***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
(OP)
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
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





RE: ***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
www.invariantlabs.com
RE: ***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
/Stig
RE: ***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
Tata but not yet tara
RE: ***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
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
RE: ***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
RE: ***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
Tata but not yet tara
RE: ***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
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
RE: ***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
Tara
RE: ***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
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
RE: ***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
RE: ***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
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
RE: ***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
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.
RE: ***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
Tara
RE: ***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
Stig
RE: ***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
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
RE: ***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
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
RE: ***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
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
RE: ***WARNING: EXCESSIVE DISTORTION AT A TOTAL OF 97 INTEGRATION POINTS
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