This document outlines boundary conditions, turbulence models, and other setup considerations for computational fluid dynamics (CFD) simulations of incompressible flows using ANSYS Fluent. It discusses inlet and outlet boundary conditions such as velocity inlet, pressure inlet, outflow, and others. It also covers turbulence modeling requirements, specifying other boundary conditions like walls, and defining fluid, solid, and porous zones. Setup of the solver, models, and determining convergence are outlined to provide the key steps for setting up an incompressible flow problem in Fluent.

1. BOUNDARY CONDITIONS FOR INCOMPRESSIBLE FLOW INLETS:
1. VELOCITY-INLET (7.3.4 of User's Guide): fixes incoming velocities
• Used for incompressible flows (similar to mass-flow inlet boundary condition that is used for
compressible flows to account for variable density)
• Pressure is calculated at the inlet
• For turbulent flows, also need to specify turbulence parameters
• For heat transfer, also need to specify inlet temperature
• For non-uniform velocity profile, use boundary profile file (7.6 of User's Guide) created from
previous simulation, analytical analysis, or experimental data.
Examples: uniform flow at inlet of pipe or duct, uniform flow for external flow, fully-developed
flow at inlet of pipe or duct
2. PRESSURE-INLET (7.3.3 of User's Guide): fixes total fluid pressure at inlet
• The total pressure, p0, is related to the static pressure, ps, through Bernoulli’s equation:
€
p0 = ps + 1
2
ρ

V
2
• Inlet flow velocity and static pressure are calculated
• Note that pressure is given as gage pressure with reference to Operating Pressure set in
Operating Conditions dialog box
Example: free boundary where there is flow in from a room at atmospheric pressure
3. INLET-VENT (7.3.6 of User's Guide): fixes ambient total pressure with inlet vent (assumed
infinitely thin) with specified loss coefficient, kL, that can be constant or a function of velocity
and is defined as
€
Δp = kL
1
2
ρ

V
2
• Similar to pressure inlet, except with a restriction at inlet
4. INTAKE-FAN (7.3.7 of User's Guide): fixes ambient total pressure with inlet fan (assumed
infinitely thin) with specified pressure jump that can be constant or a function of velocity
• Similar to pressure inlet, except with a pressure increase at inlet

2. BOUNDARY CONDITIONS FOR INCOMPRESSIBLE FLOW OUTLETS:
1. PRESSURE-OUTLET (7.3.8 of User's Guide): fixes static pressure at outlet
• Velocity at outlet is calculated
• Backflow conditions are specified to account for flow reversal (better convergence rate)
• Even if backflow is not expected in the final solution, values might be used during iteration
and should be realistic
2. OUTFLOW (7.3.11 of User's Guide): fixes exit as an outflow boundary
• Velocity and pressure are calculated
• Cannot be used with pressure inlet (problem is under-prescribed)
• Boundary conditions are the following:
1. Zero diffusion flux for all flow variables (true for fully-developed flow)
2. Overall mass balance correction
• For multiple outflow boundaries, the flow rate weighting (FRW) is used to set the percentage
of flow exiting each outlet:
€
% of flow through boundary =
FRWi
FRWi
i=1
Nbnd
∑
Example of where you must use pressure outlet instead of outflow:
3. OUTLET-VENT (7.3.12 of User's Guide): fixes ambient discharge pressure with outlet vent
(assumed infinitely fin) with specified loss coefficient, kL, that can be constant or function of
velocity and is defined as
€
Δp = kL
1
2
ρ

V
2
• Similar to pressure outlet, but with a restriction
4. EXHAUST-FAN: (7.3.13 of User's Guide) fixes ambient discharge pressure with exhaust fan
(assumed infinitely thin) with specified pressure jump that can be constant or function of velocity
• Similar to pressure outlet, but with a pressure jump
flow
pressure outlet outflow

3. TURBULENCE BOUNDARY CONDITIONS:
For the k-ε turbulence model there are two transport equations for k and ε that are 2nd
order in
space, thus need to specify two boundary conditions (at inlet and exit) for both k and ε.
1. Specify average turbulent kinetic energy (k) or turbulence intensity (I) defined as:
€
k =
3
2
ʹ′u( )2
and
€
I =
ʹ′u( )2
u
where typical range is 1% < I < 10%.
Ideally, use experimental data to measure k or I. For underdeveloped, undisturbed flow use
I = 1% (wind tunnel inlet or typical free stream air).
For fully-developed duct-flow use:
€
I = 0.16 ReDh
( )
−1/8
2. Specify turbulent dissipation rate (ε), turbulent length scale (
€
m ), viscosity ratio (µt/µ), or
hydraulic diameter (Dh):
To calculate ε from
€
m use the following:
€
ε = Cµ
3/ 4 k3/ 2
m
where
€
Cµ = 0.09
To calculate µt/µ from k and ε use the following:
€
µt
µ
= Cµ
ρ k2
ε µ
where
€
1<
µt
µ
<10
To calculate
€
m from Dh use the following:
€
m = 0.07 Dh
For turbulent flow around objects use:
€
m = 0.07 L, L = characteristic length scale
For boundary layers use:
€
m = 0.4 δ99,
€
δ99 = boundary layer thickness
For wind tunnels downstream of a wire mesh:
€
ε ≅
Δk U∞
L∞
€
Δk approximate decay of k
across domain (about 10%)
€
U∞ free-stream velocity
€
L∞ stream-wise domain length
NOTE: For turbulent heat transfer, specification of the turbulent Prandtl number controls the
turbulent heat transfer mixing and no additional boundary conditions are needed.

4. OTHER BOUNDARY CONDITIONS:
1. WALL (7.3.14 of User's Guide): fixes boundary as solid wall that bounds fluid regions
• By default, no-slip condition will be enforced
• Wall can be fixed or moving (translation or rotation)
• Can set the following thermal boundary conditions:
temperature, heat flux, convection, and/or external radiation
• Wall can have a finite thickness to model a thin layer between two zones. Can be used to
model a sheet of metal between fluid layers, a coating on a solid zone, contact resistance
between solid layers, or a thin wall with heat generation (for computer chips instead of
constant heat flux).
• For turbulent flows, can set the wall roughness by setting the Roughness Height, Ks,
(approximately the mean diameter of the roughness features) and the Roughness Constant,
Cs, which typically ranges from 0.5 to 1.0 and is hard to characterize. NOTE: Cell size should
be greater than the roughness height.
2. SYMMETRY (7.3.15 of User's Guide): fixes boundary as symmetry plane
• Used when both flow and thermal solution are symmetric about a plane to reduce
computational domain
• Use Display/Views menu and the Mirror Planes section to mirror the display
3. AXIS (7.3.17 of User's Guide): fixes boundary as axis for 2-D axisymmetric flow (use x-axis)
4. PERIODIC (7.3.16 of User's Guide): fixes boundary as periodic when geometry and flow
solution have a periodically repeating nature and will force the flow in to match the flow out
• Can have either (1) no pressure drop or (2) prescribed pressure drop
• Can specify either (1) translational or rotational periodicity
• Must link boundaries together as periodic: for FLUENT use Command Window and enter
"mesh/modify-zones/make-periodic" and select Periodic Conditions to set mass flow rate or
pressure gradient and upstream bulk temperature
Examples: flow through heat exchanger tube bundle and rotational with multiple fluid in ports
periodic
flow
periodic
symmetry
symmetry
flow
periodic

5. ZONES:
1. FLUID (7.2.1 of User's Guide): sets zone as fluid
• All active equations are solved
• Material properties must be set correctly
• Can define sources of heat, mass, momentum, turbulence, etc. within fluid zones
2. SOLID (7.2.2 of User's Guide): sets zone as solid
• Only the heat conduction equation is solved
• Material properties must be set correctly
Example: conduction through solid between heat exchanger passages
NOTE: In general, use the same edge (for 2-D)
or face (for 3-D) for the interface between
the fluid and the solid in ICEM so the mesh
nodes are the same at the fluid/solid interface.
In FLUENT, define the interface as coupled for
heat transfer across the interface. Alternatively,
you can use a non-conformal mesh.
3. POROUS MEDIA (7.2.3 of User's Guide): sets zone as porous media
• Examples of porous media include filters, packed beds, perforated plates, and tube banks
• Permeability and inertial losses for the porous media must be specified
• Heat transfer calculations assume thermal equilibrium between medium and fluid flow
• 1-D simplification of porous media model is POROUS JUMP (7.3.20 of User's Guide) for
thin membranes where pressure drop versus velocity must be specified
4. FAN (7.3.18 of User's Guide): lumped-parameter model used to determine the impact of a fan
with known characteristics (pressure rise and velocity profile at exit) upon a larger flow field
• The fan is assumed infinitely thin, thus is modeled as the interface between cells and the fan
zone type is an INTERFACE zone
5. RADIATOR (7.3.19 of User's Guide): lumped-parameter model used to add a heat exchange
element (for example a heat exchanger or condenser) with known characteristics (pressure drop
and heat transfer coefficient as a function of velocity) upon a larger flow field
• The radiator is assumed infinitely thin, thus is modeled as the interface between cells and the
radiator zone type is an INTERFACE zone
SOLID
FLUID
FLUID

6. FLUENT Summary: Outline for Model Setup
Below is a list of steps necessary to set up a convection problem in FLUENT. It only includes
the elements of FLUENT covered in ME 554. Additional models that were not covered in this
class (such as for deforming meshes, fluid structure interaction, multiphase flow, combustion,
etc. that are available in FLUENT) are not included in these steps.
1. Start FLUENT and choose: 2-D or 3-D, single precision or double precision
2. File/Read/Mesh: Import mesh into FLUENT from ICEM CFD (typically a .msh file).
3. Problem Setup
General
Mesh Check grid and verify that there are no negative volumes
Scale Change units or scale grid if necessary
Display Display mesh and visually verify mesh and boundary names
Solver
Type Select Pressure Based for pressure-correction equation derived
from conservation of mass for incompressible flow
Space For 2-D select Planar, Axisymmetric, or Axisymmetric Swirl
Time Select Steady or Transient
Units Define units for grid, properties, and calculated values
Models
Energy Turn on for conduction, convection, and compressible flow
Viscous
Model Select viscous model (inviscid, laminar, or one of the turbulence
models) based on Reynolds number for forced convection or
Rayleigh number for natural convection
k-ε Model Choose Standard for equilibrium flows; RNG or Realizable for
flows with high strain rates, swirl, rapidly changing pressures, or
separation
Near-Wall Use Standard-Wall Functions for equilibrium flows; Non-
Equilibrium Wall Functions or Enhanced Wall Functions for flows
with high strain rates, swirl, rapidly changing pressures, or
separation; make sure y+
values for wall adjacent cells are correct
Options Turn on viscous heating for high Eckert number and turbulent
compressible flows
Materials Use properties database or user defined to create new materials; for
natural convection flows set the density to Boussinesq to use this
approximation or set density to variable (typically use ideal gas for
air); change other properties to variable as well for significant
temperature changes

7. Cell Zone Cond.
Zone Use to set zone as fluid, solid, or porous
Operating Cond. Operating Pressure typically set to atmospheric (101,325 Pa)
Reference Location Only need to set this if there are no pressure boundaries.
Gravity Turn on if natural convection is significant (for Gr/Re2
> 1) and
set Operating Temperature to free stream flow temperature or
coldest boundary temperature for internal flow
Boundary Cond.
Zone Use to define boundary condition and type; for incompressible
flows typically use velocity inlet and pressure outlet; for
compressible flows must use mass-flow inlet and specify mass-
flow rate or mass flux or pressure inlet; for both of these the
specified temperature is the total temperature
Reference Values Set reference values for properties and parameters for calculations
of variables such as drag coefficient or surface Nusselt number
4. Solution
Solution Methods
Press.-Vel. Coup. Select SIMPLE, SIMPLEC (for faster convergence for some
cases), PISO (for unsteady problems), or coupled (for compressible
or natural convection)
Spatial Discret.
Gradient Select Green-Gauss Cell Based (for structured mesh) or Least
Squares Cell Based (for unstructured mesh)
Pressure Select 1st order (faster convergence), 2nd
order (for higher
accuracy), PRESTO! (for transient problems), or Body Force
Weighted (for natural convection or swirling)
Upwinding For Momentum, Energy, and Turbulent equations select 1st
order
(faster convergence), 2nd
order (for higher accuracy), Power-Law,
or QUICK (for higher accuracy on structured grids); use higher
order upwinding to reduce numerical diffusion
Solution Controls
Relaxation Set for each equation; may need to decrease for convergence;
decrease relaxation for energy to 0.7-0.9 for natural convection
and compressible flows
Advanced Use to set multigrid parameters
Monitors
Residuals Set absolute criteria to desired values (10-6
recommended)
Surface Mon. Use to check additional variables (such as total mass flow in and
Volume Mon. out) for convergence or to record results for transient problems

8. Solution Init.
Compute From Can use inlet conditions for initial values (good for k and ε)
Initialize Sets values as initial guess or initial condition for transient
Calc. Activities
Autosave Every Use to save data at any intermediate iteration or time step
Sol. Animations For transient problems set parameters to make animation(s)
File/Write/Case Save a copy of the case before iterating for a solution
Run Calculation
Check Case Use to check model setup
Calculate Enter number of iterations for a steady solution or time step,
number of steps, and maximum number of iterations for transient
File/Write/Case & Data Save a copy of the case and data after converging to a solution
5. Results
Graphics and Animations
Graphics
Contours Use to visualize contour plots of temperature, pressure, velocity,
etc.; use Colormap to change options such as number formatting
for contour plots; use Views to return to original view or to mirror
the solution for cases with symmetry; use New Surface to create a
new point, line, or plane in the flow for plotting
Vectors Use to visualize velocity vectors for solution
Animations
Playback Use to visualize animations for unsteady solutions
Plots
XY Plot Use to make x-y plots such as velocity and temperature profiles at
boundaries; data can be plotted or written to a file; for turbulent
flows verify y+
values at walls are correct for near wall treatment
Reports
Fluxes Use to output mass flow rate or heat transfer rate across boundaries
Forces Use to output forces and drag coefficients for boundaries
6. Report/Input Summary: Use to output a text file(s) summarizing model setup.
7. Define/Custom Field Functions: Use to define new variables such as the Reynolds number
as a function of the x-coordinate location.
8. Adapt/Gradient: Use grid adaptation to refine grid and improve accuracy. Refine grid until
solution is no longer significantly dependent on grid resolution.

9. NOTES ON JUDGING CONVERGENCE:
Residuals are used to monitor the convergence of simulations in FLUENT. For the pressure
based solver recall that the discretized conservation equation for a general variable φ at cell P is
written as
€
aP φP = anb φnb
nb
∑ + b
where aP is the center coefficient, anb are coefficients for the neighboring cells, and b results from
the boundary conditions and source terms. After each iteration the “scaled” residual is calculated
by summing over all cells the imbalance in the discretized conservation equation above and then
normalizing the result using the term shown in the denominator below
€
Rφ
=
anb φnb
nb
∑ + b − aP φP
Ncells
∑
aP φP
Ncells
∑
Residual definitions are often useful for judging convergence for many classes of problems, but
are sometimes misleading. As a result, there are no universal metrics for judging convergence.
Thus, it is a good idea to judge convergence not only by examining residual levels, but also by
monitoring relevant integrated quantities such as mass flux or total heat transfer.
1. If an initial guess for a solution is very good the residual values will not decrease significantly
even though a converged solution has been reached.
2. If the variable of interest is nearly zero everywhere, the residuals may not decrease
significantly. In fully-developed pipe flow, for example, the cross-sectional velocities are zero. If
these velocities have been initialized to zero, initial (and final) residuals are both close to zero.
3. If the governing equation contains non-linear source terms that are zero at the beginning of the
calculation and build up slowly during computation, the residuals may not drop significantly. In
the case of natural convection in an enclosure, for example, initial momentum residuals may be
very close to zero because the initial uniform temperature guess does not generate buoyancy. The
initial nearly-zero residual is not a good scale for the residual.
4. For some equations, such as for turbulence quantities, a poor initial guess may result in high
scale factors. In such cases, scaled residuals will start low, increase as non-linear sources build
up, and eventually decrease. It is therefore good practice to judge convergence not just from the
value of the residual itself, but from its behavior. You should ensure that the residual continues
to decrease (or remain low) for several iterations (approximately 50 or more) before concluding
that the solution has converged.