Docs: laplacianFluid

Mon, 01 Jan 0001 00:00:00 +0000

Overview

laplacianFluid solves the transient diffusion equation for a scalar field T on a static mesh. It is a direct port of the stock OpenFOAM laplacianFoam solver into the regionType framework: no velocity field, no pressure-velocity coupling, and no mesh motion are involved — only a single diffusion equation with a constant or field diffusivity DT. Despite the name T, the field is a generic passive scalar and can represent temperature or any other diffusing quantity. It is suitable as a lightweight standalone conduction region, or as one side of a multi-region coupling where only diffusive transport of a scalar is required.

Governing Equations

Diffusion

$$ \frac{\partial T}{\partial t} - \nabla \cdot \left( D_T \, \nabla T \right) = S_T $$

Symbol	Description	Unit
$T$	Transported scalar (e.g. temperature)	K (or scalar-dependent)
$D_T$	Diffusivity	m²/s
$S_T$	Source term (from `fvOptions`)	[T]/s

There is no continuity or momentum equation — laplacianFluid has no velocity field and does not support advection.

Numerical Algorithm

laplacianFluid does not run its own outer solve loop. usesPIMPLE() returns false, and solveRegion(), prePredictor(), momentumPredictor(), pressureCorrector(), and meshMotionCorrector() are all no-ops. Instead:

setCoupledEqns("T") assembles the diffusion equation as an fvScalarMatrix and registers it with multiRegionSystem.
The equation is solved through the standard coupled-matrix path (multiRegionSystem::assembleAndSolveEqns<scalar>("T")), the same mechanism used for DNA-coupled partitioned fields.
getMinDeltaT() returns GREAT, i.e. this region never constrains the global time step — deltaT must be set explicitly (no diffusion-number based adjustable time-stepping is implemented).
On write steps only, postSolve() recomputes the derived output fields gradTx, gradTy, gradTz, and DTgradT = DT * grad(T) if writeGradT is enabled (mirrors laplacianFoam’s write.H).

Non-orthogonal correction caveat: stock laplacianFoam wraps its solve in a while (simple.correctNonOrthogonal()) loop. The coupled-matrix solve path used here has no equivalent non-orthogonal corrector loop, so results will differ from laplacianFoam on non-orthogonal meshes. The closest substitute is the region’s Picard corrector (maxCorr / convergenceTolerance in fvSolution), which re-invokes setCoupledEqns() per iteration.

Sub-Models

Sub-model	Selection mechanism	Notes
`fvOptions`	`system/fvOptions`	Explicit/implicit source terms for `T`

No turbulence, transport-model, or MRF sub-models are used.

Required Fields

Field	Type	Description	Unit
`T`	`volScalarField`	Transported scalar	—
`DT`	`volScalarField`	Diffusivity — read if present, otherwise created uniform from `transportProperties`	m²/s

Additionally created at runtime if writeGradT is enabled (default true):

Field	Type	Description
`gradTx`, `gradTy`, `gradTz`	`volScalarField`	Components of $\nabla T$
`DTgradT`	`volVectorField`	Diffusive flux $D_T \nabla T$

Case Setup

Required dictionaries

constant/transportProperties – diffusivity (DT), if no DT field is supplied
system/fvSolution – T solver settings, SIMPLE.writeGradT flag
system/fvSchemes – discretisation schemes

`multiRegionProperties` entry

regions
(
 ( scalarRegion (laplacianFluid) )
);

`controlDict` (singleRegionMode)

singleRegionMode yes;
regionType laplacianFluid;

Key `fvSolution` settings

solvers
{
 T
 {
 solver PCG;
 preconditioner DIC;
 tolerance 1e-06;
 relTol 0;
 }
}

SIMPLE
{
 writeGradT true; // write grad(T) components and DT*grad(T) at write time
}

`transportProperties`

DT 4e-05; // uniform diffusivity, used if no DT field is present

Coupling

laplacianFluid exposes T via selfCoupledFieldNames(), so it is solved standalone and can also participate as a pure-diffusion side in multi-region interfaces (unlike conductTemperature, whose T is only solved through partitioned coupling):

Interface type	Exchanged fields	Coupling modes
`heatTransferInterface`	`T`, heat flux `q`	partitioned (DNA)
`defaultInterface`	`T`	partitioned (DNA)

Known Limitations

Static mesh only — meshMotionCorrector() is a no-op; moving/deforming meshes are not supported.
No non-orthogonal corrector loop — unlike laplacianFoam, the coupled solve path used here does not iterate over non-orthogonal correctors within a single time step; see the numerical algorithm note above for the workaround.

Tutorials

Tutorial path	Description
`tutorials/singleRegion/laplacianFluid/flange`	Classic OpenFOAM “flange” thermal conduction case (single-region, fixed time step)

References

Alkfri, A., Habes, C., Marschall, H., multiRegionFoam: A Unified Multiphysics Framework for Multi-Region Coupled Continuum-Physical Problems, Engineering with Computers, 2023. DOI: 10.1007/s00366-024-01974-4

multiPhysicsFoam – Diffusion