fvMeshDistributors: New library for mesh redistribution and load-balancing

Basic support is now provided for dynamic mesh redistribution, particularly for
load-balancing.  The mesh distributor is selected in the optional 'distributor'
entry in dynamicMeshDict, for example in the
multiphase/interFoam/RAS/floatingObject tutorial case when run in parallel using
the new Allrun-parallel script

distributor
{
    type            decomposer;

    libs            ("libfvMeshDistributors.so");

    redistributionInterval  10;
}

in which the 'decomposer' form of redistribution is selected to call the mesh
decomposition method specified in decomposeParDict to re-decompose the mesh for
redistribution.  The redistributionInterval entry specifies how frequently mesh
redistribution takes place, in the above every 10th time-step.  An optional
maxImbalance entry is also provided to control redistribution based on the cell
distribution imbalance:

Class
    Foam::fvMeshDistributor::decomposer

Description
    Dynamic mesh redistribution using the decomposer

Usage
    Example of single field based refinement in all cells:
    \verbatim
    distributor
    {
        type            decomposer;

        libs            ("libfvMeshDistributors.so");

        // How often to redistribute
        redistributionInterval  10;

        // Maximum fractional cell distribution imbalance
        // before rebalancing
        maxImbalance    0.1;
    }
    \endverbatim

Currently mesh refinement/unrefinement and motion with redistribution is
supported but many aspects of OpenFOAM are not yet and will require further
development, in particular fvModels and Lagrangian.

Also only the geometry-based simple and hierarchical decomposition method are
well behaved for redistribution, scotch and ptScotch cause dramatic changes in
mesh distribution with a corresponding heavy communications overhead limiting
their usefulness or at least the frequency with which they should be called to
redistribute the mesh.

tutorials/multiphase/interFoam/RAS/floatingObject/0/U

@@ -20,6 +20,8 @@ internalField   uniform (0 0 0);
 
 boundaryField
 {
+    #includeEtc "caseDicts/setConstraintTypes"
+
     stationaryWalls
     {
         type            noSlip;

tutorials/multiphase/interFoam/RAS/floatingObject/0/alpha.water.orig

@@ -20,6 +20,8 @@ internalField   uniform 0;
 
 boundaryField
 {
+    #includeEtc "caseDicts/setConstraintTypes"
+
     stationaryWalls
     {
         type            zeroGradient;

tutorials/multiphase/interFoam/RAS/floatingObject/0/epsilon

@@ -20,6 +20,8 @@ internalField   uniform 0.1;
 
 boundaryField
 {
+    #includeEtc "caseDicts/setConstraintTypes"
+
     stationaryWalls
     {
         type            epsilonWallFunction;

tutorials/multiphase/interFoam/RAS/floatingObject/0/k

@@ -20,6 +20,8 @@ internalField   uniform 0.1;
 
 boundaryField
 {
+    #includeEtc "caseDicts/setConstraintTypes"
+
     stationaryWalls
     {
         type            kqRWallFunction;

tutorials/multiphase/interFoam/RAS/floatingObject/0/nut

@@ -20,6 +20,8 @@ internalField   uniform 0;
 
 boundaryField
 {
+    #includeEtc "caseDicts/setConstraintTypes"
+
     stationaryWalls
     {
         type            nutkWallFunction;

tutorials/multiphase/interFoam/RAS/floatingObject/0/p_rgh

@@ -20,6 +20,8 @@ internalField   uniform 0;
 
 boundaryField
 {
+    #includeEtc "caseDicts/setConstraintTypes"
+
     stationaryWalls
     {
         type            fixedFluxPressure;

tutorials/multiphase/interFoam/RAS/floatingObject/0/pointDisplacement

@@ -20,6 +20,8 @@ internalField   uniform (0 0 0);
 
 boundaryField
 {
+    #includeEtc "caseDicts/setConstraintTypes"
+
     stationaryWalls
     {
         type            fixedValue;

tutorials/multiphase/interFoam/RAS/floatingObject/Allrun

@@ -4,13 +4,10 @@ cd ${0%/*} || exit 1    # Run from this directory
 # Source tutorial run functions
 . $WM_PROJECT_DIR/bin/tools/RunFunctions
 
-# Set application name
-application=$(getApplication)
-
 runApplication blockMesh
 runApplication topoSet
 runApplication subsetMesh -overwrite c0 -patch floatingObject -noFields
 runApplication setFields
-runApplication $application
+runApplication $(getApplication)
 
 #------------------------------------------------------------------------------

tutorials/multiphase/interFoam/RAS/floatingObject/Allrun-parallel

@@ -0,0 +1,17 @@
+#!/bin/sh
+cd ${0%/*} || exit 1    # Run from this directory
+
+# Source tutorial run functions
+. $WM_PROJECT_DIR/bin/tools/RunFunctions
+
+runApplication blockMesh
+runApplication topoSet
+runApplication subsetMesh -overwrite c0 -patch floatingObject -noFields
+runApplication setFields
+
+runApplication decomposePar
+runParallel $(getApplication)
+runApplication reconstructParMesh
+runApplication reconstructPar
+
+#------------------------------------------------------------------------------

tutorials/multiphase/interFoam/RAS/floatingObject/constant/dynamicMeshDict

@@ -120,4 +120,14 @@ topoChanger
 }
 
 
+distributor
+{
+    type            decomposer;
+
+    libs            ("libfvMeshDistributors.so");
+
+    redistributionInterval  10;
+}
+
+
 // ************************************************************************* //

tutorials/multiphase/interFoam/RAS/floatingObject/system/blockMeshDict

@@ -46,6 +46,7 @@ boundary
             (0 4 7 3)
         );
     }
+
     atmosphere
     {
         type patch;
@@ -54,11 +55,18 @@ boundary
             (4 5 6 7)
         );
     }
+
     floatingObject
     {
         type wall;
         faces ();
     }
+
+    internal
+    {
+        type internal;
+        faces ();
+    }
 );
 
 

tutorials/multiphase/interFoam/RAS/floatingObject/system/decomposeParDict

@@ -16,7 +16,7 @@ FoamFile
 
 numberOfSubdomains 8;
 
-method          scotch;
+method          hierarchical;
 
 simpleCoeffs
 {
@@ -25,7 +25,7 @@ simpleCoeffs
 
 hierarchicalCoeffs
 {
-    n               (2 2 1);
+    n               (2 2 2);
     order           xyz;
 }