# 3.2 Running applications in parallel

This section describes how to run OpenFOAM in parallel on distributed processors. The method of parallel computing used by OpenFOAM is known as domain decomposition, in which the geometry and associated fields are broken into pieces and allocated to separate processors for solution. The process of parallel computation involves: decomposition of mesh and fields; running the application in parallel; and, post-processing the decomposed case as described in the following sections. The parallel running uses the public domain openMPI implementation of the standard message passing interface (MPI).

### 3.2.1 Decomposition of mesh and initial field data

The mesh and fields are decomposed using the decomposePar utility. The underlying aim is to break up the domain with minimal effort but in such a way to guarantee a fairly economic solution. The geometry and fields are broken up according to a set of parameters specified in a dictionary named decomposeParDict that must be located in the system directory of the case of interest. An example decomposeParDict dictionary can be copied from the interFoam/damBreak/damBreak tutorial if the user requires one; the dictionary entries within it are reproduced below:

17numberOfSubdomains 4;
18
19method          simple;
20
21coeffs
22{
23    n           (2 2 1);
24}
25
26// ************************************************************************* //

The user has a choice of four methods of decomposition, specified by the method keyword as described below.

simple
Simple geometric decomposition in which the domain is split into pieces by direction, e.g. 2 pieces in the direction, 1 in etc.
hierarchical
Hierarchical geometric decomposition which is the same as simple except the user specifies the order in which the directional split is done, e.g. first in the -direction, then the -direction etc.
scotch
Scotch decomposition which requires no geometric input from the user and attempts to minimise the number of processor boundaries. The user can specify a weighting for the decomposition between processors, through an optional processorWeights keyword which can be useful on machines with differing performance between processors. There is also an optional keyword entry strategy that controls the decomposition strategy through a complex string supplied to Scotch. For more information, see the source code file: $FOAM_SRC/parallel/decompose/scotchDecomp/scotchDecomp.C manual Manual decomposition, where the user directly specifies the allocation of each cell to a particular processor. For each method there are a set of coefficients specified in a sub-dictionary of decompositionDict, named <method>Coeffs as shown in the dictionary listing. The full set of keyword entries in the decomposeParDict dictionary are explained in Table 3.1. Note a change in the syntax of coeffs dictionary. From version 1712 users may now specify a single dictionary with a generic name coeffs. The earlier <method>Coeffs is still supported for backwards compatibility.  Compulsory entries numberOfSubdomains Total number of subdomains method Method of decomposition simple/ hierarchical/ scotch/ metis/ manual/ simpleCoeffs entries n Number of subdomains in , , ( ) delta Cell skew factor Typically, hierarchicalCoeffs entries n Number of subdomains in , , ( ) delta Cell skew factor Typically, order Order of decomposition xyz/xzy/yxz… scotchCoeffs entries processorWeights (optional) List of weighting factors for allocation of cells to processors; is the weighting factor for processor 1, etc.; weights are normalised so can take any range of values. () strategy Decomposition strategy (optional); defaults to "b" manualCoeffs entries dataFile Name of file containing data of allocation of cells to processors "" Distributed data entries (optional) — see section 3.2.3 distributed Is the data distributed across several disks? yes/no roots Root paths to case directories; is the root path for node 1, etc. () Table 3.1: Keywords in decompositionDict dictionary. The decomposePar utility is executed in the normal manner by typing decomposePar On completion, a set of subdirectories will have been created, one for each processor, in the case directory. The directories are named processor where represents a processor number and contains a time directory, containing the decomposed field descriptions, and a constant/polyMesh directory containing the decomposed mesh description. ### 3.2.2 Running a decomposed case A decomposed OpenFOAM case is run in parallel using the openMPI implementation of MPI. openMPI can be run on a local multiprocessor machine very simply but when running on machines across a network, a file must be created that contains the host names of the machines. The file can be given any name and located at any path. In the following description we shall refer to such a file by the generic name, including full path, <machines>. The <machines> file contains the names of the machines listed one machine per line. The names must correspond to a fully resolved hostname in the /etc/hosts file of the machine on which the openMPI is run. The list must contain the name of the machine running the openMPI. Where a machine node contains more than one processor, the node name may be followed by the entry cpu= where is the number of processors openMPI should run on that node. For example, let us imagine a user wishes to run openMPI from machine aaa on the following machines: aaa; bbb, which has 2 processors; and ccc. The <machines> would contain: aaa bbb cpu=2 ccc An application is run in parallel using mpirun. mpirun --hostfile <machines> -np <nProcs> <foamExec> <otherArgs> -parallel > log & where: <nProcs> is the number of processors; <foamExec> is the executable, e.g.icoFoam; and, the output is redirected to a file named log. For example, if icoFoam is run on 4 nodes, specified in a file named machines, on the cavity tutorial in the$FOAM_RUN/tutorials/incompressible/icoFoam directory, then the following command should be executed:

mpirun --hostfile machines -np 4 icoFoam -parallel > log &

### 3.2.3 Distributing data across several disks

Data files may need to be distributed if, for example, if only local disks are used in order to improve performance. In this case, the user may find that the root path to the case directory may differ between machines. The paths must then be specified in the decomposeParDict dictionary using distributed and roots keywords. The distributed entry should read

distributed  yes;
and the roots entry is a list of root paths, <root0>, <root1>, …, for each node

roots
<nRoots>
(
"<root0>"
"<root1>"

);
where <nRoots> is the number of roots.

Each of the processor<N> directories should be placed in the case directory at each of the root paths specified in the decomposeParDict dictionary. The system directory and files within the constant directory must also be present in each case directory. Note: the files in the constant directory are needed, but the polyMesh directory is not.

### 3.2.4 Post-processing parallel processed cases

When post-processing cases that have been run in parallel the user can:

• reconstruct the mesh and field data to recreate the complete domain and fields, which can be post-processed as normal;
• post-process each segment of decomposed domain individually; or
• use ParaView via the option paraFoam -vtk and select the decomposedCase from the GUI whereby the case will be assembled internally

#### 3.2.4.1 Reconstructing mesh and data

After a case has been run in parallel, it can be reconstructed for post-processing. The case is reconstructed by merging the sets of time directories from each processor<N> directory into a single set of time directories. The reconstructPar utility performs such a reconstruction by executing the command:

reconstructPar
Executing reconstructPar without any additional options will process all stored time directories. Specifc times can be processed using the following options:
• -latestTime: latest time only
• -time N: time
• -newTimes: any time directories that have not been processed previously

When the data is distributed across several disks, it must be first copied to the local case directory for reconstruction.

#### 3.2.4.2 Post-processing decomposed cases

The user may post-process decomposed cases using the paraFoam post-processor, described in section 7.1. The whole simulation can be post-processed by reconstructing the case or alternatively it is possible to post-process a segment of the decomposed domain individually by simply treating the individual processor directory as a case in its own right.