Flow Conditions Library

Conditions in Boundaries

Atmosphere Type Option

For atmospheric flows, specifies the method by which Simcenter STAR-CCM+ computes the freestream pressure and temperature from the altitude:

Option	Corresponding Value Nodes
Standard Uses the US 1976 Standard Atmosphere as a model of the Earth's atmosphere.	None.
User Table Uses your own imported table. Make sure that you first import the table within the Tools > Table node.	Atmosphere Table Use this node to configure your own imported table from which Simcenter STAR-CCM+ extracts freestream pressure and temperature. Set Table to the imported table. Match the relevant table columns to Table: Altitude, Table: P, and Table: T. Set the corresponding units using Units: Altitude, Units: P, and Units: T.

Backflow Specification

Sets the method by which Simcenter STAR-CCM+ computes the direction of any flow that enters the simulation through an outflow boundary. For some methods, you must also set the associated Reference Frame Specification.

Pressure

Specifies how the pressure is computed.

• Environmental: Subtracts dynamic head at pressure outlet boundary.
• Static: Does not use dynamic head in the case of inflow. Pressure is maintained at the pressure specified by the user.

Direction

Direction	Corresponding Physics Value Nodes
Extrapolated Extrapolates the flow direction from the interior of the domain. In most situations, this is less stable than the Boundary Normal option. However, it is recommended for situations where the flow is known to be parallel to the pressure boundary, such as a co-flowing jet. This option is set by default for the Coupled Flow model.	None.
Boundary Normal Assumes that the incoming flow enters the simulation along a vector that is orthogonal to the boundary surface, in the specified reference frame for the boundary. This option is set by default for the Segregated Flow model and generally provides the most robust convergence. If the flow is largely parallel to the boundary, the Extrapolated option should be used instead.	None.
Components The inflow direction vector is explicitly defined in the specified reference frame. When the Reference Frame Specification is set to Lab Frame, this value is defined in the Flow Direction node under Physics Values. When the Reference Frame Specification is set to an option other than Lab Frame, this value is defined in the Relative Flow Direction node.	Flow Direction Relative Flow Direction Sets the direction vector in the chosen Coordinate System by the selected Method.
Angles Sets direction using Euler angles.	Flow Angles Defines the flow direction as the composition of rotations of a unit Reference Vector around certain axes of a reference Coordinate System. These rotations are known as Euler angles. When you set Method to Constant, set Value to the $\phi$ , $\theta$ , $\psi$ rotations. When Method is Field Function, set Angles Function to an appropriate function. You can also provide tables. Three different rotation conventions are supported to define the coordinate axes that are used, and the order in which the rotations apply. Choose a Rotation Convention as follows: X Convention (Z-X-Z): For Euler angles ( $\phi$ , $\theta$ , $\psi$ ), the first rotation is by angle $\phi$ about the z-axis, the second is by angle $\theta$ about the x-axis, and the third is by angle $\psi$ about the z-axis. Y Convention (Z-Y-Z): For Euler angles ( $\phi$ , $\theta$ , $\psi$ ), the first rotation is by angle $\phi$ about the z-axis, the second is by angle $\theta$ about the y-axis, and the third is by angle $\psi$ about the z-axis. Yaw, Pitch, Roll Convention (Z-Y-X): For Euler angles ( $\phi$ , $\theta$ , $\psi$ ), the first rotation is by angle $\phi$ about the z-axis, the second is by angle $\theta$ about the y-axis, and the third is by angle $\psi$ about the x-axis. The Axes Convention applies rotations as follows: Fixed Axes: relative to the original axes Moving Axes: relative to the rotated axes

Scalars

Specifies how scalars are computed.

• Specified: When the flow reverses, the scalar conditions that you specify at the boundary are used. Otherwise, the scalar conditions are extrapolated.
• Extrapolated: Regardless of the flow direction, the scalar conditions at the boundary are set to be equal to the scalar conditions of the immediate interior.

Fan Curve Type

Curve Type	Corresponding Value Nodes
Table	Fan Curve Table The fan curve table defines pressure rise as a function of four possible input variables. The accepted input variables, selected using Method, are: Local Velocity Mass Average Velocity Volumetric Flow Rate Mass Flow Rate After choosing the previously imported Table, set Table: X to the column that contains the input variable data, and Table: P to the column that contains the pressure rise data. Set the respective units using Units: X and Units: P. Use Pressure Rise to inform Simcenter STAR-CCM+ about the basis on which the data is defined: Standard: pressure rise is the difference between the static pressure downstream and the total pressure upstream Static to Static: pressure rise is the difference between the static pressure downstream and the static pressure upstream. This definition also matches the difference between total pressure downstream and total pressure upstream When you choose the Static to Static option, ensure that the specified fan curve is a decreasing function of the input variable. When you choose the Standard option, ensure that [specified fan curve + $\frac{1}{2}p{v}^2$ ] is a decreasing function of input variable. Of the four fan curve Method options, only the Mass Average Velocity option is not linearized, and is considered to be less robust. The other options apply a different pressure rise to each face at the fan interface or boundary. However, for some problems, it can be more meaningful to apply the same pressure rise to all of the faces on the fan interface or boundary. In that scenario, you can use the mass averaged velocity options. Enter the reference fan speed to which the performance tests apply in Data Rotation Rate, and the actual fan speed for the current simulation in Operating Rotation Rate. Simcenter STAR-CCM+ applies fan scaling laws to the reference data contained within the table. Fan Verbosity When Verbosity is On, Simcenter STAR-CCM+ prints detailed information on the behavior of the fan model.
Polynomial	Fan Curve Polynomial Models the fan pressure rise as a polynomial in one of the following variables, which you select using Method: Local Velocity Mass Average Velocity Volumetric Flow Rate Mass Flow Rate Enter the polynomial parameters using the custom property editor for Polynomial. The properties, Pressure Rise, Operating Rotation Rate, and Data Rotation Rate, have the same purpose as for the Fan Curve Table.

Flow Direction Specification

Relative Flow Direction Specification

Controls how you define flow direction. When relative, the quantities are set in the frame of reference that you apply to the boundary.

Method	Corresponding Physics Value Nodes
Boundary Normal Sets flow direction normal to the boundary face.	None.
Components	Flow Direction Relative Flow Direction Sets the direction vector in the chosen Coordinate System by the selected Method.
Angles Sets direction using Euler angles.	Flow Angles Defines the flow direction as the composition of rotations of a unit Reference Vector around certain axes of a reference Coordinate System. These rotations are known as Euler angles. When you set Method to Constant, set Value to the $\phi$ , $\theta$ , $\psi$ rotations. When Method is Field Function, set Angles Function to an appropriate function. You can also provide tables. Three different rotation conventions are supported to define the coordinate axes that are used, and the order in which the rotations apply. Choose a Rotation Convention as follows: X Convention (Z-X-Z): For Euler angles ( $\phi$ , $\theta$ , $\psi$ ), the first rotation is by angle $\phi$ about the z-axis, the second is by angle $\theta$ about the x-axis, and the third is by angle $\psi$ about the z-axis. Y Convention (Z-Y-Z): For Euler angles ( $\phi$ , $\theta$ , $\psi$ ), the first rotation is by angle $\phi$ about the z-axis, the second is by angle $\theta$ about the y-axis, and the third is by angle $\psi$ about the z-axis. Yaw, Pitch, Roll Convention (Z-Y-X): For Euler angles ( $\phi$ , $\theta$ , $\psi$ ), the first rotation is by angle $\phi$ about the z-axis, the second is by angle $\theta$ about the y-axis, and the third is by angle $\psi$ about the x-axis. The Axes Convention applies rotations as follows: Fixed Axes: relative to the original axes Moving Axes: relative to the rotated axes

Free Stream Option

You select the appropriate option as a property of the [Region] > Boundaries > [Boundary] > Physics Conditions > Free Stream Option node.

Option	Corresponding Value Nodes
Mach Number + Pressure + Temperature Default freestream option.	Mach Number Specifies the Mach number. Pressure Specifies the working pressure using the standard scalar profile methods. For turbomachinery simulations, the Radial Equilibrium method is available. The radial equilibrium pressure boundary condition is suitable for strong rotational flows where the centrifugal forces due to rotation are balanced by the radial pressure gradient force. The Radial Equilibrium method is compatible with all pressure outlet options except Average Pressure. For more information, see Radial Equilibrium. Static Temperature Sets the initial static temperature in the continuum.
Altitude + Length Scale + Reynolds Number The freestream pressure and temperature are computed internally using the specified altitude. The freestream Mach number is computed internally using the specified altitude, Reynolds number, and length scale. Adds the Physics Conditions > Atmosphere Type Option node under which you specify the appropriate atmosphere type.	Altitude Sets the height at which Simcenter STAR-CCM+ extracts the freestream pressure and temperature from the chosen Atmosphere Table. Mach Number Specify the appropriate Reynolds number and length scale values.
Altitude + Mach Number The freestream pressure and temperature are computed internally using the specified altitude. Adds the Physics Conditions > Atmosphere Type Option node under which you specify the appropriate atmosphere type.	Altitude Sets the height at which Simcenter STAR-CCM+ extracts the freestream pressure and temperature from the chosen Atmosphere Table. Mach Number Specifies the Mach number.

You can expose the freestream values that Simcenter STAR-CCM+ calculates internally by right-clicking the Free Stream Option node and selecting Print Average Pressure, Velocity, Temperature Values.

Note	The Print Average Pressure, Velocity, Temperature Values function is not compatible when the dynamic viscosity material property is set to Sutherlands Law.

Mass Flow Option

Specification Option	Corresponding Value Nodes
Mass Flux	Mass Flux Relative Mass Flux Scalar quantity for the mass flow rate per unit area. Spatial variations across the inlet can be specified using functions or tables. For more information, see Mass Flow Inlet in the Theory Guide.
Mass Flow Rate	Mass Flow Rate Relative Mass Flow Rate Specifies a mass flow rate at the outlet boundary. ${\dot{m}}_{i,\text{spec}}$ in Eqn. (827). The Mass Flow Rate represents the total mass per unit time ( $kg/s$ ) for the whole boundary. You can use field functions and tables to describe a dependence on iteration or time-step, but the mass flow rate cannot vary spatially across the boundary. The total mass flow is distributed over all of the faces of the part as described in Mass Flow Inlet in the Theory Guide. A reverse flow (negative mass flow rate) can be specified for a multiphase flow. However, this option should be used with caution.

Mass Flow Specification

Mass Flow Specification	Corresponding Value Nodes
Split Ratio	Split Ratio When there are multiple outlet boundaries on one continuum, the fraction of the mass flow passing through each of the boundaries must be specified. The specified fraction is ignored if there is only one outlet boundary in the continuum. This is a simple value with only one method of entering the data-type in a value from 0 to 1.
Mass Flow Rate At every iteration the solver makes a correction to the flow rate at this boundary to ensure that the total flow matches the specified flow rate. If the compressible solver is used, the extrapolated density is used for computing the mass flow rate. This boundary type can be used in the same continuum as a pressure outlet. However, you need to consider the following: In scenarios where the pressure outlet may act as an inlet, you need to be careful how you specify the pressure condition. In the event of reversed flow, the dynamic head is taken out of the specified pressure, which can cause an incorrect pressure profile at the pressure outlet. If you specify the mass flow rate using a field function, an average value on that boundary is used as the specified mass flow rate. The mass flow rate must be a single value, not a field function with a value that varies along the boundary.	Mass Flow Rate Relative Mass Flow Rate Specifies a mass flow rate at the outlet boundary. ${\dot{m}}_{i,\text{spec}}$ in Eqn. (827). The Mass Flow Rate represents the total mass per unit time ( $kg/s$ ) for the whole boundary. You can use field functions and tables to describe a dependence on iteration or time-step, but the mass flow rate cannot vary spatially across the boundary. The total mass flow is distributed over all of the faces of the part as described in Mass Flow Inlet in the Theory Guide.
Corrected Mass Flow Rate Becomes available when an Energy model is selected in the Physics continuum. For turbomachinery applications. Allows you to simulate the full compressor speedline from choke to surge without the need for changing boundary types. When analyzing compressor performance, the machine rotation rate is held constant and the outflow boundary rate is varied to characterize the relationship between mass flow through the compressor and the ratio of the outlet pressure to the inlet pressure. This curve is called the speedline, and each point on this speedline corresponds to an individual simulation. Towards the right of the speedline, the compressor experiences choke where no more mass flows through the machine. To the left of the speedline, the compressor experiences surge with flow reversal through the machine. The Corrected Mass Flow Rate option handles the numerical difficulties associated with these singularities and is suitable for simulating all points on the speedline. This option also allows you to specify directly the corrected mass flow delivered from the compressor to the combustor of a gas turbine engine.	Corrected Mass Flow Rate The same as Mass Flow Rate, but allows you to specify the Corrected Mass Flow Rate ( ${\dot{m}}_{i,\text{spec}}$ in Eqn. (830)).

Outlet Flow Specification

Outlet Flow Specification	Corresponding Value Nodes
Specified Split Ratios	Split Ratio When there are multiple outlet boundaries on one continuum, the fraction of the mass flow passing through each of the boundaries must be specified. The specified fraction is ignored if there is only one outlet boundary in the continuum. This is a simple value with only one method of entering the data-type in a value from 0 to 1.
Specified Mass Fluxes At every iteration the solver makes a correction to the flow rate at this boundary to ensure that the total flow matches the specified flow rate. If the compressible solver is used, the extrapolated density is used for computing the mass flow rate. This boundary type can be used in the same continuum as a pressure outlet. However, you need to consider the following: In scenarios where the pressure outlet may act as an inlet, you need to be careful how you specify the pressure condition. In the event of reversed flow, the dynamic head is taken out of the specified pressure, which can cause an incorrect pressure profile at the pressure outlet. If you specify the mass flow rate using a field function, an average value on that boundary is used as the specified mass flow rate. The mass flow rate must be a single value, not a field function with a value that varies along the boundary.	Mass Flow Rate Relative Mass Flow Rate Specifies a mass flow rate at the outlet boundary. ${\dot{m}}_{i,\text{spec}}$ in Eqn. (827). The Mass Flow Rate represents the total mass per unit time ( $kg/s$ ) for the whole boundary. You can use field functions and tables to describe a dependence on iteration or time-step, but the mass flow rate cannot vary spatially across the boundary. The total mass flow is distributed over all of the faces of the part as described in Mass Flow Inlet in the Theory Guide.
Specified Volumetric Fluxes	Volumetric Flow Rate Scalar quantity for the volumetric flow rate. The volumetric flow rate represents the total volume per unit time for the whole boundary. In cases when there are large differences between the phase densities, using the volumetric flow rate of the multiphase mixture allows a smoother outlet profile. If a constant mass flow rate is specified, the flow velocity can become unstable. For example, a bubble of air in water will experience a large velocity increase as it passes through the outlet boundary. See Specified Volumetric Fluxes.

A reverse flow (negative mass flow rate) is not supported as the volume fraction cannot be specified on the boundary.

Pressure Jump Option

Option	Corresponding Value Nodes
None	None.
Fan The pressure rise is obtained from a fan curve. At a Stagnation Inlet boundary, the pressure rise is applied in the direction going into the domain. At a Pressure Outlet boundary, the pressure rise is applied in the direction going out of the domain. Selecting this option adds the condition node Fan Curve Type.	Fan value nodes are controlled by the Fan Curve Type.
Porous Computes the pressure loss as $\alpha \rho {\left|\text{v}\right|}^2+\beta \rho \left|\text{v}\right|$ where $\alpha$ is the Porous Inertial Resistance and $\beta$ is the Porous Viscous Resistance. The pressure loss is always applied in the direction of flow.	Porous Inertial Resistance Scalar profile value for $\alpha$ . Porous Viscous Resistance Scalar profile value for $\beta$ .
Loss Coefficient Computes the pressure loss as $0.5K\rho {\left|\text{v}\right|}^2$ where $K$ is the Pressure Loss Coefficient. The pressure loss is always applied in the direction of flow.	Pressure Loss Coefficient Scalar profile entry for $K$ .

When you use the Pressure Jump Option with the Segregated Flow Solver, and the flow solution does not converge, you can resolve this problem by activating the Delta-V Dissipation in the Segregated Flow model.

Pressure Outlet Option

Provides a range of options for constraining pressure on an outflow boundary.

Option	Corresponding Physics Value Nodes
None	None.
Non-Reflecting (CF) Prevents spurious numerical reflection of the solution into the solution domain in steady, compressible, and non-isothermal simulations.	Non-Reflecting Mode Specification Specify the Number of modes to retain. Specify a number of modes less than the number of cells in the circumferential direction.
Unsteady Non-Reflecting (CF) Prevents spurious acoustic reflection in unsteady, compressible, and non-isothermal simulations.	Unsteady Non-Reflecting Length Scale Specify the Value of the reference length (typically, the domain length in the flow direction), defined as $L_{\text{ref}}$ in Eqn. (812).
Target Mass Flow Automatically applies a correction to the specified Pressure boundary value in an attempt to yield the specified mass flow rate.	Target Mass Flow Rate Sets the Massflow Rate that you want to achieve, defined as ${\dot{m}}_{\mathrm{spec}}$ in Eqn. (815). In each iteration, Simcenter STAR-CCM+ applies a Pressure Adjustment $\delta P$ to the specified pressure. The correction process is constrained by average pressure values that you set, the Minimum Allowable Avg Pressure and the Maximum Allowable Avg Pressure. The Under-Relaxation Factor enters the pressure adjustment equation, Eqn. (815), as ${\omega }_{\mathrm{spec}}$. While the adjustment is applied at every iteration, a new pressure adjustment value is computed according to the specified Update Frequency (iterations or time-steps). Activate Verbose for additional debugging output.
Pressure Jump Adds the condition node Pressure Jump Option.	None.
Average Pressure (SF) The pressure profile from the cells next to the pressure outlet boundary is adjusted so that the average of that profile is equal to the average pressure value specified under Average Pressure node. This adjusted profile is then applied to the faces of the pressure outlet boundary. The pressure at the boundary face of cell $i$ is computed as: $$P_{s,fi}=P_{s,avg,spec}+{\lambda }_{spec}(P_{s,ci}-P_{s,c,avg})$$ where: $P_{s,avg,spec}$ is the average pressure. ${\lambda }_{spec}$ is the blending factor that you select. $P_{s,ci}$ is the pressure in cell $i$ . $P_{s,c,avg}=\frac{{\displaystyle \sum _i^{}{P}_{s,ci}\left|a_i\right|}}{{\displaystyle \sum _i^{}\left|a_i\right|}}$ where $\left|a_i\right|$ is the area of the boundary face of cell $i$ . These computations are made only for faces that do not have backflow. Faces with backflow or supersonic flow are treated as for the default pressure outlet boundary condition. See Pressure Outlet. When using this option with Coupled Flow, you are advised to use the Continuity Convergence Accelerator for faster convergence. Simcenter STAR-CCM+ issues warnings to this effect.	Average Pressure Sets the average pressure $p_{avg}$ as a scalar profile. Average Pressure Adjuster Sets the factor $\beta$ that Simcenter STAR-CCM+ uses to smooth out the pressure profile that is extrapolated from cells next to the pressure outlet boundary. The value can range from 0 to 1. The default value is 0.5.

Non-Reflecting Option

This option is available only when the Coupled Flow Ideal Gas, Steady, and Two-Dimensional or Three-Dimensional models are enabled, and only on boundaries of linearly (two-dimensional) or rotationally (three-dimensional) periodic problems. It is appropriate in instances where the flow normal to the non-reflecting boundary remains subsonic.

In three-dimensional simulations, the boundary must be a surface of revolution. Furthermore, the boundary mesh must be a structured, mapped mesh of quadrilateral faces. (This requirement does not apply to steady-state calculations using the Coupled Flow model.) If these conditions are not satisfied, an error is generated during pre-processing of the boundary mesh before the application of the non-reflecting boundary condition procedure.

Reference Frame Specification

Allows you to specify a reference frame to which the boundary is associated with.

Depending on the boundary type, you define one or more of the following properties with respect to the specified reference frame:

• Flow Direction Specification
• Velocity
• Velocity Magnitude
• Flow Direction Specification
• Total Pressure
• Total Temperature
• Tangential Velocity Specification

Option	Corresponding Physics Value Nodes
Lab Frame Uses the Laboratory reference frame. This option is the default for Velocity Inlet and Stagnation Inlet boundaries.	None.
Part Reference Frame Uses the direct rotating reference frame of the region with respect to its associated part(s). This option is only available when you activate Specify by Part Subgroup under the Direct Rotating Reference Frame node. For more details, refer to Defining a Direct Reference Frame. You can visualize the reference frame specification within the [region] > Physics Values > Direct Rotating Reference Frame > [subgroup] > Direct Rotating Reference Frame Values node.	None
Region Reference Frame Uses the reference frame of the parent region. When the region is defined in a rotating reference frame, the boundary uses the reference frame of the region. You can see the region axis within the [region] > Physics Values > Axis node. If this node does not exist, the motion assigned to the region is automatically providing a region axis. For example, if you assign a rotation motion defined within the Tools > Motions node to the region, the region axis is the axis of the rotation motion.	None.
Local Reference Frame Allows you to specify a local reference frame for the boundary. You can only select a rotating reference frame. You can use when both the boundary and the region are rotating at a different RPM but have the same axis and origin. A setup where the region and boundary have different values for the RPM, axis, and origin is also possible.	Boundary Reference Frame Specification Applies the chosen Reference Frame to the containing boundary.

Flow Direction Reference Frame Specification

Provides a separate reference frame for the flow direction. The default is the reference frame currently used for Reference Frame Specification.

Adds the following value nodes:

• Total Pressure
• Total Temperature
• Flow Direction (or Flow Angles when Components or Angles is selected for Flow Direction Specification)
• Boundary Reference Frame Specification when Local Reference Frame is selected for Reference Frame Specification or Flow Direction Reference Frame Specification.

Option	Corresponding Physics Value Nodes
Lab Frame Uses the Laboratory reference frame (default). No rotation.	None.
Region Reference Frame Uses the reference frame of the parent region. When the region has a rotating reference frame attached, a physically valid setup using this condition puts the boundary in the reference frame of the region. This implies that the boundary is rotating with the region at the same RPM, and has the same rotation axis and origin as the region.	None.
Local Reference Frame This option allows the boundary to have its own frame (only rotating frame) attributes. For example, this can be used when both the boundary and the region are rotating at a different RPM but have the same axis and origin. A setup where the region and boundary have different values for the RPM, axis, and origin is also possible.	Boundary Reference Frame Specification Applies the chosen Reference Frame to the containing boundary.

Shear Stress Specification

Defines how a wall surface acts on a fluid passing across it.

Method	Corresponding Physics Value Nodes
No-Slip Relative fluid velocity tangential to the wall is set to zero. When you choose No-Slip, Simcenter STAR-CCM+ adds the Tangential Velocity Specification.	None.
Slip Fluid velocity at the wall is extrapolated from the parallel component of the velocity in the cell next to the wall. When simulating non-Newtonian fluid flow using the Viscous Flow model, the relation between the slip velocity and the shear force at the wall is given by a power-law expression.	Available only with the Viscous Flow model: Slip Coefficient The slip coefficient $k_s$ in Eqn. (1062). Slip Exponent The slip exponent $n_s$ in Eqn. (1062).
Specified Shear Allows you to model partial slip at the wall using a known wall shear force. This option is recommended for situation where there is some degree of slippage between the fluid and the wall, such as for polymer/rubber flow simulations or hydrophobic/hydrophilic fluid flow simulations.	Wall Shear Force Sets the wall shear force ${(\mathbf{T}\cdot \mathbf{a})}_f$, where $T$ is the viscous stress tensor and $a$ is the surface normal vector, as a vector profile value in the chosen Coordinate System. The wall shear force enters the momentum equation in the form of a source term in the near-wall cell. Wall Shear Velocity Derivative For a Wall Shear Force that is a function of velocity, sets the derivative of the wall shear force with respect to the x-, y-, [z-] components of velocity as a tensor profile value. The derivative is used in the linearization of the momentum equation. It is highly recommended to specify the derivative in order to improve the stability and convergence rate of the solution.

Stagnation Inlet Option

Option	Corresponding Value Nodes
None	None.
Non-Reflecting (CF) Prevents spurious numerical reflection of the solution into the solution domain in steady, compressible, and non-isothermal simulations.	Non-Reflecting Mode Specification Specify the Number of modes to retain. Specify a number of modes less than the number of cells in the circumferential direction.
Pressure Jump Adds the condition node Pressure Jump Option.	None.

Tangential Velocity Specification

When a Tangential Velocity Specification is used at a wall $f$, only the tangential component $v_{\tau }$ of the specified velocity ${\mathbf{\text{v}}}_{\text{spec}}^{\text{lab}}$ is used. If you specify a velocity with a component normal to the wall, the normal component of ${\mathbf{\text{v}}}_{\text{spec}}^{\text{lab}}$ is ignored, since the velocity ${\mathbf{\text{v}}}_f$ at the face is computed as:

$${\mathbf{\text{v}}}_f={\mathbf{\text{v}}}_{\text{spec}}^{\text{lab}}-({\mathbf{\text{v}}}_{\text{spec}}^{\text{lab}}\cdot \mathbf{\text{a}}-G_f)\frac{\mathbf{\text{a}}}{a^2}$$

()

where $\mathbf{\text{a}}$ is the face area vector and ${\mathbf{\text{v}}}_{\text{spec}}^{\text{lab}}$ is the velocity in the laboratory frame. The normal component contribution at the face $f$ can only come from the grid flux $G_f$ that is given by Eqn. (4868). That is, if the wall itself is moving at a velocity with a non-zero component in the wall normal direction.

Note that:

$${\mathbf{\text{v}}}_{\text{spec}}^{\text{lab}}={\mathbf{\text{v}}}_{\text{spec}}^{\text{mesh}}+{\mathbf{\text{v}}}_{\text{mesh}}^{\text{ref}}+{\mathbf{\text{v}}}_{\text{ref}}^{\text{lab}}$$

()

where:

• ${\mathbf{\text{v}}}_{\text{spec}}^{\text{lab}}$ is the specified velocity measured in the laboratory frame.
• ${\mathbf{\text{v}}}_{\text{spec}}^{\text{mesh}}$ is the specified velocity measured relative to the mesh.
• ${\mathbf{\text{v}}}_{\text{mesh}}^{\text{ref}}$ is the velocity of the mesh relative to the reference frame. This quantity is in Region > Physical Values > Motion Specification..
• ${\mathbf{\text{v}}}_{\text{ref}}^{\text{lab}}$ is the velocity of the reference frame relative to the laboratory frame.

The net tangential velocity in the laboratory frame is the vector sum of the tangential velocity with respect to the reference frame selected under the condition Reference Frame Specification and the velocity of the selected frame with respect to the laboratory frame.

Unless specified in an Axis node, axis of rotation is defined by information in the Motion Specification node under the Physics Values node.

Method	Corresponding Physics Value Nodes
Fixed Tangential velocity is zero with respect to the applicable reference frame.	None.
Vector Tangential velocity is specified by rotation rate with respect to the applicable reference frame.	Velocity Relative Velocity Sets the velocity vector in the chosen Coordinate System. When relative, the vector is defined within the reference frame applied to the boundary.
Rotation Rate Tangential velocity is specified as a vector with respect to the applicable reference frame.	Wall Rotation Wall Relative Rotation Sets the wall rotation rate around the axis of the reference frame applied to the containing boundary.
Local Rotation Rate Tangential velocity is defined by the rotation rate around the axis specified in the Axis node of the boundary and with respect to the applicable reference frame.	Local Axis Specifies a vector whose Origin and Direction define an axis of rotation. The local axes can be defined By Surface Subgrouping if the following prerequisites are fulfilled: Allow Per-Surface Values of the boundary is activated. Specify by Part Subgroup of the Local Axis node is activated. For more workflow of Applying Quantities by Subgroup, refer to Defining Subgroups. Wall Rotation Wall Relative Rotation As for Rotation Rate.

Velocity Specification

Controls how you define velocity on the boundary.

Method	Corresponding Value Nodes
Components Define all the components of the velocity vector.	Velocity Relative Velocity Sets the velocity vector in the chosen Coordinate System. When relative, the vector is defined within the reference frame applied to the boundary.
Magnitude + Direction Define the magnitude of the velocity vector, and take the direction based on the Flow Direction Specification.	Velocity Magnitude Relative Velocity Magnitude Sets the velocity magnitude by the selected Method. When relative, the magnitude is defined within the reference frame applied to the boundary.
Background This method is available in the Dispersed Multiphase model only. The velocity of the dispersed phase is taken from the background flow.	None.