Isotropic Hardening:Mechanical Model errors

[p282h]

Hi:

I have been trying to simulate residual stress in my mechanical model for laser scanning by importing the thermal data from Heat transfer model into the mechanical model. I have used commmercial FEA codes. My inital model is at 300K and on applying laser heat flux on the activated set of elements the temperature go as high as 2300K. Similarly, the stress should be intially high and become negligible once temperature goes beyond melting and on cooling down the stress should again increase. Although, the simulation seems to follow that trend but it aborts at 11.16 secs instead of completing at the total time step of 13 secs.


It gives the error: The strain increment has exceeded fifty times the strain to cause first yield at 136 points and aborts before completing the Step-2.

http://files.engineering.com/getfil...462-9fe6-531b9662deb7&file=THERMAL_MODEL.docx

 

[mrgoldthorpe]

Look in the msg file to see what's causing the bad convergence. Is it the displacement or force check?

Try re-setting one or two of the *CONTROLS parameters to make the convergence checks a bit less stringent.

Rstrict the maximum increment time in Step 1 to be no more than say 5% of the step time. This will prevent ABAQUS from increasing the increments too much; then having to cut-back.

You could also try:

*CONTROLS, ANALYSIS=DISCONTINUOUS

in Step 1 (check the format of that).

 

[p282h]

Hi mrgoldthorpe:

I am unable to understand what you want me to do. I just followed your advise and typed in *Controls, Analysis=discontinous; for all the steps. I thought as my material yield strength decreased with temperature, so I gave 10e11Pa when the temperature goes beyond 1873K(liquidus temperature), not to make the material yield when it becomes liquid. My analysis aborted with the same previous error when I used yield strength of 10e5Pa at 1873K and 3000K. Currently, I am running the same problem with the above modifications and will let you know. But in the mean time could you please explain to me how to figure out the bad convergence issue.

 

[mrgoldthorpe]

post the .msg file

 

[p282h]

A part of Message file:



CONVERGENCE CHECKS FOR EQUILIBRIUM ITERATION 3


AVERAGE FORCE 3.03 TIME AVG. FORCE 2.78
LARGEST RESIDUAL FORCE -7.78 AT NODE 19854 DOF 1
INSTANCE: PART-1-1
LARGEST INCREMENT OF DISP. 7.297E-06 AT NODE 19838 DOF 1
INSTANCE: PART-1-1
LARGEST CORRECTION TO DISP. 8.093E-06 AT NODE 19838 DOF 1
INSTANCE: PART-1-1
FORCE EQUILIBRIUM NOT ACHIEVED WITHIN TOLERANCE.

***WARNING: THE STRAIN INCREMENT HAS EXCEEDED FIFTY TIMES THE STRAIN TO CAUSE
FIRST YIELD AT 92 POINTS

***WARNING: THE STRAIN INCREMENT IS SO LARGE THAT THE PROGRAM WILL NOT ATTEMPT
THE PLASTICITY CALCULATION AT 12 POINTS


***NOTE: MATERIAL CALCULATIONS FAILED TO CONVERGE OR WERE NOT ATTEMPTED AT ONE
OR MORE POINTS. CONVERGENCE IS JUDGED UNLIKELY.


INCREMENT 192 STARTS. ATTEMPT NUMBER 2, TIME INCREMENT 4.261E-05

 

[Elabbasi]

Interesting problem. Usually when I see warnings that the STRAIN INCREMENT IS SO LARGE it is accompanied by a similar message stating that there is excessive distortion at xxx integration points, and/or another message stating that there are negative eigenvalues. You're not getting either it seems. If true, then you have large strains without excessively large displacements.

That could be due to the big changes that you make in Young's modulus and the Yield stress with temperature. It's tricky when you have such big changes. For example, based on your material properties, if the material is at a low temperature and has accumulated some plastic deformation. Then its temperature rises to say above 1873K the new yield is now very high, but the plastic strain that has accumulated is still there and Abaqus might be finding some cases where this change is too extreme. Couple that with the big drop in Young's modulus and it gets even harder!

Nagi Elabbasi
Veryst Engineering