Mechanical APDL Basic Analysis Guide - Ansys

Chapter 5: Solution
The PCG solver primarily solves for displacements/rotations (in structural analysis), temperatures (in thermal
analysis), etc. The accuracy of other derived variables (such as strains, stresses, flux, etc.) is dependent upon
accurate prediction of primary variables. Therefore, ANSYS uses a very conservative setting for PCG tolerance
(defaults to 1.0E-8) The primary solution accuracy is controlled by the PCG. For most applications, setting
the PCG tolerance to 1.0E-6 provides a very accurate displacement solution and may save considerable CPU
time compared with the default setting. Use the EQSLV command to change the PCG solver tolerance.
Direct solvers (such as the sparse direct solver) produce very accurate solutions. Iterative solvers, such as
the PCG solver, require that a PCG convergence tolerance be specified. Therefore, a large relaxation of the
default tolerance may significantly affect the accuracy, especially of derived quantities.
The PCG solver does not support SOLID62 elements.
With all iterative solvers you must verify that the model is appropriately constrained. No minimum pivot is
calculated and the solver will continue to iterate if any rigid body motion exists.
In a modal analysis using the PCG solver (MODOPT,LANPCG), the number of modes should be limited to
100 or less for efficiency. PCG Lanczos modal solutions can solve for a few hundred modes, but with less
efficiency than Block Lanczos (MODOPT,LANB).
When the PCG solver encounters an indefinite matrix, the solver will invoke an algorithm that handles indefinite
matrices. If the indefinite PCG algorithm also fails (this happens when the equation system is ill-conditioned;
for example, losing contact at a substep or a plastic hinge development), the outer Newton-Raphson
loop will be triggered to perform a bisection. Normally the stiffness matrix will be better conditioned after
bisection and the PCG solver can eventually solve all the nonlinear steps.
The solution time grows linearly with problems size for iterative methods so huge models can still be solved
within very reasonable times. For modal analyses of large models (e.g., 10 million DOF or larger), MOD-
OPT,LANPCG is a viable solution method if the number of modes is limited to approximately 100.
Use MSAVE,ON (the default in most cases) for memory savings of up to 70 percent. The MSAVE command
causes an element-by-element approach (rather than globally assembling the stiffness matrix) for the parts
of the structure using SOLID185, SOLID186, SOLID187, SOLID272, SOLID273, and/or SOLID285 elements that
have linear material properties. This feature applies only to static analyses or modal analyses using the PCG
Lanczos method. (You specify these analysis types using the commands ANTYPE,STATIC, or ANTYPE,MODAL;
MODOPT,LANPCG respectively.) When using SOLID186 and/or SOLID187, only small strain (NLGEOM,OFF)
analyses are allowed. The solution time may be affected depending on the processor speed and manufacturer
of your computer, as well as the chosen element options.
5.2.3. The Jacobi Conjugate Gradient (JCG) Solver
The JCG solver also starts with element matrix formulation. Instead of factoring the global matrix, the JCG
solver assembles the full global stiffness matrix and calculates the DOF solution by iterating to convergence
(starting with an initial guess solution for all DOFs). The JCG solver uses the diagonal of the stiffness matrix
as a preconditioner. The JCG solver is typically used for thermal analyses and is best suited for 3-D scalar
field analyses that involve large, sparse matrices.
For some cases, the tolerance default value (set via the EQSLV,JCG command) of 1.0E-8 may be too restrictive,
and may increase running time needlessly. The value 1.0E-5 may be acceptable in many situations.
The JCG solver is available only for static analyses, full harmonic analyses, or full transient analyses. (You
specify these analysis types using the commands ANTYPE,STATIC, HROPT,FULL, or TRNOPT,FULL respectively.)
You cannot use this solver for coupled-field applications (SOLID5 or PLANE13).
102
Release 13.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.