Difference in results with different type of mesh or dimensions of mesh

[gregorio.riva]

Hello,

I have some questions about how to choose a mesh instead of the other and how to be sure it is sufficiently fine.

I'm doing a Linear static simulation with linear material model.

I know that tet elements and brick elements should give almost the same results if they are sufficiently fine, specially if i choose the second order for the tets.

I wanted to do some tests to have the confirm about that, so i used the component you can see in the picture.
The red surface is constrained as fixed, the blue one is loaded with a perpendicular force. The red arrow points where i expect the maximum stress and where i actually get it.

I did several static linear simulations with exactly the same conditions and material, i just changed the kind of elements and the quality of the mesh. 

Bor both bricks and second order tets I used one 50% one 30% and one 20% dimension mesh (so 6 simulations).

The problem is that comparing bricks and tets simulations with the same mesh dimension i get every time much bigger stresses in the bricks one. Why is that?

And another problem is that as more i refine the mesh (for example using always brick elements) the more the stresses go up, I'm ok with that, but shouldn't the results reach a sort of convergence value at some time? It seems to me that the mesh needed to obtain that is extremely fine. So, how do i know when the mesh has the right quality for this kind of simulation?

Thanks everybody.

[John_Holtz · Accepted solution]

Hi @gregorio.riva

Here are some thoughts on your questions.

"I get every time much bigger stresses in the bricks one. Why is that?" That is a good question and observation. I do not know the answer . If you are comparing the same size elements, it could be that 1 mm brick elements and 1 mm tet elements do not have the same accuracy. It may also be related to stress concentrations; maybe one element type is more accurate or more sensitive to concentrations than the other.

"but shouldn't the results reach a sort of convergence value at some time?" The answer is yes and no. Think of a shaft with a shoulder. If the shoulder has a nice radius, the stress will converge to a result. As the radius gets smaller and smaller, the stress increases. At a radius of 0, the stress concentration factor is infinity. (There are tables that give the "stress concentration factor" based on the geometry.) 

In FEA (finite element analysis, or simulation), stress concentrations can occur mathematically at places such as corners and constraints. (These are normally referred to as "singularities".) It looks like your analysis has both at the point of maximum stress: the constraints on the pin and corner between the pin and body could be causing a singularity.

"So, how do i know when the mesh has the right quality for this kind of simulation?"

• If the stress continues to rise as the mesh becomes finer, then you have a singularity. In this case, one option is to use the stress a few nodes away from the singularity, and extrapolate the result to the singularity.
• If the location is a true stress concentration, then the stress result will converge or level off when the mesh is fine enough. The only way to know when this has been reached is by performing different analyses with finer meshes.

Some notes:

Of course, it is not necessary to use a finer mesh in the entire model. You can use refinement points, or refine edges or surfaces, to get a smaller mesh in localized areas.

The quality of the surface mesh (which you have some control over) can affect the quality of the solid mesh (which you have almost no control over). Keep in mind that a "brick" mesh generates all types of brick elements: 8-node, 6-, 5-, and 4-node elements (or tets). Sometimes, a tet element can be created "just underneath" the surface that causes a high stress at the point where it touches the surface. Some things that I do to get a smoother mesh are these:

1. For the surface mesh, change the transition rate so that the refinement creates a larger, smoother transition.  "Mesh > Mesh > 3D Mesh Settings > Options > Surface > Options > Limit adjacent mesh size".
2. For the solid mesh, change the aspect ratio to limit the distortion. Right-click on the part, "CAD Mesh Options > Create Solid Mesh > Quality" and change the "Automatic enforcement" towards smaller, or use "Upper limit" and enter a value. The current mesh quality is shown in the "Mesh > Mesh > View Mesh Results > Part". The "Max. length ratio" is what is controlled by the aspect ratio controls.

Whatever you do, don't get stressed out. 

[gregorio.riva]

Thank you,

I put a radius on the edge and the results came closer between tetras and bricks.

The strange thing is that if I do exactly the same simulation (keeping linear material etc.) with MES solver I don't get similar results...

Another question related to what you said, should i alaways consider the stresses at the end of the fixed constrained surfaces as exagerated?

[John_Holtz]

Hi Gregorio,

Glad to hear that you are getting better results with the radius.

I think that you are correct about the results at the constraints: they are the area where the results are the least accurate.