Akshay Maniyar
Ansys Employee

Hi javat33489,

Normal Stiffness Factor property appears when the Normal Stiffness property is set to Factor. It enables you to specify the Normal Stiffness Factor. Only non-zero positive values are supported. The usual factor range is from 0.01 – 10. The default value is selected by the application. A smaller value provides for easier convergence but with more penetration.

 Determining a good stiffness value may require some experimentation on your part. To arrive at a good stiffness value, you can try the following procedure as a "trial run":

  1. Use a low value for the contact stiffness to start. In general, it is better to underestimate this value rather than overestimate it. Penetration problems resulting from a low stiffness are easier to fix than convergence difficulties that arise from a high stiffness.
  2. Run the analysis up to a fraction of the final load (just enough to get the contact fully established).
  3. Check the penetration and the number of equilibrium iterations used in each substep. If the global convergence difficulty is caused by too much penetration (rather than by residual forces and displacement increments), FKN (Normal penalty stiffness factor) may be underestimated or FTOLN(Penetration tolerance factor) may be too small. If the global convergence requires many equilibrium iterations for achieving convergence tolerances of residual forces and displacements rather than the resulting penetration, FKN may be overestimated.
  4. Adjust FKN, FTOLN, or SLTO (Allowable elastic slip) as necessary and run the full analysis. If the penetration control becomes dominant in the global equilibrium iterations (that is, if more iterations were used to converge the problem to within the penetration tolerance than to converge the residual forces), you may increase FTOLN to permit more allowable penetration or increase FKN. 

Below Ansys video might help you in understanding the contact penetration.


Thank you,

Akshay Maniyar

How to access Ansys help links

Guidelines for Posting on Ansys Learning Forum