Creating loads

From the main menu bar, select LoadCreate.

A Create Load dialog box appears with a default name displayed in the Name text field.

Tip: You can also create a load using the tool in the Load module toolbox.

Type a name for the load. For more information on naming objects, see Using basic dialog box components.

Select the step in which to activate the load. Click the arrow next to the Step text field, and select from the list that appears. Loads can be created only in an analysis step; you cannot create a load in the initial step.

From the Category list on the left side of the dialog box, choose the desired category. The Category choices available are dependent upon the type of analysis procedures you are performing.

The Types for Selected Step list on the right side of the dialog box changes to a list of all the available load types.

From the Types for Selected Step list, select the load type and click Continue.

If you are creating a gravity load or an inertia relief load, the load editor appears.

If you are creating a connector force or connector moment using assembled fasteners, you can click Done in the prompt area to select a wire set from the template model.

The load editor appears.

1. Click the arrow next to the Assembled fastener field, and select from the list that appears.

   The template model name associated with the assembled fastener is displayed in the editor. The Template set list is populated with the wire sets that are associated with the referenced template model.

2. Select a wire set from the Template set list. You must ensure that the wire set has a section assignment that has the available components of relative motion for which you want to define forces.

   The appropriate fields for the available components of relative motion are displayed.

For all other load types, select the region to which you want to apply the load.

If you are creating a connector force or connector moment, you must select wires that are associated with a connector section assignment. The best approach for selecting wires is to use the default geometry set name for the wire feature (see Creating or modifying wire features for multiple connectors, for more information). If you select multiple wires, you must ensure that the connector sections assigned to the wires in the connector section assignments have the available components of relative motion for which you want to define forces or moments. If there are insufficient available components of relative motion for the connector force or connector moment, a message appears asking you to select different wires or to change the connection type.

Use one of the following methods to select the region for the load:

• Select a region in the viewport. You can use the angle method to select a group of faces or edges from geometry or a group of element faces from a mesh. For more information, see Using the angle and feature edge method to select multiple objects. When you have finished selecting, click mouse button 2.

  Tip: You can limit the types of objects that you can select in the viewport by specifying filtering options in the Selection toolbar. See Using the selection options, for more information.

  If the model contains a combination of mesh and geometry, click one of the following from the prompt area:

  • Click Geometry to apply the load to geometry or to a reference point.

  • Click Mesh to apply the load to a native or orphan mesh selection.

  By default, for most load types a set or surface is created that contains the selected objects. You can change this behavior by toggling off the option to create a set or surface in the prompt area. A default name is provided in the prompt area, but you can enter a new name.

• To select from a list of existing sets or surfaces, do the following:

  1. Click Sets or Surfaces on the right side of the prompt area. (The name of the button depends on the type of object you are creating. For example, if you are creating a pressure load, a Surfaces button appears.)

     Abaqus/CAE displays the Region Selection dialog box containing a list of available sets or surfaces.

  2. Select the set or surface of interest and click Continue.

     Note:

     The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Sets or Surfaces on the right side of the prompt area.

The load editor appears. The region to which you are applying the load is highlighted in the viewport.

Enter all of the data necessary to define the load and click OK.

Note:

If you create a connector force or connector moment that exceeds the failure criteria for a connector, the connector force or connector moment will still be applied.

For detailed information on a particular feature of the editor, select HelpOn Context from the main menu bar and then click the feature of interest or see Using the load editors.

Symbols appear in the viewport that represent the load that you just created. For more information, see Understanding symbols that represent prescribed conditions.