How to use single sheet metal part in many different assemblies?

[Anonymous]

Hi everybody!

I'm trying to figure out how to use one sheet metal part in few different assemblies.

Something like content center made for parts.

Main idea is to use one sheet metal part, as if I have to change something in original part (like adding extra flange or hole), I want it to make changes in all assemblies.

Second point is that every assembly have different parameters etc. length, width, or height, and part should read parameters of specific assembly.

This concept should help me save server disc capacity, and make it easier to manage all assemblies that are in need for redesigning.

Hope somebody has something useful or complete solution!

Feel free to ask if you need any more info.

Thanks!

[Rob67ert]

Why not make a template of the part?

[mcgyvr · Accepted solution]

I think you want iparts

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

That allows one "master" file (called the factory) to be used to create many similar versions (called members)

It still creates a file for each member..  Changes to the "master" will effect all the "members" and a single file (and ipart table) is used to manage them all

But to "save server space" should NEVER be a reason to do anything a particular way in Inventor.. Server space is CHEAP.. If thats a concern you have bigger problems..

[Anonymous]

You know @mcgyvr.... I may not know the answers to many of the questions here, but the few I do know, you always beat me to them. I need to be quicker.

[Anonymous]

mcgyvr ,

thank you for your replay. It was very helpful!

Still, I have some doubts about linking parameters to i Parts.

1. My main idea was to create stable assemblies of all our models, and use width, length and height to manipulate with dimensions.

2. And if I have to make some dimension that I haven't done before, just type those parameters and viola, there it is! AND I HAVE DONE ALL OF THIS!

But if I understood this i Part correctly, I have to make table of those dimensions inside every i Part, and then just "call" it inside desired assembly.

If you can catch me, my idea is to have many and many parameterised assemblies, and make some slight adjustment on part to effect all assemblies.

That brings us to i Parts + linking parameters of Assemblies.

Forget about disc space, that was just some random thought that I wrote.

[Anonymous]

https://www.youtube.com/watch?v=KSifiDVU7a4

this guy was on a good trail, but at the end, still not exactly what I was looking for.

Instead of manualy typing dimensions, I want it to be done by parameters source.

[Sofia.Xanthopoulou]

Hi @Anonymous,

your original question " How to use single sheet metal part in many different assemblies? " has been answered in post no. 3. Please be so kind and mark it as accepted solution, so other readers can benefit from this, too.

As for your question about the parameters I'd like to ask you to open a new thread. It would be a pity for such a good question to get lost under the wrong title. 

Thank you for your understanding

Best regards

[Curtis_Waguespack]

---

@Anonymous wrote:

...But if I understood this i Part correctly, I have to make table of those dimensions inside every i Part, and then just "call" it inside desired assembly.

---

Hi marin,

You can create Custom Parameter Columns in you iPart that allow you to enter a unique value at the time of placement. So (from memory) you should be able to right click on the iPart in the assembly and use the Change Component option to swap the component out with a new custom size that gets created right then.

http://help.autodesk.com/view/INVNTOR/2015/ENU/?guid=GUID-B7820955-D0F8-478A-8965-64ACD5CA0B54

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

[Anonymous]

I see that, but  problem is that I have hundreds of similar assemblies and I'm not goin to make hundred assemblies, I will use parameters and pack and go command, then when I have full database of assemblies, i want to be able to make a cut at (for example) part11.ipt ,  and to apply it to all hundred or whatever assemblies whereever is part11.ipt .

I hope you get me now.

Sorry but non of posts were answer to my question so far, so I'm starting to think it's not possible.

[Sofia.Xanthopoulou]

Hi @Anonymous,

I think we have a mess here... jumping from one question to the other  and honestly I have lost track ...

Let's take it step by step:

1. "Main idea is to use one sheet metal part, as if I have to change something in original part (like adding extra flange or hole), I want it to make changes in all assemblies."

- The answer to this is iParts - do we agree on this?

2. "Second point is that every assembly have different parameters etc. length, width, or height, and part should read parameters of specific assembly."

- The answer to this is iAssemblies - agreed?

3. The end of post 3 says : "Instead of manually typing dimensions, I want it to be done by parameters source."

- The answer is Post 8 - right?

Fact is, that every part/assembly in Inventor has to be unique. You cannot have one part in various assemblies, changing sizes. That is only possible with iparts - you keep the base part and create "children" depending on the base but being able to be manipulated by parameters - but - it is a separate part which will need it's space. The same concept applies to iAssemblies. 

It might not be what you were hoping for, but this is the answer to your question(s) - this is how far Inventor can go.

Unfortunately we do not have solutions for everything  

@Anonymous, for future question I'd like to ask you to try to have one question per thread and you will receive one clear answer (good or bad). This will help other readers to keep things apart and good questions don't get lost underneath "wrong" titles.

Thank you very much for posting in this community.

I am looking forward to your next posts 

Regards

[kpyoung333]

Have you ever tried using derive component with linked parameters? I used to do this for designing doors where someone would measure the LxWxD of the jamb and I would enter it into the iLogic Form for user parameters. This would update the frame and then everything else was derived off that so the casings, screen, glass, etc would update to the desired size. Additional features were added to make bottom kick plates, upper transom area, sidelights, all driven by a main Form on the base component. This bypassed any iPart or iAssembly and worked well in creating custom parts with similar constraints. Then used the Vault to copy the design and change so we could have a record and put new customer info to it. I think Curtis posted a snippet somewhere to put the Form from the base part on the top assembly but that is way farther down the line. Attached (2016) is a general example to show you what I mean. Look at the Form on Part1 and the linked parameters on other Parts. Doesn't seem many people design this way but maybe my crazy ways will help you figure something out.