Create independent copy of an assembly with Design Assistant (for dummies)

[j.pavlicek]

Hello,

I'm struggle with Design Assistant (DA) copy design. I did it before, but found it (for me) very non-intuitive.

What I need:

Copy an Assembly (Assembly1.iam) with its subassemblies (SubAssembly2.iam ÷ SubAssemblyX.iam), so I can edit them with no affect to original Assembly1.iam and its subassemblies and components.

What I tried (and achieved):

1. Actions: Open Assembly1.iam in DA, select first row, in Action column choose Copy, in Subfolder column set path to a new folder, save.
   Result: Assembly1.iam appears in the new folder. All other parts and subassemblies are linked from the original locations (any changes in these affect the original Assembly1 - obviusly.)
2. Actions: Open Assembly1.iam in DA, select all, in Action column choose Copy, in Subfolder column set path to a new folder, save.
   Result: Error during save - Content center files cannot be moved to another location.
   
3. Actions: Open Assembly1.iam in DA, select all except content center files, in Action column choose Copy, in Subfolder column set path to a new folder, save.
   Result: Error during copy because some files already exist there - all selected files are copied to the new folder, original (sub)folder structure is not preserved. This is caused mainly by bolted connections from subassemblies, they are originally stored in subfolders.

Thanks for help.

PS: I do not accept manual subfolder setting for each subassembly as solution. This is no-go for this amount of files.

[CCarreiras]

HI!

Save as -> Pack and Go

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

[j.pavlicek]

Hi, thanks for reply.

I forgot to mention that I need to keep the copy in same project.

[Mark.Lancaster]

@j.pavlicek 

Try Inventor iLogic Design Copy https://synergiscadblog.com/2014/09/23/copy-files-easily-with-ilogic-design-copy-even-without-ilogic...

[j.pavlicek]

Also I tried to Pack&Go the assembly and copy back to project, but it gives me unexpected result.

This is my case (I'm using one flanged connection assembly for simplification):

There is FlangedConnection.iam containing 2 pcs of Flanges (from the Content Center), 1 pc of sealing ( from CC) and 4 pcs of flanged connection (1 Bolted Connection created by Desing Accelerator and copied using Circular Array).

Files are placed in ...\Project_Workspace\SomeHigherLevelAssembly\FlangedConnection.iam and \Project_Workspace\SomeHigherLevelAssembly\FlangedConnection\(here are Design accelerator files) and CC files are stored in default CC folder (I want to keep copy in same project and use standard parts from CC).

When FlangedConnection.iam is saved using Pack&Go, it creates a new project folder structure in Pack&Go folder like: ...\Pack&Go_folder\Project_folder\Project_Workspace\SomeHigherLevelAssembly\Flanged Connection.iam . So I try to copy FlangedConnection assembly + belongings to a new folder ...\Project_workspace\New_folder\FlangedConnection.iam all non CC dependecies of the copied FlangedConnection.iam are linked to Project_folder\Project_Workspace\SomeHigherLevelAssembly\FlangedConnection\

Images better than 1000 words:

Pack&GoPack&Go (sub)folder containing copied assemblyDesign Assistant view of Packed&Went version of the assembly (opened in context of original Project - due availibility of Content Center parts.

[johnsonshiue]

Hi! I don't think Pack&Go is the right solution for you in this case. You want to create a brand new dataset from an existing one within the same project. This is a copy design operation. I believe you want to use iLogic Design Copy or Vault Copy Design.

P&G creates an identical copy (names and files) in a different folder. If such same named files exist in the project folder, Inventor can be confused an resolve to a wrong file in a different folder.

Many thanks!

[a_delangeT6HEN]

How is this so difficult..

[IgorMir]

Hi Johnson,

It is worth mentioning that the extra steps will still be required. Copy Design allows you to introduce prefix to the files names but it doesn't allow the user to re-name the original files. Hence the DA is needed to do so. But that, in turn - brings another issue. For whatever reason - I, for one - have never been able to get drawing's files into the DA. Which means - after editing the names for the assemblies and parts - there will be Resolving issue in each and every drawing file. Which is not a big deal if the set of drawing files is in a range of hundred plus a little. But if there are a thousand drawing files in a project - it will take some efforts to resolve them all.
Cheers,

Igor.

[IgorMir]

You need to make the Project, which was created by P&G - current. Then open the upper-most copied assembly in the DA and rename all the files in there. Close the DA, open the drawing's files in Inventor and resolve the links. You will have to just point to the corresponding re-named assembly or part file. Once done - you can transfer all of the files into your working directory. Now start Inventor and set your working (old) project as current again.

Cheers,

Igor.

[SBix26]

I've never had any difficulty to include drawing files in DA, so I wonder what's different?

My process is pretty much the same, but I start with the top-most assembly drawing.  I then select all the files under that drawing (in the upper pane), and then use the lower pane to find all "where used" files (drawings, derived parts, presentations, etc.).  In the upper pane select all, choose Action > Rename, and in the lower pane select all, choose Action > Update.  Then go through one by one: right click on the filename, select Change Name, set the new filename.  When finished click Save and you're done, except for renaming the drawings.

Note that changing the filename automatically changes the Part Number iProperty.  If you don't want the Part Number to change, you can right click on it (before saving!) and select Reset, which returns it to the original value.

---

Sam B

Inventor Pro 2024 | Windows 10 Home 22H2

[johnsonshiue]

Hi! Do you mind elaborating the issue you are having? Are these files managed by Vault or the legacy Shared project?

Many thanks!

[IgorMir]

Thanks Sam.
The waiting time for the drawings to populate the pan is quite substantial. And that's for a small assembly. But for a medium size one - I can't tell how long will that take.

Anyway, it is not a real show stopper for me since copying the whole design is a fairly seldom activity I got to do. But it is good to learn all the options should the need arise to copy designs more frequently.

Non the less - you gave me some food for thoughts how to handle the files re-naming protocol more efficiently. Thanks for that! 🙂

Cheers,

Igor.

[a_delangeT6HEN]

Dear John,
My experience is mostly in Fusion 360 but here at Folkers I work in Inventor 2024.
In Fusion it is very easy, copy and assemy and paste as new.
In effect that is what I want to achieve in inventor, simply copying a folder in windows explorer and changing file names is very inefficient.
We design speedgates, often the wings of the gates are 99% similar but not completely.
We do not use Vault.

[johnsonshiue]

Hi! If Fusion works better for you, that is great. There are similarities between the two. But, there are indeed major differences also. The reason the copy of an assembly is relatively straight forward is because Fusion supports local components. It means all components are contained inside a design.

Inventor iam file is more like a wrapper, which do not contain any geometry. But it knows where to find those part files. When copying an assembly, many files will need to be copied and the links will need to be properly remapped by Inventor.

Many thanks!

[a_delangeT6HEN]

Hi,
That is indeed what I do now, I was hoping I missed something.
Would implementing to Vault have any impact on this?

[CCarreiras]

Why not use parametric models, ready to have the configurations you need?

like this:

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

Vault will help you to make copies, but the mechanism is similar to Design copy (without Vault) but with a few more options.

[a_delangeT6HEN]

Hi,

Thank you for your time!

All my models are parametric, the issue is there are lots of shared components.
Usually I start of with a .ipt named project#-parameters.ipt and link all my part parameters this file. This part itself does not contain any geometry.
For example:
A specific type of rail which is sold at a length of 1998mm, offset a plane at the end with a parametric value and a split body modifier to adapt the length according to the input parameter. "RailLength". I add this assembly (Rail, Bolts, Nuts, Spacers, etc.), which lives in a shared folder on the network to my assembly and I change the "RailLength" parameter to suit my needs. However this means every instance of this part, also in other projects will change.
In this case I need to make an independent copy of the assembly.
In Windows explorer I copy the entire folder containing the .iam and multiple .ipt files and paste it to a location inside the inventor project. Now the .iam still uses the IPT's in the original folder, not the new folder.
This means I need to go in and tell Inventor where to find every single .ipt. This process takes a lot of time.
How do I work around that?

[CCarreiras]

Have you tried the Copy Design Tool?