Copy assembly keeping the file associations at the new folder

[Anonymous]

Hello everyone,

I have created an assembly file with a lot of sub-assemblies and parts attached to it. I'm trying to copy it to a new folder, preserving all the associations between the files in the new folder.

1. Is there any workaround for this?

2. Is there anyone who can tell their experience with this extension? http://assemblycopier.com/

Thank you in advance.

[mcgyvr]

Per your other post.. Thats what pack and go does..

You just may not be using it correctly or something..

Are you activating the newly created project file when attempting to open/modify these files?

You can also look into the ilogic copy design tool.. (check youtube for videos,etc...)

[SBix26]

I think in another topic you mentioned you are using Vault.  The easiest method to copy an assembly and all its components is Vault's Copy Design function.

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Sam B
Inventor Pro 2020.1.1 | Windows 7 SP1
LinkedIn

[Anonymous]

Hi @mcgyvr ,

Thanks for your reply here.

I am activating the new ipj file and then opening the assembly and parts files but they don't seem to be linked.

@SBix26 I have Vault 2019 but the Inventor version i'm working with is 2020, which makes it not possible to use any Vault functions. Thanks.

[Anonymous]

@mcgyvr 

The steps I'm following are:

1. Activate the ipj file

2. Change some of the values in a part

3. Open the assembly file. I notice that the "Local Update" function is grayed out (picture01)

4. I'm trying to update it through an iLogic function (picture02) but nothing happens

[SBix26]

Without Vault, the easiest way I can think of is to use Windows File Explorer to copy all the files to a new folder.  Then create a new .ipj project file in that new folder, with the Workspace defined as that new folder.  Activate the new project file, then open the copied assembly.  All should be linked as expected.

However, you now have duplicate file names of all the original files, just in different folders.  This is dangerous-- should you happen to use the wrong project file, you could do a lot of unintentional modification of files.

To rename files, you can use the Design Assistant utility.  While it is quite powerful, DA has not had a user interface update in this decade, or perhaps even in this century, so it is not as intuitive as it should be, and is quite tedious to use.  If you intend to rename, though, you might as well use DA to do the copying as well.

If I remember correctly, someone has posted pretty complete instructions for using Design Assistant to copy and rename files, but I don't have a link.  A search in the Knowledge Base should produce it.

Update: Here's a link to a video by @PaulMunford from the Knowledge Base.  The last five minutes are all about copying assemblies using Pack & Go and Design Assistant.

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Sam B
Inventor Pro 2020.1.1 | Windows 7 SP1
LinkedIn

[mcgyvr]

It looks like you have numerous parts/assemblies with the cloud icon.. I think those are Fusion 360/Team Hub files or something..

That may be your problem..

I have no idea how that would interact with a pack and go. 

Its quite easy to simply look at the properties for a file to see exactly where its saved/referenced from..

You should be tracking down these issues by looking at the file location and if they aren't ones that are stored in your newly created folders then the process will need to be changed to account for whatever is happening there..

[Anonymous]

@SBix26  thanks for your reply.

My initial file is in BIM 360, so I downloaded the folder with the assembly, parts and ipj and as per your suggestion I created a new ipj file in this folder. However the association doesn't work between the new files. I followed exactly the same steps by amending some parameters in the parts and then opening the assembly file which didn't give me the "Local update" option.

[Anonymous]

@mcgyvr thanks.

The cloud indicates that they are cloud files. The initial assembly is made in BIM 360 and the files that are the result of Pack and Go are in OneDrive. I get this icon for all the parts and sub-assemblies. 

By performing RMB-iProperties I see that all the new files are located in the new folder. Could it be an issue of OneDrive?

[mcgyvr]

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@Anonymous wrote:

@mcgyvr thanks.

By performing RMB-iProperties I see that all the new files are located in the new folder. Could it be an issue of OneDrive?

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Ok so the files are being associated correctly like you wanted..

Now we just need to figure out your process for attempting modifications to the files..

The pictures shown and the simplistic ilogic code don't tell us anything..

Please explain your process of updating the files to make a change..

Have you tried something like simply adding a new hole to any part to see if that part updates in the assembly?

[Anonymous]

@mcgyvr ,

The images are only showing that the model doesn't update.

The logic behind the model is the following:

There is the top-level assembly which contains parts and sub-assemblies. The parts and sub-assemblies don't contain any parameters but they take their values from an empty part which includes all the parameters. The top-level assembly contains planes. The distances between the planes are defined by the parameters part.

The way to test if the associations work is to amend the parameters in the part file and see if:

1.the individual parts

2. the top-level assembly

change. In this case after updating the values nothing changes.

I also tried to create a hole on one part and again, the top-level assembly file did not update.

[mcgyvr]

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@Anonymous wrote:

I also tried to create a hole on one part and again, the top-level assembly file did not update.

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And did you verify the file location of that part and ensure that the top level assembly is referencing the same part/file location?

Can you share your pack and go? Or can you duplicate another assembly that exhibits these same issues for you so we can try to replicate it?

[Anonymous]

@mcgyvr , thanks.

1. How can you see which parts/file locations the top-level assembly references?

2. I'm attaching a zipped folder of all the files here.

3. I used iLogic Design Copy and saved the new model in my c disk (not in the cloud) and it works. I will try doing the same saving the file in the cloud to see if this causes the issue.

[mcgyvr]

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@Anonymous wrote:

@mcgyvr , thanks.

1. How can you see which parts/file locations the top-level assembly references?

2. I'm attaching a zipped folder of all the files here.

3. I used iLogic Design Copy and saved the new model in my c disk (not in the cloud) and it works. I will try doing the same saving the file in the cloud to see if this causes the issue.

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Everything is working just fine for me in that zipped folder..

There are some files that are named the same as others so I needed to pick one (you should know which is which) but after that I could open the "GenericStaircaseV6.iam" file and then open the ACM_Floor and add a hole to it and it updated just fine in that top level..

I can update a part and it changes in the top level file..

You just aren't opening/modifying the correct parts.

You can easily see file locations by just looking at the properties of any part or assembly through the model browser.. You can also just right click on a file and select "open" to open/edit it.. 

[Curtis_W]

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@Anonymous wrote:

1. How can you see which parts/file locations the top-level assembly references?

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Hi @Anonymous 

Just as a tip that might help with some of this, if you open the BOM editor you can use the Column Chooser button to add File Path to the table as shown below, this will help you see where all the files in the assembly reside.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

@mcgyvr thanks.

I opened the right file as i used RMB-Open.

I tried the hole on the floor and it seems to work today; it might have not been synchronised yesterday due to OneDrive.

However when changing the parameters in the latest file nothing gets updated in the top-level assembly. I checked which file it uses and I realised it's still referencing the parameters of the initial part. The only reason I can think of is that it didn't include the parameters file (presumably because it doesn't have any geometry?) so it referenced the initial parameters. 

I will try to "pack and go" again to double-check if it contains the parameter file.

[Anonymous]

Hi @Curtis_W ,

Thank you for your advice.

Indeed I can see the components paths. However I have a part that has no geometry and contains all the parameters/values that are used in the model. This part is not shown in the BOM and unfortunately it's the file that is not linked to the top-level assembly.

[Anonymous]

Update: When I RMB-Open a component from the top-level assembly in the P&G folder it opens a component from the original directory which is not what I was aiming for. When I open a component from the P&G folder and amend it it doesn't update the top-level assembly. The iProperties show that all the sub-assemblies and parts are referenced to the original directory. The purpose was to create an independent folder with all the parts being associated with the top-level assembly within the P&G folder. 

[Anonymous · Accepted solution]

Apparently Pack&Go cannot recognise the link to cloud drive or any files stored in cloud drive unless the cloud drive is assigned with a logical drive name, as @johnsonshiue has mentioned in another post.

Also, I copied the files through iLogic Design Copy and it worked as planned, with all the parts, sub-assemblies and top-level assembly keeping the association between them within the P&G folder and cutting the link to the original directory.