How to use revise *CONTROLS command according to msg file? 1

[szleok]

I got problem on convergency

Here is my msg file:

EQUILIBRIUM ITERATION 9

AVERAGE FORCE 2.032E+03 TIME AVG. FORCE 993.
LARGEST RESIDUAL FORCE -5.84 AT NODE 95 DOF 1
INSTANCE: SOIL-1
LARGEST INCREMENT OF DISP. -7.951E-04 AT NODE 2 DOF 1
INSTANCE: SOIL-1
LARGEST CORRECTION TO DISP. 3.755E-07 AT NODE 95 DOF 1
INSTANCE: SOIL-1
FORCE EQUILIBRIUM NOT ACHIEVED WITHIN TOLERANCE.

***ERROR: SOLUTION APPEARS TO BE DIVERGING AND FIXED TIME INCREMENTS HAVE BEEN
CHOSEN. ANALYSIS TERMINATES.


I want to know how to use correct parameters for "CONTROLS command.

Thank to everyone who reply it.

 

[mrgoldthorpe]

Szleok,
You have specified fixed time increments so ABAQUS can't reduce the size of the current increment to improve convergence. Adjust your input file to allow increments to reduce: e.g.

*STATIC
** init'l time period min. max.
** time of step time time
0.5 , 5.00 , 0.0001 , 2.00

allows the increment size go go down to 0.0001 if necessary.

Regards,
MRG

http://www.analysis.demon.co.uk

 

[mrgoldthorpe]

Szleok,

In case you can't resolve your problem using my note posted earlier, here is something I put together a few years ago, using Version 5.8 or earlier for weld modeling. I think all the *CONTROL parameters specified are still in use, and in the same place in Version 6.4. Incidentally, your problem concerns not achieving equilibrium, so the 2nd tip is most appropriate.
Regards,
MRG

"By activating some of the *CONTROL facilities discussed below I have noticed reductions in solution times of more than 70% in a weld modelling problem with little or no change in the precision of results.

Firstly, in both the thermal and mechanical analyses it can save computer time by specifying more iterations per increment to prevent increments being cut-back, as follows:

*CONTROLS, PARAMETERS=TIME INCREMENTATION
** Relax checks on rate of convergence:
** IO IR IP IC IL IG
16 , 18 , 20 , 40 , 30 , 6

Secondly, a considerable amount of computer time can be saved by relaxing the convergence tolerances (which incidentally the ABAQUS manual admits are rather tight) as follows:

*CONTROLS, PARAMETERS=FIELD, FIELD=DISPLACEMENT
** ... or *CONTROLS, PARAMETERS=FIELD, FIELD=TEMPERATURE
** Relax solution tolerances:
** R_n^alpha C_n^alpha q_0^alpha q_n^aplha R_p^alpha eps^alpha
0.02 , 0.05 , , , 0.10 ,

Slacker tolerances give only very small differences in the solution that are insignificant, given the approximations inherent in weld modelling.

Finally, activating the (normally switched off) line search facility can lead to far fewer cut-backs, particularly those arising from:
'***WARNING: THE STRAIN INCREMENT HAS EXCEEDED FIFTY TIMES
THE STRAIN TO CAUSE FIRST YIELD AT - POINTS'
Activate the line search facility as follows:

*CONTROLS, PARAMETERS=LINE SEARCH
** Nls Smaxls Sminls fsls etals
4 , , , ,

Line searching is particularly powerful in the mechanical stress analysis stage of weld modelling where the solution direction is constantly changing. The line search facility obtains a better estimate of the solution at each line search iteration.

For more information see the description of *CONTROLS in the ABAQUS User Manual and the section discussing solution techniques."

http://www.analysis.demon.co.uk