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.

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.

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.

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.

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.

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.

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.

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.

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

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 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.

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.

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.

Turbulent flow can be simulated by changing the Turbulence model type to RANS (Reynolds-Averaged Navier–Stokes) or to LES (Large Eddy Simulation).

The following dependent variables (fields) are defined for this physics interface — the Velocity field u and its components, and the Pressure p.

To enable this section, click the Show More Options button () and select Stabilization in the Show More Options dialog box.

There are two consistent stabilization methods: Streamline diffusion and Crosswind diffusion. Usually, both check boxes for these methods are selected by default and should remain selected for optimal performance. Consistent stabilization methods do not perturb the original transport equation. Streamline diffusion must be selected when using equal-order interpolation for pressure and velocity.

Select the Use dynamic subgrid time scale check box to approximate the time-scale tensor in time dependent problems from projections of weak expressions. This check box is selected by default. When not selected the actual time-step is used.

To enable this section, click the Show More Options button () and select Stabilization in the Show More Options dialog box.

There is usually just one inconsistent stabilization method — Isotropic diffusion. This method is equivalent to adding a term to the diffusion coefficient in order to dampen the effect of oscillations by making the system somewhat less dominated by convection. If possible, minimize the use of the inconsistent stabilization method because by using it you no longer solve the original problem. By default, the Isotropic diffusion check box is not selected because this type of stabilization adds artificial diffusion and affects the accuracy of the original problem. However, this option can be used to get a good initial guess for underresolved problems.

If required, select the Isotropic diffusion check box and enter a Tuning parameter δid as a scalar positive value. The default value is 0.25 (a reasonable value to start with is roughly 0.5 divided by the element order). A higher value adds more isotropic diffusion.

To display this section, click the Show More Options button () and select Advanced Physics Options in the Show More Options dialog box. 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.

The Use Block Navier-Stokes preconditioner in time dependent studies check box under Linear solvers is available when the Compressibility option is set to Incompressible flow. When this check box is selected, the default solver for time dependent study steps will use the Block Navier-Stokes preconditioner in iterative solvers for the velocity and pressure. Using this preconditioner may result in shorter solution times for large time dependent problems with high Reynolds numbers.

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.

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.