creating multiple multibody parts from a single multibody part

[mjc_design]

Hi, need some advise on the above.

I have a multibody part, that i want to break off into several multibody parts.

If i create components i will end up with 70 individuals parts, when i really just want around a dozen multibody parts.

I could break off the bits one at a time into a new assembly, with every subsequent multibody part into the same assembly.

But will i have to do some re-building afterwards, or will the subsequent parts be grounded in the correct position?

Thanks

[admaiora]

Once you have your 70 parts assembly, after creating views representations, can you  create shrinkwraps with multibody style active?

[mjc_design]

Do you mean simplify?

I created my assembly containing 70 parts, and i can view rep and then simplify a number of parts together. It asks me to save the assembly and all the parts before i can do this which i don't want to do. I don't want to fill the folder with all these parts files, which i will have to go and delete afterwards.

I think i am following correctly?

[admaiora]

I mean this

There are others ways that can be possibile, but (limited to the solutions i know) you will lose your associativity to master multibody part.

[mjc_design]

Creating shrinkwraps, would mean i have a bunch of separate ipts which i would then have to build back together in an assembly. Not something i really wanted to do.

I really like make part, just means i have to do this a number of times for each multibody part i want to create. But at least they appear in my new assembly grounded and in the correct position.

Would be nice if they could add the functionality to combine make part and make components, so you could make multiple parts into a target assembly.

I'm using 2015, maybe they already have with 2016?

Thanks for your help

[admaiora]

I get your point.

Have you tried a steps workflow.

Use Make Part tool for your first sub-multibody part, inserted in your Target-01.iam assembly

Then repeat the cycle with another sub-multibody part inserting this in the same Target-01.iam assembly

And so on.

[mjc_design]

Yes, this is what i am doing now. Its a bit long winded, but i guess it's the only way for now.

[SBix26]

No, no, no, this is easy to do.  Do not use Make Components, or Make Part.  Start a new part, then use the Derived Component tool and select the master part; now you can select any number of the solids in the master part to become part of your new part.  This is the same functionality that Make Components uses, it just doesn't present you with the detailed choices.

Hope this helps,

Sam B

Inventor Professional 2016 R3 SP1 Update 1
Vault Basic 2016 SP1
Windows 7 Enterprise 64-bit, SP1

[mjc_design]

Unfortunately this is kind of the wrong way round for what i want. I'm looking to 'push' solid bodies i have in one multibody part, into an assembly made of several multibody parts. Creating dervived parts as per your suggestion would mean i have put all the pieces together again in an assembly, rather than make part which grounds the parts in place for me as i create them.

Thanks anyway

[SBix26]

This is exactly the same process that Make Components/Make Part uses, you just have to perform the steps yourself since you want something that Make Part doesn't do in its process.  It really isn't difficult...

1. New Part
2. Derive Part (select bodies)
3. Save Part
4. Place Component in assembly
   Right click > Place Grounded at Origin

Yes, it's more clicking on your part, but really not very much, and it does exactly what you want.

Sam B

Inventor Professional 2016 R3 SP1 Update 1
Vault Basic 2016 SP1
Windows 7 Enterprise 64-bit, SP1

[Curtis_Waguespack · Accepted solution]

Hi mjc_design,

I might be confused, but If I understand the quesiton correctly give these steps a try:

• Use the Make Components tool to create your 12 parts, selecting only the 12 "base" solid bodies from the list of 70 solid bodies.
• Then in the new assembly that is generated from the Make Components tool, edit part number one.
• Select the derived node from the browser, and right click in and choose Edit Derived Part
• Then in the Derived Part dialog box, choose all of the other solid bodies you want to add to this part file.
• Repeat this for parts 2-12 as needed.

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

[SBix26]

@Curtis_Waguespack - brilliant, much easier than the full manual method!

Sam B

Inventor Professional 2016 R3 SP1 Update 1
Vault Basic 2016 SP1
Windows 7 Enterprise 64-bit, SP1

[mjc_design]

Brilliant, so simple! Thanks for this

[JBerns]

@Curtis_Waguespack,

I too have struggled on how to reuse a "part" in multiple places and orientations within the multibody.

I have tried using patterns and Direct Edit with limited success.

Would you have any samples that you can share or direct me to?

The Autodesk examples (that I have found) only have single occurrences in their multibody examples.

Thank you for your time and attention. I look forward to your reply.

Regards,

Jerry

[BDCollett]

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@JBerns wrote:

@Curtis_Waguespack,

I too have struggled on how to reuse a "part" in multiple places and orientations within the multibody.

I have tried using patterns and Direct Edit with limited success.

Would you have any samples that you can share or direct me to?

The Autodesk examples (that I have found) only have single occurrences in their multibody examples.

Thank you for your time and attention. I look forward to your reply.

Regards,

Jerry

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This seems like you are trying to use the multibody environment to do what you would in an assembly,

If the body is the same, why not just create the part and reorientate it at the assembly level?

If you need a representation in the multibody in order to create other features then pattern/mirror or at the worst case direct edit should work.

You can also Copy - Paste features which might be another method you could try.

Do you have an example of your specific workflow?

[johnsonshiue]

Hi Ben and Jerry,

This is just my personal opinion based on my own experience. Multi-Solid Body workflow is indeed convenient because it all all shape definition concentrated within a part without having to deal with component definition and structure.

However, it does have drawbacks.

1) It is not suitable for large assembly. You simply cannot design a large assembly (50k) using a part. The performance will be extremely poor.

2) Inventor does not support body occurrences. As a result, each body represents a unique part. Unless the target assembly contains all unique parts, reuse would be a must. But, bodies cannot be reused unfortunately.

It is best suited for smaller design, a lot of unique parts, no reuse or exchange of parts. And, you have total control over the design.

Instead of swapping out the same part (body), I would simply set the Part Number of those parts the same. On the BOM table, the parts will roll up.

Many thanks!

[BDCollett]

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@mjc_design wrote:

Hi, need some advise on the above.

I have a multibody part, that i want to break off into several multibody parts.

If i create components i will end up with 70 individuals parts, when i really just want around a dozen multibody parts.

I could break off the bits one at a time into a new assembly, with every subsequent multibody part into the same assembly.

But will i have to do some re-building afterwards, or will the subsequent parts be grounded in the correct position?

Thanks

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I agree with you when it comes to very large assemblies but there are still ways to deal with this. Using the Master part to not only make parts but use it to define locations of parts that will not be derived or even just have basic parameters or sketch features only derived from that master location.

So in the Master you might have the same body in several places. I would name the bodies for example (Wheel, Wheel_1(ref), Wheel_2(ref) etc. When creating component only "Wheel" would be actually made into a Wheel.ipt and then using that master to position the 4 copies in the correct place based on those reference bodies. 

If you have standard parts I might model them in the master as a surface and even derive in parameters to represent them so that they update if a standard component changes.

I have used this method to design rather large assemblies with not only unique parts but that contain a lot of standard reused components. Then using Copy-Design in Vault to make new versions.

[Curtis_Waguespack · Accepted solution]

Hi @JBerns ,

Here is a quick video of the workflow that was described in the solution post.

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

[Curtis_Waguespack · Accepted solution]

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@johnsonshiue wrote:

Hi Ben and Jerry,

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🙂

[BDCollett]

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@Curtis_Waguespack wrote:

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@johnsonshiue wrote:

Hi Ben and Jerry,

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🙂

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I was going to say I also had a craving for ice-cream with that reply 🙂