Dear Mr Pryrl,

Thank you very much. Once again you have solved the problem. A tension stiffening factor as small as 2% is enough to stabilize the convergence.

Now I have a question about the compressive strength reduction (rc) in 3DNonlinearCementitious2 model: since the effect of transverse tension in the resistance of concrete in compression is taken into account in the plasticity model (though the yielding surface around hydrostatic axis), I think the strength reduction factor rc proposed by Collins and Vecchio (1986) partially accounts the same effect twice. Don’t you agree with me?

I am saying this because I imagine that in ATENA, in the calculation of rc factor only strains in cracks are accounted for and this way this factor shouldn´t be equal to 1, however I think the experimental calibration of that factor by Collins and Vecchio (1986) didn’t account for reduction of compressive strength due to transverse tensile stresses and this way Collins and Vecchio (1986) expression is too harsh if used together with a plasticity model.

Again many thanks,
Ricardo

Dear Ricardo, without seeing your modell we can only guess what might be the reason of the convergence problems.

If you are using force loading + Arc Length, you should consider if you can replace the load with prescribed displacement (and monitor the reaction instead of the external force).

Behaviour similar to your description often occurs when there is local concrete failure (especially in shear, where brittle response is typical), although later the load is fully transfered through the reinforcement. As the reinf. bars only have axial stiffness (no bending nor shear), first elongations of the bars have to develop to take over the forces previously carried by the concrete. If it is this case (check the cracks and generally the concrete damage at the end of ther step with the large convergence error), the numerical behaviour frequently stabilizes when tension stiffening is added. For heavily reinforced structures/areas, values of 10-50% are recommended (although the EC default of 40% if quite high). If you think TS is not justified in your case, you may set it to a small value of 2-5(10)% just to improve the numerical behaviour (you can see that as an equivalent of numerical viscosity commonly used in computational fluid dynamics).

Dear Mr. Pryl,
Once again, thank you for your clear explanations.

I still have one problem:
I am trying to model reinforced concrete beam-column joints in ATENA 3D – a region with large shear stresses. In beam-column joints with few reinforcements, after some steps with no problems in convergence, sometimes I get a step were I have a sudden decrease of load and ATENA can’t reach convergence – after the max. number of iterations I get errors sometimes much larger than 10-20%.

I have already tried to change the step length, the max. number of iterations and the solution method. Nothing seems to help overcome those points.

If I let ATENA continue the calculation after that problematic points I get convergence in the later steps and the load increases again (it overcomes the max. load recorded before divergence).

I think that, because of the large errors in those problematic steps, the later results are useless. On the other hand, reinforcement stresses are quite low before divergence (0.7* fy) and, since I use EC2 (Annex J) recommended detailing, I would expect that the joint would be stronger than the beam. So I am not sure If diverge means failure of concrete.

Is there any other way of overcome trouble points? Should I assume that those large errors mean that I had failure? What is the best way of evaluate the damage in concrete in order to distinguish failure from pure divergence in the mathematic process?

Many thanks for your help,
Ricardo

Dear Ricardo, yes, the values are interpolated separately for each macroelement. Normally, the results are extrapolated from the integration points (where the material is evaluated) to the surface.

If this is a problem, you can change this - set to use the value from the nearest material point instead of any interpolation/extrapolation. In ATENA Sci, this can be done directly, if you are using ATENA Engineering 3D, you have to read the step results into AtenaWin (Application - Restore FE Model from), go to Output - General options, check Nearest MP on the General output options tab and press Apply. Then, store the results (Application - Store FE Model to) and read the changed binary step results file into ATENA 3D using the File - Open other - Results by step command.