In ANSYS Fluent, you can reduce communication and improve parallel performance by increasing the report interval for residual printing/plotting or other solution monitoring reports. You can modify the value for Reporting Interval in the Run Calculation Task Page.
Solution → Run Calculation
Calculate...
Important: Note that you will be unable to interrupt iterations until the end of each report interval.
View factor computations can be accelerated through the viewfac_acc utility that uses a combination of MPI/OpenMP/OpenCL
models to speed up view factor computations. Irrespective of the number
of MPI processes launched, only one MPI process/machine is used for
computing view factors. On each machine, one MPI process spawns several
OpenMP threads that actually compute the view factors. Since only
one MPI process is required per machine, it is recommended that you
start just one MPI process per machine and specify the number of OpenMP
threads to use when running the utility outside of ANSYS Fluent. With
fewer MPI processes, the system memory usage is reduced as well. When
running the utility from inside ANSYS Fluent, the number of viewfac_acc processes will be same as the number of ANSYS Fluent processes.
If OpenCL-capable GPUs are available, then a portion of the view factor
computations are done on GPUs using OpenCL, to further speed up the
computation. At present, this capability is limited to the hemicube
method with the cluster-to-cluster option on lnamd64 and win64 machines.
When using the utility viewfac_acc outside
of ANSYS Fluent, you can specify the following command line options:
-cpu # (default = -2) The
number of OpenMP threads to launch per machine.
-2: The number of MPI processes.
-1: The total number of logical CPU cores.
0: No CPU used.
n: Up to maximum n.
-gpu # (default = 1) The
number of GPU devices to use per machine.
–1: The total number of GPU devices.
0: No GPU used.
n: Up to maximum n.
-gpu_cpu_ratio # (default
= 2.0) The ratio of the work load on 1 GPU vs 1 CPU OpenMP thread.
This is based on the time consumed by the GPU and the CPU. At the
end of the view factor computations, a recommendation is printed for
the GPU/CPU work load ratio to use in future computations.
When using the viewfac_acc utility from inside an ANSYS Fluent session, use the /define/models/radiation/s2s-parameters/compute-clusters-and-vf-accelerated text interface (TUI) command. You will only be prompted for the -gpu and -gpu_cpu_ratio options
(as described previously) and not the -cpu option, as the number of OpenMP threads to launch per machine can
be specified in the Thread Control Dialog Box (see Controlling the Threads for details).
In order to use the GPU for view factor computations, the OpenCL
library should be accessible through the appropriate environment variable
(LD_LIBRARY_PATH on lnamd64 or %path% on win64). By default on lnamd64, /usr/lib64 is searched, but if the library is installed
in another location, then that location should be specified in the LD_LIBRARY_PATH variable.
View factor computations can also be
accelerated through the raytracing_acc utility
that uses the NVIDIA Optix library for tracing the rays. The GPU available
on the machine running the host process is used in such a scenario,
except in a mixed Windows-Linux simulation where the GPU on node-0
is used. An NVIDIA GPU along with CUDA 6.0 is required for using raytracing_acc. At present, this utility is available
only on lnamd64 (Red Hat Enterprise Linux 5/6, and SUSE Linux Enterprise
Server 11) and win64 (Windows 7) machines for 3D problems. In order
to use the utility, the CUDA 6.0 library should be accessible through
the appropriate environment variable (LD_LIBRARY_PATH on lnamd64 or %path% on win64).
When using the raytracing_acc utility
from outside an ANSYS Fluent session, the command line is utility raytracing_acc <input_cluster_file> [output_s2s_file(optional)].
When using the raytracing_acc utility
from inside an ANSYS Fluent session, use the /define/models/radiation/s2s-parameters/compute-clusters-and-vf-accelerated text user interface (TUI) command.
The accelerated discrete ordinates (DO) radiation solver is computationally faster than the standard DO solver, especially when used in parallel, although it may take a larger number of iterations to converge.
After you have selected the DO model in the Radiation Model dialog box, you can enable the accelerated DO solver by using the following text command:
define → models →
radiation → do-acceleration?
If NVIDIA GPGPUs are enabled in the Fluent session, this solver will accelerate the DO computations by using the GPGPUs. In the absence of GPGPUs, this solver can still be used with the CPU cores to accelerate the DO computations. Note that the accelerated DO solver uses the first-order upwind scheme and an explicit relaxation of 1.0.
The accelerated DO solver is incompatible with some models and settings; when necessary, Fluent will automatically revert to the standard DO solver when the calculation is started and print a message about the conflict.
If you plan to use GPGPUs with the accelerated DO solver, it is recommended that you
run NVIDIA’s multi-process server (MPS) before launching ANSYS Fluent using the
following command: nvidia-cuda-mps-control -d. It is known to
improve the robustness and performance of the GPGPU computations with the multiple
Fluent processes.