Display free-body results

You can use the Free Body Results command to display the total internal forces and moments from a section of a model, summed about a selected point.

1. (Optional) Before you solve the model, make sure the Structural Output Request modeling object for your solution includes Grid Point Force results.

2. Solve the model.

3. In the Post Processing Navigator, load the results and display a post view. The post view’s displayed quantity and its result type settings do not affect the free-body results. The post view is used only to provide a view of the model in which you can select the nodes and elements for the free-body results.

4. In the Post Processing Navigator, right-click the Post View node and choose Free Body Results.

5. In the Free Body Results dialog box, from the Method list, select the method for specifying the elements for which to sum the forces and moments.Pick from Model — Select elements in the graphics window. Use the options in the Pick list to select single or multiple elements. You can select multiple elements by dragging a selection box, selecting a feature face or edge, or selecting an entire mesh. For a description of each selection method, see Free Body Results dialog box.By Element ID — Specify elements by entering the element IDs. You can enter multiple IDs by separating them with commas. After you finish specifying IDs, click Select Elements .By Group — Select an existing group of elements. Click Apply Group to apply the selection. For more information about groups, see Groups.Note: The Boolean Operation option affects how your selection is applied. By default, it is set to Add to Selection , which means each element you select is added to the set of elements included in the selection. You can also use the Boolean Operation option to remove particular elements from your selection and to further refine the selection. For more information, see Free Body Results dialog box.

6. Under Interface Definition, click Select Nodes .

7. Specify the nodes to include in the summation. You can specify only the nodes connected to the elements you selected in the previous step. You can use any of selection methods described previously for elements.

8. Under Location, click Select Location .

9. Specify the location about which to sum the forces and moments. You can select a nodal location on the model, a point location in space (specified through XYZ coordinates), or the origin of a specified coordinate system.

10. Under Reference CSYS, from the CSYS list, select the coordinate system in which the software should report the total forces and moments. Coordinate systems defined in the solver output file are listed in the Post Processing Navigator beneath the Post View node. You can also select them directly from the CSYS list in the Simulation Navigator. By default, coordinate systems are hidden in the post view.

11. Under Output & Display Options, select the appropriate options to specify how the results are displayed in the Information window and the graphics window. By default, the following options are selected:Print Information — Writes the results values to the Information window.Force Display and Moment Display — Displays both force and moment vector graphics in the graphics window. Magnitude — Displays the vector graphics in the magnitude component (that is, the square root of the sum of the X, Y, and Z components). You can choose Components to display the results in the X, Y, and Z direction components of vector data.

Learn more

Displaying free-body results

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Display free-body results, 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 } });