Newton tolerance settings for plasticity problems

[tgross]

Hello,

I am currently performing nonlinear (material and geometric) simulations using parFEAP 8.3.
I am using the full Newton Loop from the FEAP manual (with default tolerance settings):

BATCh
  PETSc ON
  DT,,0.05
  LOOP,time,20
    TIME
      LOOP,, 50
         TANG,,1
      NEXT
      STREss NODE
      REAC, all
     NEXT
END

The linear solves are performed using "-ksp_type cg -pc_type prometheus" with default tolerance settings.
Are there any suggested tolerance settings which are optimized for the combination of FEAP and PETSc?
When comparing the simulations results from parFEAP and Abaqus (same User material implementation) parFEAP needs about twice as many linear solves as Abaqus. Is it somehow possible to reduce the number of iterations by using appropriate tolerance settings in FEAP and PETSc?

Furthermore, is it possible to implement (modify the solve.XXX file) an "inexact Newton method" as proposed by Adams et al. 2004:
http://www.columbia.edu/~ma2325/adams.sc04.pdf


Best regards,
Thomas

[FEAP_Admin]

If you change the tolerances you can adjust the number needed.

To control the level of convergence for the Newton iteration you can use

TOL,,etol,residual_tol

where etol is the energy tolerance (default 10^-16) and residual_tol is the residual tolerance (default 10^-8).  Most commercial codes
have defaults that are substantially weaker, say 10^-3 on the residual.

You can control the degree of convergence for the linear solves and make it however inexact as you want with

TOL,ITER,rtol,abstol,dtol,pmaxitr

where, rtol is the residual tolerance, abstol is the absolute tolerance, dtol is the divergence tolerance, and pmaxitr is the maximum number of iterations
to take during the linear solve.  The defaults are 10^-8, 10^-16, 10^+16.  pmaxitr defaults to what ever PETSc defaults to.