Nodal pressure loads (Nastran and ANSYS)

In the Nastran and ANSYS environments, you can use the Nodal Pressure command to define the pressure that acts at nodes.

With the Normal Pressure command, you may be able to account for:

• Surface tractions that contain both normal and in-plane components.

• Pressure distributions that vary spatially.

This graphic shows a spatially varying pressure distribution in the Nastran environment.

Nodal pressure loads in Nastran analyses

In the Nastran environment, you can use the Nodal Pressure command to define the pressure that acts on the faces of shell and solid elements, and the edges of plane strain, plane stress, and axisymmetric elements. The Nodal Pressure command corresponds to the Nastran PLOAD4 bulk entry when applied to shell or solid element faces, the Simcenter Nastran PLOADE1 bulk entry when applied to plane strain or plane stress element edges, and the Simcenter Nastran PLOADX1 bulk entry when applied to axisymmetric element edges.

You can use the Nodal Pressure command to apply a pressure load to the faces of the following shell elements:

• CQUAD4

• CQUAD8

• CQUADR

• CTRIA3

• CTRIA6

• CTRIAR

You can use the Nodal Pressure command to apply a pressure load to the faces of the following solid elements:

• CHEXA

• CPENTA

• CPYRAM

• CTETRA

You can use the Nodal Pressure command to apply a pressure load to the edges of the following plane strain and plane stress elements:

• CPLSTN3

• CPLSTN4

• CPLSTN6

• CPLSTN8

• CPLSTS3

• CPLSTS4

• CPLSTS6

• CPLSTS8

You can use the Nodal Pressure command to apply a pressure load to the edges of the following axisymmetric elements:

• CQUADX4

• CQUADX8

• CTRAX3

• CTRAX6

When you solve the model, the software uses the value of the pressure at the corner nodes to compute the magnitude and direction of the equivalent nodal forces. The exceptions to this are the CPLSTS6 and CPLSTS8 elements. For these elements, the software uses the value of the pressure at the corner nodes and the midside nodes to compute the magnitude and direction of the equivalent nodal forces.

For more information, see:

• PLOAD4 in the Simcenter Nastran User’s Guide

• PLOAD4 in the Simcenter Nastran Quick Reference Guide.

• PLOADE1 in the Simcenter Nastran Quick Reference Guide.

• PLOADX1 in the Simcenter Nastran Quick Reference Guide.

Nodal pressure loads in ANSYS analyses

In the ANSYS environment, you can use the Nodal Pressure command to define both a standard pressure load on the face of selected elements or a tapered surface load. In a tapered surface load, you can assign different pressure values to each node of an element. In the ANSYS environment, the options in the Nodal Pressure dialog box correspond to the ANSYS SFE,,PRES command.

For more information, see SFE in the ANSYS Commands Reference.

Where do I find it?

Application	Pre/Post
Prerequisite	A Simulation file as the work part and displayed part and an active solutionSimcenter Nastran or ANSYS as the specified solver
Command Finder	Nodal Pressure
Simulation Navigator	Under the active solution, right-click Simulation Objects→New Load→Nodal Pressure

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Nodal pressure loads (Nastran and ANSYS), 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 } });