topic Re: Colour assignment in multi body part does not translate when that body is sent out as a separate part in Inventor Forum

Colour assignment in multi body part does not translate when that body is sent out as a separate part

AnthonyHarris90842 — Sat, 18 Feb 2023 13:36:57 GMT

I have a multi body part and I assign different colours to the the various bodies.
Then I use the make part command and click link face colour to the bodies.

When I open the new parts that are derived from the the multi body part the face colour is right but when I section that part it takes on the colour of the template that was used.

Then I have to individually go and assign that part with the face colour and this takes so much time when you have lots of bodies and many projects

Please fix this so that what ever colour you assign to the body or face it comes thru exactly like in the multibody part and we don't have to repeat the process.

Re: Colour assignment in multi body part does not translate when that body is sent out as a separate part

kacper.suchomski — Sat, 18 Feb 2023 13:51:24 GMT

I think you can submit this idea on Idea Station.

Re: Colour assignment in multi body part does not translate when that body is sent out as a separate part

AnthonyHarris90842 — Sat, 18 Feb 2023 14:14:34 GMT

Thank you KACPER

Re: Colour assignment in multi body part does not translate when that body is sent out as a separate part

johnsonshiue — Tue, 21 Feb 2023 22:58:48 GMT

Hi Anthony,

I think you are talking about the ability to link material style. The graphical section honors the material appearance style. The active material style in the part template you selected to do Make Components (Make Parts) dictates the coloring of the section. I guess you could build templates with different active material style. When you do Make Components, select the desirable template file accordingly.

Many thanks!

Re: Colour assignment in multi body part does not translate when that body is sent out as a separate part

AnthonyHarris90842 — Wed, 22 Feb 2023 00:07:05 GMT

How can you even think that is a solution when I have a few hundred parts that I need to send out.

Should I have a few hundred templates?

Re: Colour assignment in multi body part does not translate when that body is sent out as a separate part

johnsonshiue — Wed, 22 Feb 2023 01:47:37 GMT

Hi Anthony,

Unfortunately, that is the solution I can think of without using iLogic. Another way is to create an elaborated iLogic rule to make such changes automatically.

Many thanks!

Re: Colour assignment in multi body part does not translate when that body is sent out as a separate part

AnthonyHarris90842 — Wed, 22 Feb 2023 06:47:14 GMT

Hi Johnson

I cant see why this is so difficult.
I assign a colour to a body and then when I make part the part takes on that colour so that when you section it the same colour shows inside and not the template colour

Re: Colour assignment in multi body part does not translate when that body is sent out as a separate part

johnsonshiue — Wed, 22 Feb 2023 21:54:20 GMT

Hi Anthony,

The behavior you are seeing is due to the fact that the section color depends on the material appearance. But, when you use Make Components to push the bodies as individual parts, the the material style associated with the source part isn't "derived" or carried over to the pushed parts.

This behavior shows two major deficiencies. 1) Inventor does not support material style per body. You cannot assign material style to a body as other CAD tools do. 2) Except in a sheet metal part, the material style in the source part isn't derived or linked to the derived part.

Another deficiency is that the sectioned face color is based on material appearance, not the body appearance. There is no option to allow that.

I fully agree with you that the behaviors are not desirable. However, I personally cannot offer any better solution than merely explaining the behaviors. I am sorry.

Many thanks!

Re: Colour assignment in multi body part does not translate when that body is sent out as a separate part

AnthonyHarris90842 — Wed, 22 Feb 2023 23:23:50 GMT

Hi Johnson
Thank you for trying.
Is it possible for someone to write a ilogic routine that will open all my parts, check what the colour was that was assigned and on the surface and them change the derived part to that colour much as I would do it manually.

Re: Colour assignment in multi body part does not translate when that body is sent out as a separate part

johnsonshiue — Thu, 23 Feb 2023 00:30:37 GMT

Hi Anthony,

I believe it is doable. Essentially, the iLogic rule will be like a robot automating the otherwise manual process.

Many thanks!

Re: Colour assignment in multi body part does not translate when that body is sent out as a separate part

cadman777 — Thu, 23 Feb 2023 13:43:56 GMT

I'm using Inventor 2010 and now beginning to remember why I never use MBPs.

It's b/c there are too many caveats for my workflow.

This is one of them.

Re: Colour assignment in multi body part does not translate when that body is sent out as a separate part

A.Acheson — Thu, 23 Feb 2023 05:49:15 GMT

Here is a post that should get you 50% of the way there. It will access the parent part from the child part and loops through the solid bodies. You then need to find the solid body common between the two. I haven't explored this yet but if you can pin point the correct solid body through a common name etc you can drill back to the appearance on the surface. Hope that helps a bit. It would be handy if a button was set up for this very purpose within the .ale component dilaogue. Push appearance or material to all derived parts.

Re: Colour assignment in multi body part does not translate when that body is sent out as a separate part

BDCollett — Thu, 23 Feb 2023 06:59:23 GMT

I have always just used the material in combination with the BOM editor to mass select the parts I need and apply the specific material/appearance that way. If you have hundreds of different colors and materials for whatever reason that's still going to be annoying.

Re: Colour assignment in multi body part does not translate when that body is sent out as a separate part

A.Acheson — Sat, 25 Feb 2023 23:53:16 GMT

Here is a rule that will update material of derived component from the appearance of the Parent solid body. I would test this on a small non production assembly to ensure it is working as it should be.

Dim Doc As Document = ThisDoc.Document If Doc.DocumentType = kPartDocumentObject Then MessageBox.Show("This rule can only be run in an assembly file - exiting rule", "iLogic") Return End If For Each RefDoc As Document In Doc.AllReferencedDocuments 'Look at ony part files. If RefDoc.DocumentType = DocumentTypeEnum.kPartDocumentObject Then Dim RefPartDoc As PartDocument = RefDoc 'Logger.Info(RefPartDoc.DisplayName) Dim DPComps As DerivedPartComponents = RefPartDoc.ComponentDefinition.ReferenceComponents.DerivedPartComponents For Each DPComp As DerivedPartComponent In DPComps 'Logger.Info(DPComp.ReferencedDocumentDescriptor.FullDocumentName) For Each Sb As ReferenceFeature In DPComp.SolidBodies ' Logger.Info(Sb.Name) ' Logger.Info(Sb.Appearance.Name) '[Bring the correct material to the part. Appearance names must match material Names, if not use option filter! Dim MaterialName As String = Sb.Appearance.DisplayName 'Option Filter: If Appearance names don't match material Names. 'Dim MaterialName As String = "Gold" 'If Sb.Appearance.DisplayName = MaterialName Then ' 'Create Reference To another material Library ' Dim AssetLib As AssetLibrary = ThisApplication.AssetLibraries.Item("Inventor Material Library") ' 'Set The Active Library ' ThisApplication.ActiveMaterialLibrary = AssetLib 'Create Reference To the active material Library. Dim AssetLib As AssetLibrary = ThisApplication.ActiveMaterialLibrary Dim LocalMaterial As MaterialAsset Try Try LocalMaterial = RefPartDoc.MaterialAssets.Item(MaterialName) Catch Ex As Exception Dim LibMaterial As MaterialAsset = AssetLib.MaterialAssets.Item(MaterialName) LibMaterial.CopyTo(RefPartDoc) LocalMaterial = RefPartDoc.MaterialAssets.Item(MaterialName) End Try RefPartDoc.ActiveMaterial = LocalMaterial Catch Ex As Exception Logger.Info("No Material available") End Try RefPartDoc.Update '] 'End If Next Next End If Next Doc.Update

In addition here is an optional rule to derive the parent part and make an assembly. This automates the make components command.

Sub Main() 'Set a reference to the active partdocument Dim ParentDoc As PartDocument = ThisDoc.Document 'Dim DPTemplate As String = "C:\Templates\SHEET METAL.ipt" Dim DPTemplate As String = Nothing 'Set the folder for the new files Dim Folder As String = ThisDoc.Path 'Create an object collection to store the parts to put in assembly Dim PartCol As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection For Each Sb As SurfaceBody In ParentDoc.ComponentDefinition.SurfaceBodies 'Create a new part to derive the solid body in. Dim PartDoc As PartDocument = ThisApplication.Documents.Add(kPartDocumentObject,DPTemplate, True) 'Set a reference to the derivedpartcomponents. Dim Dpcs As DerivedPartComponents = PartDoc.ComponentDefinition.ReferenceComponents.DerivedPartComponents 'Create the scale definition. Dim Dpd As DerivedPartUniformScaleDef = Dpcs.CreateUniformScaleDef(ParentDoc.FullFileName) 'Set the Derived Part settings. DerivedPartSettings(Dpd, Sb) Dpcs.Add(Dpd) PartCol.Add(PartDoc) 'Set the part title to the solidbodies name. PartDoc.PropertySets.Item("Inventor Summary Information").Item("Title").Value = Sb.Name ' Save the part ThisApplication.SilentOperation = True Try PartDoc.SaveAs(Folder & "\" & Sb.Name & ".ipt", False) Catch End Try ThisApplication.SilentOperation = False Next Sb 'Use a template for a new assembly. 'Dim AssyDoc As AssemblyDocument = ThisApplication.Documents.Add(kAssemblyDocumentObject,, True) 'Find opened assembly in which the sketch part is. Dim AssyDoc As AssemblyDocument = ThisApplication.Documents.Open(Folder & "\House" & ".iam") 'Place in assembly. For Each PartDoc In PartCol ' create an empty matrix Dim mx As Matrix = ThisApplication.TransientGeometry.CreateMatrix() Dim Occ As ComponentOccurrence = AssyDoc.ComponentDefinition.Occurrences.AddByComponentDefinition(PartDoc.ComponentDefinition, mx) PartDoc.Close(True) Next End Sub Sub DerivedPartSettings(ByRef Dpd As DerivedPartUniformScaleDef, Sb As SurfaceBody) 'Set the derive style. Dpd.ExcludeAll 'Include solid, exclude the others For Each Dpe As DerivedPartEntity In Dpd.Solids If Dpe.ReferencedEntity.Name = Sb.Name Then Dpe.IncludeEntity = True End If Next End Sub

Re: Colour assignment in multi body part does not translate when that body is sent out as a separate part

AnthonyHarris90842 — Sun, 26 Feb 2023 06:49:37 GMT

Hi Alan

I have never used rules before so don't know where to start.
Any chance you do a little video to show me how to use your rule

Re: Colour assignment in multi body part does not translate when that body is sent out as a separate part

A.Acheson — Sun, 26 Feb 2023 07:56:46 GMT

Here is a nice video to show you where to set the external rules folder and how to create a rule then simply copy and paste and run. The ilogic tab is just located off the model browser tab simply press the + button. The ilogic logger is also there which will allow you to see usefull information while the rule runs.

Re: Colour assignment in multi body part does not translate when that body is sent out as a separate part

AnthonyHarris90842 — Sun, 26 Feb 2023 07:55:13 GMT

Thank you so much Alan
Highly appreciated