17.6.2.12. Line Pressure

For 3D simulations, a Line Pressure load applies a distributed force using force density loading in units of force per length. You can define force density as a vector, an axial component, or tangentially. Tangential loads can be applied to one edge only whereas vector and component loads and can be applied to one or more edges.

If a pressurized edge enlarges due to a change in CAD parameters, the total load applied to the edge increases, but the pressure (force per unit length) remains constant.

This page includes the following sections:

Analysis Types

Line Pressure is available for the following analysis types:
Dimensional Types

The supported dimensional types for the Line Pressure boundary condition include:

  • 3D Simulation

Geometry Types

The supported geometry types for the Line Pressure boundary condition include:

  • Solid

  • Surface/Shell

  • Wire Body/Line Body/Beam

Topology Selection Options

The supported topology selection options for Line Pressure include:

  • Edge

Define By Options

The supported Define By options for the Line Pressure boundary condition include:

  • Vector

    The vector load definition displays in the Annotation legend with the label Components. The Magnitude and Direction entries, in any combination or sequence, define these displayed values. These are the values sent to the solver.

  • Tangential: Supported (scoped to one edge only).

  • Components

Magnitude Options

The supported Magnitude options for Line Pressure include the following:

  • Constant. This is the only option supported for Explicit Dynamics.

  • Tabular (Time Varying)

  • Tabular (Step Varying): Supported for Static Structural analysis only.

  • Tabular (Spatially Varying): Supported for Tangential loading only.

  • Function (Time Varying)

  • Function (Spatially Varying): Supported for Tangential loading only.

Applying a Line Pressure Boundary Condition

To apply a Line Pressure:

  1. On the Environment Context tab, open the Loads drop-down menu and select Line Pressure. Alternatively, right-click the Environment tree object or in the Geometry window and select Insert>Line Pressure.

  2. Define the Scoping Method as either Geometry Selection or Named Selection and then specify the geometry.

  3. Select the method used to define the Line Pressure: Vector (default), Tangential, or Components.

  4. Define the Magnitude, Coordinate System, and/or Direction of the Line Pressure based on the above selections.

    Note:  The Direction property is not associative and does not remain joined to the entity(s) selected for its specification. Therefore, this direction is not affected by geometry updates, part transformation, or the Configure tool (for joints).

  5. For Harmonic analyses, specify a Phase Angle as needed.

Details Pane Properties

The selections available in the Details pane are described below.

CategoryProperty/Options/Description
ScopeScoping Method: Options include:

  • Geometry Selection: Default setting, indicating that the boundary condition is applied to a geometry or geometries, which are chosen using a graphical selection tool.

    • Geometry: Visible when the Scoping Method is set to Geometry Selection. Displays the type of geometry (Body, Face, etc.) and the number of geometric entities (for example: 1 Body, 2 Edges) to which the boundary has been applied using the selection tools.

  • Named Selection: Indicates that the geometry selection is defined by a Named Selection.

    • Named Selection: Visible when the Scoping Method is set to Named Selection. This field provides a drop-down list of available user-defined Named Selections.

Definition

Type: Read-only field that displays boundary condition type - Line Pressure.

Define By, options include:

  • Vector: A magnitude and direction (based on selected geometry). Requires the specification of the following inputs:

    • Magnitude

    • Direction

  • Tangential (scoped to one edge only)

  • Components: Option to define the loading type as Components (in the Global Coordinate System or local coordinate system, if applied). Requires the specification of at least one of the following inputs:

    • Coordinate System: Drop-down list of available coordinate systems. Global Coordinate System is the default.

    • X Component: Defines magnitude in the X direction.

    • Y Component: Defines magnitude in the Y direction.

    • Z Component: Defines magnitude in the Z direction.

Phase Angle (Harmonic Analysis only).

Suppressed: Include (No - default) or exclude (Yes) the boundary condition.

Mechanical APDL References and Notes

The following Mechanical APDL commands, element types, and considerations are applicable for this boundary condition.

  • Line pressure is applied using the SFE command and the SURF156 element type.

  • Magnitude (constant, tabular, and function) is always represented as one or more tables in the input file.

API Reference

For specific scripting information, see the Line Pressure section of the ACT API Reference Guide.