Products: ABAQUS/Standard ABAQUS/CAE
Parallel execution in ABAQUS/Standard:
reduces run time for large analyses;
is available for shared memory architecture platforms for the direct linear equation solver; and
is available for shared and distributed memory architecture platforms for the iterative linear equation solver.
Technical SupportSystems Information for the current version of ABAQUS).The direct sparse solver used for linear equation solution in ABAQUS/Standard can be executed in parallel to reduce the solution time for large problems. You must specify the number of parallel processors to be used, n. The direct sparse solver does not support MPI-based parallelization mode.
The direct parallel solver will process multiple fronts in parallel, in addition to parallelizing the solution of individual fronts. Since multiple fronts are processed in parallel, the direct parallel solver requires more memory than the serial solver. The memory requirements are not predictable exactly in advance since it is not determined a priori which fronts will actually be processed simultaneously.
| Input File Usage: | Enter the following input on the command line: |
abaqus job=job-name cpus=n For example, the following input will run the job “beam” on two processors: abaqus job=beam cpus=2 |
| ABAQUS/CAE Usage: | Job module: job editor: Parallelization: toggle on Use multiple processors, and specify the number of processors, n |
Parallelization of the domain decomposition-based iterative linear equation solver is achieved by mapping groups of domains to individual processors. To activate the parallel iterative solver, specify the number of CPUs for the job. Both MPI and thread-based parallelization modes are supported with the iterative solver.
For optimal performance, parallel execution of the element operations using the standard_parallel=all option is recommended when using the MPI-based parallel iterative solver.
| Input File Usage: | Enter the following input on the command line: |
abaqus job=job-name cpus=n mp_mode={mpi|threads} For example, the following input will run the job “beam” on two processors with the MPI-based domain-level parallelization method: abaqus job=beam cpus=2 mp_mode=mpi In this case half of the iterative solver domains will be mapped to each of the processors. |
| ABAQUS/CAE Usage: | Job module: job editor: Parallelization: toggle on Use multiple processors, and specify the number of processors, n: Multiprocessing mode: MPI or Threads |
MPI-based parallel execution of the element operations is available in ABAQUS/Standard. If parallel execution of the element operations is used, the solvers will automatically run in parallel as well.
Parallel execution of the element operations is supported only for static stress analyses. It is not supported for analyses that include any of the following:
adaptive meshing (“Defining adaptive mesh domains in ABAQUS/Standard,” Section 7.17.6),
crack propagation (“Crack propagation analysis,” Section 7.10.3),
element matrix output requests (“Element matrix output in ABAQUS/Standard” in “Output,” Section 4.1.1),
import (“Transferring results between ABAQUS analyses: overview,” Section 7.7.1),
matrices (“Defining matrices,” Section 2.10.1),
pressure penetration loading (“Pressure penetration loading,” Section 22.1.6),
substructures (“Substructuring,” Section 7.2),
alternative solution techniques (“Approximate implementation” in “Fully coupled thermal-stress analysis,” Section 6.5.4; “Approximate implementation” in “Coupled thermal-electrical analysis,” Section 6.6.2; “Contact iterations,” Section 8.2.2; and “Solution method” in “Convergence criteria for nonlinear problems,” Section 8.3.3), and
co-simulation (“Co-simulation: overview,” Section 7.9.1).
| Input File Usage: | Enter the following input on the command line: |
abaqus job=job-name standard_parallel=all mp_mode=mpi cpus=n |
| ABAQUS/CAE Usage: | Parallel execution of the element operations is not supported in ABAQUS/CAE. |
When running parallel execution of the element operations in ABAQUS/Standard, specifying the upper limit of the memory that can be used (see “The standard_memory parameter” in “Managing memory and disk use in ABAQUS,” Section 3.5.1) specifies the maximum amount of memory that can be allocated by each process.