• 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

The sign convention for mass flow is such that a positive value represents flow into the domain and a negative value represents flow out of the domain. Sometimes an 'outlet' can be specified as inlet with negative velocity to represent some specified mass flow rate.

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.

    Contact Resistance Heat Transfer Path

    Some typical value of thermal conductance when air gaps are not evaluated are tabulated below (reference: A Textbook fo Heat Transfer by Lienhard IV and Lienhard V) -
    Surface Pair Thermal Conductance [W/m2K]
    Copper - Copper 10,000 ~ 25,000
    Aluminium - Aluminium 2,200 ~ 12,000
    Ceramic - Metals 1,500 ~ 8,500
    Stainless steel - Stainless steel 2,000 ~ 3,7000
    Ceramic - Ceramic 500 ~ 3,000
    Thus, for a ceramic - aluminium pair (such as in electronic chips) with contact surface area of 20 [mm] x 20 [mm], the thermal contact resistance would be in the range 1.67 ~ 0.30 [K/W]. Note that contact resistance is also a function of contact area, higher the surface area lesser ther contact resistance in [K/W]. For a ceramic - ceramic pair having contact surface area of 10 [mm] x 10 [mm], the thermal contact resistance would be in the range 20.0 ~ 3.33 [K/W].
  • 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. In FLUENT, a zero thickness plane can be used to represent a fan. However, in CFX a volume is required to represent fan as momentum source coefficient. The general momentum source in CFX has unit of [kg/m3-s2]. The source can be linearlized for better convergence and stability which has unit of [kg/m3-s].

  • 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. There is no similar boundary conditions available in CFX.

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

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 and CFX, 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 the unit of permeability (α) is [m2]. Other unit of measurement is the darcy [1 darcy = 0.987 μm2], named after the French scientist who discovered the phenomenon. The unit of inertial loss coefficient (C2) is [m-1]. Inertial loss coefficient is known as Quadratic Loss Coefficient in CFX. An alternate formulation in CFX is in terms of Linear Loss Coefficient [kg/m3-s] and Quadratic Loss Coefficients [kg/m4] which are defined as A and B respectively above or Pv and Pi below.

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. All the programs FLUENT, CFX and STAR-CCM+ uses superficial velocity.

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' vs. v curve].
  3. Calculate the quadratic polynomial curve fit coefficients [A, B] from the curve Δp' vs. -v. Ensure that the intercept to the y-axis is zero.
  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:  

Porous Loss Coefficient Calculator

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

Thickness of HX - t [mm]:  
First point - V1 [m/s]:  
First point - P1 [Pa]:  
Second point - V2 [m/s]:  
Second point - P2 [Pa]:  
Third point - V3 [m/s]:  
Third point - P3 [Pa]:  
Gas Temperature - Tg [°C]:  
Gas Pressure - Pg [kPa]:  

Example calculation: x = {0.0   1.0   2.5}, Y = {0   50   75}, m1 = 50.0, m2 = 16.67, A = -13.33, B = 63.33, C = 0.0. The parabola generated by the curve fit coefficients looks like as shown below. Note that a parabola with local maxima towards higher value of X-axis may have a negative value of A or B.

Parabola through 3 points

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

Parabola through 3 points coefficients


Examples of Porous Media
One of the frequent application of porous media formulation is the heat exchangers such as automotive radiators, inter-coolers, oil-cooler and honeycombs in catalytic converters. The porous formulations can also be used in Fabric Ducts used in HVAC systems. These ducts an either be "permeable only textile fabric where air is squeezed between loose fibres" or ducts with micro-perforations with laser cut holes as low as 0.2 [mm]. Micro-perforations allow creation of variety of low velocity air patterns to suit local cooling needs. In porous fabric ducts, air is allowed to pass through the fabric with the air-flow rate controlled by the fabric weave and the internal static pressure. In non-porous fabric, no air can pass through the fabric weave and air-flow is delivered through orifices and other venting options (nozzles, micro-perforations) to achieve desired air-flow.

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

Fabric Ducts Textile Ventilation


Atmospheric Data
Reference: Analytic Combustion by 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 b-c axis Set boundary conditions (b-c) for a zone of this type
define b-c copy-bc Copy b.c. to other zones. To copy to all zones of a certain type, use wildcard character * in the name
define b-c exhaust-fan Set boundary conditions for a zone of this type
define b-c fan Set boundary conditions for a zone of this type
define b-c fluid Set boundary conditions for a zone of this type
define b-c inlet-vent Set boundary conditions for a zone of this type
define b-c intake-fan Set boundary conditions for a zone of this type
define b-c interface Set boundary conditions for a zone of this type
define b-c interior Set boundary conditions for a zone of this type
define b-c 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 b-c zone Set boundary conditions for a zone
define b-c mass-flow-inlet Set boundary conditions for a zone of this type
define b-c openchannel-threads List open channel group IDs, names, types and variables
define b-c modify-zone activate-cell-zone Activate cell thread
define b-c modify-zone append-mesh Append new mesh
define b-c modify-zone append-mesh-data Append new mesh with data
define b-c modify-zone deactivate-cell-zone Deactivate cell thread
define b-c modify-zone create-all-shell-threads Create all shells
define b-c modify-zone delete-all-shells Delete all shells
define b-c modify-zone delete-cell-zone Delete a cell thread
define b-c modify-zone extrude-face-zone-delta Extrude a face thread a specified distance based on a list of deltas
define b-c 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 b-c modify-zone fuse-face-zones Attempt to fuse zones by removing duplicate faces and nodes
define b-c modify-zone list-zones List zone IDs, types, kinds, and names
define b-c modify-zone make-periodic Attempt to establish periodic/shad flowface zone connectivity
define b-c modify-zone matching-tolerance Set normalized tolerance used for finding coincident nodes
define b-c modify-zone merge-zones Merge zones of same type and condition into one
define b-c modify-zone mrf-to-sliding-mesh Change the motion specification from MRF to moving mesh
define b-c modify-zone orient-face-zone Orient the face zone
define b-c modify-zone repair-face-handedness Reverse orientation of left-handed faces
define b-c modify-zone repair-periodic Modify the mesh to enforce a rotational angle or translational distance for periodic boundaries
define b-c modify-zone replace-zone Replace cell zone
define b-c modify-zone sep-cell-zone-mark Separate cell zone based on cell marking
define b-c modify-zone sep-cell-zone-region Separate cell zone based on contiguous regions
define b-c modify-zone sep-face-zone-angle Separate face zone based on significant angle
define b-c modify-zone sep-face-zone-face Separate each face in zone into unique zone
define b-c modify-zone sep-face-zone-mark Separate face zone based on cell marking
define b-c modify-zone sep-face-zone-region Separate face zone based on contiguous regions
define b-c modify-zone slit-periodic Slit periodic zone into two symmetry zones
define b-c modify-zone slit-face-zone Slit two-sided wall into two connected wall zones
define b-c modify-zone zone-name Give a zone a new name
define b-c 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 b-c n-r-bc general-nrbc set sigma Set NRBC sigma factor (default value 0.15)
define b-c n-r-bc general-nrbc set sigma2 Set NRBC sigma2 factor (default value 5.0)
define b-c n-r-bc turbo-specific-nrbc enable? Enable/disable non-reecting b.c.'s
define b-c n-r-bc turbo-specific-nrbc initialize Initialize non-reecting b.c.'s
define b-c n-r-bc turbo-specific-nrbc set discretization Enable use of higher-order reconstruction at boundaries if available
define b-c n-r-bc turbo-specific-nrbc set under-relaxation Set non-reecting b.c. under-relaxation factor
define b-c n-r-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 b-c n-r-bc turbo-specific-nrbc show-status Sh flowcurrent status of non-reecting b.c
define b-c n-r-bc outfl flow Set boundary conditions for a zone of this type
define b-c n-r-bc outlet-vent Set boundary conditions for a zone of this type
define b-c n-r-bc periodic Set boundary conditions for a zone of this type
define b-c n-r-bc porous-jump Set boundary conditions for a zone of this type
define b-c n-r-bc pressure-far-field Set boundary conditions for a zone of this type
define b-c n-r-bc pressure-inlet Set boundary conditions for a zone of this type
define b-c n-r-bc pressure-outlet Set boundary conditions for a zone of this type
define b-c n-r-bc radiator Set boundary conditions for a zone of this type
define b-c n-r-bc solid Set boundary conditions for a zone of this type
define b-c n-r-bc symmetry Set boundary conditions for a zone of this type
define b-c n-r-bc target-mass-flow-rate-settings/ set-method Select method for setting the mass flow flowrate
define b-c n-r-bc target-mass-flow-rate-settings/ verbosity? Enable/disable verbosity when using targeted mass flow flowrate
define b-c n-r-bc velocity-inlet Set boundary conditions for a zone of this type
define b-c n-r-bc wall Set boundary conditions for a zone of this type
define b-c n-r-bc zone-name Give a zone a new name
define b-c n-r-bc zone-type Set a zone's type
define b-c custom-field-functions/ define Define a custom field function
define b-c custom-field-functions/ delete Delete a custom field function
define b-c custom-field-functions/ example-cff-definitions List example custom field functions
define b-c custom-field-functions/ list-valid-cell-function-names List the names of cell functions that can be used in a custom field function
define b-c custom-field-functions/ load Load a custom field function
define b-c custom-field-functions/ save Save a custom field function
define b-c dynamic-zones/ create Create dynamic zone
define b-c delete Delete dynamic zone
define b-c insert-boundary-layer Insert new cell zone
define b-c insert-interior-layer Insert new layer cell zone at specified location
define b-c list List dynamic zones
define b-c remove-boundary-layer Remove cell zone
define b-c remove-interior-layer Remove interior layer cell zone
define b-c mesh-interfaces create Create a mesh-interface
define b-c mesh-interfaces delete Delete a mesh-interface
define b-c mesh-interfaces draw Draw specified sliding interface zone
define b-c mesh-interfaces list List all mesh-interfaces
define b-c mesh-interfaces make-periodic Make interface zones periodic
define b-c mesh-interfaces recreate Recreate all currently defined mesh interfaces
define b-c mesh-interfaces reset Delete all sliding-interfaces
define b-c mesh-interfaces use-virtual-polygon-approach Use new virtual polygon approach for interfaces
define b-c materials change-create Change the properties of a locally-stored material or create a new material
define b-c materials copy Copy a material from the database
define b-c materials copy-by-formula Copy a material from the database by formula
define b-c materials delete Delete a material from local storage
define b-c materials list-materials List all locally-stored materials
define b-c materials list-properties List the properties of a locally-stored material
define b-c materials data-base/ database-type Set the database type
define b-c materials edit Edit material
define b-c materials list-materials List all materials in the database
define b-c materials list-properties List the properties of a material in the database
define b-c materials new Define new material
define b-c materials save Save user-defined database
define b-c mixing-planes create Create a mixing plane
define b-c mixing-planes delete Delete a mixing plane
define b-c mixing-planes list List defined mixing plane(s)
define b-c mixing-planes set under-relaxation Set mixing plane under-relaxation factor
define b-c mixing-planes set fix-pressure-level Set fixed pressure level using value based on define/reference-pressure-location
define b-c mixing-planes set conserve-swirl enable? Enable/disable swirl conservation in mixing plane
define b-c mixing-planes set conserve-swirl verbosity? Enable/disable verbosity in swirl conservation calculations
define b-c mixing-planes set conserve-swirl report-swirl-integration Report swirl integration (Torque) on in-flow and out
define b-c mixing-planes set conserve-total-enthalpy enable? Enable/disable total enthalpy conservation in mixing plane
define b-c mixing-planes set conserve-total-enthalpy verbosity? Enable/disable verbosity in total-enthalpy conservation calculations
define b-c models acoustics auto-prune Enter the acoustics menu. Enable/disable auto prune of the receiver signal(s) during read- and-compute
define b-c models acoustics broad-band-noise? Enable/disable the broadband noise model
define b-c models acoustics compute-write Compute sound pressure
define b-c models acoustics cylindrical-export? Enable/disable the export of data in cylindrical coordinates
define b-c models acoustics display-flow-time? Enable/disable the display of flowtime during readand-compute
define b-c models acoustics export-volumetric-sources? Enable/disable the export of uid zones
define b-c models acoustics ffowcs-williams? Enable/disable the Ffowcs-Williams-and-Hawkings model
define b-c models acoustics off? Enable/disable the acoustics model
define b-c models acoustics read-compute-write Read acoustic source data files and compute sound pressure
define b-c models acoustics receivers Set acoustic receivers
define b-c models acoustics sources Set acoustic sources
define b-c models acoustics write-acoustic-signals Write on-the-y sound pressure
define b-c models acoustics write-centroid-info Write centroid info
define b-c models dynamic-mesh? Enable/disable the dynamic-mesh solver
define b-c models dynamic-mesh-controls auto-hide-cells? Enable/disable automatic hiding of skewed cells
define b-c models dynamic-mesh-controls events/ export-event-file Export dynamic mesh events to file
define b-c models dynamic-mesh-controls events/ import-event-file Import dynamic mesh event file
define b-c models dynamic-mesh-controls in-cylinder-parameter crank-angle-step Specify crank angle step size
define b-c models dynamic-mesh-controls in-cylinder-parameter crank-angle-step max-crank-angle-step Specify maximum crank angle step size
define b-c models dynamic-mesh-controls in-cylinder-parameter crank-angle-step minimum-lift Specify minimum lift for in-cylinder valves
define b-c models dynamic-mesh-controls in-cylinder-parameter crank-angle-step minimum-stroke Specify cut off point for in-cylinder piston
define b-c models dynamic-mesh-controls in-cylinder-parameter crank-angle-step modify-lift Modify lift curve (shift or scale)
define b-c models dynamic-mesh-controls in-cylinder-parameter crank-angle-step piston-data Specify piston stroke and connecting rod length
define b-c models dynamic-mesh-controls in-cylinder-parameter crank-angle-step position-starting-mesh Move mesh from top dead center to starting crank angle
define b-c models dynamic-mesh-controls in-cylinder-parametercrank-angle-step print-plot-lift Print or plot valve lift curve
define b-c models dynamic-mesh-controls layering? Enable/disable dynamic-layering in quad/hex cell zones
define b-c models dynamic-mesh-controls layering-parameter collapse-factor Set the factor determining when to collapse dynamic layers
define b-c models dynamic-mesh-controls layering-parameter constant-height? Enable/disable layering based on constant height,else layering based on constant ratio
define b-c models dynamic-mesh-controls layering-parameter split-factor Set the factor determining when to split dynamic layers
define b-c models dynamic-mesh-controls remeshing? Enable/disable local remeshing in tri/tet and mixed cell zones
define b-c models dynamic-mesh-controls remeshing-parameter cell-skew-max Set the cell skewness threshold above which cells will be remeshed
define b-c models dynamic-mesh-controls remeshing-parameter face-remeshing? Enable/disable local face remeshing at deforming zones
define b-c models dynamic-mesh-controls remeshing-parameter face-skew-max Set the face skewness threshold above which faces will be remeshed
define b-c models dynamic-mesh-controls remeshing-parameter length-max Set the length threshold above which cells will be remeshed
define b-c models dynamic-mesh-controls remeshing-parameter length-min Set the length threshold bel flowwhich cells will be remeshed
define b-c models dynamic-mesh-controls remeshing-parameter must-improve-skewness? Enable/disable cavity replacement only if remeshing improves the skewness
define b-c models dynamic-mesh-controls remeshing-parameter size-remesh-interval Set the interval (in time steps) when remeshing based on size is done
define b-c models dynamic-mesh-controls remeshing-parameter sizing-funct-defaults Set sizing function defaults
define b-c models dynamic-mesh-controls remeshing-parameter sizing-funct-rate Determine h flowfar from the boundary the increase/decrease happens
define b-c models dynamic-mesh-controls remeshing-parameter sizing-funct-resolution Set the sizing function resolution with respect to shortest boundary
define b-c models dynamic-mesh-controls remeshing-parameter sizing-funct-variation Set the maximum sizing function increase/decrease in the interior
define b-c models dynamic-mesh-controls remeshing-parameter sizing-function? Enable/disable sizing function to control size based remeshing
define b-c models dynamic-mesh-controls six-dof-parameter motion-history? Enable/disable writing position/orientation of six DOF zones to file
define b-c models dynamic-mesh-controls six-dof-parameter x-component Specify x-component of gravity
define b-c models dynamic-mesh-controls six-dof-parameter y-component Specify y-component of gravity
define b-c models dynamic-mesh-controls six-dof-parameter z-component Specify z-component of gravity
define b-c models dynamic-mesh-controls smoothing? Enable/disable spring-based smoothing in tri/tet cell zones
define b-c models dynamic-mesh-controls smoothing-parameter bnd-node-relaxation Set the spring boundary node relaxation factor
define b-c models dynamic-mesh-controls smoothing-parameter bnd-stiffness-factor Set the stiffness factor for springs connected to boundary nodes
define b-c models dynamic-mesh-controls smoothing-parameter constant-factor Set the spring constant relaxation factor
define b-c models dynamic-mesh-controls smoothing-parameter convergence-tolerance Set the convergence tolerance for springbased solver
define b-c models dynamic-mesh-controls smoothing-parameter max-iter Set the maximum number of iterations for spring-based solver
define b-c models dynamic-mesh-controls smoothing-parameter skew-smooth-niter Set the number of skewness-based smoothing cycles
define b-c models dynamic-mesh-controls smoothing-parameter skew-smooth-skew-max Set the skewness threshold above which cells will be smoothed using skewness method
define b-c 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 window aspect-ratio Set the aspect ratio of the active window
display set window axes/border? Set whether to draw a border around the axes window
display set window axes/bottom Set the bottom boundary of the axes window
display set window axes/clear? Set the transparency of the axes window
display set window axes/left Set the left boundary of the axes window
display set window axes/right Set the right boundary of the axes window
display set window axes/top Set the top boundary of the axes window
display set window axes/visible? Turn axes visibility on/off
display set window main/border? Set whether or not to draw a border around the main viewing window
display set window main/bottom Set the bottom boundary of the main viewing window
display set window main/left Set the left boundary of the main viewing window
display set window main/right Set the right boundary of the main viewing window
display set window main/top Set the top boundary of the main viewing window
display set window main/visible? Turn visibility of the main viewing wind flowon/off
display set window scale border? Set whether or not to draw a border around the color scale window
display set window scale bottom Set the bottom boundary of the color scale window
display set window scale clear? Set the transparency of the scale window
display set window scale format Set the number format of the color scale window. (e.g., %0.2e)
display set window scale font-size Set the font size of the color scale window
display set window scale left Set the left boundary of the color scale window
display set window scale margin Set the margin of the color scale window
display set window scale right Set the right boundary of the color scale window
display set window scale top Set the top boundary of the color scale window
display set window scale visible? Turn visibility of the color scale wind flowon/off
display set window text application? Show/hide the application name in the picture
display set window text border? Set whether or not to draw a border around the text window
display set window text bottom Set the bottom boundary of the text window
display set window text clear? Enable/disable text wind flowtransparency
display set window text company? Show/hide the company name in the picture
display set window text date? Show/hide the date in the picture
display set window text left Set the left boundary of the text window
display set window text right Set the right boundary of the text window
display set window text top Set the top boundary of the text window
display set window 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 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 window XY plot wind flowoptions. For a description of the items in this menu, see display/set window 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 window 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 window 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 window 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-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 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.