convergence problem in Abaqus standard

[Chen1]

I am running a model for uni-axial compression test for a rock sample, the load is applied through displacement control, where the a rigid platen is forced to move a predefined distance. I used static general step in abaqus. i am facing a convergence problem when a strain softening of the rock sample is adopted.

I am wondering how can i overcome that problem in abaqus standard.

I know that abaqus explicit has more capability to overcome convergence problem. so my question is: how can i use abaqus explicit dynamic to solve a static problem.

Again the model is similar to Uniaxial compression test, the problem comes strain softening of the material.

please help me.

 

[IceBreakerSours]

How do you *know* the softening part of the material curve is causing the solution to diverge?

Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[Chen1]

Because when i solved the same problem with elastic-perfect plastic approach, i did not find any problem.

I wish you could help me IceBreakerSour.

Thanks

 

[IceBreakerSours]

Assuming all else is the same, your answer simply says that the changing the material is the reason behind non-convergence. Have you plotted the load vs. displacement and made sure that it is the "softening" that is causing problems? How long (in the .sta file) did the analysis run? What error/warning messages do you see in the .dat and .msg files?

Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[Chen1]

Hello IcebreakerSour,

In .Sta file, 0.224 of the job has been completed. These are the error messages that i found in the .Msg file:-

***WARNING: THE SYSTEM MATRIX HAS 116 NEGATIVE EIGENVALUES.
***WARNING: THE PLASTICITY/CREEP/CONNECTOR FRICTION ALGORITHM DID NOT CONVERGE
AT 96 POINTS

***WARNING: THE SYSTEM MATRIX HAS 8 NEGATIVE EIGENVALUES.
EXPLANATIONS ARE SUGGESTED AFTER THE FIRST OCCURRENCE OF THIS MESSAGE.

8 SEVERE DISCONTINUITIES OCCURRED DURING THIS ITERATION.
8 POINTS CHANGED FROM SLIPPING TO STICKING

***WARNING: THE SYSTEM MATRIX HAS 10 NEGATIVE EIGENVALUES.
EXPLANATIONS ARE SUGGESTED AFTER THE FIRST OCCURRENCE OF THIS MESSAGE.

8 SEVERE DISCONTINUITIES OCCURRED DURING THIS ITERATION.
8 POINTS CHANGED FROM SLIPPING TO STICKING

this message repeated many times.

Again my model is just Uniaxial compression of rock sample, the rock sample is a deformable material, the platens used to apply the load are discrete rigid bodies. There is an interface between the rock sample and the rigid platens. When i solved that model assuming that the mechanical behavior of the material is elastic-perfect plastic, i did not have an problem, while when i changed the material behavior to strain softening which the actual behavior, the model diverges after 0.224 of the job.

I used solution control to overcome the divergence, i changed the residual control factor from 0.005 to 0.01, also i changed the solution correction control from 0.01 to 0.05 and i used analysis = discontinuous.

I am looking forward to your advice.

Thanks

 

[IceBreakerSours]

Try the RIKS procedure. Search the manual for details. It is a displacement control method but it will reach specified loads.

Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[Chen1]

Hello IceBreakerSour,

I used the Riks method, but unfortunately the model did not converge, only 0.29 of the job has been done, and i got that error message.
Too many attempts have made for this increment.

in the Riks method, i used the following information.
Initial arc length = 1
minimum arc legth = 1E-20
max arc length = .1

Again, this model is just a uni-axial compression test for rock sample. the properties of the rock sample are as follow:

E & Newo
300000 0.2

stress & Plastic strain
2000 0
2300 0.005
1500 0.007
900 0.01
200 0.013

As you see there is a strain softening, and that is the main cause for divergence.

 

[IceBreakerSours]

RIKS procedure is precisely used for this sort of problems. Do you need the platens? Why can't they just be analytical rigid surfaces? Have you exploited geometric symmetry? 1/2, 1/4, 1/8th symmetry.. Likewise, have you tried appropriate boundary conditions? Contact and softening are two nonlinearities, because of which Abaqus *may* be having trouble. Try to turn on the NLGEOM flag on and off and see if that helps the simulation.

Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[Chen1]

Yes i need the platens, I guess they can be analytical rigid surfaces, however there is no problem if i used a discrete rigid body, correct? I did not try the symmetric geometry. Do you think that could solve the convergence problems?