Nodal force reports

Use the Nodal Force Report command to generate reports of forces at nodes. The forces are taken from solver outputs, such as reaction forces or contact forces from Simcenter Nastran. You can use the reports to generate loads in breakout models or to display free-body diagram output in the post view. The report can also generate load summations about a point so you can evaluate interface or joint load conditions.

You can display the nodal forces with respect to the global (absolute) coordinate system or another selected coordinate system.

The Nodal Force Reports on Path command is also available to create a nodal force report along a path defined by a query curve. You can then use the nodal force reports on path as input to shear, moment, and torque diagrams. For more information, see Graphing internal forces, moments, and torque.

Note:

The Free Body Results command accessible through the Post Processing Navigator remains available for legacy purposes.

Selecting forces to be used in calculation

You can create a nodal force report from the forces in any subcase or step in a selected solution, including grid point, applied, contact, reaction, multi-point constraint, and glue forces. Because you can select any subcase or step, you can use the same elements and reference points to cycle through subcases or steps in a solution.

Defining report nodes and elements

You define the nodes and elements to be used in the nodal force calculations:

• When creating a nodal force report of a grid point force, you can specify the elements connected to the grid point force, called the nodal force report definition. If the nodal force results include more than one force, the grid point force on a node is the sum of the forces from all the elements of which the node is a part.Note: You do not define the nodal force report definition if you include more than one grid force, such as a grid point reaction force, because they are nodal forces, and internal element forces do not contribute.

• For all forces, you specify the nodes on which the forces in the report are calculated, including specifying all nodes. Specifying report nodes is optional when grid point force is the only force in the report. If you do not specify the nodes for a grid point force, the software includes all the nodes of all the elements you selected for the nodal force report definition.

You can select the elements or nodes directly or select the following entities or a combination of them:

• Polygon geometry

• Other geometries (such as curve, point, end of curve, mesh point)

• Mesh

• Groups

• Selection recipes

The software generates a nodal force report of the elements and nodes associated with the selected entities. If you change the entities, such as change the mesh size or add or delete entities from a group, the nodal force report updates accordingly.

Adding all forces and moments

You can select to have the software calculate a single net force or moment about a reference point or the origin. The forces are calculated using vector addition of all forces on the specified report nodes. The resultant moments are the sum of r x Fnode across nodes and the respective moments acting on the node (for example, grid point moment and grid point applied moment), where:

• r is the position vector from the reference point and the node.

• Fnode is the force acting on the respective node.

Post view with sum resultants

To calculate a single net force, select the Add all Forces and Moments check box in the Nodal Force Report dialog box. If you do not select the check box, the software reports the forces and moments for each node.

The resulting post view can display the results of the nodal force report at the reference location (if specified), the origin, or the centroid of selected nodes. You can choose to use the deformed coordinates to compute nodal moment arms relative to the reference point.

Calculate moments about a reference point

If you do not select to add all forces and moments, you can choose to calculate moments about a reference point. You can choose to use the deformed coordinates to compute nodal moment arms relative to the reference point.

Generating output from the nodal force report

You can output the results of a nodal force report while creating it or later, including generating a solution, with the forces and the moments of the results as loads. To generate results from a nodal force report, you must have solved the model.

For more information, see Generating nodal force report output.

Where do I find it?

Application	Pre/Post
Prerequisites	The Simulation file as the work part and displayed part and an active solutionA solved solution containing the results that you intend to use for the nodal force report
Simulation Navigator	Right-click a solution node→Nodal Force Report In a solution node, right-click the Nodal Force Report node→Nodal Force Report

How do I

Set up and generate nodal force reports

Save nodal force report results to a table field

Generate a solution from a nodal force report

Graph nodal force reports across multiple iterations

Example of creating a solution for a breakout model using a nodal force report

Learn more

Generating nodal force report output

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Nodal force reports, 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 } });