first question - I tried plotting free body resultant force vs time (nice work on the new plotting functionality by the way...) but couldnt find where I can enter the free body forces as a data set.
second question - I am having problems with converging when using non linear plastic material, I define a very simple curve, second point is yield, third is UTS and then I extend the graph to about 150% strain in order to stay within the limits of the stress-strain curve for the length of the solution, but still I have convergence issues with the material (same problem with linear material works fine). any tips on how to define a good material that will not cause convergence issues?
For question 2, it's not your defiintion of the Nonlinear material, but the time step or convergence setting for the solution. Which nonlinear solution are you using, NX Nastran Basic Nonlinear, or Advanced Nonlinear?
One of our other Femap developers is responding to your 1st question.
For Advanced Nonlinear, loads should be applied with a vs. Time function. Generally, I use a simple ramp from 0 to 1 like below and then add a 3rd value to continue at a Y value of 1 like shown below:
Then, for the Advanced Nonlinear Solver settings, I usually start with a the Number of Steps = 100 and a Time Step = .01 (for problems with contact, you may need to set the number of steps higher and the Time Step to a smaller number). For the Interation and Convergence Parameters, I start with setting the Autom Increment to 4..Total Load, Stabilize and I also activate the option for Continue if Non-Positive Definite. Total Load, Stabilize will attempt to automatically adjust the time steps.
If I get the solution to converge, I may change Auto Increment to 1..On and rerun. I usually adjust the Largest Step Multiplier to less then the default of 3.
I usually do the same, 100 steps, just one main different the the continuation of the Vs. time graph to 2, I end the graph at 1, what is the purpose of making the time go to 2?
I will try it.
SInce you cannot get your model to converge, I recommed you switch Auto Increment to 1..On and set the Largest Step Multiplier to 1.
Unless their are other problems with the model, you should be able to find what time step the model will not converge on. If this is a contact problem, I find that lowering the Time Increment value helps.
I reduced it (largest step multiplier) and it did help, I also lowered the time increment and it also helped (used extra time steps on the time where convergence was an issue), still no full convergence but better than before, I will try tweaking with it a little more and see what I get (up untill now the results look pretty good and with correlation to reality and lab tests). BTW - it is a contact problem.
Do you have any news regarding my first question - Free body forces in plotting?