Incorrect Inventor weight after sweep and shell

[Anonymous]

I have a strange issue that i can't explain so i'm reaching out to all my Autodesk friends to help me out and try to solve this problem 😉 (Or give an answer)

In attachment i have a piece of duct (Inventor 2015) that a colleague of me is designing.

At a certain point in time he's creating the second part of his duct and the weight isn't correct or adapted, after you shell the duct.

It should be more or less around 20Tons.

Does anyone have an idea how this can happen?

Just move the "EOP" up and down to see the implication.

Thanks in advance!

[mcgyvr]

Can you give us a hint for those that don't design 20 ton duct work at what specifically is wrong with the weight?

I see 19925 kg prior to moving the EOP and 23639kg after pulling the EOP all the way down..

[Anonymous]

Well that's probably the odd part ... I have a weight of 240.000 kg (240 Tons).

So i really don't know what is happening here ...

[mcgyvr]

[Anonymous]

Do you have any idea how it can be that you and me have different weights with the same part?

Is there anyway to solve my problem?

I never have experienced this ...

[swalton]

I don't have IV 2015, so I can't check, but will this part fit in a 100 meter cube?  Inventor may have issues for parts that execed this size.

[Anonymous]

The duct dimension is approx. 25m by 15m by 13m. I don't think that could be the problem ...

I have designed ducts that are bigger then this and i never had the problem.

We have our own seperate Design Data with our own Materials in it, but it never did anything out of the ordinary (We're working with quiet some time now) ... All of our colleagues have the same results.

[mcgyvr]

Is your version of Inventor up to date with any service packs/updates?

I'm using 2016 BTW..

[Anonymous]

I think so ... at the moment it is :

Let me check if it's the latest.

[hossaiy · Accepted solution]

Hi,

this is due to a bug that existed in 2015 but has since been fixed in later versions. I have attached a video below to show how to work-around it;

After employing this work-around, there are downstream issues starting from "Rectabgular Pattern 1" which looks odd but i think you'll be able to rectify that fairly easily, if not let me know and i'll look into it further.

Hope it helps & sorry for the inconvenience.

Thanks,

Yacoub Hossain

[hossaiy]

Hi,

I carried on looking at the part and noticed there was still something wrong, but i fixed it by exploying the same work around as shown previously. I have attached a part file this time (created using 2015 + sp2) which appears to be working as expected now. Let me know if i missed anything.

Hope it helps.

Thanks,

Yacoub Hossain

[Anonymous]

Thanks Hossaiy!

Can you specify what the actual bug is since we are designing ducts on a regular bases ... ? Since you split the duct i recon it has something to do with shelling bends or elbows?

[hossaiy]

Hi Q-Bixx,

Sure, the the issue is related to the shelled elbows (or the torus faces of the duct). With this particular issue, the massprop function has trouble dealing with certain torus faces (elbows) and as a result it results incorrect massprop values (not sure yet exactly what trips it up but shelled, partial torus faces appears to be key).

Splitting the torus faces appears to change things enough (without changing the actual shape) for the massprop function to avoid hitting the problem. It is restricted to torus faces. So if you do notice odd massprop values again you can probably work-around it simply by splitting any of the torus faces in the duct model and then check the massprop value again. If that doesn't work, feel free to send me an ipt to take a look, at the  following address,"yacoub.hossain@autodesk.com".

If it helps, here is a short video showing a slightly easier/quicker way of splitting the torus faces, than what i showed previously;

Hope that answers your question.

Thanks

Yacoub Hossain