Stress Discontinuities in Contact 1

[fruton]

Dear all,

I have two spherical surfaces in contact under load (no slip), and I seem to get high stresses at nodal points. Is this purely down to the need for a finer mesh? or can anyone offer any other advice on this? I am using Abaqus with C3D8 elements. I have also attached an image.

Thanks

 

[corus]

There's obvious symmetry in your results so you could halve (or even quarter) the model and get the same answers with symmetry restraints on the cut plane(s).

It looks like almost point contact so refine the mesh, preferably biased towards the region of contact.

Tara

 

[fruton]

Thanks, I noticed a much better more realistic stress profile when I refine the mesh in the contact area. Also, would it help if I have matching nodes between the two components in contact i.e. one node on one component directly contact a node on the other component?

 

[corus]

I've found that matching the nodes does give better results, and stops some penetration of the separate parts. It should converge quicker too.

Tara

 

[flash3780]

What contact method are you using? If you're using a penalty based method, you can try increasing your contact stiffness. Full Lagrangian contact is the most accurate (albeit the most finicky), from my understanding.

 

[ESPcomposites]

Here is an example of the result for a matched mesh, which should help a lot:

http://www.espcomposites.com/bolt_update.jpg

I seem to get results like you have unless the mesh is matched.

Brian

http://www.espcomposites.com

 

[fruton]

Thanks for the advice, yes I am using penalty contact (tangential) and "Hard" contact (normal), you mean opting for the "Lagrange multiplier" as the friction formulation?

 

[flash3780]

I think that "Hard" contact may be the same as a Lagrangian contact (which allows no penetration of the contact surface). Augmented Lagrange is a good compromise between a penalty and a Lagrangian contact. I'd try switching to an Augmented Lagrangian contact formulation and seeing if the problem goes away.

Here's a presentation that describes the contact options available in Ansys (other software packages use similar formulations):

http://www.scribd.com/doc/36284870/Erke-Wang-Ansys-Contact

Good luck.

 

[flash3780]

I forgot to mention; I'm not sure if ABAQUS uses symmetric contact pairs or not (they didn't used to), but you should definitely make sure that you're not using symmetric contact pairs. They make it extremely difficult to interpret contact pressure distributions.

 

[fruton]

Is it true that if you use surface to surface contact then you do not need to worry about matching nodes?

Thanks

 

[corus]

In either Node to Surface or Surface to Surface, you don't need matching nodes. It does seem to help though as it will stop any penetration of nodes.

Tara