Free Body Diagram (FBD)

Restriction: Only available in the Nastran and OptiStruct solvers in the Aerospace user profile.

Note: Result files should have element grid point forces available. The overall workflow involves two steps. Step 1: From the file loader, read all result files and model files for results in case the result file does not have topology data. The file loader is available from the Aerospace menu. Step 2: Access FBD features from the Aerospace menu.

From the menu bar, click Aerospace > Results > FBD.

The main functionalities include:

Calculate free body or resultant forces and displacements
Create cross sections and dynamic view of free body results for cross section
Show Trace plots
Create *.fbd files to show potato and VMT plots in HyperGraph 2D
Generate reports, loads and fields from free body forces and displacements

Free Body Diagram: Force

From the menu bar, click Aerospace > Results > FBD > Force.

Free Body sections: A group of elements or a cross section on which forces and moments are calculated. Existing free body sections are listed here.

Right-clicking in this area allows you to:

Create: Creates a new free body section. You will create a complete section by choosing section details in the Entity Editor of the free body section.
Import from file: Import the free body sections file (.csv file) or monitor the point3 (BDF) file in Nastran.

For existing sections, select one of the sections and right-click to create, show, hide, isolate, review, rename, delete or export to a file.

Entity Editor of free body sections

View or create/edit each FBD section from the Entity Editor. This section has the following options:

Rename, select ID and color for FBD.
Entity ID list: A free body section will be created using Elements or Cut Section. If Cut Section is selected you can either use existing cut sections by clicking the yellow button and selecting one from the list or create a new one by right-clicking and selecting create.
Node Id list: The node selection option where you can select nodes for participating in the free body force calculations. This option is applicable when you create a free body section from elements. For cross section this is not valid and is not available.
System selection: You can select the system to resolve the forces and moments calculated. The default is Analysis System. You can select global or user defined system.
Summation point: The reference point for calculating the forces and moments sum. You have the option to select:
- Centroid of the section as the reference point. This is the default.
- A node can be selected as the reference point
- An arbitrary option can be selected by entering X, Y and Z locations. You can enter this location by node by clicking on the arrow.

Load cases

List of subcases read from all result files loaded in the file loader. Sub case ID and File ID are also listed in separate columns.

FBD Plot

This tab is used to define the free body calculations and select options to plot, report and create loads and fields.

Free Body Forces/moments: Select this if free body forces are to be calculated for the free body section selected.
Resultant Force/moments: Select this for the sum of the forces/moments to be calculated at the summation point.
Select free nodes (default) if free body forces are to be shown at the cut region of the section selected. Free body forces are calculated and shown for all nodes if this option is selected. The Boundary nodes option shows the values at cut region and free edges of the free body section.
Report: There are two options: Summary Table: Creates tables with free body forces for the selected free body sections and load cases. Min/Max: Creates a table with the report of maximum and minimum values of free body forces and moments from selected load cases and free body sections. You can select multiple load cases and free body sections for reporting. Multiple load cases are not allowed for plotting FBD forces. However, multiple free body sections can be selected to plot at one time.
Load Types: Check the options to include in FBD force calculations to plot or to report.
Load Creation: Creates loads from the free body forces. Selecting this option opens a dialog to select the system to output the force and moment loads. Include file name and check the options for forces/moments to create as loads. A separate load collector is collected for each FBD section per load case.
Create Fields: Creates field with matrix as the source. You can select system to output and select forces and moments to create fields. Fields are created per FBD section per load cases. Locations, forces and moments are stored in the tables and these tables are associated to the field.
Cross Section position: Reposition the cross-section position. This option is applicable only when free body section is created using cross sections. On repositioning of the cross section, free body forcers and moments are recalculated automatically.
Select Forces and Moments: Checkboxes are given for each force and moment, the sum of two forces and moments and the sum of all forces and moments to select while plotting free body forces.

Display: Lists the options to control the free body plot display. Display options to draw arrows by constant or by magnitude, length (in %) and color of arrows for each force, moment, sum of force and moments, 2D or 3D style and arrow head location are available. You can also select for displaying values with precision.

Figure 1.

Free Body Diagram: Displacement

This option is available from the menu bar by clicking Aerospace > Results > FBD > Displacement.

You need to load the model and result files from the result file loader before selecting this option. Clicking displacement opens to a dialog to create FBD- displacements. FBD – displacement is calculated on a set of elements or nodes. Therefore, you need to create an element or node entity set.

Entity set

Lists all sets in the model.

Entity Editor

This region lists the content of the set highlighted. You can add elements or nodes to the new set or edit the content of the existing set. The drop-down menu for Entity IDs lists nodes, properties, sets and points to create or update the entity set. Select either nodes or elements and click the yellow button to open the element/node selection panel. Return to FBD- displacement after selecting the nodes/elements from the panel. Other attributes of the set Entity Editor such as set type, card image and distribution type are all set to default. You do not need to set anything other than the default values as these are not relevant to FBD-displacement.

Load cases

The list of subcases read from all result files loaded in the file loader. Sub-case ID and File ID are also listed in separate columns.

FBD Plot

Shows options to plot and create reports, loads and fields for FBD-displacements.

System to resolve in: Lists the options to select for the system for plotting and reporting of the displacements on entity sets selected. The default is Analysis system. You can select global or user defined system.
FBD summary table: Creates reports for FBD-displacements. Reports created are listed as tables in the Model Browser. These tables list set name, load case and simulation, node IDs, node locations, translational and rotation displacements in each column. You can select multiple sets and load cases/simulations for creating reports.
Load creation: Creates displacement loads from the load cases/simulation on the entity set chosen. You can select multiple sets as well as load cases to create loads. A separate collector is created for each load case and entity set selected. Selecting this option opens a dialog to define include file names and displacements to select to create loads.
Create Fields: Creates fields with matrix as the source. You can select the system to output, and there is an option to select translation and rotation displacements to create the field. Fields are created per set per load cases. Displacements are stored in the tables and these tables are associated to the field.
Select Forces and Moments: Checkboxes are given for each translation and rotation displacement. These checkboxes are also available for sum of two displacements and total sum for both translation and rotation.

Display: These display options are similar to those in FBD-Force display options.

Cross Section

You can create cross sections and use those sections in FBD-forces in this dialog. From the menu bar, click Aerospace > Results > FBD > Cross Section.

These cross sections can also be created and assigned to free body sections from the FBD- Force dialog. In this dialog you can edit the name, ID and color of the cross section.

Base location: Base location can be specified by entering position coordinates for XTAIL, YTAIL and ZTAIL. The same can be done by clicking the select position next to the position coordinate entry boxes. Clicking this opens a node selection panel. The selected node location is used for the base location.
Normal: Defines the cross-section plane by defining normal of the cross section plane. You can either enter the vector components in the entry boxes or click select direction. You can then define the direction using two or three nodes, global X, Y, Z direction or using vector or normal/parallel to screen options.

Figure 2.

Free Body Diagram- Trace Plots

You can create FBD-Trace plots along the selected node path. This creates free body sections for every intermediate cut. These free body sections are created inside a free body group entity.

From the menu bar, click Aerospace > Results > FBD > Trace Plot.

FBD Section Group

All existing free body groups are shown. Right-click and select Create to open a dialog to create free body groups.

FBD Sections Group Definition

Create new free body groups to be used for plotting trace plots.

Select Node Path: Clicking on nodes opens the Node List selection panel. Graphically you can pick the nodes along the desired path. You can select more than two nodes to define paths that may not be straight.
Select Intersect Entity: The elements to be included in the trace plot calculation. If this selection is not used, then the entire model will be considered for calculation.
Number of cuts between nodes: The integer mentioned in this entry defines the number of cross sections to be created between two consecutive nodes.
Cutting plane definition: Defines the direction of the trace plot. This has two options. By default Normal to node direction is set. This will create the path so that it runs normal to the nodes selected during node path definition. The other option is to select common direction. If this is selected, then an additional input of direction is required. Define direction from the vector definition panel by clicking direction.
System: Select the system in which forces need to be calculated. By default, trace plot forces are calculated in global system. System selection can also be defined or updated from the Entity Editor of FBD groups.

Entity Editor: Shows the details of the free body group selected. Name, Id, color, Interest Entities and system selection can be edited.
Load cases: The list of subcases read from all result files loaded in the file loader. Sub-case ID and File ID are also listed in separate columns.
Load types: Free Body Forces, SPC, MPC, internal and applied loads.

Options to plot trace diagram:

Force/Moment – Select any force or moment to plot in the trace diagram.
Arrow length (in %) to define height of arrows.
Numeric format and precision if the Show values checkbox is selected.
Plot direction: Defines the trace plot direction plane. Auto is the default option where the program itself determines the direction plane of the trace diagram. You can change it to the desired direction by selecting X, Y and Z directions in both positive and negative.
Sum to calculate either at cutting nodes or centroid of the cut sections.
Display option to plot either at cutting nodes or at centroid of the cut section.
Project System: Is applicable when trace plot is defined by selecting a user defined system. If selected in those cases free body forces are projected to the system selected. The values shown in those cases are projected values.

Figure 3.

Potato/VMT Plots

Potato and Shear/Moment (VMT) plots are created using an existing workflow in HyperGraph 2D. To keep the workflow the same as well as leverage the existing capabilities of HyperGraph, this Free Body Diagram tool has been enhanced to generate *.fbd files. These files once created can be imported in HyperGraph 2D. Then the already existing options in HyperGraph 2D Tools > Free Body Diagrams > Shear Moment or Potato can be used to draw these diagrams. Refer to the HyperGraph help for detailed documentation on creating these plots.

To create Potato and VMT plots you should have read the results file and model in the file loader available at Aerospace > Results > File Loader. Then you must create free body sections, select load cases of interest and generate the report of summary table as described in the FBD-Force option.

The Potato Plot-VMT Plot File Preparation dialog is opened by clicking Aerospace > Results > FBD > Potato/VMT Plot.

FBF Summary Table: Lists all of the summary tables that are created in FBD-Force. Select the one for potato/VMT plot.
Summation Point Coordinates: Either select the system as is in the summary table or define another system by selecting the write in user System option.

Select a file name and path to create and save the *.fbd file. Once the .fbd file is created you need to follow the existing workflow to create the potato/VMT plot from HyperGraph 2D.