Dear All,
Introduction:I am currently conducting parametric studies on Concrete Filled Double Skin Tubes(CFDST) in Abaqus. In case you are not familiar with CFDST, it is a composite structure with an outer steel tube and inner steel tube with a concrete sandwich in between them.
The problem:I am using Abaqus Riks to conduct a parametric studies which involve bending of large tapered cantilever CFDST. I have done validation against smaller scale experimental specimen which are available in the literature. The validation worked very well for me, but when I changed the size of the structure then Abaqus Riks will encounter severe convergence difficulties.
Diagnosis and attempts to solve the problem:I believe the problem is with the interaction between the steel and concrete especially when concrete fails in tension which occurs early in the analysis typically less than 10% of the ultimate load. I have tried numerous things such as modifying the concrete model in tension(e.g. inputting elastoplastic definition of concrete in tension with a small tensile strength), trying different techniques with interactions,changing element and mesh type, changing the solver settings, and I have thoroughly checked the model many times.
I also tried inputting a small value for the viscosity parameter in the Concrete model in Abaqus. This would make the model work, but the results are very wrong where the bending capacity of the structure becomes much larger than it should be.
Preliminary solution: I have decided to eliminate interactions given they are the source of the problems, so I used TIES to model the interface between the steel and concrete. The model worked very well up to failure with no problems. Hence, this verifies that interactions are the source of the problem. TIES imply that there is a perfect bond between the steel and concrete. I believe this is a reasonable assumption because I am mainly interested in the global behaviour of the structure.
Besides, researchers in the past reported that different coefficient of frictions have a minor effect on the prediction capacity CFST and CFDST. Also, EC4 and AISC assume perfect bond when calculating the bending capacity of composite sections. Hence, this justifies assumption of perfect bond is a reasonable assumption which is actually adopted by many researchers simulating reinforced concrete structures.
Conclusion: I appreciate if you can mention any suggestion or solutions to solve this problem. Please note that I am avoiding to use Abaqus/Explicit because it may give inaccurate results for a static analysis due to various issues not to mention the very long time it would take to finish the simulation. Apologies if you found this post long.However, I made it as short as possible to explain this complicated problem which is happening for a really long time.
Hi Mahmoud,
Increasing the size of structure should not result ant problem as far as I know. From my perspective, the problem you are facing could be due to many issues namely concrete material itself, mesh technique, interaction, boundary conditions, and time set up.
I do not know what kind of method you use to define the concrete material. Anyway, I would suggest you first to define the concrete by using Concrete Damage Plasticity method and see how it goes.
If you want to keep in touch wit me, I would like to help you whatever possible. I am PhD student at the University of East London and I am working on ABAQUS too.
Hi Ahmed,
I have always used the Concrete Damage Plasticity to define the concrete material in Abaqus. However, I personally believe that if I use TIES instead of interactions to model the interface, then the problem gets resolved and the model works very well.
I tried quite a lot to modify the interaction properties in Abaqus such as modifying the penalty method and scaling back the contact stiffness, but nothing seemed to work. I wonder if there are some techniques in Abaqus Standard to resolve interaction problems.
Thanks.
Hi Mahmoud
In interaction, what kind of method do you use, general contact or surface to surface?
Could you literally write down the problem you get in the error.
Thanks
Hi Ahmed,
I use surface to surface contact where a master and slave surfaces need to be assigned.
With respect to the error message, it is :" A zero displacement solution was found in the first iteration of a riks step". However, what happens before this error is that the time increment for many increments gets very tiny in the order of 1E-11, and then it would issue this error message after that.
Thanks.
A simple question please for AHMED ALBARRAM:
Why do you prefer ABAQUS ? Why not any other software like SAP2000 for solving
this construction problem ?
Hi Mahmoud Alhalaby,
I have the same problem especially with circular column. Could you guys help me?
Hi Qusay,
Try using the stabilization technique if you are using Abaqus/Standard. You can input a damping factor or a dissipated energy fraction to ease the problem in the solver settings. Also, you can try contact controls where you could damp the interaction itself. For more information on these aspects, please check the Abaqus User Manual which tells you how to do it if unsure.
Thanks Mahmoud,
These techniques are completely new to me. I did figure out how I can use a damping factor or a dissipated energy fraction, but I cannot understand what you mean by " you can try contact controls where you could damp the interaction itself", Would you mind giving more details, please?
Once again, Thanks a lot.
Hi Qusay,
If you check section 36.3.6 in the Abaqus 2016 user manual. You can find full details about it. Please note that I have tried in the past very briefly and do not know much about it. It is simply stabilizing the interaction in a similar fashion to the Abaqus Standard Stabilization solver technique. If contact and interactions are important in your study, then it may affect your results.
Anyway for both techniques, you must make sure that a small factor is applied in order for it not to influence your results. A good practice would be to request the viscous forces, damping energy and other energy magnitude. You have to check that the viscous forces and damping energy are smaller compared to forces and total energy in your problems as the manual says. Another way of checking would be to check if the reaction force is equal to the applied force. Of course at failure, they would not be equal.
Thanks a lot. I'm reading in Abaqus manual to get a comprehensive vision about these techniques. It was really great point from your side.
- Badges
- Science topic