Pressure dialog box (Nastran)

Type
Type	Specifies how the pressure load is defined.Normal pressure on 2D elements or 3D element facesDefines a pressure load normal to element faces.If you use a spatially varying field or expression to define the magnitude of the pressure load, Simcenter 3D evaluates the intensity of the pressure load at the centroid of the 2D element or the 3D element face and writes it to the P1, P2, P3, and P4 fields of the PLOAD4 bulk entry.Normal pressure on 2D elementsDefines a pressure load normal to 2D element faces.If you use a spatially varying field or expression to define the magnitude of the pressure load, Simcenter 3D evaluates the intensity of the pressure load at the centroid of the 2D element and writes it to the P field of the PLOAD2 bulk entry.Note: Do not apply this type of pressure load to 3D elements.On 2D Solid Elements (Normal to Edge) ZX, On 2D Solid Elements (Normal to Edge) XYDefines a pressure load normal to edges of elements in the axisymmetric ZX or XY plane. The option distributes the pressure to all elements (both sides) that share the polygon edge.If you use a spatially varying field or expression to define the magnitude of the pressure load, Simcenter 3D evaluates the intensity of the pressure load at the mid-span of the element edge and writes it to both the PA and PB fields of the PLOADX1/PLOADE1 bulk entry.On 2D Solid Elements ZX, On 2D Solid Elements XYDefines a pressure load by specifying values for the radial and axial component pressures.If you use a spatially varying field or expression to define the magnitude of the pressure load, Simcenter 3D evaluates the intensity of the pressure load at the mid-span of the element edge and writes it to both the PA and PB fields of the PLOADX1/PLOADE1 bulk entry.ComponentsDefines a pressure load in terms of a global or local coordinate system. For example, if you choose a local Cartesian coordinate system, you can enter pressure magnitude for each of the X, Y, and Z components.If you use a spatially varying field or expression to define the magnitude of the pressure load, Simcenter 3D evaluates the intensity of the pressure load at the centroid of the 2D element or the 3D element face and writes it to the P1, P2, P3, and P4 fields of the PLOAD4 bulk entry.On beamsDefines a pressure load on beam elements in terms of either the global coordinate system or the element coordinate system.If you use a spatially varying field or expression to define the magnitude of the pressure load, Simcenter 3D evaluates the intensity of the pressure load at the mid-span of the beam element and writes it to both the P1 and P2 fields of the PLOAD1 bulk entry.
Destination Folder
Load Container	Specifies the folder in the Simulation Navigator in which the boundary condition will be stored. The list includes the root container and existing folders that you created using the New Folder command. Examples of a root container include Load Container, Constraint Container, and Simulation Object Container.
Folder Manager	Displays a hierarchical listing of existing folders. To create a new folder, right-click any level of the hierarchy and choose New Folder.
Model Objects
Group Reference	Lets you apply the pressure load to a group.For more information, see Group Reference options.
Select Object	Lets you select the geometry or FE entities on which to apply the load. ExcludedLets you remove individual entities from within your selected object.
Stacked Smart Selector Methods	Opens the Smart Selector Methods dialog box where you can specify a progression of smart selection filters.For more information, see Smart Selector Methods dialog box.
Magnitude
Pressure	Appears when Type is set to Normal pressure on 2D elements or 3D element faces or Normal pressure on 2D elements.Specifies the magnitude of the pressure load. For more information, see Additional magnitude options.
Method	Appears when Type is set to On 2D Solid Elements (Normal to Edge) ZX or On 2D Solid Elements (Normal to Edge) XY.Defines how the magnitude of the pressure load is specified.PressureLets you specify the load applied with pressure units.Total ForceLets you specify the load applied with force units.The software calculates the pressure by distributing the total load over the area defined by revolving the edge 360° about the axisymmetric axis.
Normal Pressure	Appears when Method is set to Pressure.Specifies the magnitude of the pressure load.
Normal Force	Appears when Method is set to Total Force.Specifies the magnitude of the normal force load.
Direction
Appears when Type is set to Components.
CSYS	Sets the coordinate system that the software uses to apply the pressure load. You can select the Global Cyclic Analysis or the Global coordinate system, or you can create one of the following types of local coordinate systems: Cartesian, Cylindrical, Spherical.Note: The Global Cyclic Analysis coordinate system is available only if it is defined in the FEM.
Properties
Appears when Type is set to On beams.
Scale, X1, X2	These are display-only boxes that you cannot edit. They indicate how the Scale, X1, and X2 fields of the PLOAD1 bulk entry are specified in the Simcenter Nastran input file.For more information, see PLOAD1 in the Simcenter Nastran Quick Reference Guide.
Components
Appears when Type is set to Components or On beams.
Magnitude	Specifies the magnitude of the pressure load.
Px, Py, Pz****Pr, Pt, Pz****Pr, Pt, Pp	Appears when Magnitude is set to Expressions.Specifies the pressure magnitude for each component. The available components depend on the coordinate system type.
Specify Field	Appears when Magnitude is set to Field.Lets you select or define a field to define pressure magnitude.
Scale Factors	Appears when Magnitude is set to Field.Specifies the scale factor to apply to the field for each component.The available components depend on the coordinate system type.
Appears when Type is set to On 2D Solid Elements ZX or On 2D Solid Elements XY.
Radial Pressure	Lets you specify the magnitude of the pressure in the radial direction.
Axial Pressure	Lets you specify the magnitude of the pressure in the axial direction.

How do I

Define a pressure load normal to 2D elements or 3D faces

Define a pressure load using components

Define a pressure load on beams

Define a pressure load normal to 2D solid elements

Define a pressure load using radial and axial components

Learn more

Pressure

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Pressure dialog box (Nastran), Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });