Create and Manage FBD Cross-Section Definitions

Create and manage cross-section definitions that are used within the Resultant Force and Moment utility.

Cross-sections, are defined by an element set, node set, summation node, and a local result coordinate system.

The FBD Cross-section Manager features semi-automatic generation of element and node sets for defining cross-sections. Functionality is also available to reorder FBD cross-sections.

The FBD Cross-section Manager interface has two creation methods available for cross-section definition: manual and (semi-) automatic. The Advanced options section provides the means to semi-automatically create cross-section element and node sets for beam-like structures with regular meshes. This auto-create cross-section capability requires a continuous mesh with rows of nodes (of any orientation) to work properly. The mesh should not have any discontinuities (such as holes and gaps) and must have identifiable rows of nodes, starting from the selected nodes and progressing along the length of the selected elements.

Manually Define Cross Sections

  1. From the menu bar, click Post > Free Body > Cross Section.
    The FBD Cross Section Manager tab opens.
  2. Use the Element Set selector to specify the elements containing the nodes that define the cross-section.

    The Set Browser can be used to create the necessary element sets.

    If multiple element sets are selected, each set is added to the table as a separate cross-section definition which can be modified later by selection.

  3. Use the Node Set selector to define the nodes in each currently selected element set at which grid point data will be extracted and summed from.

    Only the nodes contained within the selected node set will be part of the grid point extraction. Use the Set Browser to create the necessary node sets.

    If multiple node sets are selected for a single element set, HyperMesh adds separate cross-section definitions to the table with the original element set and each selected node set.

  4. Use the Summation Node selector to define the node about which the grid point data will be summed.

    If no node is selected, the utility defaults to "Centroid". This option calculates the nodal averaged centroid of the coordinates of all of the nodes in the node set and creates a temporary node at that location.

    When using the "Centroid" option, a temporary node is created. If this node is deleted from the model, the loads associated with that node are also deleted.

  5. Use the Result System selector to define the coordinate system into which the grid point vector results will be transformed and output.
    If a results system is not specified, the HyperMesh "base" system is used by default.
  6. To display the element set, node set, result system and summation node which define the cross-section in the graphics display area, select the Display sections checkbox.
  7. To display the entire model in transparency mode, highlighting the currently selected element set, node set, result system and summation node, select the Show model checkbox.
    This allows you to verify a cross-section definition.
  8. Use the filter buttons on the top of the spreadsheet to select which cross-sections are required.

    Standard Ctrl/Shift–click functionality can be used to select cross-sections. Selected cross-sections can also be deleted from the database by using the Remove selection button on the right end of the filter buttons.

Each time a cross-section is created, modified, or deleted, the cross-section data is saved to the database. When the database is saved, all cross-section definitions are also saved. Therefore, cross-section definitions only need to be defined once and stored in the database. Cross-Sections can then be accessed from within the Resultant Force and Moment utility, which utilizes the cross-section definitions to perform these calculations.

Renumbering element or node sets after running the tool invalidates the link between the cross-section names and the associated sets. Therefore, it is important to avoid renumbering any element or node sets for which cross-sections are to be retained within the database.

Automatically Define Cross Sections

  1. From the menu bar, click Post > Free Body > Cross Section.
    The FBD Cross Section Manager tab opens.
  2. Use the Elements selector to choose the elements that define the entire "beam-like" component from which cross-sections will be generated.
  3. Use the Nodes selector to pick nodes for the first node set (first cross-section).

    These nodes should be at one end of the beam.

  4. To automatically display the entire model in transparency mode, highlighting the currently selected elements and nodes, select the Show model checkbox.
  5. In the Element set prefix field, enter a prefix for the name of each generated element set.

    For example, you type in "ESET" each element set will be named ESET [#], where "#" increases with each new set generated.

  6. In the Node set prefix field, enter a prefix for the name of each generated node set into the Node set prefix field.

    For example, you type in "NSET" each element set will be named NSET [#], where "#" increases with each new set generated.

  7. In the Numbering offset field, enter an offset value for generated set names.

    By default, the offset value is zero and HyperMesh generates numbered set names starting with one. If the offset value is set to a value greater than zero, the generated set names are numbered starting from that value.

  8. To have each element set contain the elements from the previous set, select the sets accumulate checkbox.
    This determines whether each progressive set also contains the elements from the previous set, or only the new "row" of elements.