Create a Section Definition

The FBD section definition portion of the tab allows you to create and manage the section definitions that are used for plotting the free body or resultant forces. This section contains tools for manually defining sections, which are defined by an element set, node set, summation node, and a local result coordinate system.
  1. From the FBD tab, click the Add new section icon to add a new section to the table.
    Warning: Whenever a new section is added, a warning icon will also be displayed in the table which indicates that it has not yet been defined. Once Elements have been picked, a green check mark will be displayed indicating that the section has now been defined.
  2. Select the elements that make up the free body and contain the nodes at which grid point data will be extracted for the section using one of the following methods.
    • Click the Elements input collector and use the extended entity selection menu.
    • Pick an individual element, or multiple elements, directly from the model in the modeling window.
    1. Click the plus icon (located next to the input collector) to add elements to the selected section.
    2. Click the minus icon (located next to the input collector) to remove elements from the selected section.
  3. Select the nodes that define the section using one of the following methods.
    • Click the Node input collector and use the extended entity selection menu.
    • Pick an individual node, or multiple nodes, directly from the model in the modeling window.
    1. Click the plus icon (located next to the input collector) to add elements to the selected section.
    2. Click the minus icon (located next to the input collector) to remove elements from the selected section.
    Note: Only the nodes contained within the selected node section will be part of the grid point extraction.
  4. Specify the coordinate system into which the grid point vector results will be transformed and output for the section using one of the following methods.
    • If Free body forces/moments are requested for plotting, three options are available: Global, Analysis and User System. If Resultant forces/moments are requested for plotting, only Global and User System will be available.
      Global System
      Force/moment results will be transformed to the global system and displayed.
      Analysis System
      Force/moment results will be shown in the analysis system of a node. Therefore, if a local system is specified in the input deck for a node, then the results shown are in this system. Otherwise, it is in global.
      User System
      Pick a user system to transform results into this system.
    • Click the System input collector and use the extended entity selection menu.
    • Pick the system directly from the model in the modeling window.
    Note: If a results system is not specified, the HyperView "base" system is used by default.
  5. Define the node about which the grid point data is to be summed for the section. Use the drop-down menu to select one of the following options:
    OptionDescription
    Centroid This default option calculates the nodal averaged centroid of the coordinates of all of the nodes in the section.
    Node Displays a Node input collector which is used to pick the summation point (using the By ID method).
    Coordinate Displays X, Y, and Z coordinate fields which are used to specify the summation point.
    This is useful for verifying free body behavior through zero-sum values for all force and moment components about any node. It is also useful for calculating the result of applied or reaction forces about any node.
    Note: If a node is not selected, the HyperView origin (0,0,0) is used by default. A dot is drawn for the summation point.