17.6.5.3. Nodal Pressure

Using Nodal Pressure, you can apply pressure on element faces. You must create a node based named selection before you can apply a Nodal Pressure. It is applicable for solid and surface bodies only. Specifically, an elemental face pressure is created only if all of the nodes of a given element face (including midside) are included. If all nodes defining a face are shared by an adjacent face of another selected element, the face is not free and will not have a load applied.

Warning:  For application to surface bodies, the Mechanical APDL solver logic for this load is such that if all of the nodes of a shell element are specified, then the load is applied to the whole element face. However, if only some nodes are specified on an element and those nodes constitute a complete external edge, then an edge pressure is created. Therefore, it is critical that you make sure that you have not selected nodes that constitute only a free shell edge. This is because shell edge pressures are input on a per-unit-length basis, and Mechanical treats this load always as a per-unit-area quantity. For more information, see the SHELL181 Element Description.

Nodal Pressures applied to shell bodies act in the opposite direction of geometry-based pressures.

Note:  A Nodal Pressure may be added during Solution Restart without losing the restart points.

This page includes the following sections:

Analysis Types

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

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

  • 3D Simulation

  • 2D Simulation

Geometry Types

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

  • Solid

  • Surface/Shell

Topology Selection Options

The Nodal Pressure boundary condition is scoped via node-based Named Selections only. For more information, see the Specifying Named Selections by Direct Node Selection Help section.

Note:  The Nodal Pressure boundary condition supports spatially varying loading on the scoped nodes for Static and Transient analyses only. For Eigenvalue Buckling and Harmonic Response analyses, only constant loading conditions are supported.

Applying a Nodal Pressure Boundary Condition

To apply a Nodal Pressure:

  1. On the Environment Context tab, click Direct FE > Nodal Pressure. Alternatively, right-click the Environment tree object or in the Geometry window and select Insert>Nodal Pressure.

  2. Click the Named Selection drop-down list, and then select the node-based Named Selection to prescribe the scope of the Nodal Pressure.

  3. Enter a magnitude for the load.

Details Pane Properties

The Details pane selections are described below.

CategoryProperty/Options/Description
Scope

Scoping Method: Read-only field that displays scoping method - Named Selection.

Named Selection: Drop-down list of available node-based Named Selections.

Definition

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

Define By: Read-only field that displays that the boundary condition is acting Normal To the surface to which it is attached.

Magnitude: Input field to define the magnitude of the boundary condition. This value can be defined as a Constant, in Tabular form as a function of Time or Step (Static Structural only), or as a Function.

Note:  Spatially varying loading (Tabular/Function) is supported for Static and Transient analyses only. For Eigenvalue Buckling and Harmonic Response analyses, only constant loading conditions are supported.

Suppressed: Includes or excludes the boundary condition in the analysis.

Load Vector Controls (Substructure Generation Analysis Only)

Load Vector Assignment: Options include Program Controlled (default) and Manual. When set to Manual, the Load Vector Number property displays.

Load Vector Number: Specify a Load Vector Number using any value greater than 1. A setting of 1 is reserved for a pre-stress Substructure Generation analysis. If multiple loads have the same Load Vector Number, the application groups these loads during the solution process to generate a single load vector that is the combined effect of all grouped loads.

Note:

  • To apply a node-based pressure, the named selections that you create must include nodes such that they define an element face.

  • Two Nodal Pressure objects that have the same scoping do not produce a cumulative loading effect. The Nodal Pressure object that was specified last takes priority and is applied, and as a result, the other Nodal Pressure object is ignored.

  • A load applied to a geometric entity and a Nodal Pressure produce a resultant effect.

  • You can apply a spatially varying Nodal Pressure to scoped nodes.

  • If a Nodal Pressure and a Direct Pressure, Direct Force, or Direct Hydrostatic Pressure share the same scoping, the Nodal Pressure always takes priority regardless of insertion order: Mechanical will ignore the Direct Pressure, Direct Force, and Direct Hydrostatic Pressure.

Mechanical APDL References and Notes

For more information on the solver representation of this load, reference the SF command in the Mechanical APDL Command Reference.

API Reference

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