Write a system/preciceDict, set compatible boundary conditions, and activate the adapter in your system/controlDict.

In order to run a coupled simulation, you need to:

  1. prepare a preCICE configuration file (described in the preCICE configuration),
  2. prepare an adapter’s configuration file,
  3. set the coupling boundaries in the OpenFOAM case,
  4. load the adapter, and
  5. start all the solvers normally, from the same directory, e.g. in two different terminals.

If you prefer, you may find an already prepared case in our Tutorial for CHT: Flow over a heated plate.

You may skip the section “Advanced configuration” in the beginning, as it only concerns special cases. You may also find more details in the Pull Request #105, especially for changes regarding the previous, yaml-based configuration format.

The adapter’s configuration file

The adapter is configured via the file system/preciceDict. This file is an OpenFOAM dictionary with the following form:

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      preciceDict;
}

preciceConfig "precice-config.xml";

participant Fluid;

modules (CHT);

interfaces
{
  Interface1
  {
    mesh              Fluid-Mesh;
    patches           (interface);
    locations         faceCenters;

    readData
    (
      Heat-Flux
    );

    writeData
    (
      Temperature
    );
  };
};

The participant needs to be the same as the one specified in the preciceConfig, which is the main preCICE configuration file. The preciceConfig can be a path and needs to be wrapped with quotation marks.

The list modules can contain CHT or/and FSI (separated by space).

In the interfaces, we specify the coupling interfaces (here only one). The mesh needs to be the same as the one specified in the preciceConfig. The patches specifies a list of the names of the OpenFOAM boundary patches that are participating in the coupled simulation. These need to be defined in the files included in the 0/ directory. The names of the interfaces (e.g. Interface1) are arbitrary and are not used.

The locations field is optional and its default value is faceCenters (with faceCentres also accepted), signifying that the interface mesh is defined on the cell face centers. The alternative option is faceNodes, which defines the mesh on the face nodes and is needed e.g. for reading displacements in an FSI scenario.

The values for readData and writeData for conjugate heat transfer can be Temperature, Heat-Flux, Sink-Temperature, or Heat-Transfer-Coefficient. Values like Sink-Temperature-Domain1 are also allowed. For a Dirichlet-Neumann coupling, the writeData and readData can be either:

readData
(
  Heat-Flux
);

writeData
(
  Temperature
);

or:

readData
(
  Temperature
);

writeData
(
  Heat-Flux
);

For a Robin-Robin coupling, we need to write and read both of Sink-Temperature and Heat-Transfer-Coefficient:

readData
(
  Sink-Temperature          // e.g. Sink-Temperature-Solid
  Heat-Transfer-Coefficient // e.g. Heat-Transfer-Coefficient-Solid
);

writeData
(
  Sink-Temperature          // e.g. Sink-Temperature-Fluid
  Heat-Transfer-Coefficient // e.g. Heat-Transfer-Coefficient-Fluid
);

For fluid-structure interaction, writeData can be Force or Stress, where Stress is essentially a force vector scaled by the cell face in spatial coordinates (with any postfix), thus, a conservative quantity as well.readData can be Displacement and DisplacementDelta (with any postfix). DisplacementDelta refers to the last coupling time step, which needs to considered in the case of subcycling.

Configuration of the OpenFOAM case

A few changes are required in the configuration of an OpenFOAM case, in order to specify the interfaces and load the adapter. For some solvers, additional parameters may be needed (see “advanced configuration”).

Boundary conditions

The type of the readData needs to be compatible with the respective boundary conditions set for each field in the 0/ directory of the case.

Read the OpenFOAM User Guide for more on boundary conditions.

CHT

  • For readData(Temperature), use type fixedValue for the interface in 0/T. OpenFOAM requires that you also give a (redundant) value, but the adapter will overwrite it. ParaView uses this value for the initial time. As a placeholder, you can e.g. use the value from the internalField.
interface
{
    type            fixedValue;
    value           $internalField;
}
  • For readData(Heat-Flux), use type fixedGradient for the interface in 0/T. OpenFOAM requires that you also give a (redundant) gradient, but the adapter will overwrite it.
interface
{
    type            fixedGradient;
    gradient        0;
}
  • For readData(Sink-Temperature) or Heat-Transfer-Coefficient, use type mixed for the interface in 0/T. OpenFOAM requires that you also give (redundant) values for refValue, refGradient, and valueFraction, but the adapter will overwrite them.
interface
{
    type            mixed;
    refValue        uniform 293;
    valueFraction   uniform 0.5;
    refGradient     uniform 0;
}

FSI

  • For readData(Displacement) or DisplacementDelta, you need the following:
    • type movingWallVelocity for the interface (e.g. flap) in 0/U,
    • type fixedValue for the interface (e.g. flap) in the 0/pointDisplacement, and
    • solver displacementLaplacian in the constant/dynamicMeshDict.
// File 0/U
interface
{
    type            movingWallVelocity;
    value           uniform (0 0 0);
}

// File 0/pointDisplacement
interface
{
    type            fixedValue;
    value           $internalField;
}

// File constant/dynamicMeshDict
dynamicFvMesh       dynamicMotionSolverFvMesh;
motionSolverLibs    ("libfvMotionSolvers.so");
solver              displacementLaplacian;

Load the adapter

To load this adapter, you must include the following in the system/controlDict configuration file of the case:

functions
{
    preCICE_Adapter
    {
        type preciceAdapterFunctionObject;
        libs ("libpreciceAdapterFunctionObject.so");
    }
}

This directs the solver to use the preciceAdapterFunctionObject function object, which is part of the libpreciceAdapterFunctionObject.so shared library. The name preCICE_Adapter can be arbitrary.


Advanced configuration

These additional parameters may only concern some users is special cases. Keep reading if you want to use nearest-projection mapping, an incompressible or basic (e.g. laplacianFoam) solver, if you are using a solver with different variable names (e.g. a multiphase solver) or if you are trying to debug a simulation.

Nearest-projection mapping

An example for for nearest-projection mapping is provided in the nearest-projection tutorial case. The preCICE documentation contains a detailed description of nearest-projection mappings in preCICE. In summary, we need to explicitly enable the connectivity option to create edges between the interface mesh points and give them to preCICE:

interfaces
{
  Interface1
  {
    mesh              Fluid-Mesh-Centers;
    locations         faceCenters;
    connectivity      false;
    patches           (interface);

    // ... writeData, readData ...
  };

  Interface2
  {
    mesh              Fluid-Mesh-Nodes;
    locations         faceNodes;
    connectivity      true;
    patches           (interface);

    // ... writeData, readData ...
  };
};

This connectivity boolean is optional and defaults to false. Note that connectivity true can only be used with locations faceNodes.

Even if the coupling data is associated to faceCenters in the solver, we can select faceNodes as locations type: the respective data will be interpolated from faces to nodes. Also, connectivity is only needed and supported for writeData. Therefore, we need to split the interface in a “read” and a “write” part, as shown above.

More details about the rationale are given in the following section.

Adapter Implementation

Since OpenFOAM is a finite-volume based solver, data is located in the middle of the cell, or on the cell face centers for a coupling interface. Mesh connectivity can be given to preCICE using the methods setMeshTriangle and setMeshEdge. Using the face centers as arguments for these methods is cumbersome. The main reason is that, although OpenFOAM decomposes the mesh for parallel simulations and distributes the subdomains to different processes, mesh connectivity needs to be defined over the partitioned mesh boundaries. This problem vanishes if we define mesh connectivity based on the face nodes, since boundary nodes can be shared among processors. Therefore, mesh connectivity can only be provided on the face nodes (not on the face centers).

As described already, the data is not stored on the face nodes, but on the face centers. Therefore, we use OpenFOAM functions to interpolate from face centers to face nodes. The following image illustrates the workflow:

nearest-projection

Data is obtained at the face centers, then interpolated to face nodes. Here, we have provided mesh connectivity and finally, preCICE performs the nearest-projection mapping. It is important to notice that the target data location is again the face center mesh of the coupling partner. In the standard CHT case, where both data sets are exchanged by a nearest-projection mapping, this leads to two interface meshes (centers and nodes) per participant. Having both the centers and nodes defined, we can skip one interpolation step and read data directly to the centers (cf. picture solver B).

Additional properties for some solvers

Some solvers may not read all the material properties that are required for a coupled simulation. These parameters need to be added in the preciceDict.

Conjugate heat transfer

For conjugate heat transfer, the adapter assumes that a solver belongs to one of the following categories: compressible, incompressible, or basic. Most of the solvers belong in the compressible category and do not need any additional information. The other two need one or two extra parameters, in order to compute the heat flux.

For incompressible solvers (like the buoyantBoussinesqPimpleFoam), you need to add the density and the specific heat in a CHT subdictionary of preciceDict. For example:

CHT
{
    rho [ 1 -3  0  0 0 0 0 ] 50;
    Cp  [ 0  2 -2 -1 0 0 0 ] 5;
};

For basic solvers (like the laplacianFoam), you need to add a constant conductivity:

CHT
{
    k   [ 1  1 -3 -1 0 0 0 ] 100;
};

The value of k is connected to the one of DT (set in constant/transportProperties) and depends on the density (rho [ 1 -3 0 0 0 0 0 ]) and heat capacity (Cp [ 0 2 -2 -1 0 0 0 ]). The relation between them is DT = k / rho / Cp.

Fluid-structure interaction

The adapter’s FSI functionality supports both compressible and incompressible solvers.

For incompressible solvers, it tries to read uniform values for the density and kinematic viscosity (if it is not already available) from the FSI subdictionary of preciceDict:

nu              nu [ 0 2 -1 0 0 0 0 ] 1e-03;
rho             rho [1 -3 0 0 0 0 0] 1;

Notice that here, in contrast to the CHT subdict, we need to provide both the keyword (first nu) and the word name (second nu). We are working on bringing consistency on this.

Additional parameters in the adapter’s configuration file

Some optional parameters can allow the adapter to work with more solvers, whose type is not determined automatically, their fields have different names, or they do not work well with some features of the adapter.

User-defined solver type

The adapter tries to automatically determine the solver type, based on the dictionaries that the solver uses. However, you may manually specify the solver type to be basic, incompressible or compressible for a CHT or FSI simulation:

CHT
{
    solverType incompressible;
};

This will force the adapter use the boundary condition implementations for the respective type.

Parameters and fields with different names

The names of the parameters and fields that the adapter looks for can be changed, in order to support a wider variety of solvers. You may specify the following parameters in the adapter’s configuration file (the values correspond to the default values):

CHT
{
   # Temperature field
   nameT T1;
   # Thermal conductivity
   nameKappa k1;
   # Density
   nameRho rho1;
   # Heat capacity for constant pressure
   nameCp Cp1;
   # Prandtl number
   namePr Pr1;
   # Turbulent thermal diffusivity
   nameAlphat alphat1;
};

Debugging

The adapter also recognizes a few more parameters, which are mainly used in debugging or development. These are optional and expect a true or a false value. Some or all of these options may be removed in the future.

The user can toggle debug messages at build time.

Coupling OpenFOAM with 2D solvers

The adapter asks preCICE for the dimensions of the coupling data defined in the precice-config.xml (2D or 3D). It then automatically operates in either 3D (normal) or 2D (reduced) mode, with z-axis being the out-of-plane dimension. Read more.

Porting your older cases to the current configuration format

In earlier versions of the adapter, we were using a yaml-based configuration format, with the adapter configuration file usually named as precice-adapter-config.yml. We moved to a OpenFOAM dictionary format in #105, to reduce the dependencies. You may also find the tutorials #69 to be a useful reference (file changes).