System requirement for half million parts assembly in Inventor

[Anonymous]

Hello everyone. i am looking for advices to purchase a computer to handle up to half million parts assembly in Autodesk Inventor. Any suggestion will be highly appreciated.

[mdavis22569]

You're asking a lot of any system ...

However if you must:

Intel® Core™ i7-6950X Processor Extreme Edition
(25M Cache, up to 3.50 GHz)
Monster m

128 gig of Crucial 128GB DDR4 2400 MHz LR-DIMM Memory Kit (4 x 32GB)

ASUS RAMPAGE V EDITION 10 LGA 2011-v3 Intel X99 SATA 6Gb/s USB 3.1 USB 3.0 Extended ATX Motherboards - Intel

2 GEFORCE 1080 video cards (with SLI set up) 

1 TB SSD

and a small generator to power it ...

you'll need 1000- 800w or better to be safe

[Anonymous]

Based on your comments, any idea how much this system cost?

Thanks.

[mdavis22569 · Accepted solution]

over 5k w/ window's, Box, monitor, key board

CPU is 1800 approx

Motherboard is 600 approx

Ram is 900

Video Cards 800 each ..so $1600 plus 40.00 for the SLI

Power Supply .. 150.00

1 TB SSD ... 500.00

plus tax, in US dollars.

Why do you have a 500K piece file?

[Anonymous]

Our product is green house buildings. A big project could have more than 500k parts. These parts include tons of nuts and bolts.in the past up to now we generate our BOM in excel. But we want to get the BOM done in Inventor, therefore we have to model up the green house in Inventor then we encounter problem with the computer. I talked to some tech from Inventor distributor, they couldn't find a solution for me. That's why I am here to get help.

[Curtis_Waguespack]

Hi newbiej,

There are different strategies to deal with this, but you'll want to attack this with a very planned use of sub assemblies ( likely with a phantom BOM designation), LODs, and maybe even virtual parts.

This will include some "outside of the box" approaches that the tech you spoke with might not be aware of.

As an example, if you derive your frame (or part of your frame) into a part file, set that part file to have a Reference BOM designation, then create a sub assembly with a phantom BOM designation, and place the derived frame part, you can then place all of your fasteners for this frame in a simplified assembly, rather than using the top level assembly, which requires more heavy lifting. The use of the phantom and reference BOM designations allows these extra files to "hide" from the BOM.

That's just an example, it might not apply to your stuff exactly, but I'm certain that a strategic approach (as apposed to everything in one giant assembly) can be used to get this done.

Also here's a related link:

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

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

[salariua]

Hi newbej,

I will be of little help here... just came in to give kudos to @Curtis_Waguespack but here's my answer on a different post regarding performance, speed, and large assemblies.

All the elements that need to move by driving the constraints or by changing the constraint value can and should still be located with constraints but the rest can be located with coordinated origin and grounded.

Another thing to consider are joints ! Although not ideal a single joint can replace 3 constraints so computing time for the position of occurrences is 3x faster.

Joints are not my favorite tool because they use faces and edges and this goes against my rule to constraint everything as much possible with the origin planes and features.

On a small list I would look at:

- Joints

- Have as many grounded components as possible

- Disable cross part file references

- Disable adaptive parts and features

- Suppress link on derived parts.

- Disable Flexible Assemblies.

I would also investigate the techniques in Large Assembly manual here:

Good Luck.

[swalton]

I deal with 5k-15k assemblies. 

• No Adaptivity
• No Bolted-Connections
• No Frame Generator
  • More of a workflow issue, than a performance issue
• Many sub-assemblies
• Fasteners in the lowest level possible
  • The hardware that attaches the sub to the top level assembly is in the sub, not the top
• Nested LODs that suppress components you "can't see from the highway"
• Substitute LODs can help, but it takes a bit to simplify a complex assembly into a simplified ipt file.
• Design Reps, not LODs in drawings
  • Copy the LODs to design reps when ready to start drawings

You might look into some iLogic button/command that grounds all components in an iam and suppresses all the constraints.  Make another another that reverses those conditions.  While in your sub-assembly, design and constrain as normal.  When the sub is complete, run the "grounding" code and place it in the top level.  If you need to edit the sub, run the "un-grounding" code and make your changes.

[Anonymous]

Thank you, your comments are very helpful to me. even i do all what you mentioned, i still need to look for a better computer to avoid crash during operation. after shrinkwrap all the subassembly the master assembly still huge. Thanks again.

[Curtis_Waguespack]

---

@Anonymous wrote:

... after shrinkwrap all the subassembly the master assembly still huge.

---

Hi newbiej,

Just be aware that if you're not employing LOD and some of the other methods mentioned above, then your shrinkwrap files could be larger than the assemblies.

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

[Anonymous]

thank you so much for your inputs.

[Anonymous]

anybody know any Inventor consultant?

[mdavis22569]

In what way ...

Where did you get your Inventor from?

Mike

[Anonymous]

some distributor from Ontario. But the Tech didn't recommand any system because he doesn't want to point me to the wrong direction.

[mdavis22569]

for how to do the large assembly?

Are there any ATC up your way to see about training and help?