Creating and editing a design response

You use the design response editor to create and configure your design responses. You associate a design response with a region of your model; however, the design response consists of a single scalar value, such as the maximum stress in the region or the total volume of the model. In addition, you can associate a design response with a particular step or a load case within a step. Design responses are used by objective functions and constraints. The design responses that are available depend on the type of optimization task you created; for more information, see Design responses.

Related Topics
Selecting the data source of a design response
Combining design responses

Context:

A design response can cover multiple models. You can incorporate multiple models into your optimization when linear perturbations about a base state are no longer sufficient as load cases. For example, you can simulate nonlinear load cases (which are not supported by Abaqus/CAE) by creating multiple copies of your nonlinear model and by creating a step in each model during which different loads and boundary conditions are applied. Each model must have the same mesh and the same section assignments, and the models must be open in your Abaqus/CAE session.

  1. From the main menu bar, select Design ResponseCreate.

    The Create Design Response dialog box appears.

    Tip: You can initiate the Create procedure in two other ways:

    • Click Create in the Design Response Manager. (You can display the Design Response Manager by selecting Design ResponseManager from the main menu bar.)

    • Click the tool in the Optimization module toolbox.

  2. From the prompt area, select the region to which the design response will be applied:

    • Select Whole Model (default) to apply the design response to the entire model.

    • Select Body (elements), and select the region to which the design response will be applied. During the optimization, the design response will be applied to the elements in the selected region.

    • Select Point (nodes), and select the region to which the design response will be applied. During the optimization, the design response will be applied to the nodes in the selected region.

    By default, Abaqus/CAE allows you to select all regions of the model. Use the Selection toolbar to change the type of object that you can select to Vertices, Edges, Faces, or Cells. For more information, see Filtering your selection based on the type of object.

    If you would rather select from a list of existing sets, do the following:

    1. Click Sets on the right side of the prompt area.

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

    2. Select the set 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 the button—Select in Viewport or Sets—on the right side of the prompt area.

  3. When you have finished selecting the design response region, click Done in the prompt area. For more information on selecting objects, see Selecting objects within the viewport.”

    The Edit Design Response dialog box appears.

  4. By default, the Optimization module assumes a design response, such as a displacement along an axis, is defined in the global coordinate system. To change the coordinate system in which the design response is defined, click for the CSYS option and do one of the following:

    • Select an existing datum coordinate system in the viewport.

    • Select an existing datum coordinate system by name.

      1. From the prompt area, click Datum CSYS List to display a list of datum coordinate systems.

      2. Select a name from the list, and click OK.

    • Click Use Global CSYS from the prompt area to revert to the global coordinate system.

    Alternatively, click to define a new datum coordinate system.

  5. From the Edit Design Response dialog box, select the Variable tabbed page.

  6. Select the variable and, if applicable, its component.

    Note:

    By default, the Optimization module displays all of the variables that are available for the selected optimization task. To avoid creating a design response that cannot be used as expected, you can display only the variables that are available for an objective function or only the variables that are available for a constraint.

  7. If you are creating an internal force or internal moment design response, you must select the nodal subset region. This region contains the nodes that form a cross section of the elements in the region in which the internal force or moment will be maximized or minimized.

  8. Select the Steps tabbed page, and specify the model and step or load case of interest. In addition, if you are performing an eigenfrequency optimization, you must select the modes of interest from the Steps tabbed page. For more information, see Selecting the data source of a design response.

  9. Select the operator that will be applied on the selected variable across the design area.

    • Sum of values: The sum of the values across the design area. For some variables (such as volume, weight, moment of inertia, and gravity) Sum of values is the only operator, and it is selected by default.

    • Minimum value: The minimum value across the design area.

    • Maximum value: The maximum value across the design area. For some variables (such as stress, contact stress, and strain) Maximum value is the only operator, and it is selected by default.

  10. If applicable, select the operator that will be applied on the selected variable across steps and load cases.

    • Sum of values: The sum of the values across the selected steps or load cases.

    • Minimum value: The minimum value across the selected steps or load cases.

    • Maximum value: The maximum value across the selected steps or load cases.

  11. Click OK to save your data and to exit the editor.