Moment load

Use the Moment command to define a concentrated moment. Moments are applied in a node’s rotational degrees of freedom. A positive moment rotates in the direction of the element's connectivity according to the right hand rule.

Note:

One-dimensional elements, such as beams and bars, do not support moment loads along the axis.

You can define the magnitude of a moment as a constant value, an expression, or a field that defines how the moment varies with time, frequency or temperature.

Defining a follower moment in Nastran analyses

In the Simcenter Nastran and MSC Nastran structural environments, you can use the options in the Direction list in the Moment dialog box to use nodes to define the direction in which the moment acts. When you define the direction of a moment by selecting nodes, the direction of that moment can change as the model deforms. This means that the moment becomes a follower moment. A follower moment depends on a structure’s geometry. As a structure deforms, a follower moment changes in magnitude and direction.

• If you select Along 2 Nodes (MOMENT1), the software uses the two nodes you select to define the vector that the moment or moment acts along. With this option, the software creates a MOMENT1 bulk data entry in your Nastran input file when you export or solve your model.

• If you select Normal to 4 Nodes (MOMENT2), the software uses the four nodes you select nodes to define a plane normal. The moment acts normal to that plane. With this option, the software creates a MOMENT2 bulk data entry in your Nastran input file when you export or solve your model.

For more information, see MOMENT1 or MOMENT2 in the Simcenter Nastran Quick Reference Guide.

Defining a follower moment in Abaqus analyses

In the Abaqus environment, you can use the Follower check box in the Follower Moment Option group of the Moment dialog box to specify that the direction of a concentrated moment should rotate with the node to which you apply it. Use this option to include follower force or moment in your analysis.

The Follower check box corresponds to the FOLLOWER parameter for the *CLOAD keyword. For more information, see *CLOAD in the Abaqus Keywords Reference Guide and Concentrated Loads in the Abaqus Analysis Guide.

Defining a moment load on a solid mesh

Because solid elements do not support rotational degrees of freedom, consult the solver's specifications to determine the best approach for applying a moment to a solid mesh.

If you are using the Simcenter Nastran environment, you can apply a moment to a section that has an area by using RBE elements. For example, to apply a moment to a 3D mesh to find the bending moment of a cylinder, you create an additional node at the center of the top circular face and connect several 1D elements (for example, RBE2s) to the nodes on the top face. Then, add a moment load to the node that you just created at the center. For this example, we will assume that the opposite circular face at the bottom is fixed.

When you create the RBEs, make sure they project from this additional center node to all nodes on the polygon face, including the coincident node beneath the node on the mesh point.

When you check the FEM using the Model Check command, the following warning might appear:

WARNING Potential problems with the rigid links may exist in the model: - Rigid Links are connected to elements which do not have rotational degrees of freedom (DOF). This may result in solver errors. - Rigid Links connected to other rigid links. (Watch for rigid loops.) - Rigid Links not connected to other elements. If solver fails, check for inconsistent degrees of freedom.

The WARNING is being triggered because the RBE elements are connected to tetrahedral elements, which have no rotational degrees of freedom. However, as long as you connect the RBEs to all of the nodes on the face in the manner shown, there will not be a problem.

Where do I find it?

Application	Pre/Post
Prerequisite	A Simulation file as the work part and displayed part and an active solutionSimcenter Nastran, Abaqus, ANSYS, or Simcenter Samcef as the specified solver
Command Finder	Moment
Simulation Navigator	Right-click the Load container→New Load→Moment

How do I

Define a force or moment load using magnitude and a single direction

Define a force or moment load normal to the model

Define a force or moment load using components

Define a force or moment load on an edge

Define a force or moment using a node ID table

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Moment load, 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 } });