Change feature color in a component, from an assembly
Hi @a81383. In a separate rule, just for temporary testing purposes, but stored in the same place as your working rule, can you try just that one line of code, but in reverse so that it 'gets' (instead of 'sets') the name of the current color or appearance of that feature in that component, or does that also throw an error? Is the component a 'top level' component, or is it down within a sub-assembly? If you can read the value, but just can't set the value, then something is making it ReadOnly. It is usually the DVR's (DesignViewRepresentations) that record things like object visibility, colors, & appearances, so maybe make sure the current DVR is not 'Locked' or something odd like that. If that line of code truly effects the document being referenced by that component, then the ModelState that the component is set to may be playing a role in this not working also, not just the ModelState setting of the main assembly. For instance, when you have components in an assembly, and ModelStates are involved, they will be representing ModelState members versions of the Document they reference. ModelState members are usually ReadOnly when the model file is open directly on your screen, but when accessed through components in an assembly they act a bit differently. If you have two components in your assembly that both represent the same base file on disk, but they are set to two different ModelStates, and you are trying to make changes to both of them by code, I believe you will need to somehow update the next one before you will be able to make changes to it. I think it has something to do with the previous edit to a document reference in that file not being fully registered yet, before trying to make another change to a different document reference in the same file, but I'm not sure. I'm not sure if this is even a problem here, since you seem to just be working with one component.
Wesley Crihfield
(Not an Autodesk Employee)
Hi @WCrihfield ,
When setting oColor equal to the feature color. It returns the correct value (see image below).
I have it set to "Default" design rep and the component model state is set to master. But there is multiple other versions of the component not set to master.
Could this be a model state issue. Where its read-only due to the multiple different model states being used and it's unable to update all of them at once?
Dim EXTCOLOR As String = Parameter("exterior_color") Dim INTCOLOR As String = Parameter("interior_color") oColor = Feature.Color("GBG", "EXT FINE") MsgBox(oColor) Select Case EXTCOLOR Case "BLK" 'Black Feature.Color("GBG", "EXT FINE") = "Black" Case "CCBN" 'Cocoa Bean Feature.Color("GBG", "EXT FINE") = "Cocoa Bean" Case "DBRZ" 'Dark Bronze Feature.Color("GBG", "EXT FINE") = "Dark Bronze" Case "SND" 'Sandtone Feature.Color("GBG", "EXT FINE") = "Sandtone" Case "TT" 'Terratone Feature.Color("GBG", "EXT FINE") = "Terratone" Case "WHT" 'White Feature.Color("GBG", "EXT FINE") = "White" End Select Select Case INTCOLOR Case "BLK" 'Black Feature.Color("GBG", "INT FINE") = "Black" Case "DBRZ" 'Dark Bronze Feature.Color("GBG", "INT FINE") = "Dark Bronze" Case "SND" 'Sandtone Feature.Color("GBG", "INT FINE") = "Sandtone" Case "WHT" 'White Feature.Color("GBG", "INT FINE") = "White" End Select InventorVb.DocumentUpdate()
Yep. I just tried it myself on a test assembly. When I did this to a regular component that did not have any custom ModelStates, it worked just fine, but when trying to do this to a component, where there were multiple components for the same file, and were set to different ModelStates, it gave me the same error as you are getting. I'm sure there is a way around this odd scenario with some trial & error testing, but you may end up having to do this by API code instead of using that iLogic shortcut snippet. The API way requires a lot more code, is more complicated though.
Wesley Crihfield
(Not an Autodesk Employee)
If you only want to change their colors at the assembly level, and not in the actual source files, then what you have there looks pretty good. That way you only have to make sure the appearance is available in the main assembly, and using the 'proxy' versions of the geometry is getting the geometry that is in the context of the assembly, so I don't think the ModelState settings of the components should matter at all. Is that code you posted working OK for you then?
If you want the color changes to effect the source files, then you do not need to get the proxy of the geometry, and will need to make sure that the 'appearance' is available as a local copy within each source document, and will need to make sure you are working with the 'factory' version document of the component's referenced file.
Wesley Crihfield
(Not an Autodesk Employee)
It finds the solid just fine but is unable to make the change. I receive the following error for both the Proxy and direct method.
Dim oADoc As AssemblyDocument = ThisDoc.Document Dim oADef As AssemblyComponentDefinition = oADoc.ComponentDefinition MyBAR = oADef.Occurrences.ItemByName("GBG GRILLE").Definition Dim oAsset As Asset Dim oLib As AssetLibrary = ThisApplication.AssetLibraries("Andersen Custom 2022") 'oAsset = oLib.AppearanceAssets("Andersen C0001 White") Dim AssyAsset As Asset Try AssyAsset = oLib.AppearanceAssets.Item("Andersen C0001 White") Catch ' AssyAsset = ThisApplication.ActiveAppearanceLibrary.AppearanceAssets("Andersen C0001 White").CopyTo(oADoc) AssyAsset = oLib.AppearanceAssets("Andersen C0001 White").CopyTo(oADoc) End Try For Each occ As ComponentOccurrence In oADoc.ComponentDefinition.Occurrences If occ.Name = "GBG GRILLE" Then Dim GBGdef As PartComponentDefinition = occ.Definition.FactoryDocument.ComponentDefinition Dim SbProxy As SurfaceBodyProxy For Each Sb As SurfaceBody In GBGdef.SurfaceBodies If Sb.Name = "FINE" Then 'Create the Proxy Body. ' occ.CreateGeometryProxy(Sb, SbProxy) ' SbProxy.Appearance = AssyAsset Sb.Appearance = AssyAsset End If Next End If Next
This line provides the following error:
Sb.Appearance = AssyAsset
There will only be a value under FactoryDocument property when the document has more than one ModelState. Otherwise it will be Nothing, and likely throw an error.
oFacDoc = CompDef.Document 'from component, then check
If CompDef.IsModelStateMember Then
oFacDoc = CompDef.FactoryDocument
Else 'keep original document reference.
End If
'''but only when you want to effect the referenced file
Wesley Crihfield
(Not an Autodesk Employee)
