OpenFOAM® v1612+: New boundary conditions
23/12/2016
New wave modelling
Integration of functionality produced by The Environmental Hydraulics Institute IHCantabria
Capabilities include:
- Wave generation
- Solitary wave using Boussinesq theory
- Cnoidal wave theory
- StokesI, StokesII, StokesV wave theory
- Active wave absorption at the inflow/outflow boundaries based on shallow water theory
The following images show some applications using the new code, supplied by IHCantabria
![[Picture]](/releases/openfoam-v1612/img/wave-models-mussels-rafts-small.png)
Mussel Raft
![[Picture]](/releases/openfoam-v1612/img/wave-models-offshore-platform-small.png)
Fixed Offshore Platform
![[Picture]](/releases/openfoam-v1612/img/wave-models-offshore-platform-2-small.png)
Jacket Offshore Platform
The baseline models are described in the reference:
Lara, J.L., Barajas, G., Maza M., Losada I.J. Wave and current interaction under smooth and rough beds with OpenFOAM, 2016
- Source code
- $FOAM_SRC/waveModels
- Examples
- $FOAM_TUTORIALS/multiphase/interFoam/laminar/waveExampleSolitary
$FOAM_TUTORIALS/multiphase/interFoam/laminar/waveExampleCnoidal
$FOAM_TUTORIALS/multiphase/interFoam/laminar/waveExampleStokesI
$FOAM_TUTORIALS/multiphase/interFoam/laminar/waveExampleStokesII
$FOAM_TUTORIALS/multiphase/interFoam/laminar/waveExampleStokesV
- Attribution
- This work was originally supplied to OpenCFD Ltd by The
Environmental Hydraulics Institute IHCantabria - see merge #88
Authors: Javier Lopez Lara, Gabriel Barajas, Inigo Losada - Integration
- The code has been restructured and updated by OpenCFD into a new $FOAM_SRC/waveModels library available to the interFoam family of solvers
- Based on the references
-
- Higuera, P., Lara, J.L. and Losada, I.J. Three-Dimensional Interaction of Waves and Porous Coastal Structures using OpenFOAM. Part I: Formulation and Validation, Coastal Engineering, 83:243-258, 2014
- Higuera, P., Lara, J.L. and Losada, I.J. Three-Dimensional Interaction of Waves and Porous Coastal Structures using OpenFOAM. Part II: Application, Coastal Engineering, 83:259-270, 2014
- Higuera, P., Lara, J.L. and Losada, I.J. Simulating Coastal Engineering Processes with OpenFOAM. Coastal Engineering, 71:119-134, 2013
- Higuera, P., Lara, J.L. and Losada, I.J. Realistic Wave Generation and Active Wave Absorption for Navier-Stokes Models, Application to OpenFOAM. Coastal Engineering, 71:102-118, 2013
New thermal lumped mass condition
The new lumpedMassWallTemperature temperature boundary condition sets a uniform temperature according to an energy balance with a lumped mass model.
The patch is specified as follows:
ceiling
{
type lumpedMassWallTemperature;
kappaMethod fluidThermo;
kappa none;
mass 1000;
Cp 4100;
value uniform 300;
}
{
type lumpedMassWallTemperature;
kappaMethod fluidThermo;
kappa none;
mass 1000;
Cp 4100;
value uniform 300;
}
- Source code
- $FOAM_SRC/TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/lumpedMassWallTemperature
- Examples
- $FOAM_TUTORIALS/heatTransfer/buoyantPimpleFoam/hotRoom
New recycled outlet
The new outletMappedUniformInletHeatAddition temperature boundary condition imposes a temperature constraint based on the average outflow temperature of a user-specified patch, with optional heat addition. This is particularly useful for heat exchanger calculations where the outflow can be recycled into the unit.
The patch is specified as follows:
inlet
{
type outletMappedUniformInletHeatAddition;
outletPatch outlet1;
Q 5; // Heat addition in W
TMin 300;
TMax 500;
value $internalField;
}
{
type outletMappedUniformInletHeatAddition;
outletPatch outlet1;
Q 5; // Heat addition in W
TMin 300;
TMax 500;
value $internalField;
}
- Source code
- $FOAM_SRC/TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/outletMappedUniformInletHeatAddition
- Examples
- $FOAM_TUTORIALS/compressible/rhoPimpleFoam/RAS/TJunction
Updated external coupled conditions
The externalCoupled function object and boundary conditions enable OpenFOAM to be interfaced to external applications, including support for multiple regions and multiple patches. To propagate the information to the external solver efficiently the geometry list is contained in a single file, but segregated by region and patch. The points and face formatting remain consistent, irrespective of the number of faces in the region.
The leading comments in the geometry exchange files have been changed from ”# ” to ”// ” to facilitate parsing of the files with OpenFOAM itself if necessary.
It is also now possible to provide explicit signalling via a message in the sentinel file, i.e. ’status=done’ to indicate that the OpenFOAM case is completed, improving the synchronization of case start and end with the external solver.