My second tutorial: cylinderInChannel

You can find the files for this tutorial under tutorials/fluids/cylinderInChannel.

Tutorial Aims

  • Demonstrate how to perform a fluid-only analysis in solids4foam;
  • Explain how a solids4foam fluid case differs from a standard OpenFOAM fluid case.

Case Overview

Diagram of the flow over a cylinder geometry and mesh

This is the classic "flow over a cylinder in a channel" test case, as analysed by, for example, Ferziger and Peric (2002). The problem is modelled as 2-D. The inlet flow velocity profile is specified (coming in from the left), and the outlet (right) gauge pressure is zero. The upper wall, lower wall and cylinder are no-slip walls.

We assume an incompressible Newtonian isothermal laminar fluid, where the Navier-Stokes governing equations take the form:

\[\nabla \cdot \boldsymbol{v} = 0\] \[\frac{\partial \boldsymbol{v}}{\partial t} + \nabla \cdot (\boldsymbol{v}\boldsymbol{v}) = \nu \nabla^2 \boldsymbol{v} - \frac{1}{\rho} \nabla p + \boldsymbol{f_b}\]

Two pressure-velocity coupling algorithms are available in this tutorial:

PIMPLE (default, pimpleFluid): a segregated predictor-corrector loop:

for all time-steps
    do
        solve momentum equation for U (terms depending on p are calculated explicitly)
        solve pressure equation for p (terms depending on U are calculated explicitly)
    while not converged
end

Newton (newtonIcoFluid): a monolithic Newton–Krylov approach that solves U and p simultaneously using PETSc SNES:

for all time-steps
    solve coupled (U, p) system with Newton–Krylov (SNES)
end

Expected Results

For Re = 100, the flow is expected to be unsteady, with vortices shedding from the cylinder.

Pressure contours (top) and velocity vectors (bottom) from Ferziger and Peric (2002)

Pressure contours (top) and velocity vectors (bottom) from Ferziger and Peric (2002)

Running the Case

The tutorial case can be run using the included Allrun script. Two fluid models are available:

./Allrun                 # default: pimpleFluid (segregated PIMPLE)
./Allrun newtonIcoFluid  # monolithic Newton–Krylov solver (requires PETSc)
./Allrun pimpleFluid     # explicit selection of pimpleFluid

The Allrun script patches constant/fluidProperties to select the requested fluid model before running; ./Allclean restores the default (pimpleFluid). The mesh in Fluent format is converted to OpenFOAM format first, and a force.pdf plot is generated afterwards if gnuplot is installed.

Tip

Remember that a tutorial case can be cleaned and reset using the included Allclean script, i.e. ./Allclean.

Analysing the Results

In the ParaView, a von Kármán vortex street is clearly visible by viewing the pressure field p:

Flow over a cylinder pressure field Pressure field

Delving Deeper

If you would like to learn more about the case, then please continue; if not, how about you check out another tutorial.

Case Structure

The case follows the typical pimpleFoam (or pimpleDyMFoam) case structure:

cylinderInChannel
├── 0
│   ├── U
│   └── p
├── Allclean
├── Allrun
├── constant
│   ├── RASProperties
│   ├── dynamicMeshDict
│   ├── fluidProperties
│   ├── physicsProperties
│   ├── polyMesh
│   │   └── …
│   ├── transportProperties
│   └── turbulenceProperties
├── cylinderInChannel.msh
└── system
    ├── changeDictionaryDict
    ├── controlDict
    ├── fvSchemes
    └── fvSolution

The only difference with a pimpleFoam case is that a constant/physicsProperties dictionary must be present, where the type of analysis is specified:

type     fluid;
//type   solid;
//type   fluidSolidInteraction;

In addition, as this is a "fluid" analysis, a constant/fluidProperties dictionary must also be present. This tutorial supports two fluid models; both coefficient sub-dictionaries are included so that either model can be selected via Allrun without editing the file manually:

fluidModel pimpleFluid;   // switched to newtonIcoFluid by Allrun if requested

pimpleFluidCoeffs
{}

newtonIcoFluidCoeffs
{}
Note

pimpleFluid requires no settings here — PIMPLE parameters are specified insystem/fvSolution as for pimpleFoam. newtonIcoFluid uses PETSc SNESoptions defined in the Up solver block of system/fvSolution.

Apart from specifying the physicsProperties and fluidProperties dictionaries, the case is equivalent to a standard pimpleFOAM case, e.g. in terms of transportProperties, RASProperties, dynamicMeshDict, U, p, fvSchemes, etc.

Code: fluidModel

For the cylinderInChannel test case, we have selected a "fluid" analysis in the physicsProperties dictionary: this means a fluidModel class will be selected; then, we specify the actual fluidModel class to be pimpleFluid (default) or newtonIcoFluid.

The code for the pimpleFluid class is located at:

solids4foam/src/solids4FoamModels/fluidModels/pimpleFluid/pimpleFluid.C

and this code directly ports the pimpleFoam solver code; in particular, see the evolve() function with pimpleFluid.C.