Multibody Parts: How to deal with multiple Part/Sub-assembly Instances

[DRoam]

What do you do when you have multiple instances of a single part, or even multiple instances of what will eventually become a sub-assembly, within a multi-body part?

Take a look at the example below. This is just part of a larger assembly that I created from a multi-body part.

How in the world could I create this using multi-body techniques but still have a proper BOM at the end?

I'm curious if anyone's come up with a good solution for this. I can only think of three options:

Option 1: Pattern/mirror bodies to create all repeated instances in the multi-body and then push them out into the assembly; demote the parts for each occurrence of a sub-assembly into a new sub-assembly file. Everything will look great, but your BOM will be screwed up because each instance of the same sub-assembly/part will be its own assembly/part file rather than an additional instance of the original.

Option 2: Only model one instance of any recurring parts in the multi-body and push that one instance into the assembly, then manually constrain additional instances. But then you completely lose the quick, simple, and robust functionality that you came to multi-body for in the first place.

Option 3: Create the multi-instance parts/sub-assemblies separately. But this only works if the parts are simple enough to be modeled independently; sometimes your reason for using multi-body is the parts are too intricately inter-related to be modeled separately. Plus, even if you could model them independently, you would then need to constrain them, eliminating the other advantages to multi-body (ease/speed/robustness).

So, has anyone come up with an ingenious method for re-using parts/sub-assemblies from multi-body parts? If so I'd love to hear it!

[SBix26]

Not sure I understand the problem with your option 2.  That is how I normally model things, and it has always been "quick, simple, and robust" for me.  Why isn't it for you, I wonder?

Sam B

Inventor Professional 2017.3
Vault Basic 2017.0.1
Windows 7 Enterprise 64-bit, SP1
Inventor Certified Professional

[WHolzwarth]

Can you upload your sample files for testing?

[mcgyvr]

Following along..

I was playing around with multi-body solids the other day and had the same question (just didn't post about it)..

[DRoam]

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@SBix26 wrote:

Not sure I understand the problem with your option 2.  That is how I normally model things, and it has always been "quick, simple, and robust" for me.  Why isn't it for you, I wonder?

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In some situations, it is very quick, simple, and robust. For example the blue plate would probably be very quick, simple, and robust to just copy, paste an additional instance, constrain the XY and YZ planes flush, then constrain the Y direction using actual part face geometry.

But what about the green gussets? Those are at odd angles and two of them are mirrors, so they would likely require 3 face-to-face constraints each to constrain, and lots of those constraints would need offsets which I would need to make sure are linked parametrically and keep up with making sure they stay linked. And if the geometry of the gussets, or what they're constrained to, happened to change, they would all become sick and I'd have to repair them. You can see, I'm quickly losing "quick, simple, and robust".

[SBix26]

Most of what I design is screwed together, so I normally constrain things by holes, and since the holes are all created in the master part, they always line up properly.  

If I were welding things together, I might put some work geometry or sketches in the master and derive those into some of the parts to give a reliable constraint partner for the additional instances.

Sam B

Inventor Professional 2017.3
Vault Basic 2017.0.1
Windows 7 Enterprise 64-bit, SP1
Inventor Certified Professional

[Curtis_Waguespack]

Hi DRoam,

It depends...

Sometimes I would do this with option 2. So the Blue, Red and Green parts would be a one multibody part, I'd then push that out as a subassembly, and then place and constrain the subassembly 2x as needed in a top level assembly. Then I might create a new part in the assembly, use the Copy Object tool to pull the 2 sub assemblies down as work surfaces, and then create the geometry for the gray part using those work surfaces

Other times (such as when the gray part is actually more than one parts and they have geometry that is based on the other parts) I might mirror the Blue, Red and Green parts in the multibody part and then create the gray part(s), but then only push out 1 copy of the Blue, Red and Green parts as a subassembly, then push out the gray parts to a new assembly as a 2nd Make Components operation, then place and constrain the subassembly in that assembly 2x as needed.

And then still other times I'd push out the part, edit the resulting derived part and include more solid bodies as described here:

http://forums.autodesk.com/t5/inventor-forum/creating-multiple-multibody-parts-from-a-single-multibo...

And then also....

For parts like those red parts that have holes and features that are secondary do not relate to the "fit" of the interrelated parts, what I prefer to do is reserve those features and not put those in the multibody, but instead push out the part and create those features in the resulting derived part. This keeps the multibody less complicated and more "nimble".

Very generally speaking I prefer not to try to load he multibody with lots and lots of parts, but instead only those parts that have "fit" geometry or are driven from a common set of parameters. The common parameters situation is where I see a lot of benefit from multibodies.

And then there are setups like this simple example has one multibody part that is then derived into other part of the assembly, and serves as the "master", which allows us to piggy back off the master geometry in a way that reduces the need of handing over parameters again and again.

Volume Assembly.zip ‏320 KB       

So, I don't know that I've cleared anything up here, but there are some options that might be worth knowing about, so that you can choose what works best, when it works best..

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