1 Assembly File 240 Variants HOW? HELP!!

[Anonymous]

I have a machine assembly that has 240 variants. They are all simple part or sub assembly swaps. I started creating these variants using LOD, but the BOMs are not correct in the drawings. How do I properly do this without having to make an assembly for each different version and have the drawing BOMs be correct?

[mcgyvr]

iAssemblies

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

[swalton]

As you have found, LOD is not the correct tool.  It is a memory management tool, not a configuration tool.  It does not play well with drawings or BOMs.

Inventor will require you to have a separate .iam/.ipn/.idw file on disk for each assembly option.  You have two options for managing the resulting files.

1. iAssemblies
   1. Create a master assembly (factory file) with a table that defines each assembly configuration.  Each configuration (member file) will be saved as a dependent copy of the factory file.  Changes to a member file must be made in the factory file.  
   2. The workflow is similar to iparts.
   3. Expect to use iParts and iAssembly sub-assemblies to build all the variations you need.
2. Saving Copies by hand or with iLogic.

Do you use Vault?

Do you know exactly what the 240 variations will be right now?

Do you expect to change the design over time after you create all 240 variations?

I might start with the iAssembly workflow if I know that I will rarely make changes to the 240 options.  

Autodesk is working on other options, but they have not been released outside of beta testing yet.  

[Anonymous]

First we are stuck on 2016, because IT won't allow us to upgrade, even though we pay for the license that allows upgrading. 

Do you use Vault?

No IT will not install for us. We have to use a shared folder on a network drive.

Do you know exactly what the 240 variations will be right now?

Yes 

10 Transformers

2 Bridges

12 Output Plates

Do you expect to change the design over time after you create all 240 variations?

Changes will come over time to components.

I am trying out the iAssembly stuff, but everything is restricted to a list. I cannot click on the model to select parts. For the bridge I need to remove one section and all of the hardware associated. This results in a table with 200 screws that I have to manually find and disable for each configuration. Then comes the washers and nuts. It would be nice to group all the hardware together under 1 table entry.

I might start with the iAssembly workflow if I know that I will rarely make changes to the 240 options.  

[mcgyvr]

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@Anonymous wrote:

I am trying out the iAssembly stuff, but everything is restricted to a list. I cannot click on the model to select parts. For the bridge I need to remove one section and all of the hardware associated. This results in a table with 200 screws that I have to manually find and disable for each configuration. Then comes the washers and nuts. It would be nice to group all the hardware together under 1 table entry.

I might start with the iAssembly workflow if I know that I will rarely make changes to the 240 options.  

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@Anonymous  You do not need to work in the iassembly table.. You can just change to "member scope" and do everything in the normal 3d model view. Factory scope/model scope toggle is on the Manage tab in the "author" section. 

You could group stuff into browser folders (I think folders were in 2016) or phantom subassemblies to quickly disable groups of fasteners.

There will not be an "easy" button to setup such an advanced model but with proper usage of Inventor it should be something entirely possible.. 

[swalton]

In the past, we have moved the mounting hardware to the sub-assembly that requires it.  That way suppressing the sub-assembly also suppresses the mounting hardware.  You could even expand on the Phantom sub-assembly idea from @mcgyvr so that your individual .ipt components are in sub-assemblies that contain the required mounting hardware.

Did you use iParts/iAssemblies to build out your Transformers, Bridges, and Plates?  That should make it a bit easier to swap out components in the top-level iAssembly.

[johnsonshiue]

Hi! Depending on how you create your assembly, there mainly two solutions. 1) iAssembly. 2) iLogic rule and iLogic Design Copy.

At the moment, Inventor assembly or part cannot represent different geometric definitions within one file at he same time. You need to have multiple files (iam and ipt). Each variation has to be its own file. Please feel free to share an example so forum experts can guide you through the best workflows available at the moment.

Many thanks!

[swalton]

I just found this link to some tutorial videos about iParts/iAssemblies and iLogic.  I have not watched them yet, but they might help explain the various configuration options currently available in Inventor.

https://www.autodesk.com/customer-success/mech-eng-webinars?mktvar002=1069928&utm_medium=email&utm_s...

[Anonymous]

I think in my specific case, due to the way that we need files and drawings saved on the system, I have no choice but to model each assembly individually. The concept behind iParts and iAssembly is good but atleast in 2016 it is very difficult to properly implement and maintain with different size and shape parts. Cable and harness cannot automatically mate to a different part with different hole locations. It is just far easier to do everything individually. Thanks for the help.

[mcgyvr]

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@Anonymous wrote:

Cable and harness cannot automatically mate to a different part with different hole locations. It is just far easier to do everything individually. Thanks for the help.

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A tip.. You can copy and paste a harness and then make it adaptive to the new assembly to quickly just move the end connector or pins without having to recreate the harness from scratch each time..

But yes.. Needing cable/harnesses to adjust to differing end connector locations is something Inventor cannot do without a different harness for each adjustment..

[Anonymous]

Is there a way to group hardware in an iassembly? so that I have 1 table entry for a specific batch of hardware? Also can a harness be an iPart with more than one configuration?

[Anonymous]

If I cannot group them, can I make an iLogic rule to enable or disable the hardware based on which cable set is enabled so that I do not have to have a ton of hardware in my iasm table?

[Anonymous]

I will add more details:

I have 3 aluminum extrusions each with 2 slots.

Each slot has a double cable lug for a total of 6 cables and 12 fasteners.

I have 2 configurations. 

Configuration 1:

2 extrusions 4 cables 8 fasteners

Configuration 2:

3 extrusions 6 cables 12 fasteners

The extrusions are a tabled iAssembly. I would like the not needed parts to disable in the main iAssembly based on the table selection from the extrusion iAssembly. The goal is to limit the amount of table entries in the main iAssembly, to greatly simplify configuration options. I cannot share the files, but I can create a dummy assembly if needed.

[johnsonshiue]

Hi! I think it is doable using iLogic. But, the devil is in the detail. Please feel free to share an example so experts can comment further.

Many thanks!

[Anonymous]

Here is a sample representation. When I select the table entry for dual I need the 6 side cable lugs to iLogic disable and the 2 top lugs to enable. When I select triple, I need the 6 side lugs to enable and the 2 top to disable. The disabled parts cannot show in the BOM. This avoids me from having to select all 8 parts in the main table as enabled or disabled. These rules will be controlled by the Output iAsm table selection, not the main table.

[johnsonshiue]

Hi! I think this is doable using iAssembly. To make member specific change, you need to change the edit scope. Go to Manage -> Author -> Edit Member Scope. Then include or exclude the lugs accordingly.

Many thanks!

[IgorMir]

Hi Wayne,

What you want to achieve is pretty straight forward indeed. I would have sent you your modified assembly but it is in IV2020 format. So, here is a screen shot of the Author Table how it should look like. And the property of lags should be changed to Normal - not Phantom as they are now. Otherwise they won't be seen in BOM. LOD has absolutely nothing to do with what you want to achieve, BTW.

Cheers,

Igor.

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@Anonymous wrote:

Here is a sample representation. When I select the table entry for dual I need the 6 side cable lugs to iLogic disable and the 2 top lugs to enable. When I select triple, I need the 6 side lugs to enable and the 2 top to disable. The disabled parts cannot show in the BOM. This avoids me from having to select all 8 parts in the main table as enabled or disabled. These rules will be controlled by the Output iAsm table selection, not the main table.

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[Anonymous]

Unfortunately, That is exactly what I DO NOT want to do. When I add the proper assembly and hardware. I end up with hundreds of options that I have to enable or disable that are not important to the configuration. I want simple main choices based on the iAssemblies and I want the hardware and associated parts to automatically enable or disable based on the selection that I choose from the iAssembly table. iLogic should be able to do this, I am just not sure how because it is a more advanced process.

The work flow should be this:

When I select dual extrusion configuration, enable dual extrusion cable set and hardware, disable triple extrusion cable set and associated hardware.

I have a few hundred more parts that go into this iAssembly and I have 240 different build configurations. I will surely make mistakes having to manually enable and disable all the parts individually, especially since the names in the table cannot be changed.

[IgorMir]

Sounds like you are looking for the "Just do it" button in the software. Sorry - can't help you on this one.

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@Anonymous wrote:

Unfortunately, That is exactly what I DO NOT want to do. When I add the proper assembly and hardware. I end up with hundreds of options that I have to enable or disable that are not important to the configuration. I want simple main choices based on the iAssemblies and I want the hardware and associated parts to automatically enable or disable based on the selection that I choose from the iAssembly table. iLogic should be able to do this, I am just not sure how because it is a more advanced process.

The work flow should be this:

When I select dual extrusion configuration, enable dual extrusion cable set and hardware, disable triple extrusion cable set and associated hardware.

I have a few hundred more parts that go into this iAssembly and I have 240 different build configurations. I will surely make mistakes having to manually enable and disable all the parts individually, especially since the names in the table cannot be changed.

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[Anonymous]

I wouldn't call using iLogic a "just do it button". Isn't the whole point of iLogic to automate certain things? What is the point of having configurations and tables, if 200 entries on that table are screws?