Simulation not converging

I am simulating a static structural simulation in which i have imported the temperature data from fluent model. But during simulation i am constantly getting an error "The solver engine was unable to converge on a solution of a nonlinear problem". I have two material in this simulation. First is structural steel (constant properties) and another one is IN718 whose properties are temp. dependent. Can anyone explain me the issues and suggest any solution for this

In the figure top material is IN718 and bottom material is Structural steel.


  • You should check what errors you have in the solver output. This will help you identify where the problem is.

  • I am constantly getting this error message "The solver engine was unable to converge on a solution of a nonlinear problem". Do you mean this ?

  • No, click the "Solution Information" tab and choose "Solver Output" from the drop down menu. This gives you a text file with information about the solver process. Near the bottom it will list the errors that caused the solution to fail. Check what these errors are.

  • Apart from this message I also saw this message

    *** WARNING ***                        CP =    494.562  TIME= 09:35:59

     Equivalent plastic strain increment has exceeded the specified limit   

     value. Since the time increment has reached the minimum value, the    

     iteration is continued with minimum time step used. 

    *** NOTE ***                           CP =    384.812  TIME= 09:34:08

     The incremental plastic strain computed in this iteration is larger    

     than the criterion of 15% leading to bisection. You may try           

     incrementing the load more slowly by increasing the number of substeps 

     or use the CUTCONTROL command to re-specify this criterion. 

    Can you suggest me what is to be done as the next step in order to debug this error.

  • You have a bisection occuring due to the plastic strain increasing very rapidly somewhere in your part, and the solver continues with the minimum step size you have set. Later, the solver fails to converge at a substep in the default 26 iterations, and since you are already at your minimum step size it aborts. You could either increase the number of iterations using the NEQIT command, or increase the maximum number of substeps.

    But before you do that you should check that the displacements and loads you have applied are correct (check units) and that the material parameters are reasonable. To find out where the solver is struggling with convergence you can change "Newton-Raphson residuals" (under solution information) from 0 to 3 and solve the model again. This gives you a new output which shows where the forces are unbalanced. You should also take a look at the force convergence plot (also under solution information) to see how the solver is doing (was it almost converging after 26 iterations, or is it diverging?)

Sign In or Register to comment.