Fluent

General computational fluid dynamics solver (cell-centered FVM). GPUs are supported.

General Information

To obtain and checkout a product license please read Ansys Suite first.

Documentation and Tutorials

Besides the official documentation and tutorials (see Ansys Suite), another alternative source is: https://cfd.ninja/tutorials

Example Jobscripts

The underlying test case are

​
#!/bin/bash
#SBATCH -t 00:10:00
#SBATCH --nodes=2
#SBATCH --ntasks-per-node=40
#SBATCH -L ansys
#SBATCH -p medium ### on Emmy
#SBATCH --mail-type=ALL
#SBATCH --output="cavity.log.%j"
#SBATCH --job-name=cavity_on_cpu
  
module load ansys/2019r2
srun hostname -s > hostfile
echo "Running on nodes: ${SLURM_JOB_NODELIST}"
  
fluent 2d -g -t${SLURM_NTASKS} -ssh  -mpi=intel -pib -cnf=hostfile << EOFluentInput >cavity.out.$SLURM_JOB_ID
      ; this is an Ansys journal file aka text user interface (TUI) file
      file/read-case initial_run.cas.h5
      parallel/partition/method/cartesian-axes 2
      file/auto-save/append-file-name time-step 6
      file/auto-save/case-frequency if-case-is-modified
      file/auto-save/data-frequency 10
      file/auto-save/retain-most-recent-files yes
      solve/initialize/initialize-flow
      solve/iterate 100
      exit
      yes
EOFluentInput
  
echo '#################### Fluent finished ############'
#!/bin/bash
#SBATCH -t 00:59:00
#SBATCH --nodes=1
#SBATCH --partition=gpu-a100:shared ### on GPU-cluster of NHR@ZIB
#SBATCH --ntasks-per-node=1
#SBATCH --gres=gpu:1             # number of GPUs per node - ignored if exclusive partition with 4 GPUs
#SBATCH --gpu-bind=single:1      # bind each process to its own GPU (single:<tasks_per_gpu>)
#SBATCH -L ansys
#SBATCH --output="slurm-log.%j"
 
module add gcc openmpi/gcc.11 ansys/2023r2_mlx_openmpiCUDAaware # external OpenMPI is CUDA-aware
hostlist=$(srun hostname -s | sort | uniq -c | awk '{printf $2":"$1","}')
echo "Running on nodes: $hostlist"
 
cat <<EOF >tui_input.jou
file/read-cas nozzle_gpu_supported.cas.h5
solve/initialize/hyb-initialization
solve/iterate 100 yes
file/write-case-data outputfile1
file/export cgns outputfile2 full-domain yes yes
pressure temperature x-velocity y-velocity mach-number
quit
exit
EOF
 
fluent 3ddp -g -cnf=$hostlist -t${SLURM_NTASKS} -gpu -nm -i tui_input.jou \
       -mpi=openmpi -pib -mpiopt="--report-bindings --rank-by core" >/dev/null 2>&1
echo '#################### Fluent finished ############'
#!/bin/bash
#SBATCH -t 00:10:00
#SBATCH --nodes=2
#SBATCH --ntasks-per-node=4
#SBATCH -L ansys
#SBATCH -p gpu-a100  ### on GPU-cluster of NHR@ZIB
### (on Emmy gpu-a100 is called gpu)
#SBATCH --output="slurm.log.%j"
#SBATCH --job-name=cavity_on_gpu
 
module add gcc openmpi/gcc.11 # external OpenMPI is CUDA aware
module add ansys/2023r2_mlx_openmpiCUDAaware
 
hostlist=$(srun hostname -s | sort | uniq -c | awk '{printf $2":"$1","}')
echo "Running on nodes: $hostlist"
 
cat <<EOF >fluent.jou
; this is an Ansys journal file aka text user interface (TUI) file
parallel/gpgpu/show
file/read-case initial_run.cas.h5
solve/set/flux-type yes
solve/iterate 100
file/write-case-data outputfile
ok
exit
EOF
 
fluent 2d -g -t${SLURM_NTASKS} -gpgpu=4 -mpi=openmpi -pib -cnf=$hostlist -i fluent.jou  >/dev/null 2>&1
echo '#################### Fluent finished ############'

Your job can be offloaded if parallel/gpgpu/show denotes the selected devices with a “(*)”. Your job was offloaded successfully if the actual call of you solver prints “AMG on GPGPU”.

Note

Ansys only supports certain GPU vendors/models: https://www.ansys.com/it-solutions/platform-support/previous-releases Look here for the PDF called “Graphics Cards Tested” of your version… (most Nividia, some AMD)

Note

The number of CPU-cores (e.g. ntasks-per-node=Integer*GPUnr) per node must be an integer multiple of the GPUs (e.g. gpgpu=GPUnr) per node.

Fluent GUI: to setup your case at your local machine

Unfortunately, the case setup is most convenient with the Fluent GUI only. Therefore, we recommend doing all necessary GUI interactions on your local machine beforehand. As soon as the case setup is complete (geometry, materials, boundaries, solver method, etc.), save it as a *.cas file. After copying the *.cas file to the working directory of the supercomputer, this prepared case (incl. the geometry) just needs to be read [file/read-case], initialized [solve/initialize/initialize-flow], and finally executed [solve/iterate]. Above, you will find examples of *.jou (TUI) files in the job scripts.

Iff you cannot set up your case input files *.cas by other means you may start a Fluent GUI as a last resort on our compute nodes. But be warned: to keep fast/small OS images on the compute node there is a minimal set of graphic drivers/libs only; X-window interactions involve high latency.

​
srun -N 1 -p standard96:test -L ansys --x11 --pty bash
 
# wait for node allocation, then run the following on the compute node
 
export XDG_RUNTIME_DIR=$TMPDIR/$(basename $XDG_RUNTIME_DIR); mkdir -p $XDG_RUNTIME_DIR
module add ansys/2023r1
fluent &