topic Re: Remove rigid body modes: When to Activate? in Fusion Design, Validate & Document Forum

Remove rigid body modes: When to Activate?

davidnfreeman — Wed, 21 Feb 2018 05:29:37 GMT

Hi,

I am trying to figure out how to simulate a shaft and sheave assembly. The force acting on the sheave is 9400N.

When the "remove rigid body modes" is activated the maximum stress on the part is 152 MPa. And with the "remove rigid body modes" de-activated the maximum stress on the part is 2050 Mpa. Any help understanding how to properly run this simulation will be most appreciated!

Also, I applied separated joints, is that the best choice for this simulation?

I haven't before shared a link on F360 so please let me know if there is any trouble opening the file written below.

http://a360.co/2GxNP7s

Thank you for any help,

David

Re: Remove rigid body modes: When to Activate?

Anonymous — Wed, 21 Feb 2018 13:53:25 GMT

You normally only remove rigid body modes when the part is not fully constrained. It shouldn't apply in your case as long as you've set up the simulation properly.

Re: Remove rigid body modes: When to Activate?

davidnfreeman — Wed, 21 Feb 2018 14:49:49 GMT

Thanks for your answer Seanathan,

I should have stated this clearly in the last post. The sheave and shaft are 'free' (degrees of freedom) because the contacts types are all separation.

I can see that the studies don't meet these criteria.

The model is fully unconstrained. That is, you have not applied any X, Y, or Z constraints to any portion of the model. In this case, the applied loads can be balanced or unbalanced.

The model is constrained, but all loads acting in the constrained direction or directions are balanced. For example, assume that the model is constrained against movement in the X direction. A force of 100 N is applied in the X direction. You must add an opposing force of 100 N in the -X direction so that the sum of forces in the X direction is zero. Loads acting in unconstrained directions may be balanced or unbalanced.

http://help.autodesk.com/view/fusion360/ENU/?guid=GUID-E34DCC0E-666C-429D-BBB6-BEFE40A7AE0C

I have run over thirty different simulations on this simple model and depending on setup have varied results, and I have no idea which results are most realistic. Also, I notice that the stress goes up with finer mesh. I have read about high-stress concentration in FEA but don't have the understanding to apply it usefully here.

It would be awesome if someone could show a procedure for realistically simulating this model and explain your interpretation of the results.

Thanks,
David

Re: Remove rigid body modes: When to Activate?

Anonymous — Wed, 21 Feb 2018 15:26:06 GMT

I'll try to take a look at your files when I get home tonight if it hasn't been answered and record a quick screencast discussing everything from the various aspects of the simulation process to results interpretation. Can you provide me with a little more details about the real world load case?

It's a steep learning curve, but it gets easier after youre over the hump.

Re: Remove rigid body modes: When to Activate?

davidnfreeman — Wed, 21 Feb 2018 23:04:27 GMT

Hi, I am in Australia so took a while to reply.

The real world case is a crane head Sheave. Of all the sheaves on the crane, this is the sheave with the greatest distance between supports (between bushings also referred to as bosses). The wire rope has 6520N (665kg) tension and changes the angle by 88 degrees, therefore the resultant force is ~9400N.

The bushings are welded to the head of the crane boom on 3mm 700mpa steel. The flange is centred on the bushings and welded on the outer side.

Thank you very much for taking a look.

Re: Remove rigid body modes: When to Activate?

Anonymous — Thu, 22 Feb 2018 04:41:33 GMT

I'm still waiting on this simulation to finish the solve (it's been running for almost an hour now), so I won't be able to get to a video tonight. But I do have some comments that should help you out.

With sharp corners, and the initial mesh set to 8%, you are going to get a stress singularity at the sharp corner in the contact region. This stress is not realistic and is probably unstable. Did you ever get convergence with this simulation?
Separation contacts are not necessarily wrong in this case (if I understand correctly that bushings are plain bearings), but they would most likely have a friction component and I don't believe they are necessary. I also don't quite understand what holds the sheave in place axially. Is it welded to the shaft?

The simulation I am running has small radii on the bushings to get rid of the sharp corner singularity, rough contacts and a very refined mesh in local contact regions. I'll let you know when it's done.

When it comes to contact regions and stress risers, there are a few ways to handle it.

If you know the design and setup well enough to know it's either a singularity or a non-issuse...it's common to simply ignore it. I do this frequently on parts that I've tested in other assemblies...and especially when the high contact stresses are still not the lowest safety margin area.
Create a very refined and detailed mesh in the contact region with small radii to eliminate the sharp corner singularity
Suppress the bushing and represent it with a different type of constraint. This isn't always available however.

Thanks,

Sean

Re: Remove rigid body modes: When to Activate?

davidnfreeman — Thu, 22 Feb 2018 06:20:29 GMT

I am surprised the simulation is running for a whole hour. The simulations of this model I ran were <5 minutes with mesh refinement set at high; I wonder how oversimplified the simulations I ran were.

I have had no convergence with the simulations. The Von Mises convergence rate was >35%.

Axially the sheave is held in place by spacers such as thin-walled steel tube. The shaft, in reality, is constrained in the bushings from spinning by a flat section on one end of the shaft corresponding to a flat on the bushing. The shaft is also constrained axially by cotter pins or circlips.

I like your suggestion of using rough contacts, 'so they can separate from each other, however, while in contact, they cannot slide relative to each other.' Source http://help.autodesk.com/view/fusion360/ENU/?guid=GUID-B43E60CD-1859-4A09-9AD4-394525DAA2D7

In Fusion how do you make manually "very refined mesh in local contact regions"? Or is this automatic with 'adaptive mesh refinement'?

Thanks,

David

Re: Remove rigid body modes: When to Activate?

Anonymous — Thu, 22 Feb 2018 18:34:17 GMT

There's a feature in fusion 360 called "local mesh refinement".

To apply it to a very limited region, I always use split faces because f360 does have a contact refinement or sphere of influence option like ANSYS.

I'll include an explanation of this in the video tonight (Texas time).

When you say mesh refinement set to high, what do you consider high? The files I opened were set to 8% I believe which would not be considered a fine mesh.

Re: Remove rigid body modes: When to Activate?

Anonymous — Fri, 23 Feb 2018 05:05:46 GMT

I've done a quick video on local refinements. I had another issue retreiving the results from the Cloud solve so I've had to start it all over again...it's taking 2-3 hours to solve for some reason. I have no clue why it's taking so long because it is not that high of an element count. I'll post another video with the results when it solves...and there's no guarantee it will converge on this one but I will at least talk through how you can identify artificially high stresses if that is the case.

Let me know if any of that is not clear.

Thanks,

Sean

Re: Remove rigid body modes: When to Activate?

davidnfreeman — Fri, 23 Feb 2018 05:20:45 GMT

Hi Sean,

That is hugely helpful! It really cleared a lot of questions up. I am looking forward to seeing your results video!

Thanks,
David

Re: Remove rigid body modes: When to Activate?

Anonymous — Mon, 26 Feb 2018 04:54:11 GMT

@davidnfreeman,

Sorry for the delay, I've been pretty busy over the weekend. I've put together a quick video to discuss my observations. A few quick notes:

-The rough contact actually does cause a little bit of an artificial peak in some regions...you will see what I'm talking about in the video

-The contact refinements are certainly helping to better calculate stresses in the contact region

-Sliding contacts may actually be a better option after all as long as the model is stabilized. Again, you will see what I mean in the video when I say stabilized. If you want to run sliding on all contacts then you may need a frictionless constraint on one end of the shaft.

Also, I use the terms frictionless and sliding interchangeably when it comes to contacts. Sorry about this, it's because ANSYS, Solidworks and F360 all have slightly different terms for them and I spend much more time in ANSYS.

Please let me know if this doesn't help!

Re: Remove rigid body modes: When to Activate?

davidnfreeman — Mon, 26 Feb 2018 06:51:11 GMT

Very helpful explanation! Your comments in the video relating the simulation to the real world were also very useful.

One question based on a statement that may not be relevant to this simulation. The following statement was actually on the page describing 'remove rigid body mode'.

"The springs account for slight imbalances that remain due to imperfect numerical balancing of the loads and acceleration forces"

So could 'imperfect numerical balancing' create an unrealistic moment force on the sheave? And with sliding contacts could the sheave potentially start rotating, resulting in high displacement and possibly also causing unrealistic stress results?

If you happen to know of an article on how forces are applied to the mesh that may be the gap (probably one of many gaps) in my understanding that makes me ask the above question?

http://help.autodesk.com/view/fusion360/ENU/?guid=GUID-E34DCC0E-666C-429D-BBB6-BEFE40A7AE0C

Thank you, Sean for your great answers.