## tips for VOF modelling using Fluent

Define -> Models ->Solver
1. Check for steady and unsteady formulation
A steady-state VOF calculation is sensible only when your solution is independent of the initial
conditions and there are distinct inflow boundaries for the individual phases. For example, since
the shape of the free surface inside a rotating cup depends on the initial level of the fluid, such a
problem must be solved using the time-dependent formulation. On the other hand, the flow of
water in a channel with a region of air on top and a separate air inlet can be solved with the
steady-state formulation.
Implicit Scheme (steady and unsteady)
In case of unsteady flow, suitable for higher time step.
Diffusive in the direction of flow.
Note for Steady State Implicit Scheme
Steady state Implicit Scheme works fine in case of good smooth uniform grid.
In case of non-uniform grid and anisotropy, there could be problems during the startup of the solution.
The best practice for implicit steady state problems is to consider problem as transient with
large time step.
Explicit Schemes ( unsteady)
Euler Explicit Diffusive in the direction normal to the flow direction.
Donor-Accepor Valid only for hex cells
Geo-Reconstruct Valid for all the cells , gives very sharp interface.
3. Solve VOF every iteration
In general, if you anticipate that the location of the interface will change as the other
flow variables converge during the time step, you should enable the Solve VOF Every
Iteration option. This situation arises when large time steps are being used in hopes of
reaching a steady-state solution.
Implicit BodyForce Treatment
When Body forces ( gravity or surface tension forces) are very large. Pressure gradient and
body forces are almost in equilibrium, if the convective and viscous terms are smaller.
So, In this treatment we only use the partial equilibrium of the pressure gradient and the
body forces to increase the stability and the convergence.
Implicit body force treatment helps to provide in some cases good pressure field at the initial start-up.
Examples involving thin film modelling
If you are interested in the sources of instability in thin film formation, turn off the Implicit body force
in case of surface tension. That reduces sources for pressure correction equation and helps to clarify real
source of instability for large time steps.
Define->Models->Viscous
Turbulent Flow
1. Initailize physically reasonable values for k and e through patch option when turning on turbulence.
2. In fluent6, fluxes are frozen at the beginning of a timestep, and the frozen flux is used
for the convection terms. Thus, if the velocity field is not conservative at time = 0,
you might face convergence problems, particularly with turbulence.
You can try to get a conservative field by iterating with no. of time steps set to 0 and
then trying the transient simulation.
3. You can start the simulation turning off the Turbulence models, and then after some time steps,
turn on the turbulence moels.
Limitation of VOF with Turbulence ( General comment)
VOF requires sufficiently fine mesh near the free surface, which is an inherent and most criticised
limitation of VOF, Especially when turbulence model is used. There is a chance that turbulence at
and near the interface are not properly represented by conventional k-epsilon models. For instance,
how you compute production of turbulent kinetic energy at the cells containing the free surface, etc.
is not clear and ambiguous at best. Unfortuantely, all this is a research issue and there isn't a quick
fix to ameliorate the situation. For gravity waves generated by submerged bodies like airfoils, it is widely
accepted that ALE approaches (mesh moving with the free surface) is more accurate and economical
than VOF methods, as long as wave-breaking does not occur.
Define->Materials
Viscosity ratio between the materials should be less than 1e5 for better stability and convergence.
Define->Phases
Selection of phases
In general problems, there is no restriction on choosing the secondary phase.
It is recommended to select the secondary phases that are advected inthe domain.
Example:
1. water bubble in air (choose water as a secondary phase)
2. Air bubble in water (choose air as a secondary phase)
Enabling Surface Tension and Wall Adhesion
Find out whether surface tension effects are important or not.
For Re << 1, check the Capillary number
For Re >> 1, check the value of weber number.
Ca = viscosity * Velocity / sigma
We = density * characteristic length * (Velocity)^2 / sigma
if Ca >> 1 or We >> 1, the surface tension effects can be neglected.
2. Reference Pressure location
The position that you choose should be in a region that will always contain the least dense
of the fluids (e.g., the gas phase, if you have a gas phase and one or more liquid phases).
This is because variations in the static pressure are larger in a more dense fluid than in
a less dense fluid, given the same velocity distribution. If the zero of the relative pressure
field is in a region where the pressure variations are small, less round-off will occur than
if the variations occur in a field of large non-zero values. Thus in systems containing air and water,
for example, it is important that the reference pressure location be in the portion of the domain filled
with air rather than that filled with water.
Use of Operating Density
For VOF calculations, Set the Operating Density to be the density of the lightest phase.
(This excludes the buildup of hydrostatic pressure within the lightest phase, improving the round-off accuracy
for the momentum balance.).
Define->Boundary Conditions
Wall
Specification of the contact angle
In Fluent, Contact angle is defined as the angle between solid and tangent to the interface measured inside the
first phase of each pair specified in the wall boudary condition panel.
Example (showing the specifiaction of contact angle in wall bc panel )
Wall Adhesion
Contact angles (deg)
water air 30
Then the contact angle will be meassured in the water phase.
Pressure outlet
Specify the correct value of Back flow Volume fraction.
For eg., If there are chances of reverse flow in the secondary phase, put the Backflow volume fraction
for secondary phase eqaul to 1. If reverse flow in primary phase, then put the value 0.
Mass Flow inlet
Reverse Flow handling in Mass Flow Inlet boundary:
If Mass Flow Inlet is not used in Mixing-Plane Model: Flux value is enforced on the boundary.
If Mass Flow Inlet is used in Mixing-Plane : The boundary is treated as pressure outlet.
Solve -> Controls -> Solution
1. Pressure Interpolation Schemes
Presto: (Genearlly recommended for VOF model)
PRESTO! was used for the segregated solver in order to avoid the "zero normal pressure gradient"
assumption adjacent to the wall.
For flows with high swirl numbers, high-Rayleigh-number natural convection, high-speed rotating flows,
flows involving porous media, and flows in strongly curved domains, use the PRESTO scheme.
One can also try the new "unstructured" PRESTO. This is the default for tri/tet meshes.
To turn it on, you need to set the rpvar "pressure/dissipation?" to #t.
Body Force Weighted:
Recommended for flow involving large body forces
Note: Please remember that if you introduce your own sources using UDF sources for momentum ,
these forces are not accumulated inside body_forces which are participating in the body-force
weighted interpolation. It could produce physically incorrect velocity vectors near free surface
unless reference density set equal to 0.0. Near the walls velocity direction will be physically incorrect
in all cases. Please use PRESTO if user sources for momentum are involved.
2. Pressure Velocity coupling:
Transient state
When used the large time step
Always use PISO + Neighor correction. ( For incompressible flow)
Neighbor correction = 1 means -> one more iteration done for to satisfy the continuity
and the momentum equation more closely.
Skewness correction is needed in case of distorted mesh, else don't use it.
It is used for the mass flux calculation at the face accurately.
Skewness-Neighor coupling - ON ( solution economical but less robust algorithm),
It is recommended not to use this in highly distorted mesh.
Increasing the number of iterations for neighbor correction and the skewness correction depends on the quality of mesh.
When used the smaller time step
PISO can be used , but computationally expansive in that case.
SIMPLE or SIMPLEC can be used with optimal relaxation factors.
Under-relaxation factor in Transient case
PISO ( not recommended for compressible flow)
Hex and quad mesh: Put all the under-relaxation factors close to 1.
Tetrahedral or triangular meshes: An under-relaxation factor of 0.7-0.8 for pressure is recommended for improved stability.
SIMPLEC
In uncomplicated problems, take all the under-relaxation factor close to 1.
In case of instability reduce the under relaxation factors or use the SIMPLE scheme.
SIMPLE
Take the defualt values. In case of instability , adjust the under-relaxation factors.
under-relaxation factor for explicit VOF
URF for Volume Fraction doesn't have any significance for the explicit VOF. ( This option removed in fluent6.2).
Steady State
Use SIMPLE or SIMPLEC is recommended.
SIMPLEC will give some advantage over the SIMPLE in terms of convergence becasue of more accurate face flux correction.
Case of Highly distorted mesh :
Use of PISO without neighbour correction and with skewness correction speeds up the convergence of
steady state problems on distorted meshes.
under Relaxation factor for steady state
The under-relaxation factors for all variables should be set to values between 0.2 and 0.5 for improved stability.
Application specific Under-relaxation Factors
For High viscosity ratio (4 - 5 orders of magnitude) problems, the lower under-relaxation factor for momentum ( 0.2 - 0.4)
is recommended to run the problem with higher time step.
For highly rotating flows, lower under-relaxation factor for momentum is recommended. ( generally, between 0.3 - 0.5).
3. Discretization Schemes
First order upwind (Default)
Second order or Quick
When the implicit or Euler explicit scheme is used you should use the second-order or QUICK discretization
scheme for the volume fraction equations in order to improve the sharpness of the interface between phases.
Summary:
While the first-order discretization generally yields better convergence than the second-order scheme,
it generally will yield less accurate results, especially on tri/tet grids. In some cases, however, you may need to
start with the first-order scheme and then switch to the second-order scheme after a few iterations.
Setting Non Iterative PISO or SIMPLEC settings (for better speed)
1. PISO noniterative mode is 1 it /per time step.
2. Under-relaxation = 1.0 for everything.
3. Termination criteria 1.e-3 for everything.
4. W-cycle for pressure amg is recommended in serial run.
Solve -> Controls -> Limits
Checking the pressure and Temperature limit
Check the minimum and maximum pressure and temperature limit specified in the panel.
If the prsssure and temperature specified in the problem goes above the prescribed limits,
increase the range.
Solve -> Initialize
initialize
The correct order of initialization is:
1. Do Init.
2. patch the domain with secondary phase.
3. Repatch velocities in all the domain, If initial velocities are non-zero.
If you don't repatch the velocity, the mass fluxes are not recalculated according to new density.
The problem with start up will come due to wrong initialization order during patch .
In case of turbulence ,Initialization of turbulence quantities (such as Turbulence KE, and Turbulence
dissipation rate) need to be reconsidered also.
Solve-> Monitors ->Residuals
If you are interested in very tight convergence, i.e order of 1e-7. The better way is to go for double precision.
Single precision solver will take large number of iterations to converge, resulting into increased solution time.
Turning off the convergence monitoring and specifying a minimum number of iterations per timestep
This can be done to speed up calculations to avoid potential problems, when at some stage iterations
do not converge completly due to roundoff accuracy in the vicinity of the convergence criteria.
Solve-> Iterate
Geo-Recon Scheme specific
To put the approprite time step in the Geo-Recon scheme
Please follow the following steps:
1. Get the minimum grid size in the direction where velocity is dominant.
2. Get the idea of maximum velocity in the domain:
3. find out the ratio
dt'' = minimum grid size / maximum velocity in the domain
4. sub-step size dt' = courant number * dt''
5. Number of sub time steps in the solution
= dt/dt'
2. Timestepping
Adaptive timestepping cannot be efficiently used with VOF because the predictor-corrector algorithm
cannot work with discontinuous systems.
Note:The Courant based global timestepping has been implemented in Fluent6.2.
Convergence problem in first time step
Generally, the first time steps in a transient VOF simulation using Geo-Reconstruct have difficulties in converging.
In fluent6, fluxes are frozen at the beginning of a timestep, and the frozen flux is used for the convection terms.
Thus, if the velocity field is not conservative at time = 0, you might face convergence problems.
You can try to get a conservative field by iterating with no. of time steps set to 0.