Warning messages related to negative eigen values while using Abaqus Standard

Hi all,

 I am working on simulation of necking in a uniaxial tension test using sheet specimens of 1 mm sheet thickness. I have given stress strain data upto a plastic strain of 1 , I am using 4 elements in the thickness direction of the sheet.My job is able to complete but with lot of warning messages as follows:

1) The strain increment has exceeded fifty times the strain to cause first yield at 286 points

2) The system matrix has 174 negative eigenvalues.

3) The strain increment is so large that the program will not attempt the plasticity calculation at 15 points

Can anyone please explain the reason for this kind of warning messages and how to resolve them. Is there any effect of these messages in the accuracy of the solution?

Thanks in advance.


Mike Graham's picture

Increment size?

1 and 3 sound like your simulations have pretty extreme changes pretty quick. Refining your time incrementation might help you to have more managable strain increments. This would be the first thing I tried. If this refinement is insufficient, the accuracy of the solution is almost certainly impacted.

Negative eigenvalues indicate some sort of instability, and I cannot guess why they happen for you.  I do not believe they necessarily indicate that your solution is inaccurate, but if I was having issues with negative eigenvalues I would at least be concerned about the reliability of my solutions.

Yixiang Gan's picture

Hi, 1) What kind of


1) What kind of material model are you using in this problem? You may need smaller time increment, or introduce STABILIZE in *Step, *STATIC part (check the ABAQUS manual, it will help).

2) What is the ratio between the thinkness of the sheet and other dimensions? Maybe a plane stress problem will be easier to get a first result for thin sheet in this case.

Dear Yixiang Gan, Thanks,

Dear Yixiang Gan,

Thanks, I am using vonmises material model. I am using the maximim time increment as 1. If I use it same as that of the initial increment size for example(0.001) I haven't recieved a single warning but my computational time has increased a lot. And I also observed that there is no effect of these negative eigen values on the problem what do you say ?

 Secondly the dimensions of the sheet are (100*25*1) mm.




dubuking's picture



 The reason for the warning message is the stability. Generally Abaqus warns such messages for the non-positive definiteness of the system matrix. Although fully implicit backward Euler method is employed during the solution procedure in Abaqus/standard, it is necessary 'small initial time increment' for the elastic-plastic transition region. This is the reason you have no warning message for small time increment (t0 = 0.001). For detaisl, see Ortiz and Popov(IJNME, 1985) and Computational inelasticity (Simo and Hughes).



chenna's picture

Check the FE model

Hi Rohit,


1.) First thing is , there is nothing to do with negative eigenvalues in your present model as you r not testing it for buckling or any kind of dynamic problems. So its purely numerical controlled. Its just numertical instability. This concept u can find in any one of the books on Numerical Methods. With enough step sizes you can get rid of those warnings.

2.)You mesh the model only with QUAD elements. TRAINGULAR elements are too stiff, which are not generally preferred in this type of analysis(Elastic-Plastic). Refine the mesh in the region of necking. This gives you better results.

2.) If possible try to input better stress-strain relations. Because with higher step size increment in stain u may not be capturing the true material behavior.

3.) Then go playing with solution controls. First go with higher step sizes in load increment. If u face problems with that go for small step sizes. If the solution converges with smaller step sizes I think you can spend enough time for that. But if its taking too much time increase step size and rerun.You must comprimise at some point between solution time and accuracy. There is always tug off war in between them. Here use Newton-Raphson method if available, which is better than its counterpart, Euler's method.

4.) Else u run the analysis in different loadsteps, with higher increments in elstic regions and smaller step sizes in elastic-plastic transition and plastic zones. I donno whether you can do it in ABAQUS. I know it can be done in ANSYS. I expect there must be something similar to this.

           Its not a very difficult to do using any of FE softwares. Its a basic E-P analysis. With little effort you can easily do it. 


         In calculating step sizes you can do some hand calculations using material data and input approximate stepsizes. This saves you a considerable amount of time in solution stage of the model.