That version of Femap is very out of date. If you look at your dat file, you will notice Femap wrote a CVISC element instead of a CBUSH. In that version of Femap, when creating the property for CBUSH(spring/damper) you need to set the formulation specifically to CBUSH instead of "default".
Since your model uses the springs to grounded nodes for stability, you need to make sure you have a nominal stiffness defined for all of the required directions to prevent all 6 rigid body motions of your structure. I would also suggest using an orientation system like basic rectangular as shown below. This makes it easier to understand the direction of each stiffness you input. If you do not use this option, then the x direction for spring stiffness is node A to node B with the orientation vector of the element determining the shear directions like a beam element.
I would strongly suggest running this model in a linear analysis and make sure the model is stable and the reactions are as expected before trying to run a nonlinear analysis.
Next your function for nonlinear spring, it is a force vs deflection curve, it has nothing to do with time, there is no "time" in a static nonlinear/sol106 analysis.
Finally in a case where stiffness needs to be updated with deflection like this, instead of using the "auto" method for iteration control, use "iter" and set the iterations before update to 1.
Thank you Joe very much for your help. I have changed the element type to Cbush but nothing changes. I do believe that the version I'm using is outdated and that causes me a lot of problem. Thank you for your other notes.
The model is stable when loaded in Z (downwards) direction only. When I apply load in Y direction (lateral) I get a problem of stability as you explained. When I use an element with an axial stiffness, the error disappears and the model runs without any problem even for nonlinear analysis.
I think the problem is with the software itself and I'm wondering if I can manually change the dat file to fix that problem.
Thank you again for your help!
There is nothing wrong with the software.
You should always create a linear static analysis before trying to solve nonlinear, if the model does not run in linear statics, it has no chance of running correctly in nonlinear.
I have attached a corrected model set up for linear statics. I changed the element formulation to CBUSH as I mentioned. I input stiffness of 500000 for X,Y,Z on the CBUSH properties based on the average value from the curves you provided and set the orientation to Basic Rectangular. You can see by looking at the dat file these changes. The solution runs, and has reasonable deflections. Now you can worry about input of the nonlinear spring curve by creating a proper function. See below for screenshots for the editing required.