The Laminar Flow Interface
The Laminar Flow (spf) interface () is used to compute the velocity and pressure fields for the flow of a single-phase fluid in the laminar flow regime. A flow remains laminar as long as the Reynolds number is below a certain critical value. At higher Reynolds numbers, disturbances have a tendency to grow and cause transition to turbulence. This critical Reynolds number depends on the model, but a classical example is pipe flow, where the critical Reynolds number is known to be approximately 2000.
The physics interface supports incompressible flow, weakly compressible flow (the density depends on temperature but not on pressure), and compressible flow at low Mach numbers (typically less than 0.3). It also supports flow of non-Newtonian fluids.
The equations solved by the Laminar Flow interface are the Navier-Stokes equations for conservation of momentum and the continuity equation for conservation of mass.
The Laminar Flow interface can be used for stationary and time-dependent analyses. Time-dependent studies should be used in the high-Reynolds number regime as these flows tend to become inherently unsteady.
When the Laminar Flow interface is added, the following default nodes are also added in the Model Builder: Fluid Properties, Wall (the default boundary condition is No slip), and Initial Values. Other nodes that implement, for example, boundary conditions and volume forces, can be added from the Physics toolbar or from the context menu displayed when right-clicking Laminar Flow.
Settings
The Label is the default physics interface name.
The Name is used primarily as a scope prefix for variables defined by the physics interface. Physics interface variables can be referred to using the pattern <name>.<variable_name>. In order to distinguish between variables belonging to different physics interfaces, the name string must be unique. Only letters, numbers, and underscores (_) are permitted in the Name field. The first character must be a letter.
The default Name (for the first physics interface in the model) is spf.
About the Physics Interface Label Names
The label for a single-phase flow interface (the node name in the Model Builder) is dynamic and is reset according to the turbulence model and the neglect inertial term (Stokes flow) property set at the physics interface level. The availability also depends on the software license.
For example, a Laminar Flow interface is added to the Model Tree. If the Low Reynolds number k-ε turbulence model is selected, the interface Label changes to Turbulent Flow, Low Re k-ε, which is the same Label that displays when the corresponding interface is added from the Model Wizard or Add Physics window.
If the Neglect inertial term (Stokes flow) check box is selected, then the Label changes to Creeping Flow, which is the same Label that displays when that interface is added from the Model Wizard or Add Physics window.
Physical Model
Compressibility
Depending of the fluid properties and the flow regime, three options are available for the Compressibility option. In general the computational complexity increases from Incompressible flow to Weakly compressible flow to Compressible flow (Ma<0.3) but the underlying hypotheses are increasingly more restrictive in the opposite direction.
When the Incompressible flow option (default) is selected, the incompressible form of the Navier-Stokes and continuity equations is applied. In addition, the fluid density is evaluated at the Reference pressure level defined in this section. The Reference temperature is set to 293.15 K.
The Weakly compressible flow option models compressible flow when the pressure dependency of the density can be neglected. When selected, the compressible form of the Navier-Stokes and continuity equations is applied. In addition, the fluid density is evaluated at the Reference pressure level defined in this section.
When the Compressible flow (Ma<0.3) option is selected, the compressible form of the Navier-Stokes and continuity equations is applied. Ma < 0.3 indicates that the inlet and outlet conditions, as well as the stabilization, may not be suitable for transonic and supersonic flow. For more information, see The Mach Number Limit.
Swirl Flow
The velocity component, , in the azimuthal direction can be included for 2D axisymmetric components by selecting the Swirl flow check box. While can be nonzero, there can be no gradients in the  direction. Also see General Single-Phase Flow Theory.
Neglect Inertial Term (Stokes Flow)
For low Reynolds number flows, the inertial terms in the Navier-Stokes equations may be neglected.
Porous Media Domains
With the addition of various modules, the Enable porous media domains check box is available. Selecting this option, a Fluid and Matrix Properties node, a Mass Source node, and a Forchheimer Drag subnode are added to the physics interface. These are described for the Brinkman Equations interface in the respective module’s documentation. The Fluid and Matrix Properties can be applied on all domains or on a subset of the domains.
Include gravity
When the Include gravity check box is selected, a global Gravity feature is shown in the interface model tree, and the buoyancy force is included in the Navier-Stokes equations.
Also, when the Include gravity check box is selected, the Use reduced pressure option changes the pressure formulation from using the total pressure (default) to using the reduced pressure. This option is suitable for configurations where the density changes are very small; otherwise, the default formulation can be used. For more information, see Gravity.
Natural convection is induced by variations in magnitude of the buoyancy force that is defined from the density. For incompressible flow, the density is constant; hence the buoyancy force is homogeneous and natural convection cannot be modeled. Nevertheless, using the Nonisothermal Flow multiphysics coupling, the buoyancy force is defined using the thermal expansion coefficient and the temperature. Hence, in this case natural convection is accounted for following Boussinesq approximation.
Use Shallow Channel Approximation
For 2D components, selecting the Use shallow channel approximation check box enables modeling of fluid flow in shallow channels in microfluidics applications. Such channels often have an almost rectangular cross section where the Channel thickness dz is much smaller than the channel width. Simple 2D components often fail to give correct results for this type of problems because they exclude the boundaries that have the greatest effect on the flow. The shallow channel approximation takes the effect of these boundaries into account by adding a drag term as a volume force to the momentum equation. The form of this term is
(3-1)
where μ is the fluid’s dynamic viscosity, u is the velocity field, and dz is the channel thickness. This term represents the resistance that the parallel boundaries impose on the flow; however, it does not account for any changes in velocity due to variations in the cross-sectional area of the channel.
Reference values
Reference values are global quantities used to evaluate the density of the fluid when the Incompressible flow or the Weakly compressible flow option is selected and to define the gravity force.
Reference pressure level
There are generally two ways to include the pressure in fluid flow computations: either to use the absolute pressure pA=p+pref, or the gauge pressure p. When pref is nonzero, the physics interface solves for the gauge pressure whereas material properties are evaluated using the absolute pressure. The reference pressure level is also used to define the reference density.
Reference temperature
The reference temperature is used to define the reference density.
Reference position
When Include gravity is selected, the reference position can be defined. It corresponds to the location where the total pressure (that includes the hydrostatic pressure) is equal to the Reference pressure level.
Turbulence
Turbulence Model Type
Turbulent flow can be simulated by changing the Turbulence model type to RANS (Reynolds-Averaged Navier–Stokes) or to LES (Large Eddy Simulation).
Dependent Variables
The following dependent variables (fields) are defined for this physics interface — the Velocity field u and its components, and the Pressure p.
If required, the names of the field, component, and dependent variable can be edited. Editing the name of a scalar dependent variable changes both its field name and the dependent variable name. If a new field name coincides with the name of another field of the same type, the fields share degrees of freedom and dependent variable names. A new field name must not coincide with the name of a field of another type or with a component name belonging to some other field. Component names must be unique within a model except when two fields share a common field name.
Advanced Settings
To display this section, click the Show button () and select Advanced Physics Options. Normally these settings do not need to be changed.
The Use pseudo time stepping for stationary equation form is per default set to Automatic from physics. This option can add pseudo time derivatives to the equation when the Stationary equation form is used in order to speed up convergence. Pseudo time stepping is triggered when the Laminar Flow interface is selected in some multiphysics coupling features and for turbulent flows. Set Automatic from physics to On to apply pseudo time stepping also for laminar flows. Set it to Off to disable pseudo time stepping completely.
When Use pseudo time stepping for stationary equation form is set to Automatic from physics or On, a CFL number expression should also be defined. For the default Automatic option, the local CFL number (from the Courant–Friedrichs–Lewy condition) is determined by a PID regulator.
Discretization
The default discretization for Laminar Flow is P1+P1 elements — that is, piecewise linear interpolation for velocity and pressure. This is suitable for most flow problems.
Some higher-order interpolations are also available, and they can be cost-effective options to obtain high accuracy for flows with low Reynolds numbers.
The P2+P2 and P3+P3 options, the equal-order interpolation options, are the preferred higher-order options because they have higher numerical accuracy than the mixed-order options P2+P1 and P3+P2. The equal-order interpolation options do, however, require streamline diffusion to be active.
Flow Past a Cylinder: Application Library path COMSOL_Multiphysics/Fluid_Dynamics/cylinder_flow