Hertz contact.zip (5.2 MB)
In the spherical contact problem, I found that the calculation results of calculix contact pressure distribution are very different from those of abaqus and ansys. The maximum contact pressure of calculix appears on the edge of the contact surface, which is obviously wrong. The maximum contact pressure should appear at Center, I don’t know if this error is caused by prepromax software or calculix software.
Welcome everyone to discuss, see the attachment for the model
This seems to be just some artifact that may disappear with further mesh refinement. I also get a small concentration in that area when I run your model without any changes but the maximum value is reported in a different location:
Anyway, it’s not a fault of PrePoMax but it can be caused by some inaccuracy of CalculiX when compared with other solvers that you’ve mentioned. Maybe ask on the CalculiX forum if you are still concerned about this.
I think you are right, this may be caused by inaccurate calculation of contact pressure by calculix, or its contact algorithm is not accurate enough. In fact, from your calculation results, the results are still different from abaqus and ansys. The contact of commercial software The pressure calculation is even better!
How did you define the surface behaviour? Is it hard, linear, exponential… And which parameters did you use? I was analyzing some Hertz contact between cylinder and plane in the last few days and my results were actually pretty accurate for pressure and Mises equivalent.
The result of the cylinder facing the plane or the sphere facing the plane is still good, but the result of the sphere facing the sphere is as shown above. In addition, I think the sphere facing the sphere is more difficult. The simplest hard is used here, and the same is true for abaqus
If I remember correctly, both abaqus and prepomax convert hard contact to linear contact with standard values and some penalties to achieve fast convergence. Maybe the default values are different, thus providing different results. What I did was to change the K value in linear contact (stiffness coefficient for the contact) to match analytical pressure, something about 5000 times of the young modulus for my materials did the job (even though documentation says 5 to 50 times, I don’t know if it is a unit problem or something else). When I forced this value, both displacement and stress fields gave values in agreement with hertz theory, but I’m not sure if this is the correct approach. Anyway, hard contact is more conservative for engineering purposes.
If you refine your mesh in the contact region, can you achieve better results? A local refinement should do good.
From many calculation examples, the calculation results of calculix’s deformation and stress during contact are still good. You said that modifying the penalty stiffness can get different contact forces. I don’t think there is a big problem, and it can also match the experimental results. I mainly I feel that the current form of contact pressure is wrong. Of course, refining the mesh can get better results than the current one, but in fact, the form of the contact pressure of commercial software is also correct when the mesh is not very dense. I’m guessing the problem is caused by calculix’s contact search algorithm. calculix’s contact search algorithm may not handle as well as commercial software.
I understand your point. Not sure on how commercial softwares handle their contact calculations, maybe they have an advantage. How does your model performs on Abaqus/Ansys contact analysis? Do you have a comparison on this so you can share with us?
From my experience in contact simulations using CalculiX parabolic FE have some problems computing the contact pressure distribution. Maybe linear FE will give you a better result.
Mesh refinement could be done only in the area of contact. You can refine a mesh around a point and then use the Grading parameter to increase the mesh size away from the point slower. Or subdivide the surface where the contact occurs.
Ok, next week I will find time to do an upload
Ok, I will try it. I also think that the maximum contact pressure of high-order elements occurs at the intermediate nodes. If linear elements are used, they need to be processed into hexahedrons.
I just used the linear criterion, and the result is a little better than the hard criterion, but still not ideal
nice，Therefore, I think that the stress averaging method is not consistent with several software. I can’t find an introduction to the contact search algorithm from calculix’s manul.
reading many benchmark test of contact analysis with Abaqus from a report, shown no large discrepancy. if i can say nearly identical results with CalculiX.
why Ansys reported near half only? make me doubt about the Ansys results. or maybe the problem is in element type using, there’s an improved versions of tetrahedral element.