Question about contact problem

[victorroda]

Hi
I need to know wich element type is better to solve contact problems with FEA.

I think the better choice are linear elements, but I need any bibliographical reference to contrast this thought.

Thanks in advice

 

[chris9]

Linear analysis is much quicker to solve than nonlinear but you can use both. You need good element shape properties such as aspect ratio, warping and distortion in the contact region.

Chris

http://www.value-design-consulting.co.uk

 

[corus]

Linear elements are better as the contact forces of mid-side nodes of quadrilateral elements are screwed up causing convergence problems. Never use quadrilateral tet elements other than in the most simplest of cases. This is for the same reason mentioned previously, and because tet elements produce less 'smooth' results causing convergence problems once again.
I've not seen any bibliographical references to this, and certainly not from the software producers.

Tata

 

[victorroda]

Thank you very much.

I'm writing a paper about the importance of precisión in geometry definition for contact problems FEA.
I've used type 'brick' linear elements because a recomendation of my supervisor, and i need to argue that decision in my paper.

So thank you very much, your answer has been very useful

 

[GregLocock]

As I sit here waiting for a non linear contact model to solve I think you may be on the wrong track. In impact type work geometry is amazingly unimportant.

Cheers

Greg Locock


New here? Try reading these, they might help FAQ731-376

http://eng-tips.com/market.cfm?

 

[corus]

Maybe in a dynamic analysis stability isn't of much concern so you can get away with quadrilateral type elements? In Abaqus at least, a non-linear problem involving contact, can be more easily solved using a dynamic analysis approach rather than a static analyis, that is if you're prepared to wait a few days for the results.

Tata

 

[chris9]

I'm doing a contact analysis right now with 10 node tets. It would run much faster with 4 node quads but it would take too long to mesh. I think solver time, accuracy and meshing effort is an important consideration.

Chris

http://www.value-design-consulting.co.uk

 

[aeroAFRIX]

I think the question itself is too general for anyone to provide a specific answer.

Element choice for contact problems depends on ( amongst other factors) whether you are performing a 2D or 3D contact FEA. Also, FEA softwares have different and sometimes unique approach to element formulations for contacts analysis.

For example, in Abaqus you use tet10 modified (C3D10M)for contact problems and impact problems that involves contact

P.S: Corus could you clarify if you were referring to 'LINEAR' elements in terms of its interpolation order? i.e. (First Order) elements are these are sometimes called Linear Elements too.

 

[Elabbasi]

In contact, there are cases where linear element (meaning no midside nodes, e.g. 4-node tets, 8-node bricks) are better and cases where quadratic elements (10-node tets, 20 and 27 node bricks) are better.

Ideally, if the contact pressure variation is smooth (when you have contact spanning multiple elements, with a smooth underlying geometry) then quadratic elements should be more accurate. In practice, the quadratic elements even in such cases sometimes give worse results. That is primarily due to issues with contact algorithms, and commercial FEA codes and academic researchers in this field have devised ways to improve results.

The most commonly used contact algorithm (in my opinion) is the master-slave algorithm with contact enforced at nodes. This algorithm does not work well with 20-node brick elements. That's because even a constant contact pressure produces tensile contact forces at the corner nodes. Using a 27-node element instead eliminates this problem. That's why Abaqus for example automatically converts 20-node bricks to 27 node bricks at slave contact surfaces. Master-slave algorithms that enforce contact at integration points do not have this issue with 20-node bricks (Ansys has this feature).

A similar problem happens with 10-node tets and that's why Abaqus recommends instead the "modified" 10-node tet for contact. This modified element is actually a patented Abaqus element which internally divides the 10-node tet into multiple 8-node bricks.

A newer generation of surface to surface master-slave contact algorithm enforcing contact more accurately than just at nodes or integration points is supposed to improve contact results with both linear and quadratic elements. Such algorithms are recently making their way to commercial codes. I know Abaqus has one (you activate it by choosing surface to surface discretization within a surface to surface contact interaction), and I believe other codes have something similar too. With these algorithms quadratic elements may finally be better for contact problems involving smoothly varying contact pressures.

Nagi Elabbasi
Veryst Engineering