Static & Implicit Dynamic steps ignore beam thicknesses in contact

[Nexes]

Hey Guys,


I've known about this forum for a while and every now and again a google search takes me here for a helpful answer or two. Now, I have a new problem and I CANT find an answer.

In short, I would like to model a dynamic process involving a moving, rigid, shell and a very much deforming beam. The beam is modelled as a 'wire' and assigned as 'pipe' section. My problem is that in both static steps (to achieve equilibrium configuration) and in subsequent implicit dynamic steps, the contact is only detected on the centreline of the beam (i.e., on the wire itself) and NOT on the edge of the section as would be the case if the beam would be modelled as an actual deformable solid.

I have a feeling this is a bug in Abaqus, as evident by shreds of information I found online. See also

http://marketing.intrinsys.co.uk/abaqus-PDir/pdf/abaqus_6.13_golden_list_of_closed issues.pdf

(search the document for 'beam', page 17). However, according to this document it should be fixed already?!

When using explicit dynamics, I can achieve the desired result by setting 'Thickness of Interfacial Layer' (Contact Properties -> Mechanical -> Geometric Properties) to the pipe's diameter but this means I cannot use static steps to achieve the equilibrium position I need (There's gravity in place as well that needs to be initiated, as well as a large initial displacement of the beam that needs to be realized before I can commence the dynamics part) because Abaqus doesn't allow static steps before explicit dynamic.


Has any one dealt with this kind of problem? Can any one confirm that this is a bug or am I doing something wrong?


Your help is much appreciated.



Kind regards!

 

[Nexes]

Ah, and I should probably add that the contact problem is NOT solved by changing from a surface-to-surface to a surface-to-node-region discretization method. I use surface-to-surface type contact formulation.

 

[cooken]

What version of Abaqus are you using? Accounting for beam thickness was introduced recently (6.12 or 6.13 I think) for the implicit solver, but only when using general contact (see edge to surface in the analysis user's manual). The default offset for contact is a radius around the wire based on the section area. You can modify this radius with contact property assignments. For contact pairs, there is no surface-surface available for beams, it always defaults back to node-surface. Check the warning messages.

The only bug that exists is when a beam comes into contact with multiple surfaces. In this case the algorithm only applies the offset for one of the surfaces and allows the rest to contact the center line.

 

[Nexes]

Fast response, thanks a lot cooken!!

I'm using 6.13, and upon checking a simple model, it seems that you are absolutely right. For general contact, the offset is taken into account properly. Now to figure out how to get general contact going in my model..

The error I get right from the get-go with General Contact is a few "Displacement increment for contact is too big", followed by a "Too many attempts made for this increment" fatal error. This is the "Initial" step, there shouldn't be any kind of movement until the next step, a simple static step.

Any ideas?

At least I know a bit more about the limitations of the program.


Regards.

 

[Nexes]

I solved that one as well!

Turns out step 1 is actually the first real step, rather than the initial step
Decreasing the initial increment size for that step did the trick.


Thanks again cooken, was stuck on this for several days!


Regards.

 

[cooken]

No problem!

Your other issue (that you solved anyway, but maybe don't fully know why) is most likely due to having small, varying gaps/overclosures between the beam and shell from the initial mesh. The smaller time increment allows the solver to resolve these, but it is better to have them resolved through strategic meshing and/or contact initialization. Convergence and solution accuracy will likely be much better (continuous pressure and therefore stress distribution, less prone to noise-like gradients).