Have you tried adaptive remeshing instead of creating finer mesh?

Try increasing the number of increments or making the increment as small as possible. Also this error shows that the solution can converge so maybe you need to define an extra BC or properly redefine one of the existing BCa

Thank you for your reply but when I use adaptive mesh the model does not work and there is a massage telling me that the model has a zero element. By the way, when I use Abaqus 6.10 the adaptive mesh works properly but in 6.14 not. I am using these values for the increments : initial :0.001. Min:1e-20. Max:0.01. The model is symmetric about x and y axis and simply supported for the rest.

Hello

try the ABAQUS mailing list

https://groups.yahoo.com/group/ABAQUS

How do you implement the Hashin criterion ?

A subroutine code for the Hashin criterion is available from

"FINITE ELEMENT ANALYSIS OF CARBON FIBER COMPOSITE RIPPING USING ABAQUS"

A Thesis Presented to the Graduate School of Clemson University

In Partial Fulfillment of the Requirements for the Degree Master of Science Mechanical Engineering

by Joy Pederson

December 2006

Little known are ABAQUS built-in models. The following might appeal to you:

VUMAT Continuum damage model for fabric reinforced composites

VUMAT Damage and failure in unidirectional fiber composite materials

These models are hidden; though the information is available from Simulia. Surf to http://www.3ds.com and register. It may be that you need special rights on the site; these can be requested from your regional SIMULIA HQ.

Good luck

Frank

Hello Mazin,

Convergence problem is something we have to learn to live with in implicit damage/fracture evolution analyses. sudden damage growth will often result in loss of stiffness and ill-conditioned stiffness matrix. In your model, please look at your damage initiation like DMICRT parameter. If damage is indeed initiated and the result is converged for that particular step, see if you can find any damage evolution in the model by looking at SDEG for example, which gives you an idea about the stiffness degradation in the elements. Usually, damage evolution in composites is modeled quite nicely and you will see convergence issues when the structure has no strength left, which you can assume as final failure. Introducing fracture mechanics, especially linear elastic fracture mechanics, can however introduce large local instabilities and dynamic modes. see if the analysis stops converging when fracture growth is initiated, this is a very likely scenario. Also looking at the job monitor you have attached, you see severe discontinuities at the non-converged iterations. This is often due to the establishment of contact, which probably indicates the fact that some cohesive elements have been deleted. 

I would try the following:

1) Assuming that you are running *STATIC analysis, try the quasi-static option in the implicit dynamic option (*Dynamic, application=quasi-static), you need a density for your material if you want to use this option. This option uses an implicit Euler integration in time, which is very dissipative and will dissipate some of the dynamic modes that could occur when fracture growth is initiated.

2) If that does not get you where you want to be, you can introduce viscous damping in the *static analysis to dissipate the dynamic modes. I prefer the first option because it does not require any viscous damping factors. 

3) as the last resort, I would try to run the analysis in EXPLICIT. Since you have a quasi-static loading, you can use mass scaling to reduce the analysis time. When I have convergence problems I cannot resolve, I often run the model in EXPLICIT to see what the mechanisms are that are probably causing the convergence problem. This can help you alot in improving the initial model.

I hope this helps.

Kind regards,

Farid

You could try a multiscale composite modeling tool like MultiMechanics  

http://multimechanics.com/abaqus

You may use the adaptive mesh. If, you find a numerical problem, you can use a fine mesh only in the known crack path.