Dear Asgar,

Clear your mind for a minute and forget about your results that derive from this FEA software. Try to see the overall picture here, so as to assess your situation. Now, when you solve the same numerical model by using the force control method (Neumann) or the displacement control method (Dirichlet) the ascending branch should be the same given that you are solving the same model. The expected difference in your results should be in the case where you have a descending branch in your curve that the force method fails to capture. So the first thing that you have to do is to compare the maximum force and the corresponding displacement that result when you apply the force control method, with the corresponding max force and displacement when you apply the displacement control method. If these two are not the same you must make sure that the ascending curves that derive from the two methods are the same up to the point where the force method stops. If this is the case, it means that the force method faces convergence issues and stops prematurely. If you get two different ascending curves then it means that either your model has errors related to your definitions of the nonlinear parameters or the extreme case that the software's algorithmic implementation is not correct (the second scenario is mostly unlike). Now the third case is the case where you don't manage to predict the experimental curve no matter what, which means that the model that your are using is not the optimum one according to the physical problem's conditions thus you should consider using a different material model and/or finite elements.

Regarding the load increment and the displacement increment, it is generally known that the smaller the load/displ increment, the more stable is your solution procedure. The stability of the nonlinear solution procedure depends on many numerical issues, that most of the times you can not control them, given that you are just a user of the software that has no capabilities in reading the numbers and having an inside view during the nonlinear analysis. Therefore, try to make as less changes as possible from analysis to analysis, in order to understand what changed and why, while never forget to apply the "overall picture concept" that I explained to you above when assessing your numerical results.

Regards

That's because the method does not converge, which may in turn be due to several reasons. Try to decrease the time step in the step module.

How can i decrease time step?

My increment size is 1e-10 and initial increment is .002

This is already a low time step. You can also try to increase the maximum number of increments, in the step module too. If that doesn't work the problem must be related to something else I think.

I very change this increment and mesh and other thing but i cant give reply

only when i increase fracture energy in damage field i can get result.

One frequent reason is that the problem becomes instable - for example, when you exceed the flow stress in an ideally plastic material. If the problem occurs directly before the specimen fractures completely, could it be that one of the fractured parts is not constrained afterwards?

my specimen have crack grows and plastic tensile a lot of but it dos'nt fracture completely and an error show that _increment smaller than specify . what can I do?

Try solving the problem by applying displacement control and not force control.This will give you an insight on what is your numerical max strength and if your model derives a descending branch.If this is the case then your numerical model is not capable of capturing the physical problem.

my BC is displacement control i use 2mm displacement for my specimen.

what is the maximum principle stress? when i decrease that i can give result .

have that high effect on p_u curve of fracture simulation?

This is my model and stress at crack tip element

i attach fig

Dear Asgar,

Clear your mind for a minute and forget about your results that derive from this FEA software. Try to see the overall picture here, so as to assess your situation. Now, when you solve the same numerical model by using the force control method (Neumann) or the displacement control method (Dirichlet) the ascending branch should be the same given that you are solving the same model. The expected difference in your results should be in the case where you have a descending branch in your curve that the force method fails to capture. So the first thing that you have to do is to compare the maximum force and the corresponding displacement that result when you apply the force control method, with the corresponding max force and displacement when you apply the displacement control method. If these two are not the same you must make sure that the ascending curves that derive from the two methods are the same up to the point where the force method stops. If this is the case, it means that the force method faces convergence issues and stops prematurely. If you get two different ascending curves then it means that either your model has errors related to your definitions of the nonlinear parameters or the extreme case that the software's algorithmic implementation is not correct (the second scenario is mostly unlike). Now the third case is the case where you don't manage to predict the experimental curve no matter what, which means that the model that your are using is not the optimum one according to the physical problem's conditions thus you should consider using a different material model and/or finite elements.

Regarding the load increment and the displacement increment, it is generally known that the smaller the load/displ increment, the more stable is your solution procedure. The stability of the nonlinear solution procedure depends on many numerical issues, that most of the times you can not control them, given that you are just a user of the software that has no capabilities in reading the numbers and having an inside view during the nonlinear analysis. Therefore, try to make as less changes as possible from analysis to analysis, in order to understand what changed and why, while never forget to apply the "overall picture concept" that I explained to you above when assessing your numerical results.

Regards

One thing to try is to require Abaqus to use more increments in each newton step.

Add

*Controls, analysis=discontinuous

to the .inp-file in the step-Definition (You can also click this somewhere in CAE.)

If the problem persists and the algrotihm still stops at (approximately) the same time value, this probably indicates that there is some inherent instability in your model.

I'm not too familiar with the damage model, but one thing to try is to add some additional hardening to the plastic law beyong that fourth point (just extrapolate linearly to 1, for example), because Damage starts at your maxps value, but the material still deforms until the damage energy is reached, I think.

Dear Asgar,

It is clear now that your model needs to be refined.Given that the thickness of your specimen is very thin, the elements that you are using derive numerical instabilities related most probably to shear locking phenomena, especially when your cracks start to develop. Try using a finer mesh and also see if abaqus has any shell elements that are shearlock free.One shell element that has this attribute is the TRIC shell element proposed by J.Argyris but i am not aware if it is incorporated in Abaqus. If this does not work, try using hexahedral elements.I believe their numerical behavior will be more stable for the case of your geometry. In other words X FEM might not work for this numerical problem due to its unique geometry so if the goal here is to practice with XFEM try modeling a different experimental setup.

Dear Asgar, It is a quite evident that it is a convergence & modelling issue, as it checks for strain within the element... Valuable opinions have been recorded by learned researchers... I would love to go with "Local Global Approach" which is also called as Submodeling... I have successfully applied this on Railway wheel and contact and is available in Thermo-Mech FE Analysis of Railwheel if interest you... However, there is also an sub-modelling paper during 96 in Abaqus Users Conf, may be of help to you

Please more describe

how can i obtain this paper?

The default parameter of attempts per increment ist 5. You can increase the number in CAE by clicking on:

Model ==> Steps ==> "Step-1" (or how you called the step after the initial step with the loads) in the model tree on the left with double-click

==> the menu bar on the top changes ==> click on "Other" ==> "General Solution Controls" ==> "Edit" ==> "Step-1" (or the other name)

==> "Specify" ==> "Time Incrementation" => "more" (the first of the three) ==> parameter "IA" ==> increase this parameter (in my calculation, I took 30)

Greets,

Thomas

Partition your surface and define small partitions as your xfem domain

i faced the same problem and it has no relation with increment size it was due to DOF , so i checked them and made some modifications until i got the analysys copmleted. wish good luck  

I hope your problem is now solved. If not, then, start with smaller loading. The problem your model is encountering is the in convergence of integration points possibly due to excessive deformation due to crack simulation. All the best out.

Some time!!!!!!!

Very much load can be causes of this error

Just:

Decrease the load

I am also getting same error whenever I apply load boundary condition while doing contact analysis. Any solution?

it is probably mesh problem. if your blank has bigger mesh for a specific region than the rigid tools, the rigid parts may exceed the contact tolerance with the specified increment. Therefore the you should reduce the blank mesh size and decrease the minimum step increment.   

I had a few similar issues with very thin PP plastic barrier cups simulations. Mine was due to Nonlinear geometry under the Step module which was on. I turned it off and it worked. 

Try to fully comprehend the physics and how discritisation etc. are governing your case. Then you will be able to sort out the issue.

@Parsa

However, if you simply turn off non-linear geometry, your simulation results will not be correct if there actually is appreciable deformation.

@ Dr. Martin Baeker,

You are totally right. Mine was a case where non-linearity would still be considered a good approximation and also I mentioned understanding the physics etc. to hint him non-linearity may not be the case for him. Honestly, I do not know his case as I did not go through answers.

General rule of thumb, It has to do with the solver and the approach as I think George Markou mentioned might also be geometry refinements. If it were me, however, I would first go with the solving method. He is ought to find out the physics and how it is governed through abaqus processors. Otherwise as you implied Doctor Baeker, any numerical simulations are not reliable yet merely numbers and colorful images.

I was also doing a contact debonding analysis by using the CZM method. I faced these problems and the solution is to maintain all the material values should be consistent. See this file and use as these as units to input values otherwise convergence problem will occur and task running will fail because these reason.

Can anyone tell me what is the meaning of the error "Too many attempts made for this increment" ?

Hello Mr. Mohamadzadeh,

I am guessing that your load is nonlinear. I am also guessing that your physics is accurate, your material definitions are perfect, and that you have used consistent units.

A STEP is conditionally stable. In a non-linear analysis, total load applied in a single STEP is broken into many smaller increments, so that the non-linear path can be followed. All we have to do is to suggest the size of the initial increment, and Abaqus chooses the rest for us (helps in saving a lot of time).

Now, if we have suggested too high an increment size, and the solution does not converge within 16 iterations (iterations are only done in Abaqus/Standard, not Explicit), Abaqus resets the increment size to 25% of the original size mentioned. The calculation is now restarted.

If the increment size is still too big, Abaqus takes 25% of the new-increment again.

This cut happens for 5 times, and if the convergence is still not achieved, then Abaqus stops the analysis with the error message: too many attempts for this increment.

There is a very simple way to solve this: try and reduce the 'Initial increment size' of the STEP (I try to reduce it by a factor of 10~50 for each unsuccessful attempt). I have had to use numbers as low as e-19.

Hope this helps.

try nleogm option it will work...because as I think u are trying crack propogation so there is geometric nonlinearity in your problem...

You can First of all check your Material Properties. Then, if material properties are correct, check interaction properties and if interactions are also ok, then finally try to mesh your model in parts by making partitions. The area of loading should have finer mesh. And if you are getting same error again, then try to remodel your problem.