• CFD, Fluid Flow, FEA, Heat/Mass Transfer

Boundary Conditions

Type of Boundary Conditions, Applications and Limitations

What is physical and mathematical significance of a boundary condition?

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.


Naming Convection of Boundaries and Cell Zones

In any practical application of CFD simulations, the computational domain may comprise of many cells zones (fluid and solid zones) and boundary zones (walls, inlets and outlets). The engineer responsible for pre-processing may not be the one who creates solver file and post-processes the results. The reviewer(s) of the mesh and simulation set-up will certainly be not the engineer who created them. In order to convey the domain information seamlessly, a naming convention should be adopted, it can be a generic system applicable for large number of projects or a specific system for particular simulation set-up. An example is outlined below with following default setting: Newtonian, stationary, adiabatic, smooth boundaries or zones can be named arbitrarily though it is recommended to chose names and identifiers meaningfully.
  1. Inlet(s) and outlet(s) should be named as b_inlet_id, b_outlet_id where 'id' stands for identifier.
  2. 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.
  3. 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.
  4. Internal planes: int_f2f_id, int_baf_id ... where 'baf' stands for thin walls or baffles.
  5. 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.
  6. All boundaries with no special setting or conditions to be applied on them can be named as 'b_def_id'.

Inlet

This is the 1st member of the pair of boundary conditions which are must for any CFD calculations in a forced convection situation. Of course a natural convection case does not required any inlet or outlet. The primary consideration of an inlet B.C. is to select between the Mass Flow Rate, Static Pressure and Total Pressure based on the actual information available about the operating conditions of the system and robustness of the solver, (the matrix inversion) algorithm which keeps running till solution is achieved. While tempting to use velocity inlet B.C. care needs to be taken to account for change in cross-sectional area when an arc is represented by a set of connected lines.

Mass Flow Inlet Boundary Condition

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 [m2/s2] and TED [m2/s3] explicitly
  • Turbulent Intensity [%] and Turbulent Viscosity Ratio (TVR) [-]
  • Hydraulic Diameter [m] and Turbulent Intensity [%]
  • Turbulent Intensity [%] and Length Scale [m]
These requirements on turbulent parameters further depends on flow type: external or internal. The length scale 'L' For external flows is typically the length scales along the flow direction.
  • 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
The setting for inlet and outlet boundary conditions in ANSYS FLUENT is shown below:

Inlet BC


Outlet

Outlet BC

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


Wall Boundary - What is physical and mathematical significance?

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:

Wall BC

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".
    • ks = Sand Roughness Height [m] or [μm], k+ = ks/h where h is characteristic height of viscous sub-layer. Please refer to the turbulence modeling page for definition of viscous sub-layer.
    • ks >> 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.
    • ks < 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, Reks is defined as Reks = ρ.u+.ks/μ and the surface roughness condition can be defined as:
      • Reks ≤ 5: hydraulically smooth and the wall surface roughness need not be activated in CFD simulations
      • 5 < Reks ≤ 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
      • Reks > 70: fully rough regime and wall surface roughness need to be activated in CFD simulations.
  • 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.
  • 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.

    Thin Wall Modeling in FLUENT

    Shell conduction can be used to account for thermal mass in transient thermal analysis problems such as thermal soaking (ramp-up) or thermal cool-down. It can also be used for multiple junctions and allows heat conduction through the junctions. Shell conduction can be applied on boundary walls as well as internal walls. Fluxes at the ends of a shell conducting wall are not included in heat balance reports. These fluxes are accounted for correctly in the ANSYS FLUENT solution, but are not listed in the flux report.
  • Wall Motion:

    Moving Wall Modeling in FLUENT

  • 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).
  • 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 (EN) and tangential direction (Eθ) is explained in following diagram.

    Particle rebounding from a wall


Periodic Boundary Conditions

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. Rotational Periodic Boundary

Symmetry Boundary Conditions

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.

CFX Recommendation on pair - combination of boundary conditions
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
FLUENT Recommendation on pair - combination of boundary conditions
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

FAN Boundary Conditions

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*x2 + ... , 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.

Rotating Domains

MRF and SMM conditions in FLUENT


POROUS JUMP Boundary Conditions

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*x2 + ... , 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.

Porous Domains

Flow geometry such as heat exchangers with closely spaced fins, honeycomb flow passages in a catalytic converters, screens or perforated plates used as protection cover at the from of a tractor engine ... are too complicated to model as it is. They are simplified with equivalent performance characteristic, knowns as Δp-Q curve. These curves are either generated using empirical correlations from textbooks or using a CFD simulation for smalled, periodic / symmetric flow arrangement. The simplified computational domain is known as "porous zone" in case it is represented as a 3D volume or pressure or porous jump in case it is represented as a plane of zero thickness. In a similar fashion, the performance data of a fan can be specified including the swirl component.

All the porous media formulation take the form: Δp = -L × (A.v + B.v2) 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 + C2.ρ/2.v2) 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 [m2]. Other unit of measurement is the darcy [1 darcy = 0.987 μm2], named after the French scientist who discovered the phenomenon.

STAR-CCM+ uses the expression Δp/L = -(Pv.v + Pi.v2) for a porous domain.

The pressure drop is usually specified as Δp = ζ/2·ρ·v2 where ζ is 'equivalent loss coefficient' and is dimensionless. Darcy expressed the pressure gradient in the porous media as v = -[K/μ]·dP/dL where 'K' is the permeability and 'v' is the superficial velocity or the apparent velocity determined by dividing the flow rate by the cross-sectional area across which fluid is flowing.

Steps to find out viscous and inertial resistances:

  1. Calculate the pressure drop vs. flow velocity data [Δp-v] from empirical correlations or wind-tunnel test or simplified CFD simulations.
  2. Divide the pressure drop value with thickness of the porous domain. Let's name it as [Δp'-v curve].
  3. Calculate the quadratic polynomial curve fit coefficients [A, B] from the curve Δp'-v. Ensure that the intercept to the y-axis is zero.
  4. In STAR-CCM+ these coefficients 'A' and 'B' can be directly used as Pv and Pi which are viscous and inertial resistance coefficients respectively.
  5. 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".
  6. Divide 'B' by [0.5ρ] where ρ is the density of fluid, to get C2 to be used in ANSYS FLUENT as "inertial resistance coefficient".
  7. 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 GUI to set porous domain in ANSYS FLUENT is as shown below. For 3D cases, direction vectors for any two principal axes need to be specified, the third direction is automatically calculated by FLUENT. However, one must be consistent in specification of direction vector and resistance coefficients.

Porous Media Setting in ANSYS FLUENT

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:  

Atmospheric Data
Reference: Analytic Combustion y Anil W. Date (Cambridge Press).

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

Binary Diffusion Coefficients

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 Dab [m2/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

Darcy Law for Porous Media
This is the basic law governing the flow of fluids through porous media such as soil, rocks and sand beds. This is analogous to other linear phenomenological transport laws namely Ohm’s law for electrical conduction, Fick’s law for solute diffusion and Fourier’s law for heat conduction. Note that Darcy’s law is a macroscopic law will hold true over regions that are much larger than the size of a single pore.

Darcy Law for Porous Media

Here:
  • Q = Volumetric flow rate [m3/s]
  • A = cross section area of the flow passage [m2
  • 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/m3], g = acceleration due to gravity [m2/s], h = height along the direction of gravity [m]
  • C = constant of proportionality [m2/Pa.s] = μ/k, μ = dynamic viscosity of fluid [Pa.s], k = permeability [m2]
In petroleum engineering, due to very low permeability of rocks, 'Darcy' unit defined by 1 [Darcy] = 0.987×10-12 [m2] is widely used. The Darcy unit can be interpreted as a flow rate of 1 [ml/s] through a rock of fluid with viscosity 1 [cP] = 0.001 [Pa.s] through a cross-section of of 1 [cm2] when the pressure drop along the direction of flow were 1 [atm/cm].

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!


Convergence Troubleshooting Strategies for Porous Media

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 (102) or three (103) 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.


Tortuosity
Tortuosity - derived from work 'tortuous' - is a measure of the geometric and flow path complexity of a porous medium. A molecule often has to traverse a path that is several times longer than the straight line between its original source and destination. Tortuosity is a ratio that characterizes the tortuous and meandering (convoluted) pathways of fluid convection and/or diffusion through the media.

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.


Surface Tension and Capillary Effect
Though CFD may not be required to solve phenomena such as capillary rise, any flow geometry where surface tension effects are comparable to viscous effects should be dealt carefully. Following chart and OCTAVE (or MATLAB) scrip summarizes the effect of pipe diameter on capillary rise and volume of liquid that can be lifted.

Capillary rise and volume of water

Some historical notes: Geovanni Borelli (1608-1675) demonstrated experimentally that h ∝ 1/r. James Jurin (1684-1750), an English physiologist who independently confirmed that h ~ 1/r and hence the capillary rise law is also known as Jurin’s Law. As the water rises in tube, the total energy of system is sum of "surface energy" and "gravitational potential energy".
  • 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. σSL - σSG + σLG cos(θ) = 0 where S, L and G refer to solid, liquid and gas phases.
  • System energy, E = σ × (2πrH) + ρ/2×(πr2H) × g
  • Capillary length, LC = [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 = 4ρr2/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

OCTAVE Script
Note that the script does not check whether the radius of the capillary is << capillary length or not. The increase in volume of liquid with increasing radii of the capillary tube is counter-intutive. Can you explain why this behaviour is observed?
%Script to calculate capillary rise and plot a curve for different radii

%Surface Tension [N/m]
%Water (at 20 C): 0.073, Glycerin: 0.063, Blood (at 37 C): 0.058, Ammonia: 0.021
%Ethyl alcohol: 0.023,	 Kerosine: 0.028, Soap solution: 0.025,   Mercury: 0.440
s = 0.073;

%Contact angle (deg) - depends on liquid-solid combination
q = 0;   %For water-glass combination

%Density [kg/m^3]
rho = 990;

%Acceleration due to gravity [m/s^2]
g = 9.806;

%Minimum radius of tube [mm]
R1 = 0.25;

%Maximum radius of tube [mm]
R2 = 1.25;

%------------------------------------------------------------------------------
dr = (R2 - R1)/25;
r = [R1: dr: R2];
h = (2000 * s * cos(q*pi/180) / rho / g ./ r) * 1000;
V = pi .* r .^2 .* h / 1000;

hold on; subplot(311); 
plot(2*r, h, "linestyle", ":", "linewidth", 2, "marker", "o");
xlabel('Tube Diameter, d [mm]'); 
ylabel('Capillary Rise [mm]'); grid on;
%  
% Format X-axis ticks
  xtick = get (gca, "xtick"); 
  xticklabel = strsplit (sprintf ("%.1f\n", xtick), "\n", true);
  set (gca, "xticklabel", xticklabel)   
%  
% Format Y-Axis ticks
  ytick = get (gca, "ytick"); 
  yticklabel = strsplit (sprintf ("%.1f\n", ytick), "\n", true); 
  set (gca, "yticklabel", yticklabel);
%
subplot(312);
plot(2*r, V, "linestyle", ":", "linewidth", 2, "marker", "o");
xlabel('Tube Diameter, d [mm]'); 
ylabel('Capillary Volume [mL or cm^3]'); grid on;
%  
% Format X-axis ticks
  xtick = get (gca, "xtick"); 
  xticklabel = strsplit (sprintf ("%.2f\n", xtick), "\n", true);
  set (gca, "xticklabel", xticklabel)   
%  
% Format Y-Axis ticks
  ytick = get (gca, "ytick"); 
  yticklabel = strsplit (sprintf ("%.2f\n", ytick), "\n", true); 
  set (gca, "yticklabel", yticklabel);
%
subplot(313);
plot(2*r, V*1000, "linestyle", ":", "linewidth", 2, "marker", "o");
xlabel('Tube Diameter, d [mm]'); 
ylabel('Capillary Volume [\muL]'); grid on;
%  
% Format X-axis ticks
  xtick = get (gca, "xtick"); 
  xticklabel = strsplit (sprintf ("%.2f\n", xtick), "\n", true);
  set (gca, "xticklabel", xticklabel)   
%  
% Format Y-Axis ticks
  ytick = get (gca, "ytick"); 
  yticklabel = strsplit (sprintf ("%.0f\n", ytick), "\n", true); 
  set (gca, "yticklabel", yticklabel);
Have you noticed why the water does not spill even when the water level is above the brink of a bowl!

Surface Tension Effect in a Bowl

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.

Four phases of capillary rise

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 ∝ t2 Capillary rise: z ∝ t Capillary rise: z ∝ t0.5 Capillary rise: z ∝ e-t

Mesh and Simulation Set-up File Review
One of the challenges for any reviewer is to understand the geometry and the naming convention used for define boundary and fluid zone. Just looking at the name of the zones, no information can be gathers if it is arbitrarily designated. Some naming convention will go a long way in making the review process easier. One of the many ways is:
  1. Use of prefixes and suffixes appropriately
  2. Name fluid zones as flu-air- or flu-water- for fluids, sol-steel- for solids, por- for porous.
  3. 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".
  4. Similarly, use bc-outlet-spr for "Static Pressure", bc-outlet-ofl for outflow...
  5. Walls with specified heat flux of heat transfer coefficient should also be named appropriately such as wf-htc- or wf-hfx- or wf-tmp-
  6. Interfaces can start with keyword if-ff- or if-ss- or if-sf-
  7. Periodic boundaries can be named as prd-trn- or prd-rot-

Result Data Interpolation
Many a times we need to interpolate the results from previous simulations into a new simulation, such as when a new mesh is generated due to refinement or coarsening. Sometimes results may be available from simulations carried out in other software (such as FLUENT or OpenFOMA) and the field variables need to be read into a new software (STAR-CCM+). Most of the commercial program provide an options to import and export data from and into CGNS and/or CSV format. The data in this format can be used to exchange result data from one program to the other.

ANSYS FLUENT - Export Data into CGNS Format

Data Import into ANSYS FLUENT:

ANSYS FLUENT - Data Import Options

Data Export into CSV Format: ANSYS FLUENT:

ANSYS FLUENT - Data Export into CSV

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+:

STAR-CCM+ Data Mapping


TUI in ANSYS FLUENT
Over the different versions, while new features have been added, the name of some of command have been altered and many have been removed / consolidated. For example, 'grid' has been replaced with 'mesh', /display/ set/ colors/ background white" has been replaced by "/display/ set/ colors/ graphics-theme-color white".
Define
/define/boundary-conditions/ axis Set boundary conditions for a zone of this type
/define/boundary-conditions/ copy-bc Copy b.c. to other zones. To copy to all zones of a certain type, use wildcard character * in the name
/define/boundary-conditions/ exhaust-fan Set boundary conditions for a zone of this type
/define/boundary-conditions/ fan Set boundary conditions for a zone of this type
/define/boundary-conditions/ fluid Set boundary conditions for a zone of this type
/define/boundary-conditions/ inlet-vent Set boundary conditions for a zone of this type
/define/boundary-conditions/ intake-fan Set boundary conditions for a zone of this type
/define/boundary-conditions/ interface Set boundary conditions for a zone of this type
/define/boundary-conditions/ interior Set boundary conditions for a zone of this type
/define/boundary-conditions/ list-zones Print out the types and IDs of all zones in the console window. You can use your mouse to check a zone ID
/define/boundary-conditions/ zone Set boundary conditions for a zone
/define/boundary-conditions/ mass-flow-inlet Set boundary conditions for a zone of this type
/define/boundary-conditions/ openchannel-threads List open channel group IDs, names, types and variables
/define/boundary-conditions/ modify-zone/activate-cell-zone Activate cell thread
/define/boundary-conditions/ modify-zone/append-mesh Append new mesh
/define/boundary-conditions/ modify-zone/append-mesh-data Append new mesh with data
/define/boundary-conditions/ modify-zone/deactivate-cell-zone Deactivate cell thread
/define/boundary-conditions/ modify-zone/create-all-shell-threads Create all shells
/define/boundary-conditions/ modify-zone/delete-all-shells Delete all shells
/define/boundary-conditions/ modify-zone/delete-cell-zone Delete a cell thread
/define/boundary-conditions/ modify-zone/extrude-face-zone-delta Extrude a face thread a specified distance based on a list of deltas
/define/boundary-conditions/ modify-zone/extrude-face-zone-para Extrude a face thread a specified distance based on a distance and a list of parametric locations between 0 and 1.0
/define/boundary-conditions/ modify-zone/fuse-face-zones Attempt to fuse zones by removing duplicate faces and nodes
/define/boundary-conditions/ modify-zone/list-zones List zone IDs, types, kinds, and names
/define/boundary-conditions/ modify-zone/make-periodic Attempt to establish periodic/shad flowface zone connectivity
/define/boundary-conditions/ modify-zone/matching-tolerance Set normalized tolerance used for finding coincident nodes
/define/boundary-conditions/ modify-zone/merge-zones Merge zones of same type and condition into one
/define/boundary-conditions/ modify-zone/mrf-to-sliding-mesh Change the motion specification from MRF to moving mesh
/define/boundary-conditions/ modify-zone/orient-face-zone Orient the face zone
/define/boundary-conditions/ modify-zone/repair-face-handedness Reverse orientation of left-handed faces
/define/boundary-conditions/ modify-zone/repair-periodic Modify the mesh to enforce a rotational angle or translational distance for periodic boundaries
/define/boundary-conditions/ modify-zone/replace-zone Replace cell zone
/define/boundary-conditions/ modify-zone/sep-cell-zone-mark Separate cell zone based on cell marking
/define/boundary-conditions/ modify-zone/sep-cell-zone-region Separate cell zone based on contiguous regions
/define/boundary-conditions/ modify-zone/sep-face-zone-angle Separate face zone based on significant angle
/define/boundary-conditions/ modify-zone/sep-face-zone-face Separate each face in zone into unique zone
/define/boundary-conditions/ modify-zone/sep-face-zone-mark Separate face zone based on cell marking
/define/boundary-conditions/ modify-zone/sep-face-zone-region Separate face zone based on contiguous regions
/define/boundary-conditions/ modify-zone/slit-periodic Slit periodic zone into two symmetry zones
/define/boundary-conditions/ modify-zone/slit-face-zone Slit two-sided wall into two connected wall zones
/define/boundary-conditions/ modify-zone/zone-name Give a zone a new name
/define/boundary-conditions/ modify-zone/zone-type Set a zone's type. You will be prompted for the ID of the zone to be changed and the new boundary type for that zone
/define/boundary-conditions/ non-reflecting-bc/general-nrbc/set/sigma Set NRBC sigma factor (default value 0.15)
/define/boundary-conditions/ non-reflecting-bc/general-nrbc/set/sigma2 Set NRBC sigma2 factor (default value 5.0)
/define/boundary-conditions/ non-reflecting-bc/turbo-specific-nrbc/enable? Enable/disable non-reecting b.c.'s
/define/boundary-conditions/ non-reflecting-bc/turbo-specific-nrbc/initialize Initialize non-reecting b.c.'s
/define/boundary-conditions/ non-reflecting-bc/turbo-specific-nrbc/set/discretization Enable use of higher-order reconstruction at boundaries if available
/define/boundary-conditions/ non-reflecting-bc/turbo-specific-nrbc/set/under-relaxation Set non-reecting b.c. under-relaxation factor
/define/boundary-conditions/ non-reflecting-bc/turbo-specific-nrbc/set/verbosity Set non-reecting b.c. verbosity level. 0 : silent, 1 : basic info. (default), 2 : detailed info. for debugging
/define/boundary-conditions/ non-reflecting-bc/turbo-specific-nrbc/show-status Sh flowcurrent status of non-reecting b.c
/define/boundary-conditions/ non-reflecting-bc/outfl flow Set boundary conditions for a zone of this type
/define/boundary-conditions/ non-reflecting-bc/outlet-vent Set boundary conditions for a zone of this type
/define/boundary-conditions/ non-reflecting-bc/periodic Set boundary conditions for a zone of this type
/define/boundary-conditions/ non-reflecting-bc/porous-jump Set boundary conditions for a zone of this type
/define/boundary-conditions/ non-reflecting-bc/pressure-far-field Set boundary conditions for a zone of this type
/define/boundary-conditions/ non-reflecting-bc/pressure-inlet Set boundary conditions for a zone of this type
/define/boundary-conditions/ non-reflecting-bc/pressure-outlet Set boundary conditions for a zone of this type
/define/boundary-conditions/ non-reflecting-bc/radiator Set boundary conditions for a zone of this type
/define/boundary-conditions/ non-reflecting-bc/shad flow Set boundary conditions for a zone of this type
/define/boundary-conditions/ non-reflecting-bc/solid Set boundary conditions for a zone of this type
/define/boundary-conditions/ non-reflecting-bc/symmetry Set boundary conditions for a zone of this type
/define/boundary-conditions/ non-reflecting-bc/target-mass-flow-rate-settings/set-method Select method for setting the mass flow flowrate
/define/boundary-conditions/ non-reflecting-bc/target-mass-flow-rate-settings/verbosity? Enable/disable verbosity when using targeted mass flow flowrate
/define/boundary-conditions/ non-reflecting-bc/velocity-inlet Set boundary conditions for a zone of this type
/define/boundary-conditions/ non-reflecting-bc/wall Set boundary conditions for a zone of this type
/define/boundary-conditions/ non-reflecting-bc/zone-name Give a zone a new name
/define/boundary-conditions/ non-reflecting-bc/zone-type Set a zone's type
/define/boundary-conditions/ custom-field-functions/define Define a custom field function
/define/boundary-conditions/ custom-field-functions/delete Delete a custom field function
/define/boundary-conditions/ custom-field-functions/example-cff-definitions List example custom field functions
/define/boundary-conditions/ custom-field-functions/list-valid-cell-function-names List the names of cell functions that can be used in a custom field function
/define/boundary-conditions/ custom-field-functions/load Load a custom field function
/define/boundary-conditions/ custom-field-functions/save Save a custom field function
/define/boundary-conditions/ dynamic-zones/create Create dynamic zone
/define/boundary-conditions/ delete Delete dynamic zone
/define/boundary-conditions/ insert-boundary-layer Insert new cell zone
/define/boundary-conditions/ insert-interior-layer Insert new layer cell zone at specified location
/define/boundary-conditions/ list List dynamic zones
/define/boundary-conditions/ remove-boundary-layer Remove cell zone
/define/boundary-conditions/ remove-interior-layer Remove interior layer cell zone
/define/boundary-conditions/ mesh-interfaces/create Create a mesh-interface
/define/boundary-conditions/ mesh-interfaces/delete Delete a mesh-interface
/define/boundary-conditions/ mesh-interfaces/draw Draw specified sliding interface zone
/define/boundary-conditions/ mesh-interfaces/list List all mesh-interfaces
/define/boundary-conditions/ mesh-interfaces/make-periodic Make interface zones periodic
/define/boundary-conditions/ mesh-interfaces/recreate Recreate all currently defined mesh interfaces
/define/boundary-conditions/ mesh-interfaces/reset Delete all sliding-interfaces
/define/boundary-conditions/ mesh-interfaces/use-virtual-polygon-approach Use new virtual polygon approach for interfaces
/define/boundary-conditions/ materials/change-create Change the properties of a locally-stored material or create a new material
/define/boundary-conditions/ materials/copy Copy a material from the database
/define/boundary-conditions/ materials/copy-by-formula Copy a material from the database by formula
/define/boundary-conditions/ materials/delete Delete a material from local storage
/define/boundary-conditions/ materials/list-materials List all locally-stored materials
/define/boundary-conditions/ materials/list-properties List the properties of a locally-stored material
/define/boundary-conditions/ materials/data-base/database-type Set the database type
/define/boundary-conditions/ materials/edit Edit material
/define/boundary-conditions/ materials/list-materials List all materials in the database
/define/boundary-conditions/ materials/list-properties List the properties of a material in the database
/define/boundary-conditions/ materials/new Define new material
/define/boundary-conditions/ materials/save Save user-defined database
/define/boundary-conditions/ mixing-planes/create Create a mixing plane
/define/boundary-conditions/ mixing-planes/delete Delete a mixing plane
/define/boundary-conditions/ mixing-planes/list List defined mixing plane(s)
/define/boundary-conditions/ mixing-planes/set/under-relaxation Set mixing plane under-relaxation factor
/define/boundary-conditions/ mixing-planes/set/fix-pressure-level Set fixed pressure level using value based on define/reference-pressure-location
/define/boundary-conditions/ mixing-planes/set/conserve-swirl/enable? Enable/disable swirl conservation in mixing plane
/define/boundary-conditions/ mixing-planes/set/conserve-swirl/verbosity? Enable/disable verbosity in swirl conservation calculations
/define/boundary-conditions/ mixing-planes/set/conserve-swirl/report-swirl-integration Report swirl integration (Torque) on in-flow and out
/define/boundary-conditions/ mixing-planes/set/conserve-total-enthalpy/enable? Enable/disable total enthalpy conservation in mixing plane
/define/boundary-conditions/ mixing-planes/set/conserve-total-enthalpy/verbosity? Enable/disable verbosity in total-enthalpy conservation calculations
/define/boundary-conditions/ models/acoustics/auto-prune Enter the acoustics menu. Enable/disable auto prune of the receiver signal(s) during read- and-compute
/define/boundary-conditions/ models/acoustics/broad-band-noise? Enable/disable the broadband noise model
/define/boundary-conditions/ models/acoustics/compute-write Compute sound pressure
/define/boundary-conditions/ models/acoustics/cylindrical-export? Enable/disable the export of data in cylindrical coordinates
/define/boundary-conditions/ models/acoustics/display-flow-time? Enable/disable the display of flowtime during readand-compute
/define/boundary-conditions/ models/acoustics/export-volumetric-sources? Enable/disable the export of uid zones
/define/boundary-conditions/ models/acoustics/ffowcs-williams? Enable/disable the Ffowcs-Williams-and-Hawkings model
/define/boundary-conditions/ models/acoustics/off? Enable/disable the acoustics model
/define/boundary-conditions/ models/acoustics/read-compute-write Read acoustic source data files and compute sound pressure
/define/boundary-conditions/ models/acoustics/receivers Set acoustic receivers
/define/boundary-conditions/ models/acoustics/sources Set acoustic sources
/define/boundary-conditions/ models/acoustics/write-acoustic-signals Write on-the-y sound pressure
/define/boundary-conditions/ models/acoustics/write-centroid-info Write centroid info
/define/boundary-conditions/ models/dynamic-mesh? Enable/disable the dynamic-mesh solver
/define/boundary-conditions/ models/dynamic-mesh-controls/auto-hide-cells? Enable/disable automatic hiding of skewed cells
/define/boundary-conditions/ models/dynamic-mesh-controls/events/export-event-file Export dynamic mesh events to file
/define/boundary-conditions/ models/dynamic-mesh-controls/events/import-event-file Import dynamic mesh event file
/define/boundary-conditions/ models/dynamic-mesh-controls/in-cylinder-parameter/crank-angle-step Specify crank angle step size
/define/boundary-conditions/ models/dynamic-mesh-controls/in-cylinder-parameter/crank-angle-step/max-crank-angle-step Specify maximum crank angle step size
/define/boundary-conditions/ models/dynamic-mesh-controls/in-cylinder-parameter/crank-angle-step/minimum-lift Specify minimum lift for in-cylinder valves
/define/boundary-conditions/ models/dynamic-mesh-controls/in-cylinder-parameter/crank-angle-step/minimum-stroke Specify cut off point for in-cylinder piston
/define/boundary-conditions/ models/dynamic-mesh-controls/in-cylinder-parameter/crank-angle-step/modify-lift Modify lift curve (shift or scale)
/define/boundary-conditions/ models/dynamic-mesh-controls/in-cylinder-parameter/crank-angle-step/piston-data Specify piston stroke and connecting rod length
/define/boundary-conditions/ models/dynamic-mesh-controls/in-cylinder-parameter/crank-angle-step/position-starting-mesh Move mesh from top dead center to starting crank angle
/define/boundary-conditions/ models/dynamic-mesh-controls/in-cylinder-parameter/crank-angle-step/print-plot-lift Print or plot valve lift curve
/define/boundary-conditions/ models/dynamic-mesh-controls/layering? Enable/disable dynamic-layering in quad/hex cell zones
/define/boundary-conditions/ models/dynamic-mesh-controls/layering-parameter/collapse-factor Set the factor determining when to collapse dynamic layers
/define/boundary-conditions/ models/dynamic-mesh-controls/layering-parameter/constant-height? Enable/disable layering based on constant height,else layering based on constant ratio
/define/boundary-conditions/ models/dynamic-mesh-controls/layering-parameter/split-factor Set the factor determining when to split dynamic layers
/define/boundary-conditions/ models/dynamic-mesh-controls/remeshing? Enable/disable local remeshing in tri/tet and mixed cell zones
/define/boundary-conditions/ models/dynamic-mesh-controls/remeshing-parameter/cell-skew-max Set the cell skewness threshold above which cells will be remeshed
/define/boundary-conditions/ models/dynamic-mesh-controls/remeshing-parameter/face-remeshing? Enable/disable local face remeshing at deforming zones
/define/boundary-conditions/ models/dynamic-mesh-controls/remeshing-parameter/face-skew-max Set the face skewness threshold above which faces will be remeshed
/define/boundary-conditions/ models/dynamic-mesh-controls/remeshing-parameter/length-max Set the length threshold above which cells will be remeshed
/define/boundary-conditions/ models/dynamic-mesh-controls/remeshing-parameter/length-min Set the length threshold bel flowwhich cells will be remeshed
/define/boundary-conditions/ models/dynamic-mesh-controls/remeshing-parameter/must-improve-skewness? Enable/disable cavity replacement only if remeshing improves the skewness
/define/boundary-conditions/ models/dynamic-mesh-controls/remeshing-parameter/size-remesh-interval Set the interval (in time steps) when remeshing based on size is done
/define/boundary-conditions/ models/dynamic-mesh-controls/remeshing-parameter/sizing-funct-defaults Set sizing function defaults
/define/boundary-conditions/ models/dynamic-mesh-controls/remeshing-parameter/sizing-funct-rate Determine h flowfar from the boundary the increase/decrease happens
/define/boundary-conditions/ models/dynamic-mesh-controls/remeshing-parameter/sizing-funct-resolution Set the sizing function resolution with respect to shortest boundary
/define/boundary-conditions/ models/dynamic-mesh-controls/remeshing-parameter/sizing-funct-variation Set the maximum sizing function increase/decrease in the interior
/define/boundary-conditions/ models/dynamic-mesh-controls/remeshing-parameter/sizing-function? Enable/disable sizing function to control size based remeshing
/define/boundary-conditions/ models/dynamic-mesh-controls/six-dof-parameter/motion-history? Enable/disable writing position/orientation of six DOF zones to file
/define/boundary-conditions/ models/dynamic-mesh-controls/six-dof-parameter/x-component Specify x-component of gravity
/define/boundary-conditions/ models/dynamic-mesh-controls/six-dof-parameter/y-component Specify y-component of gravity
/define/boundary-conditions/ models/dynamic-mesh-controls/six-dof-parameter/z-component Specify z-component of gravity
/define/boundary-conditions/ models/dynamic-mesh-controls/smoothing? Enable/disable spring-based smoothing in tri/tet cell zones
/define/boundary-conditions/ models/dynamic-mesh-controls/smoothing-parameter/bnd-node-relaxation Set the spring boundary node relaxation factor
/define/boundary-conditions/ models/dynamic-mesh-controls/smoothing-parameter/bnd-stiffness-factor Set the stiffness factor for springs connected to boundary nodes
/define/boundary-conditions/ models/dynamic-mesh-controls/smoothing-parameter/constant-factor Set the spring constant relaxation factor
/define/boundary-conditions/ models/dynamic-mesh-controls/smoothing-parameter/convergence-tolerance Set the convergence tolerance for springbased solver
/define/boundary-conditions/ models/dynamic-mesh-controls/smoothing-parameter/max-iter Set the maximum number of iterations for spring-based solver
/define/boundary-conditions/ models/dynamic-mesh-controls/smoothing-parameter/skew-smooth-niter Set the number of skewness-based smoothing cycles
/define/boundary-conditions/ models/dynamic-mesh-controls/smoothing-parameter/skew-smooth-skew-max Set the skewness threshold above which cells will be smoothed using skewness method
/define/boundary-conditions/ models/dynamic-mesh-controls/smoothing-parameter/spring-on-all-shapes? Enable/disable spring-based smoothing for all cell shapes
FILE
/file/auto-save/append-file-name-with/case-frequency Specify the frequency (in iterations or time steps) with which data files are saved
/file/auto-save/append-file-name-with/case-frequency/data-frequency Overwrite existing files when files are automatically saved
/file/root-name Specify the root name for the files that are saved
/file/max-files Set the maximum number of files. Once the maximum is reached, files will be erased as new files are written
/file/binary-/files? Indicate whether to write binary or text format case and data files
/file/confirm-overwrite? Confirm attempts to overwrite existing files
/file/define-macro Save input to a named macro
/file/export/abaqus Write an ABAQUS file
/file/export/ansys Write an ANSYS file
/file/export/ansys-input Write an ANSYS Input file
/file/export/ascii Write an ASCII file
/file/export/cgns Write a CGNS file
/file/export/nastran Write a NASTRAN file
/file/export/patran-neutral Write a PATRAN neutral file
/file/export/gambit Write GAMBIT neutral file
/file/export/ensight Write EnSight geometry, velocity, and scalar files
/file/export/fieldview Write FIELDVIEW case and data files
/file/export/fieldview-data Write FIELDVIEW case and data files
/file/export/fieldview-unstruct-mesh Write FIELDVIEW unstructured mesh-only file
/file/export/fieldview-unstruct-data Write FIELDVIEW unstructured results-only file
/file/export/fieldview-unstruct Write FIELDVIEW unstructured combined file
/file/export/execute-macro Run a previously defined macro
/file/import/abaqus/fil Read an ABAQUS .fil result file as a case file
/file/import/abaqus/input Read an ABAQUS input file as a case file
/file/import/ansys/ Import an ANSYS file
/file/import/ansys/input Read an ANSYS file as a case file
/file/import/ansys/result Read an ANSYS result file as a case file
/file/import/cfx/definition Read a CFX definition file as a case file
/file/import/cfx/result Read a CFX definition file as a case file
/file/import/cgns/data/ Read data from CGNS file
/file/import/cgns/mesh Import a CGNS mesh file
/file/import/cgns/mesh-data Import a CGNS mesh file and data file
/file/import/ensight Read an EnSight file as a case file
/file/import/gambit Import a GAMBIT neutral file
/file/import/hypermesh Read a HYPERMESH file as a case file
/file/import/nastran/bulkdata Read a NASTRAN file as a case file
/file/import/nastran/output2 Read a NASTRAN op2 file as a case file
/file/import/neutral Read a PATRAN Neutral file (zones defined by named components) as a case file
/file/import/neutral/result Read a PATRAN result file as a case file
/file/interpolate/ Interpolate data to/from another mesh
/file/read-data Read and interpolate data
/file/write-data Write data for interpolation
/file/read-bc/ Read and set boundary conditions from specified file
/file/read-case Read a case file
/file/read-case-data Read a case and a data file
/file/read-data Read a data file
/file/read-field-functions Read custom field function definitions from a file
/file/read-journal Read command input from a file
/file/read-macros Read macro definitions from a file
/file/read-profile Read boundary profile data
/file/show-configuration Display current release and version information
/file/start-journal Start recording all input in a file
/file/start-transcript Start recording input and output in a file
/file/stop-journal Stop recording input and close journal file
/file/stop-macro Stop recording input to a macro
/file/stop-transcript Stop recording input and output and close transcript file
/file/write-bc Write out current boundary conditions in use
/file/write-boundary-mesh Write the boundary mesh to a file
/file/write-case Write a case file
/file/write-case-data Write a case and a data file
/file/write-cleanup-script Write the cleanup-script-file for FLUENT
/file/write-data Write a data file
/file/write-fan-profile Compute radial profiles for a fan zone and write them to a profile file
/file/write-field-functions Write the currently defined custom field functions to a file
/file/write-macros Write the currently defined macros to a file
/file/write-profile Write surface data as a boundary profile file
DISPLAY
/display/set/windows/aspect-ratio Set the aspect ratio of the active window
/display/set/windows/axes/border? Set whether to draw a border around the axes window
/display/set/windows/axes/bottom Set the bottom boundary of the axes window
/display/set/windows/axes/clear? Set the transparency of the axes window
/display/set/windows/axes/left Set the left boundary of the axes window
/display/set/windows/axes/right Set the right boundary of the axes window
/display/set/windows/axes/top Set the top boundary of the axes window
/display/set/windows/axes/visible? Turn axes visibility on/off
/display/set/windows/main/border? Set whether or not to draw a border around the main viewing window
/display/set/windows/main/bottom Set the bottom boundary of the main viewing window
/display/set/windows/main/left Set the left boundary of the main viewing window
/display/set/windows/main/right Set the right boundary of the main viewing window
/display/set/windows/main/top Set the top boundary of the main viewing window
/display/set/windows/main/visible? Turn visibility of the main viewing wind flowon/off
/display/set/windows/scale/border? Set whether or not to draw a border around the color scale window
/display/set/windows/scale/bottom Set the bottom boundary of the color scale window
/display/set/windows/scale/clear? Set the transparency of the scale window
/display/set/windows/scale/format Set the number format of the color scale window. (e.g., %0.2e)
/display/set/windows/scale/font-size Set the font size of the color scale window
/display/set/windows/scale/left Set the left boundary of the color scale window
/display/set/windows/scale/margin Set the margin of the color scale window
/display/set/windows/scale/right Set the right boundary of the color scale window
/display/set/windows/scale/top Set the top boundary of the color scale window
/display/set/windows/scale/visible? Turn visibility of the color scale wind flowon/off
/display/set/windows/text/application? Show/hide the application name in the picture
/display/set/windows/text/border? Set whether or not to draw a border around the text window
/display/set/windows/text/bottom Set the bottom boundary of the text window
/display/set/windows/text/clear? Enable/disable text wind flowtransparency
/display/set/windows/text/company? Show/hide the company name in the picture
/display/set/windows/text/date? Show/hide the date in the picture
/display/set/windows/text/left Set the left boundary of the text window
/display/set/windows/text/right Set the right boundary of the text window
/display/set/windows/text/top Set the top boundary of the text window
/display/set/windows/text/visible? Turn visibility of the text wind flowon/off
/display/mesh-outline Display the mesh boundaries
/display/mesh-partition-boundary Display mesh partition boundaries
/display/set/colors/list List available colors
/display/set/colors/reset-colors Reset individual mesh surface colors to the defaults
/display/set/color-map/ Enter the color map menu, which contains names of predefined and user-
/display/set/colors/graphics-theme-color white Set the background (window) color to white
/display/set/colors/background/color-by-type? Determine whether to color meshs by type or by ID
/display/set/colors/foreground Set the foreground (text and wind flowframe) color
/display/set/colors/mesh-far Set the color of far field faces
/display/set/colors/mesh-inlet Set the color of inlet faces
/display/set/colors/mesh-interior Set the color of interior faces
/display/set/colors/mesh-internal Set the color of internal interface faces
/display/set/colors/mesh-outlet Set the color of outlet faces
/display/set/colors/mesh-periodic Set the color of periodic faces
/display/set/colors/mesh-symmetry Set the color of symmetric faces
/display/set/colors/mesh-axis Set the color of axisymmetric faces
/display/set/colors/mesh-free-surface Set the color of free-surface faces
/display/set/colors/mesh-traction Set the color of traction faces
/display/set/colors/mesh-wall Set the color of wall faces
/display/set/colors/mesh-interface Set the color of mesh interfaces
/display/set/colorsskip-label Set the number of labels to be skipped in the colopmap scale
/display/set/colorssurface Set the color of surfaces
/display/set/hard-copy/color-mode/color Plot hardcopies in color
/display/set/hard-copy/color-mode/gray-scale Convert color to grayscale for hardcopy
/display/set/hard-copy/color-mode/list Display the current hardcopy color mode
/display/set/hard-copy/color-mode/mono-chrome Convert color to monochrome (black and white) for hardcopy
/display/set/hard-copy/driver/dump-window Set the command used to dump the graphics wind flowto a file
/display/set/hard-copy/driver/eps Produce encapsulated PostScript (EPS) output for hardcopies
/display/set/hard-copy/driver/hpgl Produce HPGL output for hardcopies
/display/set/hard-copy/driver/image Produce SGI IRIS image output for hardcopies
/display/set/hard-copy/driver/jpeg Produce JPEG output for hardcopies
/display/set/hard-copy/driver/list List the current hardcopy driver
/display/set/hard-copy/driver/options Set the hardcopy options
/display/set/hard-copy/driver/png Use PNG output for hardcopies
/display/set/hard-copy/driver/post-format/fast-raster Enter the PostScript driver format menu. Enable a raster file that may be larger than the standard raster file, but will print much more quickly
/display/set/hard-copy/driver/post-format/raster Enable the standard raster file
/display/set/hard-copy/driver/post-format/vector Enable the standard vector file
/display/set/hard-copy/driver/post-script Produce PostScript output for hardcopies
/display/set/hard-copy/driver/ppm Produce PPM output for hardcopies
/display/set/hard-copy/driver/tiff Produce TIFF output for hardcopies
/display/set/hard-copy/driver/vrml Use VRML output for hardcopies
/display/set/hard-copy/invert-background? Exchange foreground/background colors for hardcopy
/display/set/hard-copy/landscape? Plot hardcopies in landscape or portrait orientation
/display/set/hard-copy/preview Apply the settings of the color-mode, invert-background, and landscape options to the currently active graphics wind flowto preview the appearance of printed hardcopies
/display/set/hard-copy/x-resolution Set the width of raster-formatted images in pixels (0 implies current wind flowsize)
/display/set/hard-copy/y-resolution Set the height of raster-formatted images in pixels (0 implies current wind flowsize)
/display/set/contours/ Enter the contour options menu
/display/set/clip-to-range? Turn the clip to range option for filled contours on/off
/display/set/filled-contours? Turn the filled contours option on/off (deselects line-contours?)
/display/set/global-range? Turn the global range for contours on/off
/display/set/line-contours? Turn the line contours option on/off (deselects filled-contours?)
/display/set/log-scale? Specify a decimal or logarithmic color scale for contours
/display/set/n-contour Set the number of contour levels
/display/set/node-values? Set the option to use scalar field at nodes when computing the contours
/display/set/render-mesh? Choose whether to render mesh on top of contours, vectors, etc
/display/set/surfaces Set the surfaces on which contours are drawn
/display/set/velocity-vectors/auto-scale? Auto-scale all vectors so that vector overlap is minimal
/display/set/velocity-vectors/color Set the color of all velocity vectors to the color specified. The color scale is ignored. This is useful when overlaying a vector plot over a contour plot
/display/set/velocity-vectors/color-levels Set the number of colors used from the colormap
/display/set/velocity-vectors/component-x? Set the option to use only the component of the velocity vectors during display
/display/set/velocity-vectors/component-y? Set the option to use only the component of the velocity vectors during display
/display/set/velocity-vectors/component-z? Set the option to use only the component of the velocity vectors during display
/display/set/velocity-vectors/constant-length? Set the option to draw velocity vectors of constant length. This shows only the direction of the velocity vectors
/display/set/velocity-vectors/global-range? Turn global range for vectors on/off
/display/set/velocity-vectors/in-plane? Toggle the display of velocity vector components in the plane of the surface selected for display
/display/set/velocity-vectors/log-scale? Toggle whether color scale is logarithmic or linear
/display/set/velocity-vectors/node-values? Enable/disable the plotting of node values. Cell values will be plotted if "no"
/display/set/velocity-vectors/relative? Toggle the display of relative velocity vectors
/display/set/velocity-vectors/render-mesh? Choose whether to render mesh on top of contours, vectors, etc
/display/set/velocity-vectors/scale Set the value by which the vector length will be scaled
/display/set/velocity-vectors/scale-head Set the value by which the vector head will be scaled
/display/set/velocity-vectors/surfaces Set surfaces on which vectors are drawn
MESH
/mesh/check Perform various mesh consistency checks
/mesh/mesh-info Print zone information size
/mesh/make-hanging-interface Create hanging interface between quad and tri zones
/mesh/memory-usage Report solver memory use
/mesh/modify-zones/ Enter the zone modi cation menu
/mesh/polyhedra/convert-domain Convert entire domain to polyhedra cells
/mesh/polyhedra/convert-skewed-cells Convert skewed cells to polyhedra
/mesh/polyhedra/options/parallel-migration-by-file Enable cell migration by file input/output during convert-domain
/mesh/quality Analyze the quality of the mesh
/mesh/reorder/band-width Print cell bandwidth
/mesh/reorder/reorder-domain Reorder cells and faces by reverse Cuthill-McKee algorithm
/mesh/reorder/reorder-zones Reorder zones by partition, type, and ID
/mesh/rotate Rotate the mesh
/mesh/scale Prompt for the scaling factors in each of the active Cartesian coordinate directions
/mesh/size-info Print mesh size
/mesh/smooth-mesh Smooth the mesh using Laplace or skewness methods
/mesh/surface-mesh/delete Delete surface mesh
/mesh/surface-mesh/display Display surface meshes
/mesh/surface-mesh/read Read surface meshes
/mesh/swap-mesh-faces Swap mesh faces
/mesh/translate Prompt for the translation o set in each of the active Cartesian coordinate directions
PLOT
/plot/circum-avg-axial Compute iso-axial band surfaces and plot data vs. axial coordinate on them
/plot/circum-avg-radial Compute iso-radial band surfaces and plot data vs. radius on them
/plot/fft Plot FFT of file data
/plot/change-fft-ref-pressure Change reference acoustic pressure
/plot/file Plot data from an external file
/plot/file-list Plot data from multiple external files
/plot/file-set/auto-scale? Set the range for the x and y axes. If auto-scaling is not activated for a particular axis, you are prompted for the minimum and maximum data values
/plot/file-set/background-color Set the color of the eld within the abscissa and ordinate axes
/plot/file-set/key Enable/disable display of curve key and set its wind flowtitle
/plot/file-set/labels Set labels for plot axes
/plot/file-set/lines Set parameters for plot lines
/plot/file-set/log? Use log scales for one or both axes
/plot/file-set/markers Set parameters for data markers
/plot/file-set/numbers Set number formats for axes
/plot/file-set/plot-to-file Specify a file in which to write XY plot data
/plot/file-set/rules Set parameters for display of major and minor rules
/plot/file-set/windows/ XY plot wind flowoptions. For a description of the items in this menu, see display/set/windows/xy
/plot/flamelet-curves/write-to-file? Write curve to a file instead of plot
/plot/flamelet-curves/plot-curves Plot of a curve property
/plot/flamelet-curves/histogram Plot a histogram of the speci ed solution variable using the defined range and number of intervals
/plot/flamelet-curves/histogram-set/auto-scale? Set the range for the x and y axes. If auto-scaling is not activated for a particular axis, you are prompted for the minimum and maximum data values
/plot/flamelet-curves/histogram-set/background-color Set the color of the eld within the abscissa and ordinate axes
/plot/flamelet-curves/histogram-set/key Enable/disable display of curve key and set its wind flowtitle
/plot/flamelet-curves/histogram-set/labels Set labels for plot axes
/plot/flamelet-curves/histogram-set/lines Set parameters for plot lines
/plot/flamelet-curves/histogram-set/log Use log scales for one or both axes
/plot/flamelet-curves/histogram-set/markers Set parameters for data markers
/plot/flamelet-curves/histogram-set/numbers Set number formats for axes
/plot/flamelet-curves/histogram-set/plot-to-file Specify a file in which to write XY plot data
/plot/flamelet-curves/histogram-set/rules Set parameters for display of major and minor rules
/plot/flamelet-curves/histogram-set/windows XY plot wind flowoptions. For a description of the items in this menu, see display/set/windows/xy
/plot/flamelet-curves/plot Plot solution on surfaces
/plot/flamelet-curves/plot-direction Set plot direction for XY plot
/plot/flamelet-curves/residuals Contains commands that all flowyou to select the variables for which you want to display XY plots of residual histories in the active graphics window
/plot/flamelet-curves/residual-set/auto-scale? "Set residual plot parameters. Sub-menu items are the same as file-set/ above."
/plot/flamelet-curves/residual-set/background-color Set the range for the x and y axes. If auto-scaling is not activated for a particular axis, you are prompted for the minimum and maximum data values
/plot/flamelet-curves/residual-set/key Set the color of the eld within the abscissa and ordinate axes
/plot/flamelet-curves/residual-set/labels Enable/disable display of curve key and set its wind flowtitle
/plot/flamelet-curves/residual-set/lines Set labels for plot axes
/plot/flamelet-curves/residual-set/log Set parameters for plot lines
/plot/flamelet-curves/residual-set/markers Use log scales for one or both axes
/plot/flamelet-curves/residual-set/numbers Set parameters for data markers
/plot/flamelet-curves/residual-set/plot-to-file Set number formats for axes
/plot/flamelet-curves/residual-set/rules Specify a file in which to write XY plot data
/plot/flamelet-curves/residual-set/windows Set parameters for display of major and minor rules
/plot/flamelet-curves/solution XY plot wind flowoptions. For a description of the items in this menu, see display/set/windows/xy
/plot/flamelet-curves/solution-set/auto-scale? Set the range for the x and y axes. If auto-scaling is not activated for a particular axis, you are prompted for the minimum and maximum data values
/plot/flamelet-curves/solution-set/background-color Set the color of the eld within the abscissa and ordinate axes
/plot/flamelet-curves/solution-set/key Enable/disable display of curve key and set its wind flowtitle
/plot/flamelet-curves/solution-set/labels Set labels for plot axes
/plot/flamelet-curves/solution-set/lines Set parameters for plot lines
/plot/flamelet-curves/solution-set/log Use log scales for one or both axes
/plot/flamelet-curves/solution-set/markers Set parameters for data markers
/plot/flamelet-curves/solution-set/numbers Set number formats for axes
/plot/flamelet-curves/solution-set/plot-to-file Specify a file in which to write XY plot data
/plot/flamelet-curves/solution-set/rules Set parameters for display of major and minor rules
/plot/flamelet-curves/solution-set/windows XY plot wind flowoptions. For a description of the items in this menu, see display/set/windows/xy
REPORT
/report/dpm-sample Sample trajectories at boundaries and lines/planes
/report/dpm-summary Print discrete phase summary report
/report/fluxes/heat-transfer Print heat transfer rate at boundaries
/report/fluxes/mass-flow Print mass flow rate at inlets and outlets
/report/fluxes/rad-heat-trans Print radiation heat transfer rate at boundaries
/report/forces/pressure-center Print the center of pressure on wall zones
/report/forces/wall-forces Compute the forces along the speci ed force vector for all wall zones
/report/forces/wall-moments Compute the moments about the specified moment center for all wall zones
/report/particle-summary Print summary report for all current particles
/report/path-line-summary Print pathline summary report
/report/print-histogram Print a histogram of a scalar quantity
/report/projected-surface-area Compute the area of the projection of selected surfaces along the x, y or z axis
/report/reference-values/area Set reference area for normalization
/report/reference-values/compute/ Compute reference values from zone boundary conditions
/report/reference-values/density Set reference density for normalization
/report/reference-values/depth Set reference depth for volume calculation
/report/reference-values/enthalpy Set reference enthalpy for enthalpy damping and normalization
/report/reference-values/length Set reference length for normalization
/report/reference-values/list List current reference values
/report/reference-values/pressure Set reference pressure for normalization
/report/reference-values/temperature Set reference temperature for normalization
/report/reference-values/velocity Set reference velocity for normalization
/report/reference-values/viscosity Set reference viscosity for normalization
/report/reference-values/zone Set reference zone
/report/species-mass-flow Print list of species mass fl flowrate at inlets and outlets
/report/summary Print the current settings for physical models, boundary conditions, material properties, and solution parameters
/report/surface-integrals/area Print the area of the selected surfaces
/report/surface-integrals/area-weighted-average Print area-weighted average of the specified quantity over the selected surfaces
/report/surface-integrals/facet-avg Print the facet average of the specified quantity over the selected surfaces
/report/surface-integrals/facet-max Print the maximum of the specified quantity over facet centroids of the selected surfaces
/report/surface-integrals/facet-min Print the minimum of the speci ed quantity over facet centroids of the selected surfaces
/report/surface-integrals/flow-rate Print the flow rate of the specified quantity over the selected surfaces
/report/surface-integrals/integral Print the integral of the specified quantity over the selected surfaces
/report/surface-integrals/mass-flow-rate Print the mass flow rate through the selected surfaces
/report/surface-integrals/mass-weighted-avg Print the mass-averaged quantity over the selected surfaces
/report/surface-integrals/standard-deviation Print the standard deviation of the scalar at the facet centroids of the surface
/report/surface-integrals/sum Print sum of scalar at facet centroids of the surfaces
/report/surface-integrals/vertex-avg Print the vertex average of the specified quantity over the selected surfaces
/report/surface-integrals/vertex-max Print the maximum of the specified quantity over vertices of the selected surfaces
/report/surface-integrals/vertex-min Print the minimum of the specified quantity over vertices of the selected surfaces
/report/surface-integrals/volume-flow-rate Print the volume fl flowrate through the selected surfaces
/report/uds-flow Print list of user-defined scalar flow rate at boundaries
/report/volume-integrals/mass-avg Print mass-average of scalar over cell zones
/report/volume-integrals/mass-integral Print mass-weighted integral of scalar over cell zones
/report/volume-integrals/maximum Print maximum of scalar over all cell zones
/report/volume-integrals/minimum Print minimum of scalar over all cell zones
/report/volume-integrals/sum Print sum of scalar over all cell zones
/report/volume-integrals/vol-avg Print volume-weighted average of scalar over cell zones
/report/volume-integrals/vol-integral Print integral of scalar over cell zones
/report/volume-integrals/volume Print total volume of specified cell zones
SOLVE
/solve/animate/define/define-monitor Define new animation
/solve/animate/define/edit-monitor Change animation monitor attributes
/solve/animate/playback/delete Delete animation sequence
/solve/animate/playback/play Play the selected animation
/solve/animate/playback/read Read new animation from le or already-defined animations
/solve/animate/playback/write Write animation sequence to the file
/solve/dpm-update Update discrete phase source terms
/solve/dual-time-iterate Perform unsteady iterations for a specified number of time steps
/solve/execute-commands/add-edit Add or edit execute commands
/solve/execute-commands/disable Disable an execute command
/solve/execute-commands/enable Enable an execute command
/solve/initialize/compute-defaults/ Enter the compute default values menu. You can select the type of zone from which you want to compute these values
/solve/initialize/dpm-reset Reset discrete phase source terms to zero
/solve/initialize/fmg-initialization Initialize using the full-multimesh initialization (FMG)
/solve/execute-commands/initialize/init-flow-statistics Initialize unsteady statistics
/solve/initialize/initialize-flow Initialize the flow field with the current default values
/solve/initialize/init-instantaneous-vel Initialize unsteady velocity
/solve/initialize/list-defaults List default values
/solve/initialize/repair-wall-distance Correct wall distance at very high aspect ratio hexahedral / polyhedral cells
/solve/initialize/set-defaults/ Set default initial values
/solve/initialize/set-fmg-initialization/ Enter the set full-multimesh for initialization menu. Initial values for each variable can be set within this menu
/solve/iterate Perform a specified number of iterations
/solve/mesh-motion Perform mesh motion
/solve/monitors/force/clear-all-monitors-data Discard the internal and external file data associated with the force monitors
/solve/monitors/force/clear-drag-monitor-data Discard the internal and external file data (if any exist) for the drag coefficient
/solve/monitors/force/clear-lift-monitor-data Discard the internal and external le data (if any exist) for the lift coefficient
/solve/monitors/force/clear-moment-monitor-data Discard the internal and external file data (if any exist) for the moment cofficient
/solve/monitors/force/drag-coefficient Set the parameters for monitoring the drag coeffiient
/solve/monitors/force/lift-coefficient Set the parameters for monitoring the lift coeffcient
/solve/monitors/force/moment-coefficient Set the parameters for monitoring the moment coefficient
/solve/monitors/force/monitor-unsteady-iters? Specify (for transient calculations) whether the monitors are updated every iteration or every time step
/solve/residual/check-convergence? Choose which currently-monitored residuals should be checked for convergence
/solve/residual/convergence-criteria Set convergence criteria for residuals that are currently being both monitored and checked
/solve/residual/criterion-type Set convergence criterion type
/solve/residual/monitor? Choose which residuals to monitor as printed and/or plotted output
/solve/residual/n-display Set the number of most recent residuals to display in plots
/solve/residual/n-maximize-norms Set the number of iterations through which normalization factors will be maximized
/solve/residual/normalization-factors Set normalization factors for currently-monitored residuals (if normalize? is set to yes)
/solve/residual/normalize? Choose whether to normalize residuals in printed and plotted output
/solve/residual/n-save Set number of residuals to be saved with data. History is automatically compacted when buffer becomes full
/solve/residual/plot? Choose whether residuals will be plotted during iteration
/solve/residual/print? Choose whether residuals will be printed during iteration
/solve/residual/relative-conv-criteria Set relative convergence criteria for residuals that are currently being both monitored and checked
/solve/residual/re-normalize Re-normalize residuals by maximum values
/solve/residual/reset? Choose whether to delete the residual history and reset iteration counter to 1
/solve/residual/scale-by-coefficient? Choose whether to scale residuals by coe cient sum in printed and plotted output
/solve/residual/window Specify wind flow in which residuals will be plotted during iteration
/solve/statistic/monitors Choose which statistics to monitor as printed and/or plotted output
/solve/statistic/plot? Choose whether or not statistics will be plotted during iteration
/solve/statistic/print? Choose whether or not statistics will be printed during iteration
/solve/statistic/window Specify first wind flow in which statistics will be plotted during iteration. Multiple statistics are plotted in separate windows, beginning with this one
/solve/surface/clear-data Clear current surface monitor data
/solve/surface/clear-monitors Remove all defined surface monitors
/solve/surface/curves/lines Set lines parameters for surface monitors
/solve/surface/curves/markers Set markers parameters for surface monitors
/solve/surface/list-monitors List defined surface monitors
/solve/surface/set-monitor Define or modify a surface monitor
/solve/volume/clear-data Clear current volume monitor data
/solve/volume/clear-monitors Remove all defined volume monitors
/solve/volume/list-monitors List defined volume monitors
/solve/volume/set-monitor Define or modify a volume monitor
/solve/particle-history/export-particle-data Export particle history data
/solve/particle-history/import-particle-data Import particle history data
/solve/patch Patch a value for a flow variable in the domain
/solve/set/adaptive-time-stepping Set adaptive time stepping parameters
/solve/set/bc-pressure-extrapolations Set pressure extrapolations schemes on boundaries
/solve/set/correction-tolerance/ Enter the correction tolerance menu
/solve/set/courant-number Set the fine-mesh Courant number (time step factor). This command is available only for the coupled solvers
/solve/set/data-sampling Enable data sampling for unsteady flow statistics
/solve/set/disable-reconstruction? Completely disables reconstruction, resulting in totally first-order accuracy
/solve/set/discretization-scheme/pressure Select which Pressure model is to be used. Five models are available: 10-Standard, 11-Linear, 12-2nd Order, 13-Body-Force Weighted, 14-PRESTO!
/solve/set/discretization-scheme/flow Select which Pressure model is to be used. Five models are available: 20-SIMPLE, 21-SIMPLEC, 22-PISO
/solve/set/discretization-scheme/mom Select which Momentum model is to be used. 0: !st Order UDS, 1: 2nd Order UDS, 2: Power Law, 4: QUICK
/solve/set/equations/ Select the equations to be solved
/solve/set/expert Set expert options
/solve/set/flow-warnings? Specify whether or not to print warning messages when reversed flow occurs at inlets and outlets and when mass flow inlets develop supersonic regions. By default, flow warnings are printed
/solve/set/flux-type Set the flux type
/solve/set/gradient-scheme Set gradient options
/solve/set/limiter-warnings? Specify whether or not to print warning messages when quantities are being limited. By default, limiter warnings are printed
/solve/set/limits Set solver limits for various solution variables, in order to improve the stability of the solution
/solve/set/max-corrections/ Enter the set max-corrections menu
/solve/set/multi-mesh-amg Set the parameters that govern the algebraic multimesh procedure
/solve/set/multi-mesh-controls/ Set multimesh parameters and termination criteria
/solve/set/multi-mesh-fas Set the parameters that control the FAS multimesh solver. This command appears only when the explicit coupled solver is used
/solve/set/multi-stage Set the multi-stage coefficients and the dissipation and viscous evaluation stages. This command appears only when the explicit coupled solveris used
/solve/set/numerics Set numerics options
/solve/set/predict-next-time? Applies a predictor algorithm for computing
/solve/set/p-v-controls Set pressure-velocity controls
/solve/set/p-v-coupling Select the pressure-velocity coupling scheme
/solve/set/reactions? Enable the species reaction sources and set relaxation factor
/solve/set/relaxation-factor Enter the relaxation-factor menu
/solve/set/relaxation-method Set the solver relaxation method
/solve/set/reporting-interval Set the number of iterations for which convergence monitors are reported. The default is 1 (after every iteration)
/solve/set/residual-smoothing Set the implicit residual smoothing parameters. This command is available only for the explicit coupled solver
/solve/set/residual-tolerance/ Enter the residual tolerance menu
/solve/set/residual-verbosity Set the amount of residual information to be printed. 0 (the default) prints residuals at the end of each fine mesh iteration
/solve/set/set-controls-to-default Set controls to default values
/solve/set/slope-limiter-set/ Select a new Fluent solver slope limiter
/solve/set/stiff-chemistry Set solver options for sti chemistry solutions
/solve/set/surface-tension Set surface-tension calculation options
/solve/set/time-step Set the magnitude of the (physical) time step fit
/solve/set/under-relaxation/ Set the under-relaxation factor for each equation that is being solved in a segregated manner
/solve/set/variable-time-stepping Set variable time-stepping options for VOF explicit schemes
/solve/update-physical-time Advance the unsteady solution to the next physical time level manully rather than doing it automatically with the dual-time-iterate command
SURFACE
/surface/circle-slice Extract a circular slice
/surface/delete-surface Remove a defined data surface
/surface/iso-clip Clip a data surface (surface, curve, or point) between two isovalues
/surface/iso-surface Extract an iso-surface (surface, curve, or point) from the current data field
/surface/line-slice Extract a linear slice in 2D, given the normal to the line and a distance from the origin
/surface/line-surface Define a "line" surface by specifying the two endpoint coordinates
/surface/list-surfaces Display the ID and name, and the number of point, curve, and surface facets of the current surfaces
/surface/mouse-line Extract a line surface that you define by using the mouse to select the endpoints
/surface/mouse-plane Extract a planar surface defined by selecting three points with the mouse
/surface/mouse-rake Extract a "rake" surface that you define by using the mouse to select the endpoints
/surface/partition-surface Define a data surface consisting of mesh faces on the partition boundary
/surface/plane Create a plane given 3 points bounded by the domain
/surface/plane-bounded Create a bounded surface
/surface/plane-point-n-normal Create a plane from a point and normal
/surface/plane-slice Extract a planar slice
/surface/plane-surf-aligned Create a plane aligned to a surface
/surface/plane-view-plane-align Create a plane aligned to a view-plane
/surface/point-array Extract a rectangular array of data points
/surface/point-surface Define a "point" surface by specifying the coordinates
/surface/rake-surface Extract a "rake" surface, given the coordinates of the endpoints
/surface/rename-surface Rename a defined data surface
/surface/sphere-slice Extract a spherical slice
/surface/surface-cells Extract all cells intersected by a data surface
/surface/transform-surface Transform surface
/surface/zone-surface Create a surface of a designated zone and gives it a specified name
VIEW
/view/auto-scale Scale and center the current scene without changing its orientation
/view/camera/dolly-camera Adjust the camera position and target
/view/camera/field Set the field of view (width and height)
/view/camera/orbit-camera Adjust the camera position without modifying the target
/view/camera/pan-camera Adjust the camera target without modifying the position
/view/camera/position Set the camera position
/view/camera/projection Toggles between perspective and orthographic views
/view/camera/roll-camera Adjust the camera up-vector
/view/camera/target Set the point to be the center of the camera view
/view/camera/up-vector Set the camera up-vector
/view/camera/zoom-camera Adjust the camera's field of view
/view/default-view Reset view to front and center
/view/delete-view Remove a view from the list
/view/last-view Return to camera position before last manipulation
/view/list-views List predefined and saved views
/view/read-views Read views from a view file
/view/restore-view Use a saved view
/view/save-view Save the current view to the view list
/view/write-views Write selected views to a view file
Contact us
Disclaimers and Policies

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.