1. Chapter 3 Domains and Boundary Conditions
Introduction to CFX

2. Domains
Domains are regions of space in which the equations of fluid flow or heat transfer are solved
Only the mesh components which are included in a domain are included in the simulation
Rotor
Stator
e.g. A simulation of a copper heating coil in water will require a fluid domain and a solid domain.
Selections on Domains panel affect which options are available on other panels
There can be any combination of fluid, solid, and porous domains which can be included in the CHT (Conjugate Heat Transfer) simulation
e.g. To account for rotational motion, the rotor is placed in a rotating domain.

3. How to Create a Domain (as shown earlier)
Define Domain Properties
Right-click on the domain and pick Edit
Or right-click on Flow Analysis 1 to insert a new domain
When editing an item a new tab panel opens containing the properties. You can switch between open tabs.
Sub-tabs contain various different properties
Complete the required fields on each sub-tab to define the domain
Optional fields are activated by enabling a check box

4. Domain Creation General Options panel: Basic Settings
Location: Only assemblies and 3D primitives
Domain Type: Fluid, Solid, or Porous
Coordinate Frame: select coordinate frame from which all domain inputs will be referenced to
Not to be confused with the reference frame, which can be stationary or rotating
The default Coord 0 frame is usually used
Fluids and Particles Definitions: select the participating materials

5. Domain Creation – Reference Pressure
General Options panel: Domain Models
Reference Pressure
Represents the absolute pressure datum from which all relative pressures are measured
Pabs = Preference + Prelative
Pressures specified at boundary and initial conditions are relative to the Reference Pressure
Used to avoid problems with round-off errors which occur when the local pressure differences in a fluid are small compared to the absolute pressure level
Pref
Pressure
Pressure
Prel,max=100,001 Pa
Prel,max=1 Pa
Prel,min=99,999 Pa
Prel,min=-1 Pa
Pref
Ex. 1: Preference= 0 Pa
Ex. 2: Preference= 100,000 Pa

6. Domain Creation - Buoyancy
General Options panel: Buoyancy
When gravity acts on fluid regions with different densities a buoyancy force arises
When buoyancy is included, a source term is added to the momentum equations based on the difference between the fluid density and a reference density
SM,buoy=(ρ – ρref)g
ρref is the reference density. This is just the datum from which all densities are evaluated. Fluid with density other than ρref will have either a positive or negative buoyancy force applied.
See below for more on the reference density
The (ρ – ρref) term is evaluated differently depending on your chosen fluid:

7. Domain Creation - Buoyancy
Full Buoyancy Model
Evaluates the density differences directly
Used when modeling ideal gases, real fluids, or multicomponent fluids
A Reference Density is required
Use an approximate value of the expected domain density
Boussinesq Model
Used when modeling constant density fluids
Buoyancy is driven by temperature differences
(ρ – ρref) = - ρref β(T – Tref)
A Reference Temperature is required
Use an approximate value of the average expected domain temperature

8. Domain Creation - Buoyancy
Buoyancy Ref. Density
The Buoyancy Reference Density is used to avoid round-off errors by solving at an offset level
The Reference Pressure is used to offset the operating pressure of the domain, while the Buoyancy Reference Density should be used to offset the hydrostatic pressure in the domain
The pressure solution is relative to rref g h, where h is relative to the Reference Location
If rref = the fluid density (r), then the solution becomes relative to the hydrostatic pressure, so when visualizing Pressure you only see the pressure that is driving the flow
Absolute Pressure always includes both the hydrostatic and reference pressures
Pabs = Preference + Prelative + rref g h
For a non-buoyant flow a hydrostatic pressure does not exist

9. Pressure and Buoyancy Example
Consider the case of flow through a tank
The inlet is at 30 [psi] absolute
Buoyancy is included, therefore a hydrostatic pressure gradient exists
The outlet pressure will be approximately 30 [psi] plus the hydrostatic pressure given by r g h
The flow field is driven by small dynamic pressure changes
NOT by the large hydrostatic pressure or the large operating pressure
To accurately resolve the small dynamic pressure changes, we use the Reference Pressure to offset the operating pressure and the Buoyancy Reference Density to offset the hydrostatic pressure
30 psi h
Small pressure changes drive the flow field in the tank
~30 psi + r gh
Gravity, g

10. Domain Creation General Options panel: Domain Motion Mesh Deformation
You can specify a domain that is rotating about an axis
When a domain with a rotating frame is specified, the CFX-Solver computes the appropriate Coriolis and centrifugal momentum terms, and solves a rotating frame total energy equation
Mesh Deformation
Used for problems involving moving boundaries or moving subdomains
Mesh motion could be imposed or arise as an implicit part of the solution

11. Domain Types
The additional domain tabs/settings depend on the Domain Type selected

12. Domain Type: Fluid Models
Heat Transfer
Specify whether a heat transfer model is used to predict the temperature throughout the flow
Discussed in Heat Transfer Lecture
Turbulence
Specify whether a turbulence model is used to predict the effects of turbulence in fluid flow
Discussed in Turbulence Lecture

13. Domain Type: Fluid Models
Reaction or Combustion Models
CFX includes combustion models to allow the simulation of flows in which combustion reactions occur
Available only if Option = Material Definition on the Basic Settings tab
Not covered in detail in this course

14. Domain Type: Fluid Models
Radiation Models
For simulations when thermal radiation is significant
See the Heat Transfer chapter for more details

15. Domain Type: Solid Models
Solid domains are used to model regions that contain no fluid or porous flow (for example, the walls of a heat exchanger)
Heat Transfer (Conjugate Heat Transfer)
Discussed in Heat Transfer Lecture
Radiation
Only the Monte Carlo radiation model is available in solids
There’s no radiation in solid domains if it is opaque!
Solid Motion
Used only when you need to account for advection of heat in the solid domain
Solid motion must be tangential to its surface everywhere (for example, an object being extruded or rotated)
Tubular heat exchanger

16. Domain Type: Porous Domains
Used to model flows where the geometry is too complex to resolve with a grid
Instead of including the geometric details, their effects are accounted for numerically
Images Courtesy of Babcock and Wilcox, USA

17. Domain Type: Porous Domains
Area Porosity
The area porosity (the fraction of physical area that is available for the flow to go through) is assumed isotropic
Volume Porosity
The local ratio of the volume of fluid to the total physical volume (can vary spatially)
By default, the velocity solved by the code is the superficial fluid velocity. In a porous region, the true fluid velocity of the fluid will be larger because of the flow volume reduction Superficial Velocity = Volume Porosity * True Velocity
Area Porosity
Fraction of physical area that is available for the flow to go through
Always assumed Isotropic
This setting should be consistent with the velocity used when the Loss Coefficients (next slide) were calculated

18. Domain Type: Porous Domains
Loss Model
Isotropic: Losses equal in all directions
Directional Loss: For many applications, different losses are induced in the streamwise and transverse directions. (Examples: Honeycombs and Porous plates)
Losses are applied using Darcy’s Law
Permeability and Loss Coefficients
Linear and Quadratic Resistance Coefficients
Area Porosity
Fraction of physical area that is available for the flow to go through
Always assumed Isotropic

19. Materials Create a name for the fluid to be used
Select the material to be used in the domain
Currently loaded materials are available in the drop down list
Additional Materials are available by clicking

20. Materials
A Material can be created/edited by right clicking “Materials” in the Outline Tree

21. Multicomponent/Multiphase Flow
ANSYS CFX has the capability to model fluid mixtures (multicomponent) and multiple phases
Multicomponent (more details on next slide)
One flow field for the mixture
Variations in the mixture accounted for by variable mass fractions
Applicable when components are mixed at the molecular level
Multiphase
Each fluid may possess its own flow field (not available in “CFD-Flo” product) or all fluids may share a common flow field
Applicable when fluids are mixed on a macroscopic scale, with a discernible interface between the fluids.
Creating multiple fluids will allow you to specify fluid specific and fluid pair models

22. Multicomponent Flow
Each component fluid may have a distinct set of physical properties
The ANSYS CFX-Solver will calculate appropriate average values of the properties for each control volume in the flow domain, for use in calculating the fluid flow
These average values will depend both on component property values and on the proportion of each component present in the control volume
In multicomponent flow, the various components of a fluid share the same mean velocity, pressure and temperature fields, and mass transfer takes place by convection and diffusion

23. Compressible Flow Modelling
Activated by selecting an Ideal Gas, Real Fluid, or a General Fluid whose density is a function of pressure
Can solve for subsonic, supersonic and transonic flows
Supersonic/Transonic flow problems
Set the heat transfer option to Total Energy
Generally more difficult to solve than subsonic/incompressible flow problems, especially when shocks are present
Click to load a real gas library

24. Boundary Conditions

25. Defining Boundary Conditions
You must specify information on the dependent (flow) variables at the domain boundaries
Specify fluxes of mass, momentum, energy, etc. into the domain.
Defining boundary conditions involves:
Identifying the location of the boundaries (e.g., inlets, walls, symmetry)
Supplying information at the boundaries
The data required at a boundary depends upon the boundary condition type and the physical models employed
You must be aware of types of the boundary condition available and locate the boundaries where the flow variables have known values or can be reasonably approximated
Poorly defined boundary conditions can have a significant impact on your solution

26. Available Boundary Condition Types
Inlet
Velocity Components -Static Temperature (Heat Transfer)
Normal Speed -Total Temperature (Heat Transfer)
Mass Flow Rate -Total Enthalpy (Heat Transfer)
Total Pressure (stable) -Relative Static Pressure (Supersonic)
Static Pressure -Inlet Turbulent conditions
Outlet
Average Static Pressure -Normal Speed
Velocity Components -Mass Flow Rate
Static Pressure
Opening
Opening Pressure and Dirn -Opening Temperature (Heat Transfer)
Entrainment -Opening Static Temperature (Heat Transfer)
Static Pressure and Direction -Inflow Turbulent conditions
Velocity Components
Wall
No Slip / Free Slip -Adiabatic (Heat Transfer)
Roughness Parameters -Fixed Temperature (Heat Transfer)
Heat Flux (Heat Transfer) -Heat Transfer Coefficient (Heat Transfer)
Wall Velocity (for tangential motion only)
Symmetry
No details (only specify region which corresponds to the symmetry plane
Outlet
Wall
Inlet
Symmetry
Opening

27. How to Create a Boundary Condition
Right-click on the domain to insert BC’s
After completing the boundary condition, it appears in the Outline tree below its domain

28. Velocity Specified Condition Pressure or Mass Flow Condition
Inlets and Outlets
Inlets are used predominantly for regions where inflow is expected; however, inlets also support outflow as a result of velocity specified boundary conditions
Velocity specified inlets are intended for incompressible flows
Using velocity inlets in compressible flows can lead to non-physical results
Pressure and mass flow inlets are suitable for compressible and incompressible flows
The same concept applies to outlets
Velocity Specified Condition
Pressure or Mass Flow Condition
Inlet
Inflow allowed
Inflow
allowed
Outflow

29. Pressure Specified Opening
Openings
Artificial walls are not erected with the opening type boundary, as both inflow and outflow are allowed
You are required to specify information that is used if the flow becomes locally inflow
Do not use opening as an excuse for a poorly placed boundary
See the following slides for examples
Pressure Specified Opening
Inlet
Inflow allowed
Outflow
allowed

30. Symmetry Used to reduce computational effort in problem.
No inputs are required.
Flow field and geometry must be symmetric:
Zero normal velocity at symmetry plane
Zero normal gradients of all variables at symmetry plane
Must take care to correctly define symmetry boundary locations
Can be used to model slip walls in viscous flow
symmetry planes

31. Specifying Well Posed Boundary Conditions
Consider the following case in which contain separate air and fuel supply pipes
Three possible approaches in locating inlet boundaries:
Fuel
Air
Manifold box 1
Nozzle 2 3
1 Upstream of manifold
Can use uniform profiles since natural profiles will develop in the supply pipes
Requires more elements
Nozzle inlet plane
Requires accurate velocity profile data for the air and fuel
Nozzle outlet plane
Requires accurate velocity profile data and accurate profile data for the mixture fractions of air and fuel

32. Specifying Well Posed Boundary Conditions
If possible, select boundary location and shape such that flow either goes in or out
Not necessary, but will typically observe better convergence
Should not observe large gradients in direction normal to boundary
Indicates incorrect boundary condition location
Upper pressure boundary modified to ensure that flow always enters domain.
This outlet is poorly located. It should be moved further downstream

33. Specifying Well Posed Boundary Conditions
Boundaries placed over recirculation zones
Poor Location: Apply an opening to allow inflow
Better Location: Apply an outlet with an accurate velocity/pressure profile (difficult)
Ideal Location: Apply an outlet downstream of the recirculation zone to allow the flow to develop. This will make it easier to specify accurate flow conditions
Opening
Outlet
Here we have the same case with two different setups.
Both cases have the same inflow condition: an inlet with a specified normal velocity of 50 m/s. The first case has the outflow boundary defined as an outlet with a static pressure of 0 Pascals. The second case has the outflow boundary defined as an opening with an average pressure of 0 Pascals.
Looking at the global flow characteristics, the results appear the same But if we look at the mass flow plots we start to see some differences.
The case with the opening boundary condition converges much faster as indicated by the orange arrows. More importantly, when comparing the mass flow values, the results differ by more than 10%.
Why is that?
Well let’s take a closer look at what is going on. As fluid flows towards the outlet, it separates from the pipe walls and a recirculation zone forms at the outlet.
The fluid will then tend to flow into the domain at regions of the outlet. If this backflow is prevented, as is the case with an outlet boundary condition, then the solver may take more time to converge and it may be converging towards an incorrect solution.
Outlet

34. Specifying Well Posed Boundary Conditions
Turbulence at the Inlet
Nominal turbulence intensities range from 1% to 5% but will depend on your specific application.
The default turbulence intensity value of (that is, 3.7%) is sufficient for nominal turbulence through a circular inlet, and is a good estimate in the absence of experimental data.
For situations where turbulence is generated by wall friction, consider extending the domain upstream to allow the walls to generate turbulence and the flow to become developed

35. Specifying Well Posed Boundary Conditions
External Flow
In general, if the building has height H and width W, you would want your domain to be at least 5H high, 10W wide, with at least 2H upstream of the building and 10 H downstream of the building.
You would want to verify that there are no significant pressure gradients normal to any of the boundaries of the computational domain. If there are, then it would be wise to enlarge the size of your domain. w 5h
Concentrate mesh in regions of high gradients h
10w
At least 2H
10H

36. Specifying Well Posed Boundary Conditions
Symmetry Plane and the Coanda Effect
Symmetric geometry does not necessarily mean symmetric flow
Example: The coanda effect. A jet entering at the center of a symmetrical duct will tend to flow along one side above a certain Reynolds number
No Symmetry Plane
Symmetry Plane
Coanda effect not allowed

37. Specifying Well Posed Boundary Conditions
When there is 1 Inlet and 1 Outlet
Most Robust: Velocity/Mass Flow at an Inlet; Static Pressure at an Outlet. The Inlet total pressure is an implicit result of the prediction.
Robust: Total Pressure at an Inlet; Velocity/Mass Flow at an Outlet. The static pressure at the Outlet and the velocity at the Inlet are part of the solution.
Sensitive to Initial Guess: Total Pressure at an Inlet; Static Pressure at an Outlet. The system mass flow is part of the solution
Very Unreliable: Static Pressure at an Inlet; Static Pressure at an Outlet. This combination is not recommended, as the inlet total pressure level and the mass flow are both an implicit result of the prediction (the boundary condition combination is a very weak constraint on the system).

38. Specifying Well Posed Boundary Conditions
At least one boundary should specify Pressure (either Total or Static)
Unless it’s a closed system
Using a combination of Velocity and Mass Flow conditions at all boundaries over constrains the system
Total Pressure cannot be set at an Outlet
It is unconditionally unstable
Outlets that vent to the atmosphere typically use a Static Pressure = 0 boundary condition
With a domain Reference Pressure of 1 [atm]
Inlets that draw flow in from the atmosphere often use a Total Pressure = 0 boundary condition (e.g. an open window)

39. Specifying Well Posed Boundary Conditions
Mass flow inlets result in a uniform velocity profile over the inlet
Fully developed flow is not achieved
You cannot specify a mass flow profile
Mass flow outlets allow a natural velocity profile to develop based on the upstream conditions
Pressure specified boundary conditions allow a natural velocity profile to develop