How to avoid resolving links after Pack and Go and renaming files in Inventor?

[Olina0212]

Hello everyone,

I’m having an issue related to Pack and Go workflow in Autodesk Inventor and would like to ask for best practices.

My current workflow is:

1. Use Pack and Go to create a new project from an existing one

2. Rename the assembly (.iam) and part (.ipt) files to match the new project naming

3. When opening the new assembly, Inventor asks me to Resolve Links for many parts, even though all files are already copied into the new folder

This becomes very time-consuming for large assemblies.

I would like to ask:

• Is there a way to rename files after Pack and Go without breaking references, so that Inventor does not require resolving links part by part?
• What is the recommended best practice for Pack and Go + Rename when creating a new project based on an old one?
• Should renaming be done inside Pack and Go, or is there a better tool/workflow (Design Assistant, iLogic, Vault, etc.)?

Any advice or shared experience would be greatly appreciated.
Thank you in advance.

[SharkDesign]

Pack N go is meant for sending to other people, not creating a copy for yourself. You should be using iLogic design copy or just the plain copy command in the assembly environment. 

To use iLogic (no coding required) close all files and then you'll see iLogic design copy on the ribbon. 

This will make a copy of your assembly, parts and drawings and allows you to rename the files as well. 

If you really want to use pack and go, creating a new project file in the process and using that can help to direct Inventor to the correct files, but renaming files in Windows Explorer is always going to lead to lengthy relinking tasks. 

[Olina0212]

Dear @SharkDesign 
Thank you for your detailed explanation regarding the use of iLogic Design Copy and Pack and Go.

I have a follow-up question regarding the iLogic Design Copy tool: Does this method automatically copy every file within the source folder? Specifically, I would like to create a copy that only includes the main assembly and its constituent part files.

Could you please advise if it is possible to limit the copy to these specific components only?

I look forward to your guidance.

Best regards,

[SharkDesign]

If you select the top level assembly, it will only copy all parts and sub assemblies in the assembly. Any files in the folders not used in that assembly are not copied. 
You can of course select any additional files you like in iLogic manually

[hollypapp65]

Use the Project file in Pack and go.

[IgorMir]

Pack & Go is a good and reliable tool for creating a copy of the old design. One just needs to know how to use it properly.

And the proper usage of the tool had been discussed on this forum more than enough.

Cheers,

Igor.

---

@SharkDesign wrote:

Pack N go is meant for sending to other people, not creating a copy for yourself.

[johnsonshiue]

Hi! Another thing to check is the project setting. Go to Project -> Options -> is "Use Unique File Names" set to No? If it is set to No, Inventor will prompt you to resolve files because it assumes there are files with the same name in the project cone search paths. Set it to Yes and Inventor will try to resolve files automatically.

Many thanks!

[lauri_barnhart]

Hello, @long0212le,

Just checking in—did the responses shared by @SharkDesign, @hollypapp65, @IgorMir or @johnsonshiue help clarify your question?

If so, please consider clicking the "Accept Solution" button on the post(s) that solved your problem. Doing so helps others in the community easily find useful answers.

If your question still needs more attention, feel free to reply here with an update. This way, other members can jump in with further suggestions or guidance to help you move forward.

All the best,

Lauri | Community Manager

[Olina0212]

Thank you all for your comments and advice. However, I find that neither method has fully met my expectations. Below is my current understanding; please let me know if you know of a more effective alternative.

A. Pack & Go    
Pros:      

Preserves the original physical folder structure of the project.

Project settings are linked to the new physical directory (except for "Frequently Used Subfolders").    

Cons:      

Broken links for "Frequently Used Subfolders."            

These paths do not update automatically to the new directory.            

Requires manual relinking via the Project Editor.      

Does not support file renaming.            

Pack & Go only performs a copy; it does not manage renaming.            

If renamed via Windows Explorer:                

References within the .iam are lost.                

Requires manual "Resolve Links" → high risk for large assemblies.      

Cannot package all .idw files (only those included in the assembly file).            

Only copies .idw files explicitly referenced by the .iam.            

Standalone .idw files or those following custom design workflows are omitted.

B. iLogic Design Copy    

Pros:      

Enables renaming of .iam, .ipt, and .idw files while maintaining internal reference integrity (assembly–part–drawing).      

Creates a new project from an existing one without losing assembly or part links.    

Cons:      

The physical folder structure is altered and does not match the original project (despite Project settings remaining largely identical).       In Project settings, "Workgroup Search Paths & Libraries" still point to the old project; manual adjustment is required.       Folders do not automatically rename according to the new project (directory names retain the old project name; e.g., the folder containing Frame files for the .iam).

[IgorMir]

Hi, Olina;

You are not using P&G properly, by the sound of it.
When you selecting upper assembly in the P&G Dialog box - select although all the corresponding drawings. That's if they have already been created.

Specify the stand alone location of the copied files. Desktop is usually a good option.

Select and make current (very important!) a Project file, created by P&G routine. You can even open an upper assembly in Inventor, to make sure - everything is copied properly.

Open the top assembly file in Design Assistant. All the parts will be listed in the upper pan too. If drawings were copied as well - select all of the files in the upper window (very important!) and then select Find Files in the bottom window. Make sure there is a check mark against drawing icon. It is checked by default, usually. Uncheck the ones which are not needed.

Wait for a while and all the drawings should get listed in the bottom pan as well.

Now you can carefully rename parts, assemblies in the upper window. And edit names for the drawings in the bottom pan. It is a bit of a tedious process, but a reliable one non the less.

Once finished - close DA and open files in Inventor. To make sure - all works well. When satisfied with the result - close all the files. Copy folders with new files (the folders should be renamed as well) into Inventor's work directory. Make the working Project file current again. Open assembly from your work directory to verify it. That should be it. After that you can delete files from the Desktop.

iCopy does pretty much the same thing. But it doesn't allow you to change names of the files to what's needed. You can only add prefix or suffix to it. That, probably, allows you to keep the files in the same directory prior to renaming them in DA. But I don't see it as a great bonus. Not for me anyway. 

I hope these lines have been of some assistance to you.

Cheers,

Igor.