when it is not able to converge in any iteration even with the smallest allowed time increment size and it can not reduce it further.

Hello Enas Mabrook

It depends on the problem.

For example, in nonlinear problems (e.g. contact interaction), it sometimes helps to reduce the load increment, i.e. to apply the load “more gradually”. Bring the master and slave into contact in several steps, then close and establish contact, then load as you please.

The same with plasticity. In this case, it may also help switching from load- to displacement-controlled mode. Changing or varying the yield criterion often helps as well.

If the reason for poor convergence is mesh distortion, it may, at least in theory, help to make the mesh coarser so that individual elements do not get distorted that much as strain builds up.

Finally, the easiest (and the first) thing to try is to set up the simulation with a smaller minimum time increment in the step that did not converge. This is often all it takes to make it converge (default settings are suitable mostly for problems with no convergence issues, e.g. linear elastic).

See here for many tipps:

Preprint How to get meaningful and correct results from your finite e...

You can try to adjust few settings with regard to the time increment.. If you open your .inp file , you can find similar to the one below :

##################

** STEP: Step-1

**

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

*Static

1e-3, 1., 1e-05, 1.

###################

If the simulation is coming out in first iteration, then tryto play with the numbers above esp. 1e-3 & 1e-5

(1e-3 is the inital time increment & 1e-5 is the minimum time increment that it can get to)

For my case, crystal plasticity/thermomechanical .. sometimes I had to reduce (given below) to make it work..

1e-6, 1., 1e-09, 1.

Good Luck..

you may also get better results using

*controls, analysis=discontinuous