How to correctly reuse sub-assemblies

[Jef_E]

Hello there.

I'm looking for the best modeling practice for our company. We have been using Autodesk Inventor for some years now, but we feel we aren't getting the most out of it. Maybe there are some "user related needs" that block the full potential or, we aren't using Inventor correctly ( or could be both ).

When modeling our browser tree looks a bit like this for example

- Main assembly

--- Sub-assembly [ a ]

--- Sub-assembly [ b ]

--- Sub-assembly [ c ]

--- Sub-assembly [ d ]

--- Sub-assembly [ e ]

But, when I tell you that c, d, e are identical object there is something wrong ( in my opinion ) we should not need to have 3 different assemblies for the same object.

What it should look like:

- Main assembly

--- Sub-assembly [ a ]

--- Sub-assembly [ b ]

--- Sub-assembly [ c ]

--- Sub-assembly [ c ]

--- Sub-assembly [ c ]

If we do this the result for the BOM would be

• 1x [ a ]
• 1x [ b ]
• 3x [ c ]

Looks good to me.

Now if we look to our product, it's a pressure vessel. Let's keep it very simple and name the object for the sub-assemblies

• [ a ] = Shell
• [ b ] = Manway
• [ c ] = Connection nozzle

What do we require for trace-ability when placing in the workshop : is that each sub-assembly can be ballooned with a unique indentifier.

The tag would look something like this:

• [ a ] = Shell
• [ b ] = MW
• [ c ] = {N1, N2, N3} <-- Here is a problem. Assembly [ c ] has only one iProperty that can be attached to the balloon and is for each nozzle the same.

With this problem in mind i'm back looking at the first example which allows me to balloon all sub-assemblies. But also forces me to split 3 perfectly the same items into 3 different assemblies ( not so fun ).

How is this best handeled in Inventor?

[Cadmanto]

Based on the example you outlined, the way I see it is you are correct in that you should not create three different assemblies of the exact same assembly.  It should be the same assembly inserted 3 different times.  Thus, your parts list would show a quantity of "3".  Now if there are slight differences, then there are a couple of different directions you could go.  You could either create an iassembly and have the table drive the differences or you could copy design the assembly renaming that different parts in the dialog window.  Like you know, with each design, comes different dirrectives and looks.

FYI, it would appear that this is more of a question to be posted in the Inventor forum, not the Vault forum.  Didn't see that you were even using Vault in your opening posting.

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[Jef_E]

---

FYI, it would appear that this is more of a question to be posted in the Inventor forum, not the Vault forum.  Didn't see that you were even using Vault in your opening posting.

---

Off topic : I think I am posting In the Inventor General Discussion board?

---

@Cadmanto wrote:

Based on the example you outlined, the way I see it is you are correct in that you should not create three different assemblies of the exact same assembly.  It should be the same assembly inserted 3 different times.  Thus, your parts list would show a quantity of "3".  Now if there are slight differences, then there are a couple of different directions you could go.  You could either create an iassembly and have the table drive the differences or you could copy design the assembly renaming that different parts in the dialog window.  Like you know, with each design, comes different dirrectives and looks.

---

On topic :But as I said in my opening post. I want 3x the same nozzle but I would like to see them named differently as I balloon them.

[swalton]

I don't work that way on my designs, but here is an idea:

Problem: Create a unique identifier for each instance of a common sub-assembly.

Solution: Use "placeholder" iam files to hold the unique identifier and a single instance of the common sub-assembly.

1. Create nozzle.iam with its components. 
2. Change the BOM settings for nozzle.iam to Phantom.
3. Create nozzle-instance-1.iam
4. Place nozzle.iam in nozzle-instance-1.iam
5. Add unique id info to nozzle-instance-1.iam
6. Repeat steps 3-5 as required.

This will give you a single CAD model of the nozzle that you can update and it will affect all nozzles in your design.  If you create individual drawings/partslists for each nozzle-instance.iam, you will see the components of nozzle.iam.  You will not see nozzle.iam as a sub of nozzle-instance.iam.

Another option would be iAssemblies or custom iParts

iAssemblies: http://help.autodesk.com/view/INVNTOR/2016/ENU/?guid=GUID-6E529299-CAB9-4F5C-B100-7901D877B83F

Take a look at the methods for adding new members.

Iparts: http://help.autodesk.com/view/INVNTOR/2016/ENU/?guid=GUID-9D7FF4CB-6045-4E2A-AC88-40A2F4DDF392

[Curtis_W]

Hi Jef_E,

What is missing it the ability to give each occurence an independent property. See this idea on the IdeaStation, and give it a vote:

http://forums.autodesk.com/t5/inventor-ideastation/occurrence-name-display-in-drawing/idc-p/6279429#...

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

[mpatchus]

Another possible option.???

Create derived parts from the nozzle assembly.  You could then give each item whatever properties you desire, but since they are derived, the models would update as the main nozzle assembly is updated.

[Cadmanto]

Oh, you are right, My bad!!! 

I was posting in the Vault forum and somehow thought I was still there.  Sorry!!!

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[Jef_E]

---

@Anonymous wrote:

Another possible option.???

Create derived parts from the nozzle assembly.  You could then give each item whatever properties you desire, but since they are derived, the models would update as the main nozzle assembly is updated.

---

I was going for that myself, but how would you handle the BOM? If I do this I get one line fore each nozzle in the BOM, but they exists from multiple parts.

Other thing I encountered is, what do you do for representations? When using derived assemblies, you can just switch the view or LOD representation?

What do you do when there is a single nozzle do you also derive it and then place it? because others are done that way too?