Urgent help :Abaqus solution divergence in CAE but not in Input file 3

[biofriend]

Hi Everyone

I have a very weird problem with abaqus .I have recieved an input file and when i run this,it works well . But my own made model which is exactly (100%) the same in BCs , interactions,steps,geometry ,etc. just doesnt work ,i mean it gives an error of too many attempts and exits in about half time of the total time. Since i want to develop the model i need to make my own model in CAE ,I have rechecked and recreated the model for hundreds of time (no exaggeration!),i really need help ,i'm very short with time.

Very thanks in advance

 

[johnhors]

biofriend,

Your CAE model will produce an input file to send to the solver, have you not compared this with the file you received? Comparing the two should yield some clues as to what is going wrong with your CAE model.

 

[mrgoldthorpe]

It appears that it might be a non-linear analysis (in terms of material, geometry or perhaps contact conditions). Although the BCs etc are the same, you perhaps have differences in the mesh in the CAE model, which is perhaps giving trouble in that region.

Look at the .msg file to see what is happening. Is it the residual force or displacement change convergence test that tends to fail. If the latter, where is that particular node in the mesh: are the two meshes slightly different in that region? Is there contact? If so, is that failing to converge.

In your CAE model select the option that provides the following in the step that fails
*CONTROLS, ANALYSIS=DISCONTINUOUS
(I don't use CAE to create models so don't know how you select that.) This option provides for more iterations and line-searching in severely non-linear analyses. It takes more CPU time, but it might solve your problem.

 

[biofriend]

Thanks For both of you my friends.
I have severly checked and compared the two input files.Both of them are almost the same and the mere differences are in Nodes(both in model definition part and in meshing)and just that.I discovered a weird thing.When i increase the number of elements(meshes) in order to get more precise answers , the analysis fails to converge (when the elements number is more than for example 7000)and when i reduce their number to 3000 it answers but the solution is not very reliable and precise, i was very happy that i could solve it after all but yet i have to work on it to make it more precise.
and what " mrgoldthorpe " says seems right,the non-linearity exists, but when previously when i decided to increase default iteration numbers it was of no help,time increments goes even through very small amounts of 1e-20 but it still can not converge,it seems that when it doesnt want to converge ,making time increments too small and increasing number of iterations can not be of any help sometimes.
But i still have to check about *CONTROLS, ANALYSIS=DISCONTINUOUS , i have no idea about it.

Thank you very much again and wish you all bests of luck.

 

[mizzjoey]

Basically analysis=disontinuous tells your solver that the problem would be nonlinear instead of linear, so it doesn't get confused when the values jump through the iterations.

*Controls would come after *Step. Try adding the two lines after your step specification. Did you check if the nonlinear option is swtiched to ON?
Look for NLGEOM=OFF in the step function and then change that to =ON.

Sometimes i add
*CONTROLS, PARAMETERS=FIELD, FIELD=DISPLACEMENT
,100.0

This sets the displacement ctrl to 100% instead of the 5% default. The values in 2nd line are force tol, disp tol.

I'm sure the documentation has some instructions about ctrl settings. Try looking up the *Controls in the manual. If you say your model has nonlinearity, usually the high jumps in stress/strain exceeds the default settings for the iteration to continue - subsequently the solver drops the job.

hope this helps,
jo

 

[biofriend]

Thanks mizzjoey ,
I didn't completely get all of what you have said,
Nlgeom is on,thats ok cause the step is visco and its very vital.
Do you mean step controls or contact controls?
"Try adding the two lines after your step specification" where is should do this? what do you mean by line?
and this : *CONTROLS, PARAMETERS=FIELD, FIELD=DISPLACEMENT
,100.0
sorry i wasn't sure about these so i decided to ask you,
thanks very much for your help.

 

[mizzjoey]

No worries

Your input deck should go like this

*Step, name=Step-1
<step options>
**
*Controls, analysis=discontinuous
*Controls, parameter=field, field=displacement
, 100.
**
<Then you proceed with your boundary conditions and such>
**
*End step

Easy huh? You can use this line to relax the tolerance of your Standard solver. But I suggest you go through the manual as you use the cards. You may not understand it at first (i know I didn't), but as you go back to the manual btwn manipulating the software some things will reveal their mysteries to you

Good luck!
jo

 

[biofriend]

Many thanks to you all my friends and especially
Dear mizzjoey

this is possibly(hopefully)my last question and then the case is broken;
I searched and added and changed these :
1- Using quasi newtonian instead of newtonian
2- time incrementation:chose discontinuous analysis
3- added to line search algorithm(changed N from default of 5 to 10 and etha(accuracy) from 0.1 to 0.01)

AND IT WORKED!!!
but how much the result is reliable ??? ,i know some alteration like stabilization may mystify the reliablity of the results, and here the values of results are a little suspicious, are these changes that i made safe ?

I'm very thankful for your time

 

[biofriend]

Once again
Although these thechniques help the solution to converge but as i increase the number of mesh elements it fails again. In the message there is a sign of one/more elements excessively distorted . I checked adjust inistial overclosure in interaction module and also checked automatic tolerances but it still exists . I think i need to use adaptive remeshing to avoid this excessive distortion which also doesn't apparently works with quadratic elements. What's your idea? Am i right?

Thanks again

 

[mrgoldthorpe]

biofriend,
I suspect the problem is that you are are using non-linear geometry in conjunction with non-linear material behaviour (creep) and a lot of mesh refinement, since you said above on 17 Oct 08 17:11: "...as i increase the number of mesh elements it fails again. In the message there is a sign of one/more elements excessively distorted..." Are you aware what NLGEOM does? It updates the nodal coordinates by the displacement increment at each increment. If you have excessive displacement and a fine mesh you can get distorted elements, and so poor convergence.

We via eng-tips don't quite know what you are doing, but you are obviously changing the mesh to be different to the 'input file' version you first received. You must stop and think about what your objectives are, and why you are doing what you are doing.

A more detailed description and perhaps a drawing would be handy.

 

[mizzjoey]

I would agree with mr goldthorpe.

To biofriend, i'm always happy to make a friend in eng-tips
Please bear in mind that how successfully your analysis proceeds depends also on how you expect the model to behave vs its setting-up. When you run an analysis you should have a reasonable 'guess' or idea what results you expect, how your components should deform or interact with each other for example (might come with more experience, so I understand your difficulty at this stage; I still haven't developed an intuition myself). This is why some mesh might give you results and some might not even when you use the same component with same dimensions.

I suggest what you do is look at your deformed body (the nonconvergence). Do you see any area where the mesh has distorted too much? Any idea what caused this distortion and if there is another option/method of meshing that may avoid the mesh distortion? May I also suggest you compare the deformed body of the converged analysis with the one that did not converge? Capturing the image and linking it here would be a good idea as well, so we can see how it looks like and give suggestions. That is, if you don't have confidentiality issues

jo

 

[biofriend]

Hi
Dears mrgoldthorpe,mizzjoey
Thanks

I am very happy to make good firends like you too,I mean it.
At the moment,due to some complexities i have to do some multitasking to which i am not at all accustomed(single time,single job).In a few days(about5-6 days) i will provide you with some photos so that you can have a mental picture of it,The confidentiality exists but not in this level and besides i know that you will keep it in the closet

I wish you all bests

 

[biofriend]

First of all I have to apologize for the interval between my replies,
I was on a trip to other cities for a couple of weeks.

For a better understanding of the model:
there are two photo links below the message,
As you might see in the photos, the physical model is very simple:
An axisymmetric model of a pipette sucking an spherical gel inside.
Material model : 3 parameters viscoelastic (SLS) for the gel
Analytical rigid for pipette


The main problem which arises everywhere is "too many attempts" problem which I think may be due to excessive distortion of the elements.

The important remark is :

For the instantaneous Elasticity when I put the real value it doesn't converge but when I multiply it by 10 it works. This suggests that the harder the gel is , it is more likely for the process to be converged.
However it is clear that I can not manipulate the real values and increase them in order to elicit an answer!
Changing meshing quality also helps but just a little and can not thoroughly eliminate the problem.

What is your opinion? what shall I do now?

Thanks

Photos :
1-

http://files.engineering.com/getfile.aspx?folder=b701fb87-7f6e-4d16-9700-63d1623e7cec&file=1.JPG

2-

http://files.engineering.com/getfile.aspx?folder=55bd768e-91cc-40f4-9949-34b896f2b9c2&file=2.JPG

 

[biofriend]

P.S

As far as i know , dynamic/explicit works well in these kind of problems but since the density of the gel is unknown,this method can not be securely exploited.

 

[mrgoldthorpe]

biofriend,

In any kind of large deformation problem like yours the mesh eventually becomes excessively distorted, and so the accuracy of affected elements declines until a converged solution becomes impossible. Tricks like altering *CONTROLS will only delay the inevitable, depending how far you are drawing the gel up the pipette.

I think you'll have to remesh the latest reasonably converged solution (with not too much element distortion) and *MAP SOLUTION to the new mesh. (You mention adaptive meshing above.)

By the way, why not use first order elements? Your mesh looks fine enough to do this.

As a matter of interest, what are the main output results you require of the analysis? Do these necessitate a highly refined mesh of second order elements?

 

[biofriend]

Dear mrgoldthorpe

Thanks for your prompt ersponse,
I have used tri elements,first order as they show a higher resitence to distortion.Actually its better to obtain the highest accuracy to fit the experimental data but since i'm still experimenting the simulation it was reasonable to use 1st order elements.
My required outputs include the length of aspiration and also tension distribution.The latter is very sensitive to meshing.

Adaptive meshing fails whenever I try to use it the same as the job does.May be it's because I don't know how to use this feature yet.I have to give it a second look and try to learn it more precisely.
Yours,

 

[biofriend]

Hi

As much as i have percieved,Explicit is the only/best way in combination with ALE adaptive meshing to tackle this type of problems.It is clear that it helps the process to go further but it still fails due to distortion:

" There are a total of 2 excessively distorted elements

The elements contained in element set ErrElemExcessDistortion-Step1 have distorted excessively."

What do you recommend me to change safely and effectively? frequency,number of sweeps or use adaptive mesh controls...?

Many thanks for your sense of altruism

 

[xerf]

Some remarks:

*If you expect large elastic strains (>5...10%) you should not use *Elastic but rather hyperelastic.

*If you start altering the values of the control parameters you accept that your solution might contain errors or even even be completely wrong despite the convergence.

 

[biofriend]

Dear Xerf

For the first remark
The material model is considered to be viscoelastic at the time ,I may consider the effect of hyperelasticity later.
And to the 2nd is absolutely yeah!
Unless you're fully aware of what you are changing,which I at the time do not know.

Thanks and regards