OpenFOAM support

How to get OpenFOAM

The easiest way to start is to get binary packages for your Linux distribution. For example, to get OpenFOAM v2412 on Ubuntu:

# Add the signing key, add the repository, update:
wget -q -O - https://dl.openfoam.com/add-debian-repo.sh | sudo bash

# Install OpenFOAM v2412:
sudo apt-get install openfoam2412-dev

As these steps change your .profile, you need to log out and in again to make OpenFOAM fully discoverable.

Supported OpenFOAM solvers

We support mainstream OpenFOAM solvers such as pimpleFoam and solids4Foam for FSI, buoyantPimpleFoam, buoyantSimpleFoam, and laplacianFoam for CHT, or pimpleFoam and sonicLiquidFoam for FF. Our community has, additionally, tried the adapter with multiple different solvers that support function objects.

Supported OpenFOAM versions

OpenFOAM is a project with long history and many forks, of which we try to support as many as possible. Since several HPC systems only provide older versions, we try to also support a wide range of versions.

We provide version-specific release archives and respective Git branches for:

• OpenCFD / ESI (openfoam.com) - main focus:
  • OpenFOAM v1812-v2412 or newer
  • OpenFOAM v1612-v1806 (not tested)
• OpenFOAM Foundation (openfoam.org) - secondary, consider experimental:
  • OpenFOAM 10
  • OpenFOAM 9
  • OpenFOAM 8
  • OpenFOAM 7
  • OpenFOAM 6
  • OpenFOAM 5.x
  • OpenFOAM 4.0/4.1 (not tested)

Known not supported versions: OpenFOAM v1606+ or older, OpenFOAM 3 or older, foam-extend (any version).

Availability of OpenFOAM packages

We use the Ubuntu repositories of each OpenFOAM vendor for testing. Quick reference for maintainers:

• OpenCFD / ESI (openfoam.com):
  • PPA repository
  • More details on the OpenFOAM documentation.
• OpenFOAM Foundation (openfoam.org):
  • PPA repository
  • More details on the OpenFOAM documentation.
• foam-extend:
  • The project distributes pre-built Debian packages as release artifacts on SourceForge.

The following table gives an overview, including versions that we do not support, but which might be useful for future or historical reference.

Differences between OpenFOAM versions

We take into account the following relevant differences between OpenFOAM versions, compared to the latest OpenCFD version. This list is important for maintainers of version-specific ports of the adapter.

OpenFOAM v1612-v1806

• clockValue: The clockValue.H header is not available (used in preciceAdapterFunctionObject.H).
  • Disable the timers feature, controlled by the ADAPTER_ENABLE_TIMINGS preprocessor variable (set in Allwmake).
• dictionary access: In dictionaries (essentially: in the preciceDict), some methods are not available. These are mainly used in the configuration step in Adapter.C, but also in ForceBase.C.
  • Replace preciceDict.get<fileName>("...") with static_cast<fileName>(preciceDict.lookup("...").
  • Replace preciceDict.get<word>("...") with static_cast<word>(preciceDict.lookup("...")).
  • Replace preciceDict.get<wordList>("...") with static_cast<wordList>(preciceDict.lookup("...")).
  • Replace preciceDict.findDict("...") with preciceDict.subDictPtr("...").
• Db access: In the macro that deals with adding checkpointed fields, some methods are not available.
  • Replace mesh_.sortedNames<GeomField>() with mesh_.lookupClass<GeomField>().sortedToc().
  • Replace mesh_.thisDb().getObjectPtr<GeomField>(obj) with &(const_cast<GeomField&>(mesh_.thisDb().lookupObject<GeomField>(obj))).
• Pointers: std::unique_ptr is not available.
  • Replace std::unique_ptr<T> with Foam::autoPtr<T>.
  • Replace calls to pointer .reset(), such as ForceOwning_.reset(new volVectorField(, with ForceOwning_ = new volVectorField(. Adjust the number of closing parentheses.
  • Replace calls to pointer .get();, such as ForceOwning_.get(), with ForceOwning_.ptr().

OpenFOAM 4 and 5

OpenFOAM 4 was released in June 2016 (GitHub mirror, Doxygen).

OpenFOAM 5 was released in July 2017 (GitHub mirror, Doxygen).

Same as in OpenFOAM v1612-v1806.

OpenFOAM 6

OpenFOAM 6 was released in July 2018 (GitHub mirror, Doxygen). Compared to OpenFOAM 5:

• adjustTimeStep: In the function objects interface, adjustTimeStep() was renamed to setTimeStep().
  • Replace adjustTimeStep() with setTimeStep(), both for the function object and the adapter members.
• setDeltaT: The Time method setDeltaT(..., false) was replaced by setDeltaTNoAdjust(...).
  • Replace setDeltaT(timestepSolver_, false) with setDeltaTNoAdjust(timestepSolver_).
• Case files:
  • In system/fvSolution, replace residualControl with outerResidualControl.

Related work in the adapter: PR #33.

OpenFOAM 7

OpenFOAM 7 was released in July 2019 (GitHub mirror, Doxygen). Compared to OpenFOAM 6:

• fileName: fileName::DIRECTORY was renamed to fileType::directory.
  • Replace this in the Adapter.C.

Related work in the adapter: PR #91.

OpenFOAM 8

OpenFOAM 8 was released in July 2020 (GitHub mirror, Doxygen). Compared to OpenFOAM 7:

• Function objects: Function objects changed behavior, and the execute() method is now also executed at start. See the adapter issue #179 and PR #180.
  • In the beginning of preciceAdapterFunctionObject::read(), add this->executeAtStart_ = false;.
• Thermophysical models: Some properties were moved from the previous TurbulenceModels and transportModels to the new ThermophysicalTransportModels and MomentumTransportModels.
  • In Make/options, replace the following include paths:
    • Remove the include paths to transportModels/incompressible, transportModels/compressible, transportModels/twoPhaseMixture, transportModels/interfaceProperties, transportModels/immiscibleIncompressibleTwoPhaseMixture, TurbulenceModels/turbulenceModels, TurbulenceModels/compressible, TurbulenceModels/incompressible.
    • Add include paths to ThermophysicalTransportModels, MomentumTransportModels/momentumTransportModels, MomentumTransportModels/compressible, MomentumTransportModels/incompressible, transportModels.
    • Remove the linking paths to compressibleTurbulenceModels, incompressibleTurbulenceModels.
    • Add linking paths to thermophysicalTransportModels, fluidThermoMomentumTransportModels, incompressibleMomentumTransportModels.
  • In CHT/KappaEffective.H:
    • Remove the header inclusions turbulentFluidThermoModel.H, turbulentTransportModel.H.
    • Include the headers fluidThermoMomentumTransportModel.H, kinematicMomentumTransportModel.H, thermophysicalTransportModel.H.
    • Remove the variable declarations for turbulence_ (2x), nameRho_, nameCp_, namePr_, nameAlphat_, rho_, Cp_, Pr_ from the compressible and incompressible variants.
    • In the incompressible variant’s constructor signature, remove the nameRho, nameCp, namePr, nameAlphat.
    • Add a new declaration: const Foam::thermophysicalTransportModel& thermophysicalTransportModel_; for each one of the turbulence_ removed.
  • In CHT/KappaEffective.C:
    • Replace all instances of turbulence_ with thermophysicalTransportModel_ and update the respective comments.
    • Replace compressible::turbulenceModel and incompressible::turbulenceModel with thermophysicalTransportModel.
    • Replace turbulenceModel::propertiesName with thermophysicalTransportModel::typeName.
    • In the incompressible variant, remove all lines of code working with nameRho_, nameCp_, namePr_, nameAlphat_ from the constructor (which ends up with an empty body) and the extract() method. Replace the usage of kappaEff_temp with thermophysicalTransportModel_.kappaEff()().boundaryField()[patchID].
    • Replace the const dictionary& CHTDict with const dictionary CHTDict.
  • In CHT/HeatFlux.C and in CHT/HeatTransferCoefficient.C:
    • Replace KappaEff_Incompressible(mesh, nameRho, nameCp, namePr, nameAlphat) with KappaEff_Incompressible(mesh).
  • In FSI/ForceBase.H:
    • Remove the header inclusions immiscibleIncompressibleTwoPhaseMixture.H, turbulentFluidThermoModel.H, turbulentTransportModel.H.
    • Include the headers fluidThermoMomentumTransportModel.H, kinematicMomentumTransportModel.H.
  • In FSI/ForceBase.C, in the ForceBase::devRhoReff():
    • Replace compressible::turbulenceModel with compressible::momentumTransportModel.
    • Replace incompressible::turbulenceModel with incompressible::momentumTransportModel.
    • Replace cmpTurbModel::propertiesName with cmpTurbModel::typeName.
    • Replace turb(mesh_.lookupObject<>()) with turb = mesh_.lookupObject<>() (where const cmpTurbModel& turb).
    • Replace turb.devRhoReff() with turb.devTau().
    • Replace turb.devReff() with turb.devSigma().
    • Replace U(mesh_.lookupObject<>()) with U = mesh_.lookupObject<>() (where const volVectorField& U).
  • In FSI/ForceBase.C, in the ForceBase::mu():
    • Remove the line typedef immiscibleIncompressibleTwoPhaseMixture iitpMixture;.
    • Replace the type iitpMixture with fluidThermo and rename the respective object from mixture to thermo.
    • Replace "mixture" in the lookups with basicThermo::dictName.

Related work in the adapter: PR #130.

OpenFOAM 9

OpenFOAM 9 was released in July 2021 (GitHub mirror, Doxygen). Compared to OpenFOAM 8:

• Function objects: The setTimeStep() method was removed.
  • Remove the method from the preciceAdapterFunctionObject.H and preciceAdapterFunctionObject.C. Adjust the comments for the equivalent method in Adapter.H.
  • Impact: See limitations in adjustable time step size (#261).
• Thermophysical models: Different libraries need to be linked and different headers need to be included:
  • In Make/options, remove the linking of fluidThermoMomentumTransportModels and incompressibleMomentumTransportModels.
  • In Make/options, link to transportModels, momentumTransportModels, incompressibleMomentumTransportModels, compressibleMomentumTransportModels.
  • In CHT/KappaEffective.H, replace the headers fluidThermoMomentumTransportModel.H and kinematicMomentumTransportModel.H with momentumTransportModel.H.
  • In FSI/ForceBase.H, replace the header fluidThermoMomentumTransportModel.H with compressibleMomentumTransportModel.H.
  • In FSI/ForceBase.C, add the header fluidThermo.H.
  • In FSI/ForceBase.C, replace:
    • compressible::momentumTransportModel with compressibleMomentumTransportModel
    • incompressible::momentumTransportModel with incompressibleMomentumTransportModel. Further down, replace the usage const incompressible::momentumTransportModel& with const icoTurbModel&.
• Triangulation: In Adapter.C:
  • Replace the header faceTriangulation.H with polygonTriangulate.H.
• Case files:
  • In constant/dynamicMeshDict, replace solver with motionSolver.
  • In system/fvSolution, replace residualControl with outerCorrectorResidualControl. This was already renamed to outerResidualControl in OpenFOAM 6.

Related work in the adapter: PR #221.

OpenFOAM 10

OpenFOAM 10 was released in July 2022 (GitHub mirror, Doxygen). Compared to OpenFOAM 9:

• Function objects: The method fields() has been made pure virtual, meaning it needs to be implemented.

  • In preciceAdapterFunctionObject.H, implement it as (more of a workaround to avoid implementation):

    virtual wordList fields() const
    {
        return wordList::null();
    }
    

• Physical properties and models: The physicalProperties was replaced by transportModels.
  • In Make/options, replace physicalProperties with transportModels in the included paths and in the linked libraries.
  • In FSI/ForceBase.H, replace kinematicMomentumTransportModel.H with incompressibleMomentumTransportModel.H.
  • In FSI/ForceBase.C, replace basicThermo::dictName with physicalProperties::typeName.
• Fields V0 and V00: The fields V0 and V00 have been removed or renamed (not sure to what).
  • In Adapter.C, method preciceAdapter::Adapter::setupMeshVolCheckpointing(), guard each of these two fields with a if (mesh_.foundObject<volScalarField::Internal>("V0")) (and if (... ("V00")), respectively). Alternatively, remove the implementation of this method altogether.
  • Impact: This might lead to stability issues in FSI simulations with implicit coupling. Check your results.
• Case files: Several changes to the tutorials are needed, read the discussion.

OpenFOAM 11

OpenFOAM 11 was released in July 2023 (GitHub mirror, Doxygen). We do not yet know which are relevant changes. Please help us port the adapter to OpenFOAM 11.

Related work in the adapter: PR #310.

OpenFOAM 12

OpenFOAM 12 was released in July 2024 (GitHub mirror, Doxygen). We do not yet know which are relevant changes. Please help us port the adapter to OpenFOAM 12.

foam-extend

We have not yet documented all related changes that would make the adapter work for foam-extend. See the repository precice/foam-extend-adapter for the latest state and please contribute to this page.

Related work in the adapter: PR #302.

Notes on OpenFOAM features

End of the simulation

The adapter (by default) ignores the endTime set in the controlDict and stops the simulation when preCICE says so.

Let’s see this with more details. During the simulation, both the solver and preCICE try to control when the simulation should end. While in an explicit coupling scenario this is clearly defined, in an implicit coupling scenario the solver may schedule its exit (and therefore the last call to the adapter) before the coupling is complete. See how function objects are called for more details on this.

In order to prevent early exits from the solver, the solver’s endTime is set to infinity and it is later set to the current time when the simulation needs to end. This has the side effect of not calling any function object’s end() method normally, so these are triggered explicitly at the end of the simulation.

Function Objects

In principle, using other function objects alongside the preCICE adapter is possible. They should be defined before the adapter in the system/controlDict, as (by default and opt-out) the adapter controls when the simulation should end and explicitly triggers (only) the end() methods of any other function objects at the end of the simulation. If the end() of a function object depends on its execute(), then the latter should have been called before the preCICE adapter’s execute().

If you want to test this behavior, you may also include e.g. the systemCall function object in your system/controlDict:

functions
{

    systemCall1
    {
        type        systemCall;
        libs        ("libutilityFunctionObjects.so");

        executeCalls
        (
            "echo \*\*\* systemCall execute \*\*\*"
        );

        writeCalls
        (
            "echo \*\*\* systemCall write \*\*\*"
        );

        endCalls
        (
            "echo \*\*\* systemCall end \*\*\*"
        );
    }

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

}

Writing results

As soon as OpenFOAM writes the results, it will not try to write again if the time takes the same value again. Therefore, during an implicit coupling, we write again when the coupling timestep is complete. See also a relevant issue.

Adjustable timestep and modifiable runTime

In the system/controlDict, you may optionally specify the following:

adjustTimeStep  yes;
maxCo           0.5;

runTimeModifiable yes;

The adapter works both with fixed and adjustable timestep and it supports the runTimeModifiable feature. However, if you set a fixed timestep and runTimeModifiable, changing the configured timestep during the simulation will not affect the timestep used. A warning will be shown in this case.