Plastic analysis in CCX, time steps/convergence question

JSC

Hi everyone,
I am trying to check ultimate capacity for a cantilver beam subject to bending. The beam is a CHS (circular hollow section) in steel grade S355 modelled with HEX20 elements (very fine mesh) and having a load at the end causing a bending moment and shear at the fixed boundary (wall). I am running the model in CCX, non-linear quasi static mode with 10 time steps, tough I have allowed the "automatic time stepping". The materials tangent modulus has been altered between something very low up to a more realistic level of 2-3GPa.
The sections is categorized as a "Class 2" section in e.g. the Eurocodes, meaning that full plasticity is possible but it lacks some rotational capacity to develop full rotational hinges.
In one scenario, when I run the model with a very low tangent modulus, it fails to converge at the last time step, which corresponds to a load approx 13% over the theoretical limit given by the plastic modulus. I get very fine and detailed steps just up to the last stage and where the solutions also looks reasonable.
So here is my question: Is it safe to assume that the lack of convergence is due to that the solver has found a limit, (in this case looking like an in-elastic buckling of the tube wall close to the fixed boundary)? The solver performs solutions for time steps 9.771s, 9.754s, 9.617s, 9.344s etc. i.e. very small load increases just up to the point where it exits ( my time line was 0s-10s).
Or to rephrase the question; is it reasonable to assume that the ultimate load capacity is 97.71% of the applied loading?
Many thanks in advance for any input on this,
Jan

Victor

Yes, it may be correct that the final converged step is the limit of stability. From your list of times, that wouldn't be 9.771 s because it subsequently backed off from that.

However, I'm not sure that's safe. Some other things to consider:

Don't trust the mesh to be correct just because it's very fine. You should also run it with coarser meshes to ensure it has reached mesh convergence.

If you load it with a displacement instead of a force, it should properly continue through the instability region which would give you more confidence. You can then read the external force from the solution.

Consider adding an initial imperfection or small load to help initiate buckling in case it's sensitive to that.

I assume the load is ramped linearly with 100% load at 10 s.

JSC

Hi Victor,
Thank you very much for the quick reply and your valid pointers!

I agree there are more things to consider, like imperfections, internal stresses, load introduction (which is a bit more complicated than explained) etc.

A run with coarser mesh did however not indicate any buckling, I guess the stiffer elements prevents that.

I will try loading it with a displacement, but I am not really confident with how to interpret the external forces in this context.

Yes, the load is ramped up linearly, 100% at 10s.

I guess my overall goal is to see when and how the item fails and to get a feel for what the safety margin looks like - I have other aspects in the model to consider and would like to justify that the capacity given by the plastic modulus is valid in this case. (In additon there are also safety factors applied to the load).

My interpretation, I may be wrong, of a "class 2" item is that some parts of a section, subject to bending moment, will show post elastic buckling which prevents the formation of a plastic hinge with rotational capacity, e.g. when local inelastic buckling occurs a loss of capacity takes place therefore the load limit is set to what the plastic modulus admits.

Kind regards,
Jan

JohnM

I second Victor's comment about the displacement versus force. If you model a stiff "holder" where the load is currently applied, you might be able to use a single displacement, which is very handy for post-processing.
Convergence is very sensitive to the slope on bilinear kinematic.
When using automatic time step, it's worth limiting the maximum time step. This is true of any analysis where "stuff is still happening" at the end of the loading event.

JSC

Thanks JohnM!
I take it you mean that the load introduction area/zone should be sufficienlty stiff to avoid issues there?

I have noticed that the tangent modulus greatly affects the convergence, esp. that the lower it gets the harder to get convergence. However some codes like DNV gives advise on tangent modulus for common steel grades and they all appears to be towards a more realistic level; 1.5-2.2 GPa for S355 which is helps convergence.

By limiting the max time step do you mean the actual step size, which seems to be automatically adjusted and hard to affect, or the amount of "overload" e.g. 110% instead of 120%? I guess the latter is obviously helpful for convergence.

JohnM

Gluing some "stiff" elements to the load point allows you to distribute the load from a single point. Think of it as a poor-man's rigid region constraint. Victor has added some features recently that may do this for you, but I still use this trick. See attached example, note that the full force vs deflection can be determined by looking at reaction at deflection node. Also in example, auto-time stepping with .05 max limit.

JSC

Thanks a lot JohnM!

I do seem to get convergence even for an extremly low tangent modulus when applying a deflection (for a ramped up load load and a higher tangent modulus it also converges). In both cases it seems clear that post elastic buckling takes place. Then it's of course another question of how accurate the solution is, but that will be up to model detailing, BC's etc.