topic iLogic Design Copy failure in Inventor Forum

iLogic Design Copy failure

AnufrievSergey — Wed, 03 Mar 2021 11:18:32 GMT

Hi, all.

iLogic Design Copy is great instrument! It works wery well, but i find some issue.

If you uncheck boxed renaming - renaming procedure stops at all (copying error). Please fix this.

I need to rename only those parts, which get influence, from my iLogic parameters, not all parts.

More info at the pictures below.

Re: iLogic Design Copy failure

johnsonshiue — Wed, 03 Mar 2021 22:50:33 GMT

Hi Sergey,

The behavior does not sound right to me. I need to work with the project team and see why it behaves this way. Hopefully, it can be fixed soon.

Many thanks!

Re: iLogic Design Copy failure

MjDeck — Tue, 09 Mar 2021 22:05:42 GMT

@AnufrievSergey , it looks like you are creating copies of each file in the same folder. Is that true? The source folder is the same as the target (destination) folder?

Re: iLogic Design Copy failure

AnufrievSergey — Wed, 10 Mar 2021 06:05:02 GMT

Good morning, Mike. Yes, the folder is the same.

Re: iLogic Design Copy failure

MjDeck — Wed, 10 Mar 2021 15:50:16 GMT

We weren't expecting the source and destination to be the same. We can make changes to support that workflow in future.
It looks like there's no workaround with iLogic Design Copy. Have you considered using Copy Design in Vault instead?

Re: iLogic Design Copy failure

AnufrievSergey — Tue, 16 Mar 2021 09:41:41 GMT

Yes, our company use Vault with a part name generator. It will be great generate names for 'iLogic Design Copy' files from Vault name generator. I just don't know how.

Re: iLogic Design Copy failure

MjDeck — Thu, 18 Mar 2021 14:29:42 GMT

I'm not familiar with Vault Copy Design myself, but I think it's worth a try. You can set the "Reuse" option on individual files to avoid copying and renaming them. If you have questions about Copy Design, it's best to ask them on the Vault forum.
But I'm wondering why you want to create a copy in the same folder. How are you planning to use the copy?

Re: iLogic Design Copy failure

AnufrievSergey — Thu, 01 Apr 2021 11:33:19 GMT

Good day, MJ.

I use storage stackable trolley for aluminium alloy profiles different shapes. Each profile need to be store by own trolley with exact dimension. And this dimensions are parametric, I call it general dimensions. See picture.

Some parts are depends from general dimensions, some parts not. All trolleys is a same project and need to be saved in one folder, but parts can be save in a several subfolder. But in a "iLogic Copy Design" i can choose only vault project root. I not except that my experience in a "iLogic Copy Design" is poor. And if you can explain how can i save all parts of three trolley: 800x600x400, 800x400x400, 800x400x600 (it is LxWxH in mm), in a same folder or subfolders, it will be wery helpful. I have some unified parts and have a parts witch depend from general dimensions.

Thanks, please excuse me for delay answer.

Re: iLogic Design Copy failure

MjDeck — Thu, 01 Apr 2021 13:27:16 GMT

I think Vault Design Copy would be better for what you're trying to do.

Re: iLogic Design Copy failure

AnufrievSergey — Fri, 02 Apr 2021 06:24:19 GMT

Hi, "Vault Design Copy" good too. I just need to adjust my file name generator now. Thanks.

Re: iLogic Design Copy failure

paulm — Fri, 15 Sep 2023 18:55:32 GMT

edit. i made an error. sorry.

Re: iLogic Design Copy failure

chrisw01a — Tue, 19 Sep 2023 16:47:38 GMT

@MjDeck wrote:
We weren't expecting the source and destination to be the same. We can make changes to support that workflow in future.
It looks like there's no workaround with iLogic Design Copy. Have you considered using Copy Design in Vault instead?

MjDeck,

Can we please get a copy of the source code for iLogic Copy Design? I need to figure out how you are iterating through "AllReferencedDocuments" when .ipt's with model states are involved. Our program (calling Apprentice Server) is having an issue where Document.AllReferencedDocuments is recognizing two copies of the same document due to the document having two model states. This is blowing up our program. Any help is appreciated.

Re: iLogic Design Copy failure

MjDeck — Fri, 15 Sep 2023 19:42:30 GMT

@chrisw01a , it's not an Apprentice bug. They really are two separate documents, although they are in one single ipt file. In Inventor 2022 and later, a model state file contains one factory document, plus one member document for each model state.
When a model state component is placed in an assembly, the assembly contains a reference to one of the member documents.
If you place two different model states of the same file, then the assembly contains references to two different model state member documents.
To avoid trying to copy the same file twice, you could keep a HashSet or Dictionary of the filenames that have been processed.

Re: iLogic Design Copy failure

chrisw01a — Fri, 15 Sep 2023 20:03:01 GMT

I see. We are already keeping a dictionary to make sure we don't create any duplicate file suffixes. In fact, that is exactly the part where it is blowing up.

So if we have two parts in the source folder:
12345-101.ipt
77777-101.ipt

We are exiting the program because in our destination directory, this would cause duplicate part names.
Unfortunately this model state issue is creating this scenario naturally so the program finds:
12345-101.ipt
12345-101.ipt
And it determins that this will create a duplicate in our destination folder so we exit.

I'm not sure how to fix this to allow for both cases.

There is nothing else I can call from Apprentice to eliminate the duplicate?

Thanks for the reply.
Chris

Re: iLogic Design Copy failure

MjDeck — Fri, 15 Sep 2023 20:26:07 GMT

You can use the File.AllReferencedFiles property. Sample:

For Each fileX As Inventor.File In openedDoc.File.AllReferencedFiles Debug.Print("referenced file: {0}", fileX.FullFileName) Next

However, that doesn't give you the Document. And unfortunately, it looks like each member document has a separate NeedsMigrating flag. You have to activate the model state and save it in order to migrate its document. Let me double-check that behavior.

But I would recommend using openedDoc.AllReferencedDocuments as you are now. But add a new dictionary of filenames (in addition to what you have now) to avoid adding names twice.

Re: iLogic Design Copy failure

MjDeck — Fri, 15 Sep 2023 20:47:55 GMT

You can get a list of Documents from a File. So if you want to use AllReferencedFiles:

For Each fileX As Inventor.File In openedDoc.File.AllReferencedFiles Debug.Print("referenced file: {0}", fileX.FullFileName) For Each docX As Inventor.ApprenticeServerDocument In fileX.AvailableDocuments Debug.Print(" needs migrating = {0}", docX.NeedsMigrating) Next Next

Re: iLogic Design Copy failure

chrisw01a — Sat, 16 Sep 2023 17:59:22 GMT

@MjDeck wrote: In Inventor 2022 and later, a model state file contains one factory document, plus one member document for each model state.

MjDeck,

Given your examples, is there a way to determine if the document is a factory document vs member document? This could help me a lot.

Re: iLogic Design Copy failure

MjDeck — Sun, 17 Sep 2023 23:50:04 GMT

Here's a sample function to test for factory and member documents. This could be improved by to defining an Enum and returning that instead of an integer.

''' <summary> ''' Returns: ''' 0 if the document is not a model state document ''' 1 if it is a model state factory ''' 2 if it is a model state member ''' </summary> Private Function GetModelStateDocumentType(doc As Inventor.ApprenticeServerDocument) As Integer If doc.DocumentType = Inventor.DocumentTypeEnum.kPartDocumentObject Then Dim compDef As Inventor.PartComponentDefinition = doc.ComponentDefinition If compDef.IsModelStateFactory Then Return 1 If compDef.IsModelStateMember Then Return 2 ElseIf doc.DocumentType = Inventor.DocumentTypeEnum.kAssemblyDocumentObject Then Dim compDef As Inventor.AssemblyComponentDefinition = doc.ComponentDefinition If compDef.IsModelStateFactory Then Return 1 If compDef.IsModelStateMember Then Return 2 End If Return 0 End Function

Here's some info about the model state API.

Re: iLogic Design Copy failure

chrisw01a — Mon, 18 Sep 2023 19:03:39 GMT

Thank you a bunch. I am having to do my regular work at the moment but will get back to it soon.

Re: iLogic Design Copy failure

Yijiang.Cai — Thu, 09 Nov 2023 06:39:34 GMT

This idea has been implemented within Autodesk Inventor 2024.2. Please review the Inventor 2024.2 What's New article here. For more information regarding how you may leverage the feature, and please review this page. Special thanks to everyone who cast a vote for it.