Basic openfoa mtutorialsguide

Basic guide to OpenFOAM tutorials
Disclaimer: OpenFOAM® is a registered trademark of OpenCFD Limited, the producer OpenFOAM
software. All registered trademarks are property of their respective owners. This guide is not approved or
endorsed by OpenCFD Limited, the producer of the OpenFOAM software and owner of the
OPENFOAM® and OpenCFD® trade marks.
©Rapid OF Blog Basic OpenFOAM Tutorials Guide v1.0 1

1. Introduction
Practically every question on how to learn OpenFOAM is answered by directing the aspiring
student to tutorials provided with the package. They are instructed to “simply” go through the
tutorials, run and play with them and learn through practice.
It is not far from the truth - we learn best by practice and any time you want to learn something
really well you need to practice it to drill the procedures into your memory. Theory is of course
fundamental, but it’s practice that makes the student skillful in any given field.
There are tens of solvers in OpenFOAM and each of them has few tutorials, so there is a lot to
work through. Naturally, at the beginning you will want to work on the field you are most
interested with, or need for your work or study, and thus you will need to choose a relevant
tutorial(s).
What I want to give you in this guide is a short instruction on each of listed tutorials. I will not go
deep into physics, equations and so on – instead I will cover what happens in each of them from
the procedural side. How the case is set up, are there some additional steps taken, ho the mesh
is set up and some general remarks on physics and boundary conditions.
The tutorials, as found in OpenFOAM installation, are divided by solvers names – each solver
has its own set of tutorials (few of them have only one).
Below you will find a list of solvers with descriptions taken from OpenFOAM official
documentation (to be found in UserGuide.pdf in OF installation or here
http://www.openfoam.org/features/standard-solvers.php). For each solver I have listed the
tutorials available (OF release 2.3.0), a short description of what is done and a screenshot of
the results.
Based on this list you can quickly select the one most useful for you at the time and use it to set
up a case you want to simulate.

2. Basic
laplacianFoam - Solves a simple Laplace equation, e.g. for thermal diffusion in a solid
Tutorial name Description
flange Steady state heat transfer on a flange.
Dirichlet boundary conditions used, two
different temperatures. Includes mesh
conversion from Ansys mesh.
potentialFoam - Simple potential flow solver which can be used to generate starting fields for
full Navier-Stokes codes.
cylinder Solves potential (inviscid steady state) flow around a 2D cylinder. Uses
symmetry boundary condition. /system/controlDict shows how to
automatically generate analytical solution.
pitzDaily Potential flow over backward facing step. Potential flow solver can be
used to generate initial conservative velocity fields for any case (using
appropriate geometry). Utility to use: mapFields
ScalarTransportFoam - Solves a transport equation for a passive scalar
Name Description
pitzDaily Convection-diffusion problem with
temperature being convected with
velocity through Pitz- Daily problem
geometry.

3. Incompressible
adjointShapeOptimization - Steady-state solver for incompressible, turbulent flow of non-
Newtonian fluids with optimization of duct shape by applying ”blockage” in regions causing
pressure loss as estimated using an adjoint formulation
pitzDaily Runs optimization of
Pitz – Daily case to
reach Ua, pa
conditions at the exit.
Applies blockage
(alpha) in regions
which need to be
modified to reach the
desired conditions.
boundaryFoam - Steady-state solver for incompressible, 1D turbulent flow, typically to generate
boundary layer conditions at an inlet, for use in a simulation. Specify inlet velocity and get inlet
distributions of model-relevant turbulence variables.
boundaryLaunderSharma Generates velocity distribution using Launder Sharma k-
epsilon turbulence model. Kinematic viscosity applied using .xy
file. Cyclic symmetry applied on front and back sides.
Generates a ./graphs directory with .xy files with velocity and L-
S k-epsilon model variables distribution for each saved time
step.
boundaryWallFunctions Generates velocity and other turbulence variables distributions
using wall functions formulation. In this case inlet velocity = 0.
boundaryWallFunctionsProfile Uses formulation as the above but ./Allrun script is provided
which runs the case for a set of nu values 9different Re),
generates u+ and y+ values and generates plot comparing the
results with Spalding law.

Figure I-1
Comparison of velocity profiles for the three tutorials
Figure I-2
Comparison of OpenFOAM solution to Spalding law

icoFoam - Transient solver for incompressible, laminar flow of Newtonian fluids
cavity Lid-driven flow in a square shaped
cavity; incompressible and laminar,
basic hex mesh. Widely described in
OpenFOAM user guide.
cavityClipped The above case solved on a geometry with one bottom corner being cut out.
cavityGrade Cavity tutorial using mesh grading
elbow Incompressible laminar flow through
an elbow with side pipe. Imports
mesh from a .msh file.
nonNewtonianIcoFoam - Transient solver for incompressible, laminar flow of non-Newtonian
fluids. Viscosity curve is defined in /constant/transportProperties file.
offsetCylinder Flow of shear-thickening fluid around a
cylinder.

pimpleDyMFoam - Transient solver for incompressible, flow of Newtonian fluids on a moving
mesh using the PIMPLE (merged PISO-SIMPLE) algorithm
mixerVesselAMI2D Solid body motion case (mesh
topology unaltered) with arbitrary
mesh interface. Straight vanes
mixer rotor rotates inside mixer
vessel.
movingCone Simple illustration of mesh
topology technique. A 2D cone is
translated through the domain and
the mesh topology is altered in
line with the movement. Cone
translation induces fluid
movement in the opposite
direction.
oscillatingInletACMI2D Simple illustration of solid body
movement technique +
oscillations set up in
dynamicMeshDict file. Part of the
mesh moves in relation to the rest
but its topology remains
unaltered. Includes also setup of
Arbitrary Mesh Interface.
propeller Propeller rotation simulated as a
solid body movement. Mesh
created with snappyhexmesh.
Refined mesh created by
running ./Allrun.pre which
includes surfaceFeatureExtract.
K-epsilon turbulence model used.
Tutorial also shows how to
calculate forces and moments on
the surface of the propeller.

wingMotion Wing rotation simulated as mesh
deformation. Mesh set up with
snappyHexMesh, initial flow field
(on fixed wing) calculated with
simpleFoam, then mapped onto
initial mesh for pimpleDyMFoam.
K-omega SST turbulence used,
moving mesh set up in
/constant/dynamicMeshDict
Picture to the right shows grid
points displacements.
pimpleFoam - Large time-step transient solver for incompressible, flow using the PIMPLE
(merged PISO-SIMPLE) algorithm
channel395 LES simulation of a flow through a
square shaped channel with
nonuniform initial velocity and
pressure distributions (a vector/value
applied to each node). Cyclic
symmetry boundaries at inlet, outlet
and sides of the channel.
elipsekkLOmega Turbulent flow of air around an
ellipse. kkL Omega (RANS)
turbulence model used. Shows also
how to build mesh automatically from
a smaller block (mirroring and
transformations).
pitzDaily Well known Pitz Daily case solved by
pimple. K-epsilon turbulence used,
uniform inlet velocity and mesh
graded to fit the areas of greatest
velocity gradients.

TJunction Turbulent (k-epsilon) flow of air-like
fluid through T-Junction – a duct with
two outlets. Created to test a case
with two outlets, so mesh is not
refined. Flow induced by pressure
difference.
TJunctionFan As above + fan represented by
baffles introduced in the inlet duct
(createBafflesDict in /system
directory).
pisoFoam - Transient solver for incompressible flow
– les:
motorBike First runs motorBike case using simpleFoam and Spalart-Allmaras RANS
turbulence modeling. The mesh is set up using snappyHexMesh. Next,
clones the calculated flow field and copies LES setup files into case folder,
then runs the case using LES turbulence modeling.
pitzDaily Large Eddy simulation of Pitz-
Daily case. Mesh set up in the
same as for simpleFoam solver.
1-equation eddy SGS model.
k at inlet set as uniform fixed
value.
Does not converge to final
solution within the time specified.
pitzDailyMapped Geometry and overall setup as
above, k at the inlet set as
mapped.

– ras
cavity Flow of air in a cavity, induced by the
movement of the upper wall. Basic mesh not
including boundary layers what is clearly
visible. Turbulence modeled with k-epsilon
model.
cavityCoupledU General setup the same as for the case
above. Coupled PbiCCCG solver for U
vector used. It offers performance benefits if
the number of iterations in each direction is
similar (uniform orthogonal mesh).
shallowWaterFoam - Transient solver for inviscid shallow-water equations with rotation
squareBump Simulates waves propagation on a
square shaped domain excited with a
central force represented as a height
difference. Run setFields before running
the case.

simpleFoam - Steady-state solver for incompressible, turbulent flow
airFoil2D Steady state flow of air around
airfoil, Newtonian fluid model,
Spalart-Allmaras turbulence, C-
type 2D mesh (imported from
external mesher)
mixerVessel2D Air, k-epsilon turbulence, uses
m4 utility to create input file for
blockMesh (allows to use
mathematical formulations to
specify points location). Round
shape container with internal
rotor. Movement of rotor
simulated with the use of
additional, rotating frame of
reference, set up in fvOptions.
motorBike RANS k-omega SST flow model
run on a motorbike + rider
model. Mesh created with
snappyHexMesh tool, initial flow
conditions created with
potentialFoam, forces and
moments calculated through
controlDict defined functions,
streamlines extracted for
external post processing.
pipeCyclic Swirling flow in a pipe. Cyclic
mesh settings shown along with
parametric mesh setup (needs
to have Code Stream
activated), uses realizable k-
epsilon turbulence model.

pitzDaily Steady turbulent (RANS, k-e)
flow over backward facing step.
blockMesh hexagonal 2D mesh
showing advanced edge grading
approach to mesh refinements.
pitzDailyExptInlet Geometry as above, inlet velocity time dependent (from experiment), set
up through type timeVaryingMappedFixedValue utility (needs separate file
with the values defined for U), K-epsilon turbulence model. Streamlines
for post processing generated through additional option in ControlDict.
turbineSiting Calculates wind velocity field
over a hill. Uses k-epsilon
turbulence model (RANS) with
model coefficients adjusted to be
appropriate for atmospheric
boundary layers modeling.
Terrain geometry created from a
STL file using snappyhexMesh.
SRFSimpleFoam - Steady-state solver for incompressible, turbulent flow of non-Newtonian
fluids in a single rotating frame
mixer 3D simulation of a mixer section with
one blade, cyclic boundary
conditions on sides, k-omega SST
turbulence model, in this case
Newtonian fluid used, but possible to
use non-Newtonian fluids.

4. Compressible
rhoCentralFoam - Density-based compressible flow solver based on central-upwind schemes
of Kurganov and Tadmor
biconic25-55Run35 Laminar flow in a double cone duct.
Flow enters from a high velocity free
stream. Already converged solution
imported on blockMesh. Pressure
sampled on walls.
forwardStep Laminar supersonic (Ma=3) flow
through a duct with straight vertical
obstacle. Artificial inviscid gas used,
defined in
constant/thermophysicalProperties to
have the sound of speed = 1m/s.
Development of shock waves can be
observed.
LadenburgJet60psi Cyclic symmetry solution of air laminar
flow field. Initial state loaded from
external source.
obliqueShock Simulation of an oblique shock wave
development. The shock is created
using two different velocities-Mach
numbers at the inlet and top wall of the
domain. Laminar flow and normalized
gas (a = 1m/s) models used.
shockTube Development of a pressure wave in a
simple tube. Wave generated using
setFields to assign pressure and
temperature in specific location

wedge15Ma5 Normalized inviscid gas flow in a
domain with conical obstacle. Top
and bottom boundaries are set as
symmetry planes, thus the case in
fact models a flow over a cone. Flow
velocity is 5m/s, thus – Ma=5 and
shock wave development is observed.
rhoLTSPimpleFoam – Local time stepping transient solver for laminar or turbulent flow of
compressible fluids.
angledDuct Flow of air through a duct with
porosity. Temperature dependent
(Sutherland's) transport model
used, k-epsilon turbulence. Porosity
added in system/fvOptions file.
Mesh created using m4 utility.
rhoPimplecFoam - Transient solver for laminar or turbulent flow of compressible fluids
angledDuct Set up precisely as other angleDuct
cases. Differences due to solver
and run time can be observed.

rhoPimpleDyMFoam - Transient solver for laminar or turbulent flow of compressible fluids for
HVAC and similar applications with moving mesh capability
annularThermalMixer Simulates a mixing process in a mixer
equipped with static baffles on the
external walls and moving rotor in the
center. Rotor movement treated as
solid body motion. Initial conditions set
through /constant/caseSettings –
imported into 0 folder with appropriate
command in boundary conditions files.
Mesh created with snappyHexMesh.
There are two inlets of gas inner
(colder and faster) and outer (warmer and slower).
rhoPimpleFoam - Transient solver for laminar or turbulent flow of compressible fluids for HVAC
and similar applications
les pitzDaily Simulation of air flow through a
tube with backward step and a
nozzle at the exit. Inflow is set
as a turbulent with 2%
fluctuation in the flow direction
and 1% cross flow. 1 equation
eddy SGS model used.
ras angledDuct Flow of air though a square
shaped duct with a porous
section. Porosity added in
system/fvOptions file. Mesh
created using m4 utility; k-
epsilon turbulence used.

cavity Flow of air inside a square shaped
cavity, induced by the movement of
upper wall. K-omega SST
turbulence model used on a very
coarse mesh, thus the results are
only provisional.
mixerVessel2D Mixing of air in a simple straight
vaned 2D mixer. K-epsilon
turbulence used. Movement of
rotor introduced as additional frame
of reference.
rhoSimplecFoam - Steady-state SIMPLEC solver for laminar or turbulent RANS flow of
compressible fluids.
squareBend Flow of air through a 180deg bend.
k-epsilon turbulence, Sutherland
transport models used. Lack of
boundary layer grid – simple
blockmesh grid used.

rhoSimpleFoam - Steady-state SIMPLE solver for laminar or turbulent RANS flow of
compressible fluids
angledDuctExplicit
FixedCoeff
Air flow through square shaped
angled duct with a porosity section
(explicit porosity source).
sonicFoam - Transient solver for trans-sonic/supersonic, laminar or turbulent flow of a
compressible gas
laminar forwardStep Supersonic (Ma=3) flow over
rectangle forward facing step.
Normalized inviscid gas used for
which sound speed = 1m/s.
schockTube Simulation of air behavior when
half of the tube is set to have 10x
lower pressure. Eventual
equalization of pressure can be
observed. SetFields utility used
to set the initial pressure
distribution and sample tool used
to generate p, T and magU
distributions along the central
line of the tube.
ras nacaAirfoil Launder-Sharma k-epsilon,
imported mesh with techniques
shown how to overcome high
skewness; contains also
technique to calculate the airfoil
force coefficients.

prism Supersonic flow of air around a
prism. Top and bottom
boundaries are free stream. k-
epsilon turbulence model used.
Mesh including prism boundary
layer created using blockMesh.
sonicLiquidFoam - Transient solver for trans-sonic/supersonic, laminar flow of a compressible
liquid
decompressionTank Models what happens when a valve of
pressurized water tank is opened. Includes
modeling of compressible liquid (barotropic
model) and pressure waves propagation.

5. Multiphase
cavitatingFoam - Transient cavitation code based on the homogeneous equilibrium model from
which the compressibility of the liquid/vapour ”mixture” is obtained
LES throttle 2D case of water flow through
a narrow duct (throttle). Flow is
induced by pressure difference
between two chambers;
barotropic compressibility model
used, Newtonian fluid model
used for both water and vapor.
Initially no vapor is present in the flow. Flow acceleration creates
pressure drop and induces cavitation around the flow jet.
throttle3D Essentially 2D case, in terms of
hydraulic setup. The mesh is
refined and 10 cells are used in
the “depth” direction (z) instead
of 1. refineMesh utility used on
topological sets (topoSet).
RAS throttle Flow set up as for les/throttle.
Turbulence modeled with k-
omega SST.

compressibleInterDyMFoam - Solver for 2 compressible, isothermal immiscible fluids using a
VOF (volume of fluid) phase-fraction based interface capturing approach, with optional mesh
motion and mesh topology changes including adaptive re-meshing.
sloshingTank2D Movement of water inside a cyclically heeling sloshing tank.
compressibleInterFoam - Solver for 2 compressible, isothermal immiscible fluids using a VOF
(volume of fluid) phase-fraction based interface capturing approach.
deepCharge2D 2D case of the physical setup described
below. The same utilities and settings
used otherwise.
Picture to the left shows the water
volume fraction (alpha.water) at time
step 50. Picture below shows static
pressure contours at one of the initial
steps.
deepCharge3D Before the start of the calculation, there
is a volume filled with water up to half of
its height. setFields utility is used to
insert a sphere of 10x the pressure and
(T+278) inside the water column of
initially uniform pressure and
temperature. Expansion of the sphere is
simulated on a basic hexagonal mesh
(blockMesh).

compressibleMultiphaseInterFoam - Solver for more than 2 compressible, isothermal
immiscible fluids using a VOF (volume of fluid) phase-fraction based interface capturing
approach
damBreak4phase Simulation of 4 immiscible
fluids release. First picture
shows the initial state,
second – end state. The
fluids become sorted by
specific weight. Laminar
case.
interDyMFoam - Solver for 2 incompressible, isothermal immiscible fluids using a VOF (volume
of fluid) phase-fraction based interface capturing approach, with optional mesh motion and
mesh topology changes including adaptive re-meshing.
damBreakWithObstacle 3D dam brake case – a column of
water released against centrally
located obstacle. Mesh dynamically
refining to the front of the wave based
on volumetric fraction of water. Mesh
adaptation set through
constant/dynamicMeshDict.
DTCHull Duisburg Test Case container ship
hull simulation. Mesh created with
snappyHexMesh and refined using
surface STL file. The hull movement
treated as solid body movement with
6 degrees of freedom (no mesh
changes). k-omega SST turbulence
model used.

floatingObject Floating of a cuboid simulated as internal
mesh deformations. Floating object
inserted into a basic hex mesh with
topoSet utility. K-epsilon turbulence
model used.
mixerVesselAMI 3 D simulation of mixing tank. Movement
of the rotor modeled as solid body
motion. Simulates mixing water with air.
Mesh created with snappyHexMesh and
refined with surfaceFeatureExtract utility
and 3 separate STL files for Gas Inlet,
Stirrer and Outlet.
sloshingTank2D Sloshing tank simulated as solid body motion (mesh unaltered).
libsampling tool used to extract walls pressure (ControlDict)
sloshingTank3D 3D case of a solid body motion sloshing
tank water movement simulation.
testTubeMixer Test tube rocking on rotating table.
Modeled as slid body Motion, mesh is
unaltered. Motion described in
dynamicMeshDict.

interFoam - Solver for 2 incompressible, isothermal immiscible fluids using a VOF (volume of
fluid) phase-fraction based interface capturing approach.
laminar capillaryRise Natural wall contact driven rise of
water in a capillary channel.
ConstantAlphaContactAngle =
45deg set in 0/alpha.water file.
damBreak Release of a water column in
air environment against a
vertical obstacle. Laminar flow
model used and basic coarse
hexagonal mesh.
les nozzleFlow2D LES simulation of high
velocity fuel jet with static
air atmosphere. refineMesh
utility used to improve mesh
quality at the fuel-air
interface.
ras damBreak Release of water column in air
environment against a vertical
obstacle. Transient RANS
turbulent flow modeling with k-
epsilon turbulence model, water-
air surface tension has to be set
in constant/transportProperties
file. Initial water column set with
setFields utility.

damBreakPorous
Baffle
Dam break case with additional vertical porous baffle
extending from the mid-length of the center obstacle.
CreateBaffles utility used, along with setFields – for initial
distribution.
waterChannel Gravitational flow of
water through a
narrow channel,
originating in a
slightly higher placed
chamber. The
channel mesh is built
using extrudeMesh
utility. K-omega SST
turbulence model
used. Inlet, outlet and atmosphere fluxes calculated using
additional entries in ControlDict.
weirOverflow Water flowing over weir
barrier. RANS turbulent
flow modeling with k-
epsilon turbulence model.
setFields used for initial
water distribution along
with initial conditions
attached in 0 directory,
which specify water flow
rate.

interMixingFoam - Solver for 3 incompressible fluids, two of which are miscible, using a VOF
method to capture the interface
damBreak Dam break case with 3 phases of
which 'water' and 'other' are miscible.
The miscibility is expressed through
diffusion coefficient to be found in
/constant/transportProperties file.
Initial phases distribution in space set
by setFields utility.
interPhaseChangeDyMFoam - Solver for 2 incompressible, isothermal immiscible fluids with
phase-change (e.g. cavitation). Uses a VOF (volume of fluid) phase-fraction based interface
capturing approach, with optional mesh motion and mesh topology changes including adaptive
re-meshing.
propeller A ship propeller simulation including
cavitation. Propeller mesh is created with
snappyHexMesh including surface
refinements. It is embedded in rotating block
of the domain mesh (solid body rotation).
Mesh is not refined along the simulation.
Initially no vapor is present in the water and
relative propeller water motion is 0. Flow
velocity is then ramped up to 15m/s within
0.01s and propeller rotation – to 628 1/s. Picture to the right shows
propeller velocity with vapor volume overlayed as contours.

interPhaseChangeFoam - Solver for 2 incompressible, isothermal immiscible fluids with phase-
change (e.g. cavitation). Uses a VOF (volume of fluid) phase-fraction based interface capturing
approach
cavitatingBullet Simulation of water cavitation caused by
rapid movement of a bullet. The apparent
bullet speed it 20m/s, flow is laminar and
initially no water vapor is present in the
domain. Mesh created with snappyHexMesh.
LTSInterFoam - Local time stepping (LTS, steady-state) solver for 2 incompressible, isothermal
approach
DTCHull Set up virtually the same as
InterDyMFoam example for the same
geometry. Lacks information on the hull
movement due to static mesh. Thanks to
local time stepping the speed of
calculation is significantly higher than for
dynamic mesh and global time step.
Options included in ControlDict extract
forces and moments for every saved time
step.

MRFInterFoam - Multiple reference frame (MRF) solver for 2 incompressible, isothermal
approach
mixerVessel2D Water (0.25 volume) and air being mixed in a simple 2D mixer. Laminar
flow model used; rotor movement introduced as an additional rotating
frame of reference.
MRFMultiphaseInterFoam - Multiple reference frame (MRF) solver for incompressible fluids
which captures the interfaces and includes surface-tension and contact-angle effects for each
phase
mixerVessel2D Mixing of 4 varying density phases. Rotor movement set using additional
rotating frame of reference. Simple multiphase settings: separate transport
properties for each phase and phase-to-phase surface tension set in
/constant/transportproperties.

multiphaseEulerFoam – Solver for n incompressible fluids with one phase dispersed, e.g. gas
bubbles in a liquid.
bubbleColumn Simulation of air bubbles rising up inside a water
columns. Inlet is located at the bottom, where
volumetric ratio of air and water is 0.5 each and the
inflow velocity of air is 0.1 m/s. Flow is laminar and
mesh is created in blockMesh. Initial water column
created with setFields utility.
dambreak4hase Water, oil, mercury and air released from the
left wall against the obstacle in the center.
Laminar flow model used and coarse mesh –
88x142x1. Interfacial interactions, pair by
pair, described in
/constant/transportProperties.
damBreak4phase
Fine
Fine mesh (344x570x1) simulation of the
case described above. Pockets of entrapped
air visible.
Picture for the previous case shows the same
time snapshot – The overall flow structure is
similar, but differences in multiphase structure
is clearly visible.
mixerVessel2D Straight vanes quasi 2D mixer with 4 different
density fluids and spinning rotor at the center.
The rotor spins thanks to the usage of
additional rotating frame of reference
assigned to the rotor mesh cells. Interfacial
interactions (drag, heat transfer...) included in
constant/interfacialProperties and
transportProperties file.

multiphaseInterFoam - Solver for n incompressible fluids which captures the interfaces and
includes surface-tension and contact-angle effects for each phase
damBreak4phase 4 phases present. Phase properties set in
/constant/transportproperties. In this case
each phase has a separate transport model
defined and on phase-phase level only the
interfacial surface tension (sigma) is defined).
dambreak4phase
Fine
Fine mesh case of the simulation described
above. Details of multiphase structure
differences visible, while overall flow shape is
very similar.
settlingFoam - Solver for 2 incompressible fluids for simulating the settling of the dispersed
phase
dahl Sludge settling simulation. Volumetric
fraction Alpha initially is very low, but with
inflow it reaches the maximum packing limit.
Transport properties of the sludge set in
/constant/transportProperties file.

tank3D Settling of sludge in a tank with one inlet (the
ribs), 3 outlets (on top side) and a conveying
belt (bottom, far end). Properties set as for the
previous case.
twoLiquidMixingFoam - Solver for mixing 2 incompressible fluids.
lockExchange Density difference driven mixing of water and 1%
more dense sludge inside an inviscid walls
column. Kelvin-Helmholtz instabilities develop.
twoPhaseEulerFoam - Solver for a system of 2 incompressible fluid phases with one phase
dispersed, e.g. gas bubbles in a liquid
laminar bubbleColumn Laminar case of air being
released from the bottom of
still water column. Air bubbles
diameter kept constant
(constant/phaseProperties)

bubbleColumnIATE Interfacial Area Transport
Equation used to estimate air
bubbles diameters distribution
(constant/phaseproperties).
The equation calculates the
rate of bubbles break up and
coalescence. Qualitative
difference in the air behavior
clearly visible as the air tends
to form larger voids throughout
the simulation time.
fluidizedbed Laminar case of particles
column being injected with air
stream from the bottom. Even
though the drag model used is
the same as for RAS case
described below, the flow
pattern differs dramatically.
mixerVessel2D Simple straight vanes mixer
where half of the internal
volume is initially filled with
water. Rotor movement
introduced as additional
rotating frame of reference.
m4 script used to create
blockMesh input and rotor
defined using topoSet.
LES bubbleColumn Inflow of air at the bottom with
0.1 m/s and alpha = 0.5.
Separate files for air and water
thermophysical and turbulence
properties.
/constant/phaseProperties file
contains phase properties i.e.:
surface tension, drag,
blending, aspect ratio, heat
transfer, virtual mass and
other.

RAS bubbleColumn Initial boundary conditions set
up exactly as in LES case.
Here, k-epsilon turbulence
model is used and the case
converges within the
simulation time to a stable 2-
phase flow pattern, unlike LES
case.
fluidizedBed Simulation of dispersed
particles column behavior
when hot air is blowed in
from the bottom. Particles
are assumed to be of
spherical shape and
constant radius
(constant/phaseProperties).

6. Heat transfer
buoyantBoussinesqPimpleFoam - Transient solver for buoyant, turbulent flow of
incompressible fluids
hotRoom Shows how constant
temperature point heat source
influences the behavior of a
static volume of air. Natural
convection occurs. K-epsilon
turbulence model and
Boussinesq Newtonian fluid
model used.
BuoyantBoussinesqSimpleFoam - Steady-state solver for buoyant, turbulent flow of
incompressible fluids
hotRoom Set up exactly as transient
solver case above. For this
simple case, steady state solver
takes half the pseudo-time steps
to converge. Slight difference in
the maximum velocity value can
be observed
iglooWithFridges A half-sphere of cold air with two
warm cubes placed inside.
Simulation shows development
of natural air convection.
Snappyhexmesh used to create
mesh, k-epsilon turbulence used.

buoyantPimpleFoam - Transient solver for buoyant, turbulent flow of compressible fluids for
ventilation and heat-transfer
hotRoom Hot room case, as described
above. Does not use Boussinesq
approximation; equation of state
employed instead.
buoyantSimpleFoam - Steady-state solver for buoyant, turbulent flow of compressible fluids
buoyantCavity Natural convection of air inside a
closed cavity, of which one of the
vertical walls is hot and the other –
cold. Temperature difference of 19.6
deg drives an up-flow of hot and
down-flow of cold air. k-omega SST
turbulence model used and basic
mesh. Tutorial also provides a
technique to obtain values relevant to
be compared with experiment.

circuitBoardCooling Cooling of two high
temperature baffles
representing circuit boards.
Heat is transferred to air flowing
through the domain. One of the
baffles generates heat at
100W/m2.
externalCoupledCavity Buoyant cavity case with
boundary conditions modified
using “external” procedure. For
this case temperatures of the
walls are increase by 1deg
each time step until they
equalize.
hotRadiationRoom Room with a 227deg C cube in
one of the corners, filled with
27degC air. The radiation of the
cube is modeled to show how it
influences the temperature of
the air. Natural convection
develops, driven by the heat of
the cube and cold ceiling and
floor. k-epsilon turbulence
modeling is used.
hotRadiationRoomFvDOM Case set up as above, but
Discrete Ordinates model is
used instead of P1, to simulate
the influence of radiation.

chtMultiRegionFoam - Combination of heatConductionFoam and buoyantFoam for conjugate
heat transfer between a solid region and fluid region
multiRegionHeater “T” shaped solid heater is
surrounded by water in the
bottom section, by two
solids on the sides of the
upper section and by air
over the top. The bottom of
the heater is 500deg warm,
the temperature in the rest
of domain is 300deg initially.
Additionally, there is 0.01m/s
flow in X direction assigned to the air and water. Left solid is isolated
from the heater.
snappyMultiRegionHe
ater
General arrangement as
above, only air used at the
bottom instead of water,
and no thermal isolation
used for left solid. Mesh
created with
snappyHexMesh. Top air is
given initial velocity of
0.1m/s, 10 times more than
the bottom.

chtMultiRegionSimpleFoam - Combination of heatConductionFoam and buoyantFoam for
conjugate heat transfer between a solid region and fluid region, including steady-state turbulent
flow of compressible fluids
heatExchanger Forced flow of air through a
bundle of warm water filled
pipes. There is a straight
vanes rotor at the bottom
(fvOptions->MRF and
createBaffles) and the water
is modeled as a porous
region. There are two
domains – each with
separate blockMesh and
separate set of
thermophysical properties
and boundary conditions.
multiRegionHeaterRa
diation
Initial box divided into 3
solid and 2 fluid zones
(topoSet,
splitMeshRegions). Each
zone has its own fvSolution,
fvSchemes,
thermophysicalProperties
and boundary condition files
generated. The heater is
200deg hotter than the rest
and heat transfer to the
neighboring solids and air
can be observed along with natural convection inside the air domain.

Basic openfoa mtutorialsguide

Recommended

Recommended

More Related Content

What's hot

What's hot (20)

Viewers also liked

Viewers also liked (8)

Similar to Basic openfoa mtutorialsguide

Similar to Basic openfoa mtutorialsguide (20)

Recently uploaded

Recently uploaded (20)

Basic openfoa mtutorialsguide