Pressure Inlet and Pressure Outlet

Pressure inlet and outlet conditions are typically assigned in computational fluid dynamic analysis (CFD), at the opposite end of the model to a flow rate or a different pressure.

Here are a couple of typical examples of combinations that are used:

Flow Driven Analyses

In those cases where we know the flow rate conditions, the recommended boundary condition combinations for the inlet and outlet region are the following:

Pressure Driven Analyses

In those cases where we know the pressure conditions, the recommended boundary condition combinations for the inlet and outlet region are the following:

Pressure Inlet

The pressure inlet boundary condition defines an inflow condition based on the known pressure value (P) at the boundary. It is used when no flow rate is known, or if a flow rate (or velocity) is assigned at the outlet.

The turbulent flow quantities are matched with the values specified for the Initial Conditions and are thus not required as inputs.

Pressure Outlet

The pressure outlet boundary condition defines an outflow condition based on the flow pressure $P$ at the outlet. This is usually used when there is a flow rate (or velocity), or a higher pressure assigned at the inlet.

All relevant unknown flow quantities e.g. temperature in case of compressible flow, and other quantities including turbulence, are calculated from the interior of the domain with gradients of the quantities fixed to zero value.

Pressure Inlet and Outlet Input Methods

The pressure values at the inlet and the outlet can be assigned using the following types:

1. Total pressure (inlet only)
2. Fixed (inlet and outlet)
3. Mean (outlet only)

These three types are described in detail below:

1. Total Pressure

The total pressure expression, defined by velocity vector U and density $\rho$:

$$\begin{array}{}\text{(1)}& p=p_0–0.5\rho |\overrightarrow{U}{|}^2\end{array}$$

Under certain conditions, the user might need to specify a parameter Gamma $(\gamma )$ which is used in transonic and supersonic cases.

The pressure $p$ is calculated at the boundary based on the fixed total pressure $p_0$ that must be specified. The velocity $U$ and static pressure $p$ are adjusted accordingly until they converge to a stable configuration.

Additionally, the user can also input values in the form of a table by uploading a .csv file or entering the values manually. The following figure highlights the icon which serves this purpose.

Correct dependencies should be chosen. In this case, the uploaded file contains values that are dependent on time only.

2. Fixed Value

This prescribes the pressure value on a certain boundary of the domain. This value could be constant or dependent on time and/or space coordinates. Either static or gauge pressure can be used depending on the analysis type.

Similar to the Total pressure input value, the Fixed value option also allows you to input a table. In this case, the uploaded file contains values that are dependent on time or space coordinates.

3. Mean Value

This is only used at an outlet where it is not clear that flow passes over the boundary uniformly. The average pressure over the boundary would equal this assigned value. Unlike the fixed value, not every region on the boundary needs to have the same value.

Turbulence

SimScale allows for the definition of turbulence at the velocity inlet. The user has three options to choose from.

• Automatic
• Turbulent intensity and mixing length
• Fixed Value

The values can either be fixed or driven by a formula or a table for space or time-dependent conditions.

1. Automatic

When automatic is assigned a fixed turbulence value of 5 $$ is chosen for the turbulent intensity $(I)$. The turbulent mixing length $(L)$ is calculated as 0.07 $(D_h)$, where  $(D_h)$ is the hydraulic diameter of the boundary face.

2. Turbulent Intensity and Mixing Length

When the Turbulent intensity and mixing length option is selected, the user can specify the turbulent intensity $(I)$ and the turbulent mixing length $(L)$.

3. Turbulence Fixed Value

Fixed Value allows the user to directly specify the turbulent kinetic energy in $[\frac{m^2}{s^2}]$ and the specific dissipation rate $[\frac{1}{s}]$.

Modified Pressure

The modified pressure, also known as non-hydrostatic pressure, is used for the boundary condition definition in analysis types that take buoyancy effects into account. The formula below shows the correlation between the modified static pressure $p_{rgh}$ and the static pressure $p$:

$$\begin{array}{}\text{(2)}& p_{rgh}=p–\rho gh\end{array}$$

In equation 2, $\rho$ is the density of the fluid, $g$ is gravity, and $h$ is the height of the column of the fluid. Combined, the $\rho gh$ term represents the hydrostatic pressure.

The following analysis types use modified pressures in the definition of boundary conditions:

• Convective heat transfer
• Conjugate heat transfer v2.0
• Conjugate heat transfer (IBM)
• Multiphase

Hydrostatic Pressure (Multi-purpose)

This feature allows applying a hydrostatic pressure profile at pressure inlet and outlet boundary conditions in Multi-purpose analysis type when gravity magnitude is non-zero. The following formula shows how hydrostatic pressure $P_h(\overrightarrow{x})$ is calculated at each boundary:

$$\begin{array}{}\text{(3)}& P_h(\overrightarrow{x})=P–\rho (\overrightarrow{x})\overrightarrow{g}\cdot \left(\overrightarrow{x}–\frac{\overrightarrow{g}}{|\overrightarrow{g}|}{h}_{\text{ref}}\right)\end{array}$$

Where $P$ is the static pressure, $\overrightarrow{g}$ is the the gravity vector, $\overrightarrow{x}$ is the position vector and $h_{ref}$ is the reference height where hydrostatic pressure is equal to the static pressure. Both $\overrightarrow{x}$ and $h_{ref}$ are with respect to the global coordinate system.

In the user interface, after selecting the pressure inlet or pressure outlet boundary condition, you can enable hydrostatic pressure with a toggle. If activated, you must specify a reference height ($h_{\text{ref}}$, default 0 $m$).

Parametric Studies with Pressure Conditions

Users can sweep through different pressure levels using SimScale’s parametric experiment capabilities. To learn more about this capability, make sure to check this article:

How to Run Parametric Studies in SimScale?

Last updated: April 21st, 2025