Hi Valentina,

why don't you try using a dynamic implicit solver instead of the static one and with a smaller initial time increment? For simulations with softening the static solver can be unstable and creates convergence problems.

In any case, it would be better if you increase the maximum number of increments.

Federico.

Hi Federico, thank you for your reply.

As you have suggested I try with Dynamic, so I have a question: I have to delete the static step and I have to change in this new step the BC and the constraints?

Valentina

If you delete your static you will lose the BCs that have been created in that step and you will have to recreate them. In this case that you have very few BCs it is the quickest way.

Federico

This is a classical problem if you simulated damage in any Abaqus (or any finite element solver). Convergence is difficult to achieve. So you need to modify the default convergence setting. So for each increment, Abaqus will solve the equilibrium problem iteratively. If after X iterations, it still does not convergence, it will show that "I made too attempts to solve it.. but I can't".. what you need to do is to tell Abaqus .."Hey.. you need to work harder.. try iterate more!!"

Practically how you do this is to go to step module... click "Other" .. click "General solution control"... a window pop out... click your step name... click edit... choose Specify... change to Time incrementation tab.. modify I0 = 20 (initially it is 4)..IR = 40 (initially 8).. click more and find Ia = 20 (initially 5).. this is the setting Abaqus used when doing iteration... to understand the meaning of each, read the abaqus documentation. But these are the most important ones. (without sacrificing the accuracy)

Hi Valentina, if you want to simply increase the maximum number of increments that abaqus standard will do, you have to add in the .inp file the bold snippet that I've added down here.

** STEP: Step-1

*Step, name=Step-1, nlgeom=YES, INC=1000

*Static

0.1, 1., 1e-15, 1.

Set this parameter equal to the maximum number of increments in a step (or in a single loading cycle for direct cyclic analysis). This value is only an upper bound. The default value is 100.

Try to provide BC to the directions with unnecessary movement which won't affect the analysis output. Sometimes it works.

Monitor the messages and try to detect why the solution is not converging. The messages will guide you to instance causing the problem and the direction which needs restraints or needs some enhancement in the interface properties.

Good luck.

Thanks to everyone,

I have solved this problem but now I have applied a change in the model; I have created one solide (fiber + cohesive element) then I have made a partition, I have applied a cohesive section to cohesive element but now the fiber is a solide composite by three ply.

The program is working but it take much time when I add the fiber and the interface (= cohesive element). So I ask you if it's correct the strategy of tie constraint or I am making some mistakes somewhere.

Kind regards

Valentina