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

In the following example, you want to perform further analysis of the bulkhead shown in the figure in a local breakout model. To create a solution for the breakout model, you create a nodal force report from the global model, and generate a solution with only the loads from the bulkhead of interest. You use the results of the solved solution step TipTorque in the Global solution.

After you create the solution, you would export it and import it to the local model.

Set up the nodal force report

Set up a nodal force report using the results from the TipTorque solution step.

1. Right-click the Global solution and choose Nodal Force Report .

2. In the Nodal Force Report Name box, type Station3 as the name for the nodal force report.

3. From the Forces Type list, select Grid Point.

4. Select the Grid Point Force check box.

5. In the Solution Step group, from the Step list, select Specify Index.

6. In the Specify Index box, type 2, the index number for TipTorque.

7. Select the nodes and elements from which to generate the nodal force report. Click Select Object and in the main graphics window, select the elements that represent the bulkhead of interest. Click Select Object and in the main graphics window, select the nodes of the bulkhead.

8. From the Create Output list, select Post View.

9. Click OK.The Station3 nodal report appears in the Nodal Force node of the Simulation Navigator and a post view shows a free-body diagram of the grid forces.

Generate a solution from the nodal force report

1. In the Simulation Navigator, in the Nodal Force node, right-click Station3 and choose Create Solution.

2. In the Create Solution from Nodal Force Report dialog box, type Station3_Solution as the name of the solution.

3. Notice that Subcase Selection is set to TipTorque because it was the only solution step you included in the nodal force report.

4. Specify the loads to create:To create a table field of force loads, select the Force check box.To create a table field of moment loads, select the Moment check box.

5. Click OK to create the solution.The graphics window displays the loads created. A single arrowhead indicates a force load and a double arrowhead indicates a moment load.The new solution appears in the Simulation Navigator under the Simulation file. The fields appear in the Simulation Navigator in the Fields container, and the loads appear in the Load Container.

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

Learn more

Nodal force reports

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

Example of creating a solution for a breakout model using a nodal force report, 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 } });