## Computational Fluid Dynamics Software: SimFlow

SimFlow is a CFD Analysis and Modeling for Windows and Linux. Easy and intuitive Computational Fluid Dynamics (CFD) Software for your everyday CFD Analysis. # Incompressible Single-Phase Solvers

For the incompressible and single-phase solver, the system of equations is simplified by eliminating density from the equations. Thus, density is not required for these solvers. Instead, it is required to operate on kinematic fluid properties, such as kinematic fluid viscosity or kinematic pressure.

## Assumptions

The incompressible solvers assume the density to be constant. This fact comes straight from the definition: “incompressible” means that there is no compressibility effect and density is constant. The incompressible flow assumption usually works well for all fluids at low Mach numbers (about Mach 0.3), as it does for modelling air winds at normal temperatures. The second condition is a “Single-phase” flow which determine only one fluid in a considered domain. These two conditions ensure a constant density throughout the whole domain, independent of other parameters.

## Solver Simplification

If the case consider incompressible single-phase fluid flow, the system of equations is simplified by eliminating the density from the equations. All equations are divided by the constant density. So, Incompressible Navier-Stokes equation does not contain any density at all, so the density can not vary and affect the flow. Fluid density for this case are implicitly applied through kinematic viscosity, which is expressed by the dynamic viscosity divided by the density. The kinematic fluid viscosity unit is $$\frac{m^2}{s}$$ which corresponds to dynamic viscosity divided by the reference density.

## Consequences

Incompressible flow solvers in OpenFOAM operate using a kinematic pressure instead of a physical pressure. Kinematic pressure is defined as pressure divided by fluid density, and it is expressed in $$\frac{m2}{s2}$$. When using incompressible flow solvers in SimFlow always use kinematic pressure values at boundary conditions to obtain correct results. When you analyze the results, remember that the pressure field in ParaView displays values of kinematic pressure. Therefore, you must multiply the values of kinematic pressure by the fluid reference density in order to calculate the pressure field expressed in Pa.

Similar applies to the forces calculated at the boundary. The displayed result is expressed in $$\frac{m^4}{s^2}$$ (Newton divided by $$\frac{kg}{m^3}$$). In order to compute actual force you will need to multiply this value by a reference density.

By analogy, flow rate is expressed by Volumetric Flow Rate instead of Mass Flow Rate. This also requires scaling these values by the density.

## Multiphase incompressible solvers

All the consequences described in the previous section do not apply to multiphase solvers. In case of multiphase solvers density can not be directly removed from the equation, because each phase might be associated with different density. Thus, the pressure and the forces are expressed in [Pa] and [N].

## Pressure is relative

The pressure in incompressible Navier-Stokes equation is present only under the gradient:

$\frac{\partial \mathbf{u}}{\partial t}+(\mathbf{u} \cdot \nabla)\mathbf{u} = -\nabla p_k + \nu \cdot \Delta \mathbf{u}$

where $$p_k = \frac{p}{\rho_{ref}}$$ is kinematic pressure.

There is no additional equation bounding pressure with other variable (e. g.: gas state equation). Therefore, there is no bounds for the pressure value. Solving N-S equation will provide information on pressure distribution, but not its exact value. It is irrelevant if pressure is equal 1[bar] or 1[Pa] as long as pressure difference between the same points is the same. A good analogy is integration constant. We can integrate differential equation with respect to integration constant, because when we re-apply the result under derivatives the constant will cancel out.

### Add any constant to the result

The consequence of the above is a fact that we can add any constant value to the pressure result. It is very common to specify pressure value at the outlet to be equal 0. In this situation, we can read the pressure result as a gauge pressure, relative to unknown ambient pressure. We are free to add any constant value (1 bar for instance) at the postprocessing step.

### Reference Pressure

There is one more implication for the fact that pressure result is relative. The exact result is unspecified, because infinite number of pressure fields can satisfy N-S equation. Usually when we specify boundary conditions we enforce pressure at the inlet or outlet (it can be fixed to 0 value). Fixing pressure at the boundary constraints pressure value, and thus result is unique in numerical sense (by analogy to integration the boundary condition is additional information allowing to compute integration constant).

Situation is slightly different when all the boundaries of the fluid domain are walls. Typical pressure boundary condition at the wall is “Zero Gradient” ($$\vec{n} \cdot \nabla p = 0$$), which does not apply constraint to pressure value. The resultant pressure equation is singular, and there is no unique numerical solution to it. To be able to solve such equation and find pressure distribution, we must provide pressure constraints by other means. One approach is to enforce pressure to be equal to specific value in particular point in space. In SimFlow you can specify Reference Pressure value and location under the Operating Conditions panel.

## List of Solvers

These rules are applicable for the incompressible single-phase solvers:

• Buoyant Boussinesq SIMPLE
• Overset Laplacian Dynamic Mesh
• Overset SIMPLE
• SIMPLE
• SRF SIMPLE

Transient Solvers

• Buoyant Boussinesq PIMPLE
• DPM
• DPM Dynamic Mesh
• Ico
• Overset Laplacian Dynamic Mesh
• Overset PIMPLE Dynamic Mesh
• PIMPLE
• PISO
• SRF SIMPLE 