Generating nodal force report output

You can generate the output of a nodal force report when you create it or any time after:

• To generate the output when you first create the report, in the Nodal Force Report dialog box, set Create Output to the desired output and click OK.

• To create the report later, in the Simulation Navigator, right-click the nodal force report and select the output type.

Post views

A post view that you create from the results of a nodal force report consists of a contour plot. The following figure shows a wireframe display with arrows on the nodes of the report that represent the forces and moments. The values of the arrows equal the values of the respective forces and moments.

Nodal force report displayed in a post view

For nodal force reports with sum resultants, an arrow appears at the reference location, if specified, or at the origin. The arrow length and color represent the values of the respective forces and moments. The legend color bar and header display the values. You select the Add all Forces and Moments check box in the Nodal Force Report dialog box to calculate sum resultants.

Post view with sum resultants

You can also display the arrow that represents the sum resultants at the centroid of the nodes that comprise the nodal report. To set the centroid display, in the Display dialog box, select the Display at Centroid check box when the Color Display list is set to Arrows.

To generate a post view of a nodal force report, in the Simulation Navigator, right-click the nodal force report and choose Create Post View.

As with other post view displays, you can use the Edit Post View command to further refine the post view display generated from the nodal force report results.

Post views for multiple nodal force reports

You can overlay post views of nodal force reports in a single viewport or display multiple nodal force reports in a single post view.

• Overlay the post views of nodal force reports in a single viewportYou can overlay the post views of nodal force reports in a single viewport. The Overlay command is available when you right-click a nodal force report in the Simulation Navigator. The Post Processing Navigator lists the post views displayed in a single viewport.Two post views of nodal force reports overlaid in a single viewport

• Display multiple nodal force reports in a single post viewYou can create one post view that contains several nodal force reports. The color scale in the post view legend reflects the values for all the nodal force reports. To display multiple nodal force reports in a single post view, select the nodal force reports in the Simulation Navigator, and then right-click and choose Create Post View. Multiple nodal force reports displayed in a single post view

To display multiple nodal force reports, the reports must:

• Belong to the same solution.

• Have the same load cases and the same type of coordinate system.

• Have sum resultants calculated with the Add all forces and moments check box in the Nodal Force Report dialog box selected.

If more than one nodal force report is displayed in a post view, you cannot edit the nodal force reports. You can change the post view display, such as set the display to arrows.

Table fields

You can save nodal force report results to a table field. You can treat the field like any other field: plot, export, or save this field to an AFU file, or use it to define field-based boundary conditions in subsequent analyses.

The options for the independent and dependent domains depend on the type of results in the nodal force report. Which dependent domain you select depends on how you intend to later use the table field. In general, the nodes or coordinates are the independent domain and the forces and moments are the dependent domain. When forces and moments are summed with respect to a reference point in the nodal force report, a subcase ID, time, or frequency can be the independent domain. When multiple iterations exist in a subcase or step, you can create tables of fields.

To generate a table field from a nodal force report, in the Simulation Navigator, right-click the nodal force report and choose Create Table Field.

The new field appears in the Simulation Navigator in the Fields container.

For more information, see Table fields and Save nodal force report results to a table field.

Table field file

After you create a nodal force report, you can export the results as a field (.fld) file. You can select forces, moments, or both. If you select both, the software stores the moments and forces in the same field file. The moments are listed first, followed by the forces. The description in the file lists the name of the nodal force report and the force type, such as grid or reaction force.

For more information about exporting a field to a file, see Exporting and importing fields and Save nodal force report results to a table field.

Solution

You can create a new solution within the active Simulation file, with the forces and the moments in the nodal force report as field-based loads. Creating a solution is helpful if you want to generate loads from a global model (an assembly) and use them in a local breakout model for further analysis. The output of the nodal force report from the global model acts as load input to the local breakout model. After creating the solution, you export it from the global model and import it into the local model. The local breakout model can be a subassembly or component model.

To generate a solution from a nodal force report, in the Simulation Navigator, right-click the nodal force report and choose Create Solution.

The new solution appears in the Simulation Navigator under the Simulation file. In addition, the fields appear in the Simulation Navigator in the Fields container, and the loads appear in the Load Container.

The graphics window displays the loads created. A single arrowhead indicates a force load and a double arrowhead indicates a moment load.

For more information, see Generate a solution from a nodal force report and Example of creating a solution for a breakout model using a nodal force report.

Graph across multiple iterations

You can graph the forces and moments in a nodal force report. The solution on which the nodal force report is based must contain multiple iterations of time or frequency. The X-axis is defined as the iterations in the nodal force report and the Y-axis is defined as the forces or moments. You specify a prefix to identify the graphs from the nodal force report.

The software creates graphs for each load you select. It stores them in the Graphs node of the Post Processing Navigator with the prefix you selected. The following example shows graphs generated using the Nodal Force Report prefix from a nodal force report of grid point force results.

For more information, see Graphing results across multiple iterations and Graph nodal force reports across multiple iterations.

Information window and print

The software lists the forces and moments in the Information window. You can print the results from the Information window.

To view and print the results of a nodal force report, in the Simulation Navigator, right-click the nodal force report and choose Print Information.

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

Nodal force reports

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Generating nodal force report output, 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 } });