Maximum stress of bearing

Recently, I was doing the analysis of the maximum stress of bearing. First, I generated the hexahedral mesh of bearing and imported it into prepomax. Then, I applied 600N force to the half of the inner ring of bearings and checked the maximum stress of the inner ring and found that the result was quite different from the theoretical value.The theoretical maximum stress of the inner and outer rings is 1784.83Mpa and 2031Mpa respectively, but the simulation results are 932.5Mpa and 1011Mpa respectively. Can you tell me whether it is a problem caused by the meshes or some boundary conditions or loads?

I’d rather avoid applying boundary conditions to surfaces involved in contact. Also, try further refining the mesh, it’s very important if you want to obtain accurate contact stresses. You may even try utilizing submodeling to focus on the region of interest and use highly refined mesh:

But after I refine the mesh,Why the results don’t converge?

Well, maybe the refinement is still insufficient. Or you encountered stress singularity ( but I’d expect the first issue to be the case.

Could you tell me how should i apply boundary conditions to balls?

It would be best to avoid applying BCs to them at all (other than e.g. symmetry if you analyze half of the ball in a reduced model. Look for some research papers describing bearing FEA.

(post deleted by author)

thanks very much! i’ll try it

This is the latest result after I refined the contact surface of the inner and outer rings of the bearing. The stress cloud map of the roller surface shows that the maximum contact stress is not in the center of the contact surface. Do you know what caused this?

Apart from von Mises stress, check contact outputs. Especially CPRESS but also COPEN. Look at the other side of the interface - see what those contacting surface segments look like in bot undeformed and deformed state.

thanks very much! I have found the fault.Besides, Do you know how to add local coordinates by keywords? Or are there any guidelines for adding keywords?

What was it ?

You can use the Keyword Editor to add new keywords following the CalculiX syntax (described in CalculiX user’s manual). If you want to apply boundary conditions in local CSYS, check this thread: *TRANSFORM (R and C)

I should look at the S33 not the mises stress, the maximum stress in the z direction is shown in the center of the contact surface.

I meet with a problem again, it occurs “job failed” when I dense the mesh, but I don’t know exactly what caused it, could you give me some advice? Thanks a lot!

There’s no specific error here, just “Job failed - no results exist”. Try exporting the input file and submitting the analysis from the command line (detailed description here: Using standalone CalculiX), maybe you will get more specific error messages.

Also, go to Tools → Settings → Calculix → Number of processors and set your number of CPUs because currently, you are running the simulation on just 1 core.

I think it was caused by a lack of memory, and when I used a computer with more memory, it works well. Besides, do you know how to check the the normal stress of a point on a surface.

That’s very likely, I’ve seen such issues in CalculiX with large meshes before.

You can select the stress tensor component of interest and use Query → Vertex/Node to check the value at a given node.

but from this, i can’t know the normal stress of a point on a face.

After selecting the stress component (like S11 here), you have to use the Query tool to check the value at a given node. Unless you are talking about normal stresses in a different coordinate system, aligned with a face in your model. This would be tricky since PrePoMax doesn’t support such a functionality. ParaView with its Calculator filter could help you but it would still require some manual transformations (using proper formulas).

yes. I just mean it. And I have studied Tutorial-Hertz contact you posted,but i confused that you checked S33,neither contact stress nor mises stress.