I believe that 1 x 10^10 is the limit that triggers the high max/min stiffness warning.
To put it in a simple example, imagine adding 1 x 10^6 and 1 X 10^-4 (a max/min ratio of 10^10). The result is 1.0000000001 x 10^6. That is getting close to the limit of precision in today's computers (15 or 16 digits normally), so some precision can be lost in the calculation. How the inaccuracy propogates through the solution is difficult to predict. So my suggestion is to be cautious when using results from analyses with such warnings. If you understand why the warning occurs in each model and "know" that it should not influence the answer, then it may be safe to use the results.
As with any analysis, you should check all of the results (displacement, stress, reactions, temperature, heat flows, etc) to check for potential errors.
John Holtz, P.E.
Senior User Experience Designer, Simulation
Current version of Mechanical & Multiphysics: 2013 SP1 (2013.01.00.0012 28-Jun-2012)
I'm not very clear on your question.
But a ratio like this seems too large for current double precision solver.
Usually, it causes unstable, bad accuracy results.
If this response answers your concern, please mark it as "solved".
This value is calculated by measuing the max and min diagonal terms in the system stiffness matrix. Usually it will print as a warning as you see in the log file to indicate your matrices might have some problem. However, under some cases such as when MPCs are used with Penalty method, or some initial boundary condition is used, this warnig can also be seen.
As long as the solver does not give you error messages, you can pretty much ignore it. But as John suggested, do be cautious you observe the results is against your intuitive. If that happens, this warning might give you some clue to check your modeling details.
I have seen only two models that produced problematic results relating to this stiffness warning. The stress results were obviously incorrect, as they appeared in "spots" on the model... like a 12 year old's acne problem. In these cases, the stiffness warning exceeded 1e20. In these cases, the models contained "Gap" or "Boundary Elements" where the stiffness was defined. Changing these gap and boundary element's stiffness to 1e10 solved the problem both times.
Customer Support Engineer
285 Kappa Drive
Pittsburgh, PA 15238