Applying a load to the frame

Now that you have constrained the frame, you can apply a load to the bottom of the frame. In Abaqus the term load (as in the Load module in Abaqus/CAE) generally refers to anything that induces a change in the response of a structure from its initial state, including:

  • concentrated forces,

  • pressures,

  • nonzero boundary conditions,

  • body loads, and

  • temperature (with thermal expansion of the material defined).

Sometimes the term load is used to refer specifically to force-type quantities (as in the Load Manager of the Load module); for example, concentrated forces, pressures, and body loads but not boundary conditions or temperature. The intended meaning of the term should be clear from the context of the discussion.

Context:

In this simulation a concentrated force of 10 kN is applied in the negative 2-direction to the midspan of the frame; the load is applied during the linear perturbation step you created earlier. In reality there is no such thing as a concentrated, or point, load; the load will always be applied over some finite area. However, if the area being loaded is small, it is an appropriate idealization to treat the load as a concentrated load.

  1. In the Model Tree, click mouse button 3 on the Loads container and select Manager from the menu that appears.

    The Load Manager appears.

  2. At the bottom of the Load Manager, click Create.

    The Create Load dialog box appears.

  3. In the Create Load dialog box:
    1. Name the load Force.
    2. From the list of steps, select Apply load as the step in which the load will be applied.
    3. In the Category list, accept Mechanical as the default category selection.
    4. In the Types for Selected Step list, accept the default selection of Concentrated force.
    5. Click Continue.

    Abaqus/CAE displays prompts in the prompt area to guide you through the procedure. You are asked to select a region to which the load will be applied.

    As with boundary conditions, the region to which the load will be applied can be selected either directly in the viewport or from a list of existing sets. As before, you will select the region directly in the viewport.

  4. In the viewport, select the vertex at the bottom center of the frame as the region where the load will be applied. Name the associated set center.
  5. Click mouse button 2 in the viewport or click Done in the prompt area to indicate that you have finished selecting regions.

    The Edit Load dialog box appears.

  6. In the dialog box:
    1. Enter a magnitude of -10000.0 for CF2.
    2. Click OK to create the load and to close the dialog box.

      Abaqus/CAE displays a downward-pointing arrow at the vertex to indicate that the load is applied in the negative 2-direction.

  7. Examine the Load Manager and note that the new load is Created (activated) in the analysis step Apply load.
  8. Click Dismiss to close the Load Manager.