Fill out the form to download

Required field
Required field
Not a valid email address
Required field
Required field

  • Set up your own cloud-native simulation in minutes.

    • Documentation

    SimScale DocumentationSimulation SetupBoundary ConditionsPressure (Structural Analysis)

    Pressure (Structural Analysis)

    In the Pressure boundary condition, a distributed load is applied on a face (or set of faces). It is useful to model the loads applied through the surface in contact with fluids or other solids, where the resultant of the load is in the normal direction of the face.

    pressure boundary condition panel
    Figure 1: Pressure boundary condition panel for structural analysis

    The parameters of the boundary condition are:

    1. Pressure (P): The magnitude of the applied pressure. It can be a constant or variable value.
    2. Assignment: Set of faces where the pressure load will be applied.

    Supported Analysis Types

    The following analysis types support the usage of the pressure boundary condition:

    Resultant Force Magnitude and Direction

    The pressure load value (P) is defined in units of force (N, lb., etc.) per unit of surface area (m2, sq. in., etc), thus the total applied force depends on the total area of the assigned face (or set of faces):

    $$ F = P A \tag{1}$$

    For a positive pressure applied, the direction of the resulting force is opposite to the face-normal, i.e. it points inwards towards the solid region. A negative pressure value will result in a force pointing outwards in the direction of a face-normal.

    The statement above is valid in the case of a single planar face, or set of adjacent faces lying on the same plane. If the assigned faces are not planar or do not belong to the same plane, then the resulting force is computed taking into account the normal of each face in a vector sense:

    $$ \vec{F} = \Sigma( -P \vec{A}) = \Sigma (-P A \vec{n}) \tag{2}$$

    For curved faces, this turns into an integral statement with infinitesimal areas, and the normal of each mesh element is used to numerically compute the resulting force.

    Variable Pressure

    Variable pressure values can be specified with the use of the formula or table inputs. The allowed functions for pressure are:

    • Time-dependent: The pressure varies with respect to time (variable t) in a non-linear or dynamic simulation. This is useful for example to ramp up the load from zero in non-linear simulations, where a sudden application of load leads to numerical divergence, or in naturally time-varying loads for dynamic simulations.
    • Coordinate-dependent: The pressure varies with respect to the position in space (variables X, Y, Z). This is useful, for example, in the case of hydrostatic pressure, where the load varies with respect to height.

    It is important to know that in coordinate dependent functions, the variables X, Y, and Z refer to the coordinates in the original, undeformed configuration. Thus, this feature can not be used to model deformation-dependent pressure functions (for example, contact with a spring).

    Case of Large Deformations

    For large deformations, as those allowed in non-linear or dynamic simulations, the normal directions of the assigned faces are subject to change. In that case, the resulting load will always keep the original direction computed in the undeformed configuration. Thus, the usage of the Pressure boundary condition might not yield correct results.

    If you need the applied force direction to be updated with the deformed configuration of the solid, please use the follower pressure boundary condition.

    An example of the pressure boundary condition applied on a thick plate can be seen below:

    von mises stress color plot of thick plate under pressure
    Figure 2: Stress contour on a thick plate under pressure load.

    Last updated: October 30th, 2023

    Contents