Suppressing features of part with model states from Assembly

[Marcus_Chong]

Is there a way to suppress or activate a feature (extrusion, revolve, etc) of part model state from assembly with iLogic?

[dalton98]

Here is an example of that:

Dim oAss As AssemblyDocument = ThisApplication.ActiveDocument
Dim oOcc As ComponentOccurrence = oAss.ComponentDefinition.Occurrences.Item(4)
Dim oCompDef As PartComponentDefinition = oOcc.Definition
Dim oPartDoc As PartDocument = oOcc.Definition.Document
Dim oMSDoc As PartDocument
oMSDoc = oPartDoc.ComponentDefinition.ModelStates.ActiveModelState.Document
oMSDoc.ComponentDefinition.Features.Item("Extrusion1").Suppressed = True

 Edit.... I tried this again and it didnt work for me. using the 'ActiveModelState' was giving me trouble. This seems to be working(for now)...........

Dim oAss As AssemblyDocument = ThisApplication.ActiveDocument
Dim oOcc As ComponentOccurrence = oAss.ComponentDefinition.Occurrences.Item(4)
Dim oPartDoc As PartDocument = oOcc.Definition.Document
Dim oMSDoc As PartDocument
oMSDoc = oPartDoc.ComponentDefinition.ModelStates.Item("9FT").Document

oOcc.Edit
oMSDoc.ComponentDefinition.Features.Item("Extrusion1").Suppressed = False
oOcc.ExitEdit(ExitTypeEnum.kExitToPrevious)

[Marcus_Chong]

Hi,

I tried with your rules, but I am not sure why it is giving me some error.. would you mind share with me your file to study as I am still very new in this area. I have put down some notes below as per my understanding.. correct me if I am wrong.

Dim oOcc As ComponentOccurrence = oAss.ComponentDefinition.Occurrences.Item(4) ---> this is to access to Item 4 counted from the model tree

Dim oPartDoc As PartDocument = oOcc.Definition.Document --> this is to access Item 4 part document as oOcc has been defined to Item 4

Dim oMSDoc As PartDocument
oMSDoc = oPartDoc.ComponentDefinition.ModelStates.Item("9FT").Document --> this is to access the model states called 9FT

oOcc.Edit --> to edit the occurrences

oMSDoc.ComponentDefinition.Features.Item("Extrusion1").Suppressed = False --> to edit the feature

oOcc.ExitEdit(ExitTypeEnum.kExitToPrevious) ---> is this to close the .ipt file?

I created part and assembly to test on the rule as below, but giving me problem.. I have attached the files which give me error.. 

Hope you can advise me on this

-------------------------------

Dim oAss As AssemblyDocument = ThisApplication.ActiveDocument
Dim oOcc As ComponentOccurrence = oAss.ComponentDefinition.Occurrences.Item(1)
Dim oPartDoc As PartDocument = oOcc.Definition.Document
Dim oMSDoc As PartDocument
oMSDoc = oPartDoc.ComponentDefinition.ModelStates.Item("Model State1").Document

oOcc.Edit
oMSDoc.ComponentDefinition.Features.Item("Extrusion2").Suppressed = True
oOcc.ExitEdit(ExitTypeEnum.kExitToPrevious)

[dalton98 · Accepted solution]

Yes all of those are correct. We're still on inventor 2022..... so i cant access those. You might have better luck actually opening the model state document and changing it there. You can set the document visibility to false.

Dim oAss As AssemblyDocument = ThisApplication.ActiveDocument
Dim oOcc As ComponentOccurrence = oAss.ComponentDefinition.Occurrences.Item(4)
Dim oPartDoc As PartDocument = oOcc.Definition.Document
If oPartDoc.ComponentDefinition.IsModelStateMember Or _
oPartDoc.ComponentDefinition.IsModelStateFactory Then
	Dim oModelState As String = oPartDoc.ModelStateName
'	Dim oPartDoc As PartDocument
	oPartDoc = ThisApplication.Documents.Open(oPartDoc.FullDocumentName, False)
	oPartDoc.ComponentDefinition.ModelStates.Item(oModelState).Activate
	oPartDoc.ComponentDefinition.Features.Item("Extrusion1").Suppressed = False
	oPartDoc.Save
	oPartDoc.Close
End If

oAss.Update 

[Marcus_Chong]

Thank you very much!