Issue with contact elements 1

[Dave442]

Hi all,

I am trying to model the expansion of a stent, a small metallic medical device which is expanded within an occluded blood vessel to improve blood flow through the vessel.

I have created a finite element model of the stent geometry (SOLID185) and have simulated its expansion using a rigid cylinder subject to displacement boundary conditions. The expansion of the stent is driven by frictionless contact between the rigid surface (target surface - TARGET170) and the inner surface of the stent (contact surface - CONTACT174). The nonlinear solution seems to converge well with no load bisection or unexpected error messages.

When I enter the post-processor, the deformed shape of the model seems ok, however, if I plot stresses and strains I have noticed some odd results (please see linked image). This only seems to occur on the surface which has been meshed over with contact elements??

http://files.engineering.com/getfile.aspx?folder=e8dafc2b-c92c-4473-a5f1-7588f1a8390f&file=01.pdf

I have never used surface-surface contact elements before and was wondering if anyone has an idea whats going wrong? I have tried using different elements / keyoptions with no luck!

Many thanks,
Dave

 

[kan123]

Have you unselected the contact elements before generating the plot? Their presence could mess up the nodal averaging.

Are the dark blue patches in the same locations as the actual contact? Could the pressure be high enough to affect the calculation of local von Mises stress?

If this is your first use of surface-surface elements, it might be worth your effort to build a simple sample problem where you know what the correct results should be. It's been a few years, but I vaguely remember that it was hard to plot the pressure distribution because the results were arbitrarily assigned to one side of the interface for each pair of elements. But this should not affect the results for the underlying solid elements.

If all else fails, you might have better luck with node-surface elements (with the cylinder as the surface).

 

[kan123]

Oh, and you can plot contours of the component stresses. This might show that one particular direction (like normal to the contact surface) is causing the unexpected result.

 

[Dave442]

Hi kan123,

Thanks very much for your suggestions. I didn't realise that I had to unselect the contact elements before investigating results, I have never used contact elements before!

I used the following command:

ESEL,U,TYPE,,2,3

and the problem seems to have gone. Plotting nodal / element contours of equivalent and component stresses there doesn't seem to be anything out of the ordinary.

Many thanks!
Dave