×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Mesh Convergence Issue

Mesh Convergence Issue

Mesh Convergence Issue

(OP)
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.

RE: Mesh Convergence Issue

(OP)
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.

RE: Mesh Convergence Issue

How about posting some pictures ?

RE: Mesh Convergence Issue

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

RE: Mesh Convergence Issue

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.
 

RE: Mesh Convergence Issue

(OP)
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.

RE: Mesh Convergence Issue

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

RE: Mesh Convergence Issue

"coarse"

RE: Mesh Convergence Issue

Of course!

RE: Mesh Convergence Issue

(OP)
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.

RE: Mesh Convergence Issue

(OP)
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.

RE: Mesh Convergence Issue

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.

RE: Mesh Convergence Issue

(OP)
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.

RE: Mesh Convergence Issue

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?

RE: Mesh Convergence Issue

(OP)
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.  

RE: Mesh Convergence Issue

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

RE: Mesh Convergence Issue

(OP)
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.  

RE: Mesh Convergence Issue

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

www.engtran.com
niswug.org
 

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources