- CFD, Fluid Flow, FEA, Heat/Mass Transfer: FEEDBACKS/QUERIES - FB@CFDYNA.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). These are the operating conditions which govern both the micro- and macro behaviors of these variables. A suitable choice of boundary conditions is as good as a good test set-up! Intuitively, a boundary condition implies that "it is known what happens" on a particular boundary.

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.

- Inlet(s) and outlet(s) should be named as b_inlet_id, b_outlet_id where 'id' stands for
__id__entifier. - Walls with boundary conditions (other than adiabatic): w_tpr_id, w_hfx_id, w_htc_id, w_rot_id w_mov_id, w_rgh_id, w_s2s_id where 'rgh' stands for rough walls, s2s stands for coupled solid walls.
- Cell zones: fld_air_id, fld_wtr_id, fld_oil_id, fld_nnw_id, fld_rot_id, por_mom_id, por_thm_id, sld_alm_id, sld_stl_id, sld_src_id ... where 'nnw' stands for non-Newtonian fluids, 'src' stands for solid zones with heat source and/or sink and 'por' stands for porous (fluid) zones.
- Internal planes: int_f2f_id, int_baf_id ... where 'baf' stands for thin walls or baffles.
- Non-conformal interfaces: if_f2f_id, if_s2s_id, if_sta_rot_id, if_por_fld_id, if_por_por_id where 'sta' stands for 'stationary' zones and 'por' stands for 'porous' zones.
- All boundaries with no special setting or conditions to be applied on them can be named as 'b_def_id' or dumy-id1, dumy-id2 or empt-id1, empt-id2 or fblk-id1, fblk-id2 where dumy stands for dummy, empt for empty and fblk for flow-blockers.
**This is especially important while dealing with assemblies with large number of solids and fluid zones.**

**Non-Newtonian Fluids**: Most of the fluids behave such that shear stress is linear function of strain rate with zero initial threshold value of shear stress. However, there are some material where shear stress is non-linear function of strain rate with non-zero initial threshold value of shear stress (yield point) before which flow cannot start. Various type of such material also known as Bingham plastic and Herschel-Bulkley are described below.

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 viscous sub-layer. Please refer to the turbulence 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 roughness 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 conductivity of the solid. Some typical value of thermal conductance when air gaps are not evaluated are tabulated below (reference: A Textbook fo Heat Transfer by Lienhard IV and Lienhard V) -Surface Pair Thermal Conductance [W/m ^{2}K]Copper - Copper 10,000 ~ 25,000 Aluminium - Aluminium 2,200 ~ 12,000 Ceramic - Metals 1,500 ~ 8,500 Stainless steel - Stainless steel 2,000 ~ 3,7000 Ceramic - Ceramic 500 ~ 3,000 **Baffles or Zero Thickness Wall or Two-sided Wall**: A wall that forms interface between regions such as fluid-solid interface are called two-sided walls. When a wall is used to represent thin baffle, a fluid zone will be on each side of the wall. Such zones in FLUENT are automatically split into two identica wall jones by adding suffix '-shadow'. They are coupled unless "Temperature or Heat Flux" boundary conditions are used on one of them. In other words, different temperature and heat flux values can be specied on the two sides of a**Zero Thickness Wall**.**Shell Conduction**: If a thickness is specified to a wall then thermal resistance across the wall thickness is imposed though conduction is considered in the wall in the normal direction only. If the walls are of nearly uniform thickness and the conductive heat transfer needs to be accounted 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.FLUENT creates a shadow wall by adding suffix ':external' to the walls on which shell conduction is switched ON.

- TUI to delete all shell conduction zones: mesh modify-zones delete-all-shells. Note that once shell conduction settings are turned off (deleted), the old data filev(solution with shell conduction) cannot be read with new case file (without shell conduction).
**Wall Motion**:**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).**TUI for Radiation Setting**: /define/models/radiation discrete-ordinate? , , , , where comma is used to accept default values. The 4 inputs needed are (1)Number of θ divisions (2)Number of φ division (3)Number of θ pixels and (4)Number of φ pixels.- The TUI to define emissivities for the walls is: /define/b-c/wall <wall name> , , , , , , , , , 0.40 , , , , where the emissivity is 0.40 and comma is used to accept default values. This TUI command sets the wall as OPAQUE. Also note that the TUI operation does not accept multiple wall zones and hence the setting has to be provided using a loop on multiple face zones of type wall.
**DPM (Discrete Particle Modeling)**: In DPM simulations dealings with solid-liquid or solid-gas where particles or droplets interact with walls, the boundary conditions need to be specified as per expected behaviour. When a solid particle hits the wall, it may either reflect or get captures (stick to the wall). Elastic impact is not realistic even at particles with diameters at micron level. Hence, an appropriate coefficient of restitution need to be specified. Usually, particles traveling at lower velocity (how much lower - it is not a unique value) and smallers ones tend to get captured by the wall. The wall-particle interaction phenomena results in deposition of dust particles on solar panels, leaves of the trees, window panes and the blades of a rotating ceiling fan. Gravity can also have significant effect on dust deposition for particles with diameters > 50 [μm]. For liquid droplets, there are 4 different types of wall-droplet interactions: Splash, Stick, Rebound and Breakup. The rebound with known coefficient of restitution in normal direction (E_{N}) and tangential direction (E_{θ}) is explained in following diagram.

**Natural Convection (Buoyancy-driven Flows)**

- Use Boussinesq approximation to start the simulation. Specify correct density and expansion factor of the fluid
- Initialize the domain with small velocity say 0.02 or 0.05 [m/s] in the direction opposite to the gravity
- Alternatively, solve a force convection flow with small velocity is expected inlet(s) and then switch on to natural convection mode
- Turn-on radiation once flow and temperature fields have stabilized

As per FLUENT User's Manual: "The boundary pressures that you input at pressure inlet and outlet boundaries are the **redefined pressures** as given by equation above. In general you should enter equal pressures, p'_{HS} at the inlet and exit boundaries of your ANSYS FLUENT model if there are no externally-imposed pressure gradients. **For example, if you are solving a natural-convection problem with a pressure boundary, it is important to understand that the pressure you are specifying is p' _{HS}.** Therefore, you should explicitly specify the

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.

Except shell and tube heat exchangers, for most engineering problems it is impractical and sometimes impossible to correctly model individual fins and tubes of a heat exchanger core. In cross-flow heat exchangers such as automotive radiators, air is called primary fluid (the heat sink) and water or coolant as auxiliary (secondary) fluid (the heat source). There are multiple approaches to model such heat exchangers when combined with surrounding systems and sub-systems.

The heat exchanger models were designed for 'compact' heat exchangers, implying that the primary fluid side flow is unidirectional. The auxiliary fluid is assumed to flow through a large number of parallel tubes, which can optionally double back in a serpentine pattern to create a number of **passes**. One can independently choose the direction of principal auxiliary fluid flow, the pass-to-pass direction and the direction of external primary fluid flow. Pressure loss is modeled as a momentum sink in the momentum equation and heat transfer is modeled as a heat source in the energy equation.

Lumped Model | Macro Model | Dual Cell Model | |

Accounts for the pressure loss and auxiliary fluid heat rejection | Simple-effectiveness-model | Number-of-Transfer-Units (NTU) model | Number-of-Transfer-Units (NTU) model |

Core modeled as volumetric heat source | Compute auxiliary fluid inlet temperature for a fixed heat rejection or total heat rejection for a fixed auxiliary fluid inlet temperature | NTU method for heat transfer calculations | |

- | Auxiliary flow is modeled as 1D flow | Auxiliary flow modelled on a separate mesh (other than the primary fluid mesh) |

**Heat Exchangers Models in STAR-CCM+**

**Single stream option**: in this case only one of the fluid streams (usually the cold stream) is modeled explicitly - by specifying the heat exchanger enthalpy source, while the second stream is assumed to have a uniform temperature that user specifies. This is activated by using option**Heat Exchanger**for**Energy Source Option**for the individual Region node.- Heat Exchanger Exit Temperature Specification is used to choose between specifying the heat transfer rate and predicting the outlet temperature or vice versa.
- When this condition is choosen to be 'Inferred', the heat transfer rate can be specified by accessing the Heat Exchanger Energy Transfer physics value node.
- For a heater, the hot stream [e.g. coolant path in automotive radiator] is assumed to have an infinite thermal capacitance and the specified heat exchanger temperature T
_{H}refers to the constant temperature of the hot stream. - For specified heat exchanger energy transfer rate Q, the inlet cold stream [e.g. air in automotive radiators] temperature T
_{CI}, and the cold stream specific heat Cp_{C}, an energy balance could be used to predict the cold stream exit temperature T_{CO}as T_{CO}= T_{CI}+ Q / Cp_{C}/ m_{C}where m_{C}is mass flow rate of the cold fluid. - Heat Exchanger First Iteration: This node specifies the iteration from which the heat exchanger enthalpy source is active and begins its contribution to the source term of the energy equation.
- It is recommended to active the source term when the flow is beginning to conform to its expected pattern, at least in terms of direction. As per user manual, 50 iterations is a good estimate to get a reasonable conformity.

**Dual stream option**: here both the streams are modeled explicitly by defining two overlapping regions and creating a heat exchanger interface between them. This model supports**fluid-solid interface**where the heat exchange occurs between a solid region and a fluid region and**fluid-fluid interface**where the heat exchange takes place between two fluid regions. For a fluid-fluid type heat exchanger, following options are available for specifying heat transfer rate in the heat exchanger:- UAL Polynomial [UAL is function of cold flow velocity], UAL Table [UAL is a table of the cold flow velocity], UAL Map [map of curves to specify the UAL directly when multiple heat exchanger curves]: UA refers to the product of the Overall heat transfer coefficient (U) and the Area of the heat exchanger (A). UAL refers to the local (or cell value of) heat transfer coefficient (in W/K), with L referring to local.
- UAG [U.A Global] Table
- Q Table [table of the cold stream mass flow rate for one value of hot stream mass flow rate], Q Map [series of curves from which it calculates UAL].

**Basic option:**This option solves for a simpler version of the energy equation using only the convective term and the source term to yield a solution.**Heat Exchanger Topology:**- When using the
**basic option**, ensure that the core mesh is constructed of uniform cells. - In other words, all the cells in the heat exchanger region must be of comparable cell volume, as the cell volumes do not enter the calculation of the UAL table in the basic model.
- The accuracy of results that the
**actual dual stream**heat exchanger predicts does not depend on the uniformity of the mesh. - The topology must contain two identical regions with a different continuum associated with each region.
- Both the regions [hot and cold streams] should be created from the same mesh continuum. To ensure this, copy the [core region of the radiator] region after the volume mesh has been generated.
- Once the two overlapping regions exist, the heat exchanger interface can then be created by selecting the two regions and choosing Create Interface from the right-click menu. While selecting the two regions, select the region representing the cold stream before the region representing the hot stream.
- The mesh alignment option should be activated so that a conformal match is obtained across mesh interfaces. STAR-CCM+ does not automatically generate a conformal mesh across interfaces for the trimmed cell mesh type. Operations > Automated Mesh > Meshers > Trimmed Cell Mesher node and activate Perform Mesh Alignment.
- Create a block shape part around the core which required for the volumetric controls that define mesh refinement. Geometry > Parts node and select New Shape Part > Block.

- When using the
**Actual option:**UAL Map method is available with the**actual dual stream**heat exchanger option only.

- In both the options, heat is added or removed from the core cells as a source or sink term in the corresponding fluid energy equation. It is assumed in this section that both the streams exist only in a single phase (liquid or gas) and no phase change occurs inside the heat exchangers.

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. In

- 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.
**Interior types boundaries don't have a strict 'boundary' or 'interface' conditions, they simply pass information along.**Values at interior faces follow the interpolation and reconstruction rules. Coupled walls are similar in that they mostly pass information along but they have interface conditions (they match fluxes). - 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.

Sometimes, the axis of the fan or MRF domain does not pass through origin. If the geometry or mesh was created in some other units (not in meters), scaling the domain in ANSYS FLUENT may change the location of axis. That is the coordinates of a point on axis of the fan may not be same when the mesh is scaled into meter in ANSYS FLUENT. This is bacause scaling of a 3D space needs some reference point: centroid of the geometry or orgin are two ideal options. The X, Y and Z coordinates on axis of a fan can be estimate by calculating

Let (x_{0}, y_{0}, z_{0}) is the centre of circle passing though 3 points (x_{1}, y_{1}, z_{1}), (x_{2}, y_{2}, z_{2}) and (x_{3}, y_{3}, z_{3}). From equality of distance (radius): (x_{0} - x_{1})^{2} + (y_{0} - y_{1})^{2} + (z_{0} - z_{1})^{2} = (x_{0} - x_{2})^{2} + (y_{0} - y_{2})^{2} + (z_{0} - z_{2})^{2}. This simplifies to following set of equations. Note that this is valid only when the points are truely 3D that is the circumcircle is not aligned with either of the axes.

2(x_{2}-x_{3}) x_{0} + 2(y_{2}-y_{3}) y_{0} + 2(z_{2}-z_{3}) z_{0} = (x_{2}^{2} - x_{3}^{2}) + (y_{2}^{2} - y_{3}^{2}) + (z_{2}^{2} - z_{3}^{2}) ... [2]

a_{1} x_{0} + b_{1} y_{0} + c_{1} z_{0} = d_{1} ... [4]

a_{2} x_{0} + b_{2} y_{0} + c_{2} z_{0} = d_{2} ... [5]

a_{3} x_{0} + b_{3} y_{0} + c_{3} z_{0} = d_{3} ... [6]

**For 2D plane when it is aligned to one of the Cartesian planes (XY or YZ or ZX): **

First point | X11: | X12: | ||

Second point | X21: | X22: | ||

Third point | X31: | X32: | ||

This is opposite 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. There is no similar boundary conditions available in CFX.

- 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.

**Examples of porous materials**: note that a material which does not allow convection of fluid (e.g. brick, soil, cotton...) may allow diffusion of the fluid (brick, cotton...) such as water. In general, most of the applications of porous domain in CFD simulations refer to convection phenomena such as flow through the radiator core and honeycomb in a catalytic converter.

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.

Most of the time the pressure drop across a porous domain are reported in terms of v

In FLUENT and CFX, 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. **Note that FLUENT takes 1/α as input for porous regions. ** This is a measure of flow resistance and the unit of permeability (α) is [m^{2}]. Other unit of measurement is the darcy [1 darcy = 0.987 μm^{2}], named after the French scientist who discovered the phenomenon. The unit of inertial loss coefficient (C_{2}) is [m^{-1}]. A good knowledge of soil permeability, also termed hydraulic conductivity is needed for estimating the quantity of seepage under dams and dewatering to facilitate underground construction. The degree of pore saturation with water is one of significant factors affecting the soil water permeability. The permeability coefficient has unit of [m/s] and is calculated by Q.L/A/H where Q is the leakage flow rate [m^{3}/s], L is the length of height of porous domain [m], A is cross-section area [m^{2}] and H is applied hydraulic head [m]. The value of soils varies from 10^{-4} to 10^{-10} [m/s]. Clay is the most porous sediment but is the least permeable which acts as an aquitard, impeding the flow of water.

Inertial loss coefficient is known as Quadratic Loss Coefficient in CFX. An alternate formulation in CFX is in terms of Linear Loss Coefficient [kg/m^{3}/s] and Quadratic Loss Coefficients [kg/m^{4}] which are defined as A and B respectively above or P_{v} and P_{i} below.

STAR-CCM+ uses the expression Δp/L = -(P_{v}.v + P_{i}.v^{2}) for a porous domain. Here P_{v} is Viscous Loss Coefficient and has unit [kg/m^{3}/s] and P_{i} is known as Inertial Loss Coefficient having unit [kg/m^{4}]. Note that it is the coefficient of v^{2} which is called **Inertial** which is contrary to the fact that viscous pressure drop is proportional to v^{2}.

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' vs. v curve].
- Calculate the quadratic polynomial curve fit coefficients [A, B] from the curve Δp' vs. -v. Ensure that the intercept to the y-axis is zero.
- In STAR-CCM+ these coefficients 'A' and 'B' can be directly used as P
_{v}and P_{i}which are viscous and inertial resistance coefficients respectively. - Divide 'A' by dynamics viscosity of the fluid to get
**inverse of permeability that is 1/α**to be used in ANSYS FLUENT as "viscous resistance coefficient". - Divide 'B' by [0.5ρ] where ρ is the density of fluid, to get
**C**to be used in ANSYS FLUENT as "_{2}**inertial resistance coefficient**". - 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.

When pressure drop is linear function of velocity, it is known as Darcy's Law: Δp = - μ/α × v. This option is implemented explicitly in COMSOL.

In case porous domain is not aligned to any coordinate direction, the direction of unit vector along the flow and across the flow directions can be estimated from following Javascript program. Note that empty field is considered as 0.0. There is no check if a text value is specified in the input fields and the calculator will result in an error.

First point - X1: | |

First point - Y1: | |

First point - Z1: | |

Second point - X2: | |

Second point - Y2: | |

Second point - Z2: | |

Porous Loss Coefficient Calculator

Note that the loss coefficients are assumed to be (and most of the time they are so) parabalic. Hence, only 3 sets of points are required to derive the parabolic equation. It is recommended that the first point is close to no-flow conditions, second point close to the mid-point of operation and the last point towards the highest flow rate conditions. In the table below, P_{i} refers to pressure drop across the porous domain at V_{i}. Air is assumed to be the working fluid. Sutherland law is used to find out viscosity of air at specified temperature.

Thickness of HX | TH | [mm] | |

First point | V1 | [m/s] | |

First point | P1 | [Pa] | |

Second point | V2 | [m/s] | |

Second point | P2 | [Pa] | |

Third point | V3 | [m/s] | |

Third point | P3 | [Pa] | |

Gas Temperature | Tg | [°C] | |

Gas Pressure | Pg | [kPa] | |

Example calculation: x = {0.0 1.0 2.5}, Y = {0 50 75}, m_{1} = 50.0, m_{2} = 16.67, A = -13.33, B = 63.33, C = 0.0. The parabola generated by the curve fit coefficients looks like as shown below. Note that a parabola with local maxima towards higher value of X-axis may have a negative value of A or B.

The formula to derive A, B and C are as follows:

If the porous domain is not inclined the coordiate system of the entire model, a local coordinate system needs to be created to specify viscous and inertial loss coefficients. Most pre-processors such as FLUENT and STAR-CCM+ have option to create a coordinate system based on origin and two points which can be selected graphically using left mouse button. In case it is to be specified using a direction vector such as in macros or scripts, following transformation matrix should be used.

Note that the transformation matrix is for rotation about z-axis. Thus, a vector in Laboratory Reference Frame (1.0, 0.0, 0.0) shall become (cosθ, -sinθ, 0.0) when rotated by angle θ about z-axis.

Porosity provides information on the overall pore volume of a porous material and is defined as the ratio of the nonsolid volume (voids) to the total volume of the nonwoven fabric. The air permeability and porosity of fabric duct are inter-dependent. An increase in porosity (the free space) should lead to decrease in permeability (resistance to the air flow). From flow point of view, a volume based definition of porosity may not provide a direct relation to the the flow velocity which depends on flow area perpendicular to the flow direction.

There is decrease in atmospheric pressure and temperature with altitude as compared to height above sea level. Why sea level is considered as reference datum? This is because the lquids maintain uniform level and any point anywhere in the sea is expected to be same radial distance from the centre of the Earth.

p [Pa] = 101325 * (1 - 2.25577E-05 × H)^{5.2559} where altitude H is in [m].

T [K] = 288.15 - 0.0065 × H. You may use the following calculator to estimate ambient pressure and tempearture at higher altitudes. There is option to chose altitude in [m] or [ft]. However, the outputs are in SI units.

Altitude, H | |

Unit | |

In situations with multi-component flows (such as leakage of fuel or refrigerant) where diffusion dominates the correct specification of binary diffusion coefficient is very important. Following table specifies value at 1 [atm] and 300 [K]. Reference: Analytic Combustion by Anil W. Date.

Pair | D_{ab} [m^{2}/s] |

H2O - air | 24.0E-6 |

CO - air | 19.0E-6 |

CO2 - air | 14.0E-6 |

H2 - air | 78.0E-6 |

O2 - air | 19.0E-6 |

SO2 - air | 13.0E-6 |

NH3 - air | 28.0E-6 |

CH3OH - air | 14.0E-6 |

C2H5OH - air | 11.0E-6 |

CH4 - air | 16.0E-6 |

C6H6 - air | 8.00E-6 |

C8H18 - air | 5.00E-6 |

C8H16 - air | 7.10E-6 |

C10H22 - air | 6.00E-6 |

O2 - H2 | 70.0E-6 |

CO2 - N2 | 11.0E-6 |

CO2 -H2 | 55.0E-6 |

C6H14 - N2 | 8.00E-6 |

C8H18 - N2 | 7.00E-6 |

C10H22 - N2 | 6.40E-6 |

Here:

- Q = Volumetric flow rate [m
^{3}/s] - A = cross section area of the flow passage [m
^{2} - L = Length of flow path along the direction of flow [m]
- ΔP = pressure drop along the direction of flow = [p - ρgh] [Pa], ρ = density of fluid [kg/m
^{3}], g = acceleration due to gravity [m^{2}/s], h = height along the direction of gravity [m] - C = constant of proportionality [m
^{2}/Pa.s] = μ/k, μ = dynamic viscosity of fluid [Pa.s], k = permeability [m^{2}]

Dupuit-Thiem equation (based on Darcy Law in cylindrical coordinate system) is a widely used formula to estimate pressure drop across the wall for a known (oil extraction) flow rate in a circular reservoir that has a constant pressure at its outer boundary.

**Dust Accumulation in Air Filters**: There are many application of air filters such as automotive air cleaners. Dust Holding Capacity (DHC) is one of the key parameters of such filters. The filter are orthotropic porous media where the porous loss coefficients are different along the 3 directions. However, any CFD simulations to deal with dust accumulation will be a transient simulation where the behaviour of porous domain will change depending upon duct collection level and spatial distribution. This is because filter may not collect dust uniformly and hence permeability will change non-uniformly. For most practical applications, change in pressure drop can be assumed to be a linear function of duct loading (the amount of dust trapped in filters). *How does one model the trapping of dust particles in the pores of the filter? *Neither the filter pores nor the diameters of the particles are uniform in size and shape!

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.

In the fluid mechanics of porous media, tortuosity is the ratio of the length of a streamline to that of the straight-line distance between those points. A measure of deviation from a straight line. It is the ratio of the actual distance traveled between two points, including any curves encountered, divided by the straight line distance. Tortuosity is used by drillers to describe wellbore trajectory, by log analysts to describe electrical current flow through rock and by geologists to describe pore systems in rock and the meander of rivers.

A related concept is fractal which is used to describe the effective length of rivers and used even for trading in stock markets.

[2]: A method for aerodynamic drop break-up that has been widely implemented is known as the Taylor Analogy Break-up model or TAB. The TAB model approximates a drop as a damped oscillator system and tracks a deformation parameter. When the deformation parameter is sufficiently large, break-up is assumed.

- σ: surface tension of liquid which is measure of cohesive force between liquid molecules.
- H: Capillary rise (or depression) - lower point of the meniscus. Note that the capillary effect is the net effect of competitive forces adhesion (force between liquid and solid molecules) and cohesion. Contact angle is a constant property of liquid-solid interface and affects capillary rise.
- If contact angle is zero, the liquid surface is parallel to solid surface and the liquid is said to wet the solid completely. The equation relating to the contact angle and surface tension between all 3 interfaces namely liquid-solid, liquid-gas and solid-gas is known as Young's equation. σ
^{SL}- σ^{SG}+ σ^{LG}cos(θ) = 0 where S, L and G refer to solid, liquid and gas phases. - System energy, E = σ × (2πrH) + ρ/2×(πr
^{2}H) × g - Capillary length, L
_{C}= [2σ/ρ/g]^{0.5}~ 4.0 [mm] for water at room temperature. - Under dynamic condition when liquid level is increasing in the capillary tube, its rise is resisted by a combination of gravity, viscosity, fluid inertia and dynamic pressure.
- The timescale required to establish Poiseuille flow is, t = 4ρr
^{2}/μ where μ is the dynamic viscosity. For water and 0.50 [mm] tube: t ~ 1.2 [s], for 0.20 [mm] tube: t = 0.2 [s]. If rise timescale is less than this value, inertia of liquid mass dominates and inertial overshoot results in oscillation of liquid column about steady state (equilibrium) height. - Note that the capillary rise predicted is 15 [m] for micro-pores (r =1.0 μm ie. 1.0E-6 m).
- The nature of wetting depends on the choice of liquid as well as on the nature of the surface. For example, water spreads on a clean glass surface but beads up on a glass sheet coated with a monolayer of dimethyloctylchlorosilane (generating a hydrophobic surface).
- Spreading of liquid also depends on the nature of the surrounding fluid. For example, oil droplets on a surface under water have a different contact angle than an oil drop in air. In both the cases, the fluid pairs are immisible.

Surface tension and angle of contact with water and some of the non-metals are tabulated below as per www.accudynetest.com.

Surface Tension of Water with | Abbreviation | [N/m] | [°] |

Silicone Oxide | Glass | 0.0725 | ~ 0 |

Poly-Vinyl-Chloride | PVC | 0.0379 | 85.6 |

Poly-Tetra-Fluoro-Ethylene | PTFE | 0.0194 | 109 |

Poly-Amide-6-6 | Nylon-66 | 0.0422 | 68.3 |

Poly-Methyle-Meth-Acrylate | PMMA (Acrylic, Plexiglass) | 0.0375 | 70.9 |

Poly-Ethylene-Terephthalate | PET | 0.0390 | 72.5 |

Poly-Carbonate | PC | 0.0440 | 82.0 |

Acrylonitril Butadine Styrene | ABS | 0.0385 | 80.9 |

Poly-Ethylene | PE | 0.0316 | 96.0 |

Poly-Propylene | PP | 0.0305 | 102 |

One of the applications of capillary effect combined with fully-developed laminar (Poiseuille) flow is pipetting. Pipetting process is aspiration of a pre-determined volume of liquid by creating a vacuum above a tapered capillary tube (known as tip). The pressure in the pipette chamber during the process is in a dynamic equilibrium and is affected by the ambient pressure, viscosity, surface tension and density of the liquid, and the speed of the piston movement. The suction (aspiration) of liquid in pipette tips normally undergo following 4 phases:

**Acceleration phase**: The rate of decrease of pressure the pipette chamber is higher than the rate of increase of pressure caused by reduction in gas volume due to aspirated volume of the liquid. Thus, the fluid-gas interface will tend to accelerate.**Uniform speed phase**: The pressure in the cavity reduced uniformly and is balanced by actual pressure increase due to reduction in gas volume caused by suction of fluid.**Deceleration phase**: the piston speed slows down, but the total pressure difference between the inside and outside of the pipette chamber is still high to keep the fluid moving. The liquid suction speed gradually slows down and finally maintains the balance.**Balancing phase**: the pipetting operation is completed and the static equilibrium is achieved between pressure, surface tension and hydrostatic forces.

Regime-I | Regime-II | Regime-III | Regime-IV |

Initial boundary effects important | Viscous effect negligible | Poiseuille flow: inertia effect negligible | Late viscous regime |

Surface tension forces dominant | Capillary rise resisted by fluid inertia | Lucas-Washburn law applies | Fluid rise approaches steady state height |

Capillary rise: z ∝ t^{2} | Capillary rise: z ∝ t | Capillary rise: z ∝ t^{0.5} | Capillary rise: z ∝ e^{-t} |

- Use of prefixes and suffixes appropriately
- Name fluid zones as f-air- or f-water- for fluids, s-steel- for solids, por- for porous.
- Add bc-inlet-tpr for "Total Pressure" boundary condition at inlet, bc-inlet-mfl for "Mass Flow" boundary condition or bc-inlet-vel for "Velocity Inlet".
- Similarly, use bc-outlet-sprs for "Static Pressure", bc-outlet-oflo for outflow...
- Walls with specified heat flux of heat transfer coefficient should also be named appropriately such as wf-htc- or wf-hfx- or wf-tmp-
- Interfaces can start with keyword if-ff- or if-ss- or if-sf-
- Periodic boundaries can be named as prd-trn- or prd-rot-

**The format of the standard transient profile file:**

( (inletvel transdata 3 0) (time 1 2 3 ) (invel 6 5 4 ) )Here '3' denotes the number of data points (number of rows in tabular format). '0' indicated that data is not time-periodic, use '1' for a time-periodic dataset. 'invel' shall appear as drop-down in boundary condition panel. Note:

- All quantities, including coordinate values, must be specified in
**SI units**. - Profile names (e.g. 'inletvel' in this example) must have all
__lowercase__letters - Data can be either in column or row format.

The data set used above can also be specified as described below:

( (inletvel transdata 3 0) (time 1 2 3 ) (invel 6 5 4 ) )

__Tabular Transient Profiles__

inletvel transdata 3 0 time invel 1 6 2 5 3 4

**Interpolation file format: ANSYS FLUENT**

2 --the interpolation file version 3 --dimension (2 or 3) 25000 --total number of points 3 --total number of fields (velocity, pressure...) included x-velocity --field variable to be interpolated pressure --field variable to be interpolated -0.100000 --x-coordinate of first node in the list -0.200000 --y-coordinate of first node in the list -0.300000 --z-coordinate of first node in the list ... ... ... 1.000000 --x-coordinate of last node in the list 2.000000 --y-coordinate of last node in the list 3.000000 --z-coordinate of last node in the list 0.500000 --x-velocity at first node in the list 0.100000 --x-velocity at second node in the list 0.200000 --x-velocity at third node in the list ... ... ... 5.000000 --x-velocity at last node in the list 100.0000 --pressure at first node in the list 200.0000 --pressure at second node in the list 300.0000 --pressure at third node in the list ... ... ... 500.0000 --pressure at last node in the list

At the end is a list of the field values at all the points in the same order as their names. The number of coordinate and field points (x-velocity and pressure in this case) should match the number given in line 3 (25000 in this case). Note that it cannot interpolate heat generation rate (W/m^{3}), though internal energy, enthalphy, heat transfer coefficient... can be interpolated. In other words, no volumetric source/sink term can be interpolated in the fluid region. On the boundaries, all field variables are available for interpolation.

**Data Export into CSV Format: ANSYS FLUENT**:

The header in CSV files for FLUENT and STAR-CCM+ uses different variable names. In STAR-CCM+ variables has to be specified with appropriate units: e.g. "Absolute Pressure (Pa)", "Velocity Magnitude (m/s)", "Velocity[i] (m/s)", "Velocity[j] (m/s)", "Velocity[k] (m/s)", "X (m)", "Y (m)", "Z (m)"... Note the space between variables and unit. The x-component of velocity is accessed by Velocity[i].

**Data Mapper: STAR-CCM+**:

Using a user field function, the table data which provides the variations of velocity with time can be imported and then defined as follow:

interpolateTable(@Table("VelData"), "Time", LINEAR, "VelMPS", $Time)

Here the field function type should be vector. For boundaries such as inlet, in the “Physics Values” option of the boundary in the “Method” field, select Field Function, and then right below this, select the field function defined earlier.

The name of the table is VelData, Time is the name for the first column in the .csv file, LINEAR (other option available is SPLINE) is the interpolation method creating values between the discrete time values specified in the table, VelMPS is the name of the second column in the table (corresponding to the velocity magnitude), $Time specifies that the velocity is function of time. In case velocity is function of spatial coordinates say y-axis: $${Position}[1] can be used in place of $Time to specify that the position coordinate is aligned with the y-axis (1 = y-direction, use '0' for x-direction and 2 for z-direction).

References:

- STAR-CCM+ User Guide Version 10.02
- ANSYS FLUENT User Guide V15.0
- Break-up and atomization of a round water jet by a high-speed annular air jet: J. C. Lasheras, E. Villermaux And E. J. Hopfinger
- Modeling Aerodynamic Break-Up Of Liquid Drops In A Gas Flow With Molecular Dynamics Analogy Methods: Alexander L. Brown And Flint Pierce, Sandia National Laboratories, PO Box 5800, Albuquerque, NM, 87185-1136, USA

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