***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS 1

[Fabi0]

Hi

i'm working with the simulation of a back up roller bearing: the load had a nominal value and a max value:

Nominal = 205KN
Max= 650KN

The material has been characterized in elastic and plastic behaviour (Elastic-->E,poisson; Plastic-->isotropic, with 4 point of stress-strain curve).

I need to investigate phenom like ratcheting in the inner ring, so i need to undestand where material go over yield stress and how much.

The model has 4 static step (i believe static it's right, by reading abaqus documentation):
1- i get contact applying gravity to outer ring
2- i apply a small portion of nominal load and shut down the gravity
3- nominal load
4- max load

After a lot of singularity problems (i have a lot of contact even if i've used simmetry) solved by use of CONTACT CONTROL, AUTOMATIC TOLERANCE and DAMPING FACTOR over the whole model (not CONTACT CONTROL, AUTOMATIC STABILIZATION), now i'm dealing with another problem:

***WARNING: THE STRAIN INCREMENT HAS EXCEEDED FIFTY TIMES THE STRAIN TO CAUSE FIRST YIELD AT 65 POINTS
***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS IN SOLID (CONTINUUM) ELEMENTS
***NOTE: ELEMENTS ARE DISTORTING EXCESSIVELY. CONVERGENCE IS JUDGED UNLIKELY.
***NOTE: SEVERE CONTACT OVERCLOSURES EXIST. CONVERGENCE IS JUDGED UNLIKELY.

It'e my first analysis that take in plasticity, so i'm completely out of ideas about how solve this problem.

Maybe i need to use Kinematic in Plastic definition of material?
Should i use less coarse mesh? (but contact work right, in elastic behaviour)

I've read about remeshing, but my mesh uses HEX element, so no remeshing...

Fabi0

 

[InvariantL]

When I get these multiple problems, usually my mistake is that I haven't been careful in entering the data for the yield point and plastic properties of the material. I would double check it and make sure you didn't use the wrong units, omit a factor of 10, etc. These errors can make the material extremely soft such that it can't support any stress without deforming excessively.

http://www.invariantlabs.com

 

[portliner]

Use full-integration HEX-elements in the contact areas. Make a test and apply a given displacement instead of a given force.

/Stig

 

[corus]

Use linear elements, C3D8. The quadratic elements are a waste of time as they rarely work. For your first step use a fixed displacement rather than gravity to get contact, but make sure everyting remains in the elastic domain. Your 2nd step is a waste of time as the 3rd step will apply only a proportion of the load if it's ramped on and you use a small time step.

Tata but not yet tara

 

[Fabi0]

You're right, i've ereased second and third step.

The problem is that i've a lot of element, and to keep them to a reasonable number, i have to use some "very stretched" element near contact zone (square face side =0.1; non square face side=0.5).
With hex elements i can't do better, if i do refine mesh again the computational time will be too long (more than 800K elements right now).

I prefer use hex than tet in hertz contact, so the only things i believe could solve problem is ALE remeshing....

Fabi0

 

[Fabi0]

One more picture

 

[corus]

As a first step to the problem I'd assume plane strain and model it in 2D. This will give you results that represent the centre of all the regions. From these results you may be able to simplify the 3D problem to a sub region to which you can apply symmetry restraints to represent the whole body.

Tata but not yet tara

 

[Fabi0]

Do you mean submodeling?
Because the model i posted is the result of the application of two symmetry planes on the whole bearing: the model is so 1/4 of the bearing...i can't apply more symmetry cut off, there's no more.

Fabi0

 

[corus]

To me it looks like you've taken 180 degrees of the whole structure. In fact you have a series of rollers for which symmetry could apply around each half of a roller. This would considerably cut down the size of the model if you just took one half segment. This is assuming there isn't something else that adds asymmetry to it all, but I can't see it.

Tara

 

[Fabi0]

Yes i've take 180° of the structure: the deformation of the bearings is no more symmetric, 90° up has a different deformation than 90° down.

So you mean that i could apply another symmetry not on the whole model but on the single rolles?
As a matter of fact, i've costrained the middle plane of each roller to move only in radial direction....so, if i understanded what you told me, i've only to remove an half from each roller. But in this way i consider a wrong roller stiffness.
Excuse me if i've understood, but i really can't get your point about symmetry and the relationship with 2d analysys

Fabi0

 

[Fabi0]

By the way: yes, i've took 180° of the bearing original 360°. But i've also took L/2, where L is bearing lenght.

 

[corus]

Unless your loads are not symmetric then I can't see why your displacements differ. The bearings appear to be placed evenly around the circumference and as you suggest will displace radially (along a plane passing through their centreline).If that is the case then you could take the radial line (from the centre of the whole structure) from one bearing to the radial line to the adjacent one, and apply symmetry restraints, ie. there is no cirucmferential displacement along those planes. Taking it further the results will be symmetric about the plane between the two radial planes, so you could apply symmetry there too.

I don't know how many bearings there are, but say for example there were 24 bearings, then your model will be 360/48 degrees of the whole structure.

For all cases use L/2 for the length and apply symmetry on that plane too, as you have done.

Tara

 

[Fabi0]

Ehm....probably it's my fault (my english is not so good), but what you see in the picture is ONE bearing.

The cilinder are the roller between the inner and the outer ring.
So i need to investigate how outer rings deflect under a (single) radial load, and how roller bring that load to the inner ring (it's full because is a sort of shaft) because there are problem on the inner ring, caused by an high radial load.

Maybe a Cinema4D render of the bearing may help

Tell me if i've again misunderstand your idea or if you believe that the cilinder are the bearing.

By the way, thx a lot for your support!!

Fabi0

PS: in the render attached you will see the baering without the outer ring, so you can see the four row of rollers. Axially there's no problem, so i've erased from model all axial rollers, and all the cage, grease provider and so on. What you see in the .cae model is an half (180°) of two rows of roller, with a small portion of inner and outer ring.

 

[corus]

Other than the end block on the outside, the whole structure shows cyclic symmetry around each of the cylinders/bearings/whatever you want to czll them. I've sketched on to the picture the symmetry planes I refer to.

Tara

 

[portliner]

From the picture of the mesh the number of element could probably be reduced by using TETs in the regions outside the contact-zones. This will create a non-compatible mesh but give accurate results in the contact zones anyway.

Stig

 

[Fabi0]

Stig:
yes, infact that is the "next" method i'll apply if i can't obtain a solution, even if TETs generally make more elements than HEX...do you know if there's a way to have two different HEX mesh in the same part? Like if there is two part joined with TIE ?

Corus:
forgive my poor ability in understanding. I've get what you mean with simmetry, but to apply that i need to undestand how to costrain that plane: the only way i know to get a smart description of its behavior is to pass throught a submodeling, then getting a submodel drive boundary condition to that plane. Can you confirm that? Can i drive a 3d solid model by a 2d analysis?

Fabi0

 

[corus]

Don't use tet elements whatever you do. This will increase the number of elements and nodes in the model and the results from using tets are irregular at best.

You don't need sub modelling to apply symmetry. For the angled plane just define a local co-ordinate system to that plane and apply the standard symmetry condition in that co-ordinate system. For the opposing vertical plane just use the global co-ordinate system.

I'm not sure what you mean by a 2D analysis driving a 3D model in submodelling. It's not possible anyway. My suggestion was to use a 2D plane strain analysis which would give valid results for the bearing away from its free ends. You could use lots of elements then, and even include the full 360 degrees of the bearing, for what it'd be worth.

Tara

 

[Fabi0]

Thx again for your reply and time Corus. I wish to understand fem like you a day.

I know that I can apply symmetry to the angle plane by use of local co-ordinate sistem (like i did with rollers to give them only radial displacement).

The reason I suppose to need submodeling is that the radial force (P) is partitioned on the rollers (so i have some Pi --> P = sum (Pi*cos(angle_i) ), but how P is partitioned depends by outer ring deformation: probably i could use 2D model to calculate Pi, and then i can use the symmetry to the angled plane.

Fabi0

 

[corus]

I see now. You have a direct force acting in the X direction on the bearing and have decided to apply it in a sinusoidal pressure distribution around 180 degrees of the outer bearing so that the sum is equal to the nett force P, in that direction. You then are using symmetry for 180 degrees that includes half of the pressure distribution, whilst the remaining 90 degrees has no load. The whole thing must be restrained on the outer 'square' block. In that case the loading is asymmetric and everything I've said previously was bollocks, as we say.

I'd try and reduce the problem with some reasonable assumptions to make is simpler to model. The central region appears to be a solid block of material that will have negigible deformation. You could replace that by an analytical rigid surface and so only model the contact of the outer regions, restrained by contact with the rigid body. This will reduce the number of elements needed. In your initial run, use elastic properties to get the thing working. When that works, introduce your inelastic properties.

Alternatively, you could assume that the pressure distribution on the outer ring transfers its load as point loads on the inner set of rollers (as point contact is being made), in the same distribution. You then only need to model contact between the inner rollers and the central block, which you'd model using solid elements.



Tara