Loads on Geometry

You can apply loads to geometrical entities and map them to the FE mesh using the Load on Geom panel.

One advantage is that you can remesh a model without deleting complicated loads or boundary conditions. After remeshing, loads or boundary conditions that have been applied to geometrical entities can be remapped to the new mesh.

You can apply loads to geometry by using the following panels: Forces, Moments, Constraints, Pressures, Temperatures, Flux, Velocities, and Accels. These are the same panels used to apply loads to a mesh.

There are two ways to map loads on geometry to the mesh associated with this geometry (loads on mesh):
  • Manually, using the Load on Geom panel
  • Automatically, by exporting the FE deck, using the Export tab.

The Model Browser allows separate or simultaneous visualization of loads on mesh and loads on geometry.

To visualize loads on mesh and/or loads on geometry, right-click on the load in the Model Browser. From the toolbar, click (Elements/Geometry). This icon determines what the other buttons act on; right-click the button (or left-click the small triangular downward arrow) to reveal a drop-down menu of options. You can select Elements, Geometry, or both.
  • When Elements is selected, you control the display of loads applied to elements.
  • When Geometry is selected, you control the display of loads applied to geometric entities.
  • Both means that you can control the display of both types of loads independently, and load collectors may contain one type or both types simultaneously.
  • Use the none, all and reverse buttons to assist in selecting which loadcols should be displayed.
Note:

Loads on mesh and loads on geometry can be displayed together, similar to the simultaneous display of both elements and geometry belonging to a specific component.

A geometrical entity can be associated with one mesh or multiple meshes (component or components) and/or with one load collector or multiple load collectors.

One load collector stores both loads on geometry and loads on mesh. The mesh, or multiple meshes, is associated with the geometrical entities to which the loads on geometry have been applied. Each load type is stored in a dedicated section of the same load collector.

Terminology and Definitions

geometrical entities
A point, a line, or a surface.
loads on geometry or geometry loads
Loads applied to geometrical entities.
loads on mesh or mesh loads
Loads applied to mesh (nodes or element).
Loads can be applied directly to mesh or applied by mapping them from loads on geometry.
load mapping
The process of mapping geometrical loads to mesh loads. The loads are mapped from the geometrical entities (to which the geometrical loads are applied) to the mesh that is associated with the geometrical entities.

Application of Loads to Geometry

You can apply loads to geometrical entities in a way similar to the manner in which loads are applied to mesh. The process includes two basic steps.

  1. Creating a load collector by using the Collector panel.
  2. Applying loads to the geometry using one of the following panels on the Analysis page: Forces, Moments, Constraints, Pressures, Temperatures, Flux, Velocities, and Accels.
    To apply a load to a geometrical entity, first create a load collector in which the loads applied to geometrical entities will be stored. Next, access an HyperMesh load panel (such as Forces, Constraints) located on the Analysis page, and choose the create subpanel. Third, select a geometrical entity on which the loads will be applied (points, lines, or surfaces) using the panel selection box, define the load or boundary condition parameters in the same way you would for the application of the load or boundary condition on a FE mesh entity, such as a node, and click create. HyperMesh stores the loads/boundary conditions in the database and displays them in the modeling window.
    The following chart specifies the geometrical entities to which loads can be applied, in each of the load application panels listed above.
    Panel Geometrical Entities
    Accels Panel points, lines and surfaces
    Constraints Panel points, lines and surfaces
    Flux Panel points
    Forces Panel points
    Moments Panel points
    Pressures Panel surfaces

    nodes on edge: lines (for 2D solid elements)

    nodes on face: surfaces (for 3D solid elements)
    Temperatures Panel points, lines and surfaces.
    Velocities Panel points, lines and surfaces.

    Refer to the specific panel for detailed information about creating, reviewing and updating loads and constraints.

Exporting Loads

Export sessions that contain loads on geometry, loads on mesh that have been applied directly to mesh, and loads on mesh that have been mapped from loads on geometry.

When saving the model as an HM database, all load types are saved and are retrieved when you open the .hm file. When exporting the model using an export template, only the loads on mesh are exported. The loads on mesh that are exported may have been applied directly to mesh, mapped from geometry to mesh, or both.

The all/displayed option on the Export tab allows you to determine which loads are exported.

If all is selected, all the loads on geometry that have not been mapped (if any), are mapped to loads on mesh and all the loads on mesh are exported.

If displayed is selected, all the displayed loads on mesh are exported. All the loads on mesh, both displayed and hidden, that are associated with the displayed loads on geometry are exported as well. If any loads on geometry are displayed and have not been mapped, they will automatically be mapped to loads on mesh and exported as well.

Visualization of Loads on Geometry and Loads on Mesh

The Display panel allows you to visualize loads on mesh and loads on geometry.

Visualize loads on mesh and loads on geometry either individually or together by setting the collector type to loadcols and using the toggle between elems and geoms.

The elems option controls the display of loads on mesh while geom controls the display of loads on geometry. A simultaneous display is similar to the display of both elements and geometry belonging to a specific component.
Note: A major graphical display difference between loads on geometry and loads on mesh is the density of the arrows. Multiple arrows represent loads on mesh (one arrow per node or element); a single arrow for each geometrical entity represents loads on geometry. The basic length of the arrow also differs. For the same arrow magnitude percentage setting or uniform size setting within the load application panels, an arrow that represents a load on geometry is longer than arrows representing loads on mesh.

Create Load Collectors

  1. In the Model Browser, right-click on the white area and select Create > Load Collectors.
  2. In name field, enter a load collector name.
  3. Click color and select a color from the pop-up menu.
  4. If creating a generic load collector:
    1. Click the switch and select no card image.
    2. Click create.
    3. Click return
  5. If creating a specific load collector:
    1. Click the switch and select card image.
    2. Click card image = and select the card image type.
    3. Click create/edit.
    4. Enter the relevant data in the card image.
    5. Click return.