Question on Designating Target and Contact Surfaces

[nodalDOF]

I have a problem where i am modeling a cylindrical (steel) bar embedded in concrete and i am trying to smulate shear test. For this case I have some doubt regrading designation of contact and target surfaces. As per ansys contact technology guide the following applies

3.5. Designating Contact and Target Surfaces:
For flexible-to-flexible contact, the choice of which surface is designated contact or target can cause a different amount of penetration and thus affect the solution accuracy. Consider the following guidelines when designating the surfaces:

(a)If a convex surface is expected to come into contact with a flat or concave surface, the flat/concave surface should be the target surface.

(b)If one surface has a fine surface mesh and, in comparison, the other has a coarse mesh, the fine mesh should be the contact surface and the coarse mesh should be the target surface.

(c)If one surface is stiffer then the other, the softer surface should be the contact surface and the stiffer surface should be the target surface.

However, there was no explination regarding precedence. Here a canvex surface (That is stiffer) is coming in to contact with a concave surface (concrete). So as per guideline (a) The concave suface should be "Target" surface. But, this is less stiffer than the steel ( as per guideline (c) the same should be "contact surface"). Is there a precedence for this designatons?

Thanks,
Nodal DOF.

 

[cbrn]

Hi,
at the expense of twice the contact-computation time, the best I see in these cases is to enable the option of "Symmetric" contact.

Regards

 

[nodalDOF]

Cbrn,

Thanks for your reply. Seems like a good option for small models. I did not observe any significant cange in the results by switching the contact and target surfaces as long as the aurfaces are in contact. However, the results deviated when they started to seperate.

Thanks,
Nodal DOF

 

[cbrn]

Hi,
from what you notice, it seems that the combination of factors which "guide" the calculation of the contact stiffness is intrinsecally "quasi-symmetric", so there is only very small difference by reversing the contact pair. Keep in mind that the calculation of the contact pair takes anyway into account the properties of both the materials in contact. "Problem" may arise when separation occurs, or, worse, when the contact is initially open. In this case, the auto-calculated pinball factor, which depends on the underlying thickness, plays a significant role, as well as the fact that, being the bodies not in contact, the stiffness is estimated using only the properties of the "CONTACT" elements; thus you can understand why the results strongly differ by reversing the pair.
If you also set "update contact stiffness -> each equilibrium iteration", then there is very little to worry about.
The "symmetric" option does not in any way multiply the entire solution time by two! It only doubles the contact stiffness calculation time, which is a fraction of the total contact calculation time and an even smaller fraction of the total solution time. You can use this feature even with models having 1.5 Milion DOFs or so. It may be more efficient, in particular cases, to run "symmetric" and "update... at each substap" instead of "asymmetric" + "update... each equilibrium iteration". But be careful, it depends: think carefully about the implications of each option...

Regards

 

[nodalDOF]

cbrn,

Thanks for your suggestion. I am implementing symmetric option for my contact model. Initially i thought they would take too much time (my current models run for 1-2 days). However, some of my contacts started seperating in half the way through because of applied loads and BCs resulting in unconverged solutions. In this case as you mentioned the results started deviating from the moment the separation starts. Thanks for your help.

NodalDOF