Unresolved links when opening .iam

[saltedfish]

I created a quickie model for my boss, composed of a few separate parts. Essentially created one solid, then a second, and threw them together in an assembly. I sent the resulting .iam file to my boss for review, and he informed me he was unable to open it because the assembly was referencing file paths that were broken when he tried opening it from his machine. Specifically, it opened a "Resolve Links" dialogue.

Is there a way to sever these dependencies and create an assembly that is wholly self-contained? I can't imagine why I'd want something I'm sending someone to look for file paths specific to my machine. Inventor help pages mention how to repair the links, but there has got to be a way to make Inventor package everything in one bundle.

Thanks in advance.

[VinodBalasubramanian]

How did you manage to send it. Did you use a packngo option. Can you confirm if you just copied them and sent to your boss or used packngo function to collect all necessary files associated to the model.

https://grabcad.com/library/tutorial-how-to-pack-and-go-in-autodesk-inventor-1

[EvanGu]

Hi,

When you save your assembly and pass it to someone else, have you tried Save As->Pack and Go? This command packages everything that has dependency with your top assembly.

[bob_holland]

@saltedfish,

You can also derive the whole assembly into a single part.

That way it is only one part file:

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2014...

You can then break the links to the original parts and assemblies:

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2016...

We hope that this helps.

Thank you.

[SteveMDennis]

@saltedfish

As the others have pointed out, by default Inventor uses a reference model for parts in an assembly, the parts are NOT local to the assembly. If you are using project files the references are relative but they may be absolute in other instances.

We have a few workflows that would help you in your scenario as mentioned, Pack and Go, derive to make it a single part (but the file size will blow up if there are too many parts in the assembly), etc.

It all depends on what you are trying to do. You could have also just sent the part files along with the assembly file.

[Paul.Normand]

Hi,

An Inventor iam file does not actually contain any of the parts or sub-assemblies in the file. Assembly components are external reference files that are loaded when you open the file. If the files are not available, then they are unresolved. If they are on the network, they can be found if the path is specified in the project file (ipj).

If you send the parts along with the assembly file, then Inventor can find the files it needs. If there are more than a couple of files, there is a handy utility called Pack n Go that will find all of the files and package them up for you in a zip file. In file explorer, right-click on an assembly file to access Pack n Go. 

Here's a video that walks you through the process:

https://www.youtube.com/watch?v=AfchaMjhm_M

Hope that helps,

Paul

[saltedfish]

I tried using the Save As -> Pack and Go and it resulted in a mess of files and folders on my desktop. Am I supposed to zip those files and send them all to the recipient?

Edit: it appears deriving the assembly is the way to go. Given the low part count, file size shouldn't be an issue.

[SteveMDennis]

Unknown to me you can use pack and go and NOT create a zip file. Apparently you need to make sure you check the option to create a zip file when using pack and go. So yes you can use pack and go to create the zip automatically. Why we don't check that by default I have no idea, I'm gonna look into that with the team.

[saltedfish]

At this point, I've determined that I want to derive the assembly so that it is a single file I can send. However, I cannot find the Derive button on the Manage > Insert area on the ribbon. Do I need to enable something to make the assembly eligible for deriving?

Also, when attempting to pack and go, I do not even see an option to have Inventor zip it up for me.

[sundars]

Hi there,

You can create a new part file (ipt) and derive your assembly into the part file - this will make a single IPT which has the assembly derived into it. Now break link on the assembly by RMB clicking on it in the browser.

Then save the IPT and voila you will have a stand-alone IPT. Bear in mind, this will create a fairly large IPT file depending on how big the assembly you derived into it is.

For the zip option in Pack-n-go, you should be able to find the checkbox on the left side of the pack-n-go dialog below "Skip Templates" - It should be called "Package as .zip"

-shiva

Inventor Development

[Paul.Normand]

And if you are using Inventor 2018, you can use the Shrinkwrap command right in the Assembly 3D Model ribbon to create a single part from the assembly.

(This method means you don't have to start a part file and then use Derive in the Modify tab)

As Shiva suggested in the alternate (2017) workflow, right click the parent entry in the part file browser, right-click and break the link.

[saltedfish]

Alright, here's the scoop:

I followed @sundars advice and made a new .ipt and used the Derive function to pull in the .iam bits. This resulted in an .ipt with the solids in it, but I cannot manipulate the separate pieces of the assembly in the resulting .ipt -- even after selecting the "Maintain each solid as a solid body" option in the Derived Assembly window. And after breaking the link.

@Paul.NormandI am using Inventor 2015, I just learned, so this limits my options I guess.

Thanks to everyone so far for helping me out, I really appreciate the time you're taking to give me a hand.

Also, there is absolutely no zip option in my Pack and Go dialogue, which makes sense if I'm two years out of date. It's like I'm back in the dark ages of the 90s where I have to do this by hand.

[SteveMDennis · Accepted solution]

@saltedfish

If you want to still use the assembly as an assembly and have the assembly functionality you can't use derive or shrinkwrap. You need to keep the assembly structure using pack and go or something like that.

Derive, shrinkwrap, etc. turn the assembly into a multi LUMP part file, you can use part commands like move body, etc. but you will not be able to drag the body like in the assembly, edit constraints, etc. it IS a part after the derive.

The assembly environment is when you have an IAM and referenced IPT files, there is NO local parts/bodies in our assembly world.

[saltedfish]

I got it. So my only option for sending a model containing multiple parts to someone is to pack and go it and send them a zip and hope they know what to do with it? That seems terribly clumsy, but workable. I'll do that.

[SteveMDennis]

If you want them to have the full assembly capabilities (mechanistic move, etc.) yes.

Pack and Go should collect all the files (keep the hierarchy or not, up to you) zip it up ,etc.

The recipient unzips and opens the assembly, everything should work w/o any resolve dialog or errors.

[bob_holland]

@saltedfish

Another option that you can look at is Inventor's Connected Design:

https://knowledge.autodesk.com/search-result/caas/CloudHelp/cloudhelp/2017/ENU/Inventor-Help/files/G...

Inventor Connected Design enables online 3D design reviews with others not on your network who need to participate in the design process. Use Inventor Connected Design to easily collaborate securely on a view-and comment-only copy of your 3D model with your customers and remote project stakeholders: Create a Design Share to share an Inventor model free of intellectual property with others not on your network who need to participate in the design process. For example, create a Design Share for a customer to request approval on a design, or to provide easy access to your field sales team for on-site 3D design demos. Design Shares give customers easy access to designs you want to share. Your collaborators can review the 3D viewable of the model and post comments.

This may give the person that you are collaborating with all the information that they need.

Good luck.

[saltedfish]

That's a handy piece of information to have. Not quite applicable here, since my boss does need the models themselves to create prints from, but I'll keep it in mind going forward. Have a good one!