CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS (http://www.cfd-online.com/Forums/ansys/)
-   -   Problem of contact on Ansys Workbench 11 (http://www.cfd-online.com/Forums/ansys/76041-problem-contact-ansys-workbench-11-a.html)

Benjaminleb May 12, 2010 10:19

Problem of contact on Ansys Workbench 11
 
2 Attachment(s)
Hello,

I have some difficulties with a contact between two bodies. I am creating a model of the knee articulation. The patella is supposed to slide naturally along the Femur when the leg is flexing whereas in my model the patella rotates without sliding. I put a "Frictionless contact" between the patella and the femur, but the patella seems to rotate around one point and to get fatter without sliding.. Have you got an idea?

Thank you very much.

mechanicaldesign May 13, 2010 02:35

Hi Benjaminleb,

In my opinion, the contact which must you used here is:

-Augment Lagrange with frictional. Coeficient of friction must be entered in the next manner: artificial (you will enter an very small coef. for example 1e-3) or real (which corresponding to real coef. of material used);

The contact region must be refined. If you want to retain an hexaedral mesh, you must choose hexaedral method for all components, and after that enter size option for every component, in a manner in which you will obtained an satisfied results.
Much more than that, if your penetrability exceed your imposed values, you can increase the stiffness factor manualy (by default must be 1, but you must increased to 5, 10, 20,etc.), to decrease the penetration betweens components (this tehnique is very useful in pretension, to obtain a much good results). This option will be increase the computational time.
In this case of study you must used enough substeps in a manner in which solution converge. In my opinion, is enough to used betweens 10 and 30 substeps. From some test you are only person which decide the optimum number of substeps to obtained a good results.

So, keep in touch about your results from your study, following the sugestion presented anerior. I waiting good news, and maybe some image or movies with some results.

Best regards.:)

Benjaminleb May 13, 2010 11:59

Thank you so much for your nice reply, I keep you informed!

Best regards.

Benjaminleb May 24, 2010 18:12

Better, but penetration persists...
 
3 Attachment(s)
Hi,

I followed your advices, and now the first step works well (if it is under 8 degrees) but the patella penetrates from the second step, whatever the degree I put. For instance if I put 2 steps:
- First step : 0 to 8 degrees (the patella slides)
- Second step : 8 to 10 degrees (the patella penetrates)

And if I put only one step from 0 to 10 the patella penetrates from the beginning.

Have you got an idea??

Thanks a lot!

mechanicaldesign May 28, 2010 02:07

Hi Benjaminleb,

If I understand corectly your problem, the part which penetrate the lower bone, must sliding on the surface of their bone. So, if want to do it works, and to convergence the solution, you must used some advance option from contact.

So, If you use contact criterium of Augment Lagrange, made the next modification on contact which cause your trouble:

-settup contact with update stiffness from contact option, and only to contact which cause trouble;
-increase the number of substepts;

After this setup, rerun the problem and observe what happends;

-if it don't work , put the option normal stiffness from automatic to manual, and here will be present the factor K which representing the stiffness contact. By default is 1, but you can decrease for example to 0.1 and rerun the problem;
-increase the number of substeps (somethimes this option can resolve your problem by default);

Don't forget to put frictional coeficient betweens surfaces which made a contact.

I wait good news and pictures (without values).

Best regards.


All times are GMT -4. The time now is 15:51.