17.6.2.1. Pressure

A Pressure load applies a constant pressure or a varying pressure in a single direction (x, y, or z) to one or more flat or curved faces. A positive value for pressure acts into the face, compressing the solid body.

Note:  You can add a Pressure load during a Solution Restart. By default, the application sets the Applied By property to Direct.

This page includes the following sections:

Analysis Types

Pressure is available for the following analysis types:

Note:  Eigen response (an Eigenvalue Buckling Analysis or a Modal Analysis) and Harmonic Response (Full) analyses take into account any pressure load stiffness contribution applied in a linked Static Structural analysis.

Dimensional Types

The supported dimensional types for the Pressure boundary condition include:

  • 3D Simulation. For 3D simulations, a Pressure load applies a pressure to one or more faces.

  • 2D Simulation. For 2D simulations, a Pressure load applies a pressure to one or more edges.

Geometry Types

The supported geometry types for Pressure include:

  • Solid

  • Surface/Shell

  • Wire Body/Line Body/Beam

Topology Selection Options

The supported topology selection options for the Pressure boundary condition include:

  • Face: Supported for 3D only. If you select multiple faces when defining the pressure, the same pressure value gets applied to all selected faces. If a constant pressurized face enlarges due to a change in CAD parameters, the total load applied to the face increases, but the pressure (force per unit area) value remains constant.

  • Edge: Supported for 2D only. If you select multiple edges when defining the pressure, the same pressure value gets applied to all selected edges.

  • Nodes. Not supported for Harmonic Response analysis. When you scope to nodes, the load behaves as a Nodal Pressure and follows all of the requirements of that loading condition.

  • Element Face: Supported for 3D only.

  • Element

Considerations for Face and Edge Scoping

Keep the following in mind when using Face and Edge scoping:

  • You cannot apply a single Pressure load on multiple edges of different surface bodies when the bodies include both a 3D surface body and a 2D surface body.

  • 3D Faces or 2D Edges automatically update their direction at each substep and "follow" the changing normal for large deflection analyses.

Define By Options

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

  • Components

  • Vector. While loads are associated with geometry changes, load directions are not.

    Note:  The Components and Vector options apply pressure in a constant direction and as a result do not contribute to any pressure load stiffness.

  • Normal To (default)

  • Normal To: Real - Imaginary: Supported for Harmonic Response analysis only.

  • Vector: Real - Imaginary: Supported for Harmonic Response analysis only.

  • Components: Real - Imaginary: Supported for Harmonic Response analysis only.

Applied By Options (Mechanical APDL solver only)

When you are using the Mechanical APDL solver, the Pressure boundary condition also displays the Applied By property for all of the above Define By options. Applied By has two options:

Surface Effect

(Default for non-Mode Superposition.) The Surface Effect option applies pressure using the surface effect elements created on the top of the scoped geometry.

Direct

(Default for Mode Superposition and when a crack is defined under the Fracture folder.) In 3D analyses, the Direct option applies pressure directly onto the faces of solid or shell elements. In 2D analyses, the Direct option applies pressure directly onto the edges of plane elements.

Considerations and Limitations for the Applied By Options

Keep the following in mind when you specify the Surface Effect and Direct options for Applied By:

  • If you scope two Pressure objects to the same geometry, and specify the loads in the same direction, using the Direct option, the pressures do not produce a cumulative loading effect. The Pressure object that you specified last takes priority and is applied, and as a result, the application ignores the other Pressure object.

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

  • A pressure applied using the Surface Effect option and a pressure applied with the Direct option produce a resultant effect.

  • When you scope a Pressure to a solid body as well as a shell body, the application does not display the annotation arrow for the loading direction (via the Direction property).

  • During a structural analysis, you can also create a spatially varying load using the Vector type option. A spatially varying load allows you to define the pressure in tabular form or as a function.

  • If your analysis includes some combination of a Pressure, a Force, and a Hydrostatic Pressure load, and 1) all are set to the Direct option and 2) share the same scoping, 3) have the same Direction, whichever load was written to the input file last, overwrites all previous loads.

  • If you have a Nodal Force and a Pressure applied using the Direct option and they share the same scoping, they produce a resultant loading effect.

  • Applying a Pressure load Normal To faces (3D) or edges (2D) could result in a pressure load stiffness contribution that plays a significant role in analyses that support pre-stress (Pre-stressed Full Harmonic, Pre-stressed Modal, and Eigenvalue Buckling) because they use the Static Structural Solution as a starting point.

Note the following limitations on using the Direct option for the Applied By property when the Define By property is set to Vector or Components:

  • Not supported for vertices and edges of Solid bodies and Line Bodies.

  • Not supported on bodies associated with Condensed parts.

  • Not supported if the model has any crack defined under the fracture folder.

  • Not supported if the analysis includes a Nonlinear Adaptive Region object and 1) the Loaded Area property is set to Initial and 2) the Large Deflection property (Analysis Settings > Solver Controls) set to On.

  • In a multiple step analysis, if you define more than one load (Pressure, Force, or Hydrostatic Pressure) using the Direct option and a Nodal Pressure, and they share the same scoping, deactivation of a particular load step in one of these loads could delete all the other loads in that load step and following steps.

Magnitude Options

The Magnitude options for Pressure include:

  • Constant

  • Tabular (Time Varying)

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

  • Tabular (Harmonic Index Varying): Supported for Harmonic Response (Full) analysis only when a Cyclic Region object is defined. By default, at least two harmonic index entries are required when defining a Harmonic Index dependent tabular load.

  • Tabular (Sector Number): Supported for Harmonic Response (Full) analysis only when a Cyclic Region is defined. By default, at least two entries are required to define a dependent tabular load.

  • Tabular (Frequency Varying): Supported for Harmonic Response analysis only. By default, at least two frequency entries are required when defining a frequency dependent tabular load. The Pressure boundary condition in a Harmonic Response (Full, linked MSUP, or standalone) can be defined in such a way that it is fully frequency dependent. That is, the magnitude of the load as well as the Phase Angle of the load can be dependent upon the frequency definitions.

  • Tabular (Spatially Varying)

  • Function (Time Varying)

  • Function (Spatially Varying)

    Note:  Harmonic Response Analysis only: Spatially varying Tabular and Function data is supported for the Normal To and Normal To: Real-Imaginary loading types. The Phase Angle property supports Spatially varying Tabular definition but does not support Function definition.

  • Table Name: Supported for the Mechanical APDL solver only. A multi-variable table of numeric values that defines the pressure distribution for the selection. The Magnitude field automatically lists the names of all tables that contain pressure or pressure components as dependent variables.

  • New Table : Supported for the Mechanical APDL solver only. Select this option to create a new multivariable table of pressure or pressure component values. You can then assign this table as the Magnitude.

Applying a Pressure Boundary Condition

To apply a Pressure:

  1. Select the Pressure option from the Environment Context tab. Alternatively, right-click the Environment tree object or in the Geometry window and select Insert>Pressure.

  2. Define the Scoping Method. Options include Geometry Selection, Named Selection, and Crack Growth. Based on your selection, specify a geometry or select a SMART Crack Growth option from the drop-down list of the Crack Growth property.

  3. Specify the Define By property. Options include:

    • Components

    • Components: Real – Imaginary (Harmonic Response only)

    • Vector

    • Vector: Real – Imaginary (Harmonic Response only)

    • Normal To (default)

    • Normal To: Real – Imaginary (Harmonic Response only)

  4. Specify the Applied By property as needed: Surface Effect (default non-Mode Superposition) and Direct (Mode Superposition default).

  5. Specify the Loaded Area property as needed: options include Deformed (default) and Initial.

  6. Based on your Define By property selection, specify the following additional properties as required:

    • Magnitude (including component magnitudes)

    • Check the box next to Magnitude to parameterize the magnitude.

    • Direction

    • Coordinate System

    • Graphics Controls

    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).

    • 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.

  7. 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

Scope

Scoping Method: Use this property to select a geometric entity, either through manual selection or using a Named Selection, or you can specify a SMART Crack Growth object. Options include Geometry Selection (default), Named Selection, and Crack Growth. Note that the Crack Growth option is only available when a SMART Crack Growth object is defined under the Fracture folder during a 3D Static Structural analysis.

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

Crack Growth: Visible when the Scoping Method is set to Crack Growth. This property provides a drop-down list of available SMART Crack Growth objects. This property enables you to apply the pressure to the new crack faces the application generates during the smart crack growth process or to these new crack faces in addition to the initial crack faces of the crack associated with the SMART Crack Growth object.

Shared Reference Body: This property is a scoping feature used to apply a Pressure to shared faces or edges between two bodies. When you have properly scoped the geometric entities, using either Geometry Selection or an appropriate Named Selection, the property provides a drop-down list of the names of the bodies that share the scoped features. By selecting a body from this list, you are specifying that the pressure be applied to its surface or edge. Once selected, the Geometry or Named Selection property displays a parenthetical of the shared face or edge, "1 Shared Face/1 Shared Edge," to indicate the condition.

Note:

  • When working with the shared edges of a 2D model, the Applied By property must be set to Direct.

  • Edges can be shared between a surface and line body, but the line body cannot be specified as the Shared Reference Body or the property becomes invalid.

Definition

Type: Read-only field that describes the object - Pressure.

Define By: Options include:

  • Normal To: Requires a Magnitude entry.

  • Normal To: Real - Imaginary (Harmonic Analysis only): Real and imaginary magnitude. Requires the specification of the following inputs:

    • Magnitude - Real

    • Magnitude - Imaginary

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

  • Vector: Real - Imaginary (Harmonic Analysis only): Real and imaginary magnitude and direction (based on selected geometry). Requires the specification of the following inputs:

    • Magnitude - Real

    • Magnitude - Imaginary

    • Direction

  • 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.

    • X Phase Angle (Harmonic Analysis only)

    • Y Phase Angle (Harmonic Analysis only)

    • Z Phase Angle (Harmonic Analysis only)

    Note:  Selection of a Coordinate System rotated out of the global Cartesian X-Y plane is not supported in a 2D analysis.

  • Components: Real - Imaginary (Harmonic Analysis only): Option to define the loading type as real and imaginary 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 - Real: Defines magnitude (Real) in the X direction.

    • X Component - Imaginary: Defines magnitude (Imaginary) in the X direction.

    • Y Component - Real: Defines magnitude (Real) in the Y direction.

    • Y Component - Imaginary: Defines magnitude (Imaginary) in the Y direction.

    • Z Component - Real: Defines magnitude (Real) in the Z direction.

    • Z Component - Imaginary: Defines (Imaginary) magnitude in the Z direction.

Applied By: (Mechanical APDL solver only.) This property defines how the load is applied, either by creating surface effect elements or by direct application on the scoped geometry. Options include:

  • Surface Effect: Default option for all analyses except Mode Superposition analyses.

  • Direct: Default option for Mode Superposition analyses and when solution restart points are available.

Loaded Area: Options include Deformed (default) and Initial. The Initial option treats the scoped surface area as a constant throughout the analysis. For the Deformed option, the application incorporates the change in the surface area as a result of deformation throughout the analysis. The selection for this property can be of significance during large deflection problems.

Apply To: Visible when the Scoping Method is set to Crack Growth. Options include:

  • New Crack Faces Only (default): Select this option to apply a normal pressure load to the new crack faces the application generates during the smart crack growth process.

  • Both Initial and New Crack Faces. Select this option to apply a normal pressure load to new crack faces as well as the initial crack faces of the crack associated with the SMART Crack Growth object.

    Important:

    • For all analytical cracks, such as Pre-Meshed Crack, Arbitrary Crack, etc., the application highlights the nodes from the initial crack top face and bottom face components for either of the Apply To property options. However, for the New Crack Faces Only option, even though the application highlights the nodes of the initial crack faces, the application only applies the load to the new crack faces generated during crack growth.

    • When you scope the Initial Crack property of a SMART Crack Growth object to a Crack Initiation object, the application does not highlight any nodes.

    Note:  If you apply a Pressure to the initial crack faces using the Both Initial and New Crack Faces option and another Pressure is scoped to the crack face Named Selections or the nodes belonging to these named selections, they do not produce a cumulative effect. The Pressure object that you specified last takes priority and is applied. As a result, the application ignores the other Pressure applied on these crack face named selections.

Non-Cyclic Loading Type: This property is available for a Full Harmonic Response analysis when a Cyclic Region is present in the model. Options include:

  • No (default). The loading is purely cyclic. That is, the load applied to the base sector is applied to each and every sector.

  • Harmonic Index. The non-cyclic loading can be specified for one or more harmonic indices. This is also known as "engine-order loading" (or traveling wave excitation). A Harmonic Index entry is required.

  • Sector Number: This property enables you to select the desired Sector onto which you apply the non-cyclic load.

Important:  When you specify the load as Tabular, the Independent Variable property displays and is set to Harmonic Index by default. The Harmonic Index property is hidden as their values are entered in the table.

Harmonic Index: This property displays when the Non-Cyclic Loading Type property is set to Harmonic Index. Where NS is Number of Sectors, enter a value from:

1 to NS/2; if NS is even.
1 to (NS-1)/2; if NS is odd.

Sector Number: This property displays when the Non-Cyclic Loading Type property is set to Sector Number. You use this property to specify the desired sector onto which you want to apply the non-cyclic load. If you choose Tabular for the Magnitude property, you can then set the Independent Variable property to Sector Number and then specify your loading using the Tabular Data window.

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

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.

Pressure Table Options (Mechanical APDL solver only)

If you selected the name of a table under Magnitude to define the pressure load on the boundary, the following options are available.

  • Parameterization: Check the box next to Magnitude to parameterize the table.

  • Spatial Coordinate System (read only)

  • Graphics Controls (if applicable)

For details, see Specify Pressure Loads with Tables.

Mechanical APDL References and Notes

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

  • When you set the Applied By property to Surface Effect, the Pressure is applied as a surface load through the surface effect elements using the SF or SFE command using the SURF154 (3D) and SURF153 (2D) element types.

  • When you set the Applied By property to Direct, a Pressure is applied directly on to the element faces using the SFCONTROL and SFE ,,PRES commands. Refer to SFCONTROL command for a list of supported solid elements, shell elements, and plane-2D elements.

  • When using a SMART Crack Growth object as the scoping method, the application uses the CGROW,CSFL,PRES command to apply a pressure to the new crack faces generated during crack growth.

  • Magnitude (tabular and function) is always represented as a table in the input file.

  • A table is a special type of numeric array that enables the Mechanical APDL solver to calculate (through linear interpolation) the values between entries in a multi-dimensional table of numeric data. The solver applies these interpolated values across the selected geometry when it computes the solution. See the discussion in Array Parameters.

API Reference

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