- CFD, Fluid Flow, FEA, Heat/Mass Transfer
- +91 987-11-19-383
- amod.cfd@gmail.com

Boundary Conditions

The boundary conditions of any problem is used to define the upper and lower limits of the field variables (albeit in absence of any source or sink). Basically, they are the operating conditions which governs both the micro- and macro behavior of these variables. A suitable choice of boundary conditions is as good as a good test set-up!

There are different (combination) of boundary conditions. For example, in a structural simulation, the number of boundary conditions can be varied to ensure the force- and moment balance of the entire system. This can be achieved by applying boundary condition at just one node or at 6 different nodes! Similarly, in any fluid problem, there must be an entry and an exit for the fluid (as an exception buoyancy-driven flow can be omitted for the time being). This most basic condition is termed as "Inlet" and "Outlet" boundary conditions in CFD parlance, though the choice of "field variables" such as velocity, pressure, temperature, mass flow rate, may vary as per problem set-up.

Some other considerations during application of Inlet B.C. is "Fully Developed Flow" Vs "Developing Flow". For example, if you are a beginner learning tips and trick of CFD by trying to simulate HTC and correlating it with Dittus-Boelter equation, make sure that the flow regime is fully developed. Sometimes, the inlet of the problem set-up is moved upstream the actual location to get the flow a bit developed. Specification of turbulence parameters (turbulent kinetic energy, TKE and turbulent eddy dissipation, TED) should be based on actual measurement of as far as possible. When there are any source of momentum such as centrifugal fan in the computation domain or sharp edges, the overall result gets affected by the turbulence set at the inlet. Followings are the methods to specify turbulence:

- Specify TKE [m
^{2}/s^{2}] and TED [m^{2}/s^{3}] explicitly - Turbulent Intensity [%] and Turbulent Viscosity Ratio (TVR) [-]
- Hydraulic Diameter [m] and Turbulent Intensity [%]
- Turbulent Intensity [%] and Length Scale [m]

- External Flows
- Length Scale = 0.07 x L
- Turbulent Intensity: Based on upstream condition
- Turbulent Viscosity Ratio: 1 < TVR < 10

- Internal Flows
- ~ Length Scale = Hydraulic Diam.
- Turbulent Intensity: 0.16 x Re
^{-1/8} - Turbulent Viscosity Ratio: 1 < TVR < 10

**Boundary source**: Inlet can also have a boundary source define to model heat sources such as solar radiation.

Walls are required to store a liquid or contain the expansion (mixing) of gases. Since all the fluid flow has to be contained inside walls or at least in a channel, wall B.C. is natural extension into the numerical simulation process. Wall are not only the source of 'turbulence' that gets generated in the flow domain, its surface characteristics becomes important if certain assumptions gets violated. In any CFD software it is not necessary to create 'named' 2D regions for the walls. This is because any faces of a 3D region which do not explicitly have a 2D region assigned to them, are automatically assigned to the default B.C. 'wall' having 'Adiabatic' condition. In case one wishes to create walls such as "Isothermal / Rotating / Heat Flux Wall", it must be created during the pre-processing. Typically, there is no flow across the wall boundary conditions. However, in case of permeable or porous walls, flow does occur across the wall. Similarly, in case of suction or blowing (for example transpiration cooling in Gas Turbine Blades), the mass flow rate specifications are required on the wall boundary conditions.

The setting for wall boundary conditions in ANSYS FLUENT is shown below: Typical classification of wall B.C. is:-
**No-slip**: Velocity of fluid at wall boundary is same as fluid velocity. -
**Free slip**: Velocity component parallel to wall has finite value (computed by the solver), but the velocity normal to the wall and shear stress both set to zero. Zero gradients for other field variables are not enforced in slip wall conditions. -
**Wall Roughness**: Walls are assumed to be hydraulically smooth so long the "sand roughness height" is inside the Laminar Sub-layer. Roughness is also called "Rugocity". Typically roughness is caused by small protrusions over the mean surface of a manufactured component. Any such "technical roughness" can be converted into a "equivalent sand roughness".- k
_{s}= Sand Roughness Height [m] or [μm], k^{+}= k_{s}/h where h is characteristic height of viscouns sub-layer. Please refer to the tubulence modeling page for definition of viscous sub-layer. - k
_{s}>> h: In this case roughness element take up all of the boundary layer and hence the viscosity is of no further importance (also call "Fully Rough Regime" where flow is independent of Reynolds Number. - k
_{s}< h: Here roughness elements are still completely within the purely viscous sub-layer and the flow can be assumed to be "hydraulically smooth", that is, there is no difference as compared to the ideal smooth surface. - Roughness Reynolds number, Re
_{ks}is defined as Re_{ks}= ρ.u^{+}.k_{s}/μ and the surface rougness condition can be defined as:- Re
_{ks}≤ 5: hydraulically smooth and the wall surface roughness need not be activated in CFD simulations - 5 < Re
_{ks}≤ 70: transitionally smooth and wall surface roughness can be activated in CFD simulations though the impact of pressure drop or wall shear stress may not always be noticeable - Re
_{ks}> 70: fully rough regime and wall surface roughness need to be activated in CFD simulations.

- Re

- k
**Contact Resistance**: By default, the walls are assumed to have zero thickness. This setting can be used specify the typical contact resistance between fluid-solid such as fouling factors or the contact resistance between solid-solid. If the thickness of the wall needs to be modeled to account for conductive resistance normal to the plane only (no conduction along the plane), contact resistance value can be specified as [t/k] where t = thickness of the wall and k is thermal conducitivity of the solid.**Shell Conduction**: If the walls are of nearly uniform thickness and the conductive heat transfer needs to be acccounted for both in-plane and through-the-plane conduction, this feature can be used. The user needs to specify only the thickness and thermal conductivity of the solid as described in case of contact resistance.**Radiation**: Walls can be defined as opaque, semi-transparent or transparent to model radiation effects. An opaque wall participate by absorbing, reflecting and emitting radiation. A semi-transparent wall will transmit radiation through it as well. On the other hand, these properties of a solid may be different for infra-red radiation and solar radiation. For example, glass is transparent to solar radiation (that is solar radiation can pass through a glass wall without any reflection/absorption) whereas it is opaque/semi-transparent to infra-red radiation (it traps these waves by refection and absorption).

Strictly speaking, this is not a boundary condition. That is, any numerical simulation can proceed without it. However, this is a great tool to reduce the computational effort and resource if the flow can be envisaged to be symmetrical about a plane or pair of planes. It must be noted that there is a subtle difference between geometrical symmetry and periodicity. Periodic interfaces are treated as if one side of the interface has been translated or rotated to align with the second side of the interface. The periodic type determines the type of transformation (translational or rotational) used to map one side of the interface to the other.

- They must be in pairs.
- They have to be physically identical.
- There is a symmetry. But, unlike a symmetry BC, there is a flow normal to the BC
- The flow field in at one BC is equal to the flow field out at the other
- Types of periodic boundaries
- Transnational Periodic BC: In this case the two sides of the interface must be parallel to each other such that a single translation transformation can be used to map Region List 1 to Region List 2. Flow around a single louver in a whole array in a heat exchanger fin is an example
- Rotational Periodic BC: In this case the two sides of the periodic interface can be mapped by a single rotational transformation about an axis. Flow domain through an Axial Flow Fan can be reduced using rotational periodic B.C.

Strictly speaking, this also is not a boundary condition. That is, any numerical simulation can proceed without it. However, this is a great tool to reduce the computational effort and resource if the flow can be envisaged to be symmetrical about a plane or pair of planes. It must be noted that the geometrical symmetry does not guarantee symmetry of the flow. Similarly, cases where micro-structure of flow eddies are being captured such "Large Eddy Simulation" or "DES – Detached Eddy Simulation", symmetry cannot be used owing to inherent 3D nature of the eddies.

- By definition, a symmetry BC refers to planar boundary surface. If 2 surfaces which meet at a sharp angle & both are symmetric planes, set each surface to be a separate named boundary condition, rather than combine them into a single one.
- Velocity component normal to the Symmetry Plane Boundary = 0. Scalar variable gradients normal to the plane is also =0
- If a particle reaches symmetry plane, it is reflected back.
- Symmetric geometry doesn't necessarily imply that the flow field is also symmetric. For example, a jet entering at the centre of a symmetrical duct will tend to flow along one side above a certain Reynolds number. This is known as the Coanda effect. If a symmetry plane is this situation, an incorrect flow field will be obtained.

Solver Behaviour | Inlet | Outlet |

Most Robust | Velocity or Mass Flow Rate | Static Pressure |

Somewhat Robust | Total Pressure | Velocity or Mass Flow Rate |

Sensitive of Guess (Initialization) | Total Pressure | Static Pressure |

Unreliable | Static Pressure | Static Pressure |

Not possible (divergence guaranteed) | Any | Total Pressure |

Solver Behaviour | Inlet | Outlet |

Most Robust | Velocity or Mass Flow Rate | Static Pressure |

Somewhat Robust | Velocity or Mass Flow Rate | Outflow or Outlet-vent |

Only for incompressible flows | Velocity Inlet | Outflow |

Not available | Any | Mass Flow Rate |

Not for compressible | Specified Velocity | Any |

A fan is considered to be **infinitely thin**, and the discontinuous pressure rise across it is specified as a function of the velocity through the fan. The relationship may be a __constant__, a **polynomial - of the form a + b*x ^{2} + ... **, or piecewise-linear, or piecewise-polynomial function, or a user-defined function.

- Fan should be modelled so that a pressure rise occurs for forward flow through the fan.
- Since the fan is considered to be infinitely thin, it must be modeled as the interface between cells, rather than a cell zone. Thus the fan zone is a type of internal face zone (where the faces are line segments in 2D or triangles/quadrilaterals in 3D).
- Thun when mesh is read into ANSYS FLUENT, the fan zone is identified as an interior zone.
- You can use the Surface Integrals dialog box to report the pressure rise through the fan as described by following steps.
- Create a surface on each side of the fan zone - just upstream and downstream to create two new surfaces.
- In the Surface Integrals dialog box, report the average Static Pressure just upstream and just downstream of the fan. The pressure rise through the fan is difference of downstream and upstream values.
- While generating contour plots, turn off the display of node values to see the different values on each side of the fan. If node values are displayed, the cell values on either side of the fan will be averaged to obtain a node value, and you will not see distinct (pressure, temperature, velocity ...) values on the two sides of the fan.

This is oppostive to the fan boundary conditions define above and like fan is also is considered to be **infinitely thin membrane**, and the discontinuous pressure drop across it is specified as a function of the velocity through the fan. The relationship may be a __constant__, a **polynomial - of the form a + b*x ^{2} + ... **, or piecewise-linear, or piecewise-polynomial function, or a user-defined function.

- It should be modelled so that a pressure drop occurs for forward flow through the porous jump.
- Porous jump should be used (instead of the full porous media model) whenever possible because it is more robust and yields better convergence.
- The porous jump model is applied to a face zone, not to a cell zone.
- By default ANSYS FLUENT uses and reports a superficial velocity inside the porous medium, based on the volumetric flow rate, to ensure continuity of the velocity vectors across the porous medium interface.
- You can use the Surface Integrals dialog box to report the pressure drop through the POROUS JUMP membrane as described by following steps.
- Create a surface on each side of the fan zone - just upstream and downstream to create two new surfaces.
- In the Surface Integrals dialog box, report the average Static Pressure just upstream and just downstream of the porous jump membrane. The pressure drop through the membrane is difference of upstream and downstream values.
- While generating contour plots, turn off the display of node values to see the different values on each side of the fan. If node values are displayed, the cell values on either side of the fan will be averaged to obtain a node value, and you will not see distinct (pressure, temperature, velocity ...) values on the two sides of the fan.

All the porous media formulation take the form: Δp = -L × (A.v + B.v^{2}) where v is the 'superficial' flow velocity and negative sign refers to the fact that pressure decreases along the flow direction. The 'superficial velocity' is calculated assuming there is no blockage of the flow. L is the thickness of the porous domain in the direction of the flow. Here, A and B are coefficients of viscous and inertial resistances.

In FLUENT, the equation used is: Δp/L = -(μ/α.v + C_{2}.ρ/2.v^{2}) where α is known as 'permeability' and μ is the dynamic viscosity of fluid flowing through the porous domain. This is a measure of flow resistance and has unit of [m^{2}]. Other unit of measurement is the darcy [1 darcy = 0.987 μm^{2}], named after the French scientist who discovered the phenomenon.

STAR-CCM+ uses the expression Δp/L = -(P_{v}.v + P_{i}.v^{2}) for a porous domain.

Steps to find out viscous and inertial resistances:

- Calculate the pressure drop vs. flow velocity data [Δp-v] from empirical correlations or wind-tunnel test or simplified CFD simulations.
- Divide the pressure drop value with thickness of the porous domain. Let's name it as [Δp'-v curve].
- Calculate the quadratic polynmical curve fit coefficients [A, B] from the curve Δp'-v. Ensure that the intercept to the y-axis is zero.
- In STAR-CCM+ this coefficients 'A' and 'B' can be directly used as P
_{v}and P_{i}which are viscous and inertial resistances respectively. - Divide 'A' by dynamics viscosity of the fluid to get inverse of permeability that is 1/α to be supplied as input in ANSYS FLUENT.
- Divide 'B' by [0.5ρ] where ρ is the density of fluid, to get C
_{2}to be supplied as input in ANSYS FLUENT. - The method needs to be repeated for the other 3 directions. If the flow is primarily one-directional, the resistances in other two directions need to be set to a very high value, typically 3 order of magnitude higher.

The rate of convergence slows a porous region is defined such that pressure drop is relatively large in the flow direction (e.g. the permeability is low or the inertial factor is large). This slow convergence can occur because the porous media pressure drop appears as a momentum source term yielding a loss of diagonal dominance in the matrix of equations solved. The best remedy for poor convergence of a problem involving a porous medium is to supply a good initial guess for the pressure drop across the medium. You can supply this guess by patching a value for the pressure in the fluid cells upstream and/or downstream of the medium. It is important to recall, when patching the pressure, that the pressures you input should be defined as the gauge pressures used by the solver (i.e. relative to the operating pressure defined in the simulation).

Another possible way to deal with poor convergence is to temporarily disable the porous media model and obtain an initial flow field without the effect of the porous region. Once an initial solution is obtained, or the calculation is proceeding steadily to convergence, enable the porous media model and continue the calculation with the porous region included. (This method is not recommended for porous media with high resistance.)

Simulations involving highly anisotropic porous media may, at times, pose convergence troubles. This issue can be addressed limiting the anisotropy of the porous media coefficients to two (10^{2}) or three (10^{3}) orders of magnitude. Even if the medium's resistance in one direction is infinite, it is not needed to set the resistance in that direction to be greater than 1000 times the resistance in the primary flow direction.

The content on CFDyna.com is being constantly refined and improvised with on-the-job experience, testing, and training. Examples might be simplified to improve insight into the physics and basic understanding. Linked pages, articles, references, and examples are constantly reviewed to reduce errors, but we cannot warrant full correctness of all content.

Copyright © 2017 - All Rights Reserved - CFDyna.com

Template by OS Templates