number will not have this, only the file name.

I would like to have some code that runs prior to save via a trigger where if the file name ends in REF or MOCK (also Ref, ref, Mock, mock, maybe create a list of "triggers" and if the filename contains a trigger then set a bool to true?), it will prompt the user with a message ("it seems like you have a "REF" or "MOCK" part, would you like to override the color?") and if the user selects "Yes", then the color will be set to "Pink".

Catch:  This rule should work for parts, sheetmetal parts, assemblies, weldments, etc.

Thank you in advance.

[D.Motshagen]

Hi @chandra.shekar.g,

Do you also have a part of code for clearing the override on the appearance?

Clear Override cannot be chosen as name

thanks.

[Darkforce_the_ilogic_guy]

I have this code.. that will remove all Color(will clear override the color) . on all View in the file.. I have try to remove some code that are unit to where i use it .. so I hope i did it right so I did not break the code 😀

For assembly 

	Dim oAsmCompDef 'As AssemblyComponentDefinition

 
oAsmCompDef = ThisApplication.ActiveDocument.ComponentDefinition
 
 Dim oViewReps As DesignViewRepresentations
oViewReps = oAsmCompDef.RepresentationsManager.DesignViewRepresentations


'define view rep
Dim oViewRep As DesignViewRepresentation


Dim NumberOfView = oViewReps.Count
' get Manager of Representations

 Dim dViewRepMgr As RepresentationsManager
 dViewRepMgr = oAsmCompDef.RepresentationsManager

 'Get active Representation View
 Dim dViewRep As DesignViewRepresentation
 dViewRep = dViewRepMgr.ActiveDesignViewRepresentation

 
 

For i = 1 To NumberOfView


oViewReps.Item(i).Activate


'---------------------
Dim oAsmDoc As AssemblyDocument
oAsmDoc = ThisDoc.Document


Dim objColl As ObjectCollection 
objColl = ThisApplication.TransientObjects.CreateObjectCollection 

Dim oOccurrence As ComponentOccurrence
For Each oOccurrence In oAsmCompDef.Occurrences

	Call objColl.Add(oOccurrence)

 
 iLogicVb.UpdateWhenDone = True

Next
oAsmCompDef.ClearAppearanceOverrides(objColl)
'-------------------------
iLogicVb.UpdateWhenDone = True

Next

For Part

Sub Main

Dim doc = ThisDoc.Document
	Dim sDocumentSubType As String = doc.SubType
	doc.AppearanceSourceType = AppearanceSourceTypeEnum.kMaterialAppearance
	
	If sDocumentSubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Or sDocumentSubType = "{4D29B490-49B2-11D0-93C3-7E0706000000}" Then  	' = "Sheet Metal and Part"
	ChangeView	
		
	End If
	
	End Sub 
	
	Public Sub debug(txt As String)
	Trace.WriteLine("NTI : " & txt)
End Sub
		
	Sub ChangeView
	
	'''New Code Begun
	''' Here
	debug("Start Run Function Change View")
	Dim doc As PartDocument
 doc = ThisDoc.Document
 debug("Load This Document Variabel")
 ' get AssemblyComponentDefinition
 Dim partDef As PartComponentDefinition 
 partDef = doc.ComponentDefinition
 debug("Loaded Variabel 2")
 ' get Manager of Representations
 Dim dViewRepMgr As RepresentationsManager
  dViewRepMgr = partDef.RepresentationsManager
debug("Loaded Variabel 3")
Dim dViewRep As DesignViewRepresentation
 dViewRep = dViewRepMgr.ActiveDesignViewRepresentation
 debug("Loaded Variabel 4")
Dim oName As String 
oName = dViewRep.Name 
debug("Loaded Variabel 5")
' get the first Representation view
  dViewRep = dViewRepMgr.DesignViewRepresentations.Item(oName)		
	'New code Ende
'set a reference to the part component definintion.

'Dim oPartCompDef As PartComponentDefinition

'oPartCompDef = ThisDoc.Document.ComponentDefinition
debug("Loaded Variabel 6")
'define view rep collection
Dim oViewReps As DesignViewRepresentations
oViewReps = partDef.RepresentationsManager.DesignViewRepresentations'oPartCompDef.RepresentationsManager.DesignViewRepresentations
debug("Loaded Variabel 7")
Dim NumberOfView = oViewReps.Count
debug("Loading Variable Change view")
Try
For i = 1 To NumberOfView 
debug("Run For LOOP")	
oViewReps.Item(i).Activate
debug("Run For LOOP2")	




ClearOverride


	

iLogicVb.UpdateWhenDone = True
Next


	
	

Catch
debug("Run Error Code 13")
End Try
Try
dViewRep.Activate

Catch
	debug("Run Error Code 14")
	dViewRepMgr.DesignViewRepresentations.Item(1).Activate
End Try
End Sub 


Sub ClearOverride
	Dim doc = ThisDoc.Document
	doc.AppearanceSourceType = AppearanceSourceTypeEnum.kMaterialAppearance
	End Sub
	

[D.Motshagen]

Hi @Darkforce_the_ilogic_guy,

Thanks for your reply.

I found the solution to my problem:

'clear override material appearence
'Found at: https://forums.autodesk.com/t5/inventor-ilogic-and-vb-net-forum/clear-all-appearance-overrides-in-part-with-ilogic/m-p/8226065/highlight/true#M88140

Dim oDoc As PartDocument 
 	oDoc = ThisApplication.ActiveDocument 
oDoc.AppearanceSourceType = AppearanceSourceTypeEnum.kMaterialAppearance

This will do the trick.