Mesh Convergence Issue

[jrw501]

Hello, I'm new to FEA/FEM and was wondering if anyone has encountered the following problem with mesh density sensitivity before:

For some background, I'm using ABAQUS to model seismic isolation bearings to determine stability/critical behavior at various displacement levels.

Anyway, I've created 3 mesh sizes: a coarse mesh with roughly 3000 elements, a medium mesh with roughly 18000, and a fine mesh with roughly 72000 elements. The models have resulted in the solution from the fine mesh being somewhere in between the solutions of the coarse and medium, i.e. the solutions are not asymptotically approaching some value like I've seen in most literature (not on this subject, but in general). Is this "oscillation" of results indicative of something typical (such as accumulation of error from a mesh that's "too fine") -- does anyone have any suggestions or insight? I can provide more information regarding the model if needed.

Thanks in advance.

 

[jrw501]

In case this is helpful, I probably should've added that the results from the medium mesh are about 10% smaller than the fine mesh, and the results of the coarse are about 10-15% larger than the fine mesh.

I guess another question I had was should I just invest time in creating a 4th mesh somewhere in between the current medium and fine (or perhaps beyond the fine mesh).

Thanks again.

 

[johnhors]

How about posting some pictures ?

 

[prex]

You should specify what kind of elements are you using (2D, 3D) and what is the stress level you are using to compare the results. Is this a local peak level or some general stress across a section in the model?
In the former case, the mesh refinement could be involved, but the interest in it could be minor; in the latter, with so much difference in an undisturbed portion of the model, there would be serious worries as to the validity of your approach.
I would use one model only, not certainly a fourth one, to be satisfied of the general distribution of stresses before going on, then a second model to analyze changes, mainly whether they are generalized or only local.

prex

http://www.xcalcs.com

: Online engineering calculations

http://www.megamag.it

: Magnetic brakes and launchers for fun rides

http://www.levitans.com

: Air bearing pads

 

[ColonelSanders83]

You should also specify if the stresses you are witnessing are all in the same local area or if they are jumping around in your model.

It is also important to ask if you are looking at stresses from averaged elements. Generally speaking the difference in stress between fully averaged and no averaging in an element should not fluctuate more then %5 for a refined mesh.

 

[jrw501]

I'm using C3D8H and C3D8I elements (3D solid elements) -- the bearings are composite elements of steel and rubber, the steel is using the incompatible modes, the rubber is using the hybrid formulation since it's nearly incompressible. The criteria being used to determine instability is when the horizontal stiffness (=shear force/lateral displacement) becomes negative (so we're not too concerned with particular stresses). Perhaps I should be looking at some element stresses to see why we are getting different results though. I'll post some pictures momentarily.

 

[jrw501]

b1: medium mesh elevation
b2: medium mesh results
b3: fine mesh perspective

The main difference between the meshes is the number of elements radially and the bias of each element outward to maintain an aspect ratio of approximately unity.

 

[jrw501]

http://files.engineering.com/getfile.aspx?folder=2acc2d83-290f-41cf-ace2-3895617f41f9&file=b2.JPG

http://files.engineering.com/getfile.aspx?folder=af3092f0-8a03-4179-aff3-3849fcda3f46&file=b3.JPG

 

[crisb]

They all look course to me, but I dont really understand the problem. Have you tried:
b4: finer
b5: even finer?

 

[johnhors]

"coarse"

 

[crisb]

Of course!

 

[jrw501]

I suppose relative to some meshes these are somewhat coarse, but the "fine" mesh takes about 24-36 hours to run locally and the operation needs to be performed multiple times for each mesh size. As far as what's being done, the bearing is being shear under constant axial load -- at some point the bearing's (only modeled in half space for efficiency) horizontal stiffness (the slope of the horizontal force-displacement curve) goes to 0 which is denoted as the critical displacement for a given axial load. We do this for multiple axial load levels and plot the axial load - critical displacement curves so we can start to see when the bearing becomes unstable for a given load.

 

[jrw501]

I meant to add that it is these locations of critical displacements that are varying for each mesh size. So under axial load X, I get critical displacements a, b, and c for the various mesh sizes where a~1.1c and c~1.1b.

 

[crisb]

Second order elements would probably give better results than the 8 node bricks you appear to be using. However if you are having problems running a model with 72000 elements then it may not be an option. Why is it taking so long to run, 72000 elements should be a very modest model to run.

 

[jrw501]

I would guess part of the reason it takes so long to run is that the problem becomes numerically difficult to solve as the horizontal stiffness starts approaching 0. I'm not using any really high performance computers either. I was tending away from 2nd order elements because some of the elements are undergoing appreciable distortion and I've read that first order elements give better results when this is the case. The coarse mesh runs in about 2-5 minutes and the medium mesh runs in about 2 hours.

 

[crisb]

Just out of interest how are you applying the shear load. Is it applied as a pressure, or prescribed displacement? Displacement loading is sometimes better for "collapse" type analysis. Also I haven't understood how you are applying symmetry, as the plane of symmetry appears to be distorting?

 

[jrw501]

The shear load is being applied as a prescribed displacement as you guessed. The real bearing is circular (annular), but only half of the bearing has been modeled (which is probably most easily seen in the 3rd image when looking at the top) to reduce the number of elements. The plane of symmetry is a vertical plane when looking at the elevation.

 

[ktop]

The aspect ratio of the elements near the OD is pretty bad. You can see it in the behavior of the elements near the bottom turning inside out. You might want to try meshing it so that all the "rubber" elements are roughly the same size.

KTOP

 

[jrw501]

That's a good point, I'll try fixing the elevation aspect ratio. I actually think I may be starting to observe convergence similar to what is seen in the displacement-mesh density graph shown here:

http://machinedesign.com/article/converging-on-an-accurate-solution-0413.

I'm going to give a better look at convergence of stresses to anticipated values, a denser mesh, and the point you bring up KTOP.

Thanks.

 

[kellnerp]

Here is a little something that shows how you might manually create a more even mesh on a cylinder. This will allow you to have better control over aspect ratio. This is quite a bit more work than what you have started with, but may help with results. Enjoy.

Meshing a Cylinder

TOP

TOP

http://www.engtran.com

niswug.org