Manually resizing and remeshing

To learn about the impact of a remeshing rule on the mesh generated by Abaqus/CAE, you can manually apply a rule and view its impact on the resulting mesh. However, before you can remesh your model, you must run an analysis and create an output database that contains error indicator output variables. You can then change the sizing methods and constraints and view the impact of the modified rule on the generated mesh. When you are confident that a remeshing rule is capturing your intent, you can use the same rule to control several iterations that are driven by automatic remeshing. You can also use manual remeshing to continue an adaptivity process that ended prematurely.

Related Topics
What is the difference between automatic adaptive remeshing and manual adaptive remeshing?
When do I need to use manual adaptive remeshing?
Understanding adaptivity processes
In Other Guides
About adaptive remeshing

Context:

For more information, see What is the difference between automatic adaptive remeshing and manual adaptive remeshing?, and When do I need to use manual adaptive remeshing?.

  1. From the main menu bar, select AdaptivityManual Adaptive Remesh.

    Abaqus/CAE displays the Manual Adaptive Remesh dialog box.

    Tip: You can also manually resize and remesh using the tool, located with the mesh tools in the Mesh module toolbox. (For more information, see Using the Mesh module toolbox.)

  2. In the ODB field, enter the name of the output database that contains the error indicator output variables. Abaqus/CAE uses the error indicators to drive the remeshing algorithm.

    Abaqus/CAE displays the following information about each of the remeshing rules in the output database:

    • The name of the rule.

    • A description of the error indicator output variable that was used by the rule.

    • The percentage target error. This is the value you specified when you created the remeshing rule. If you selected fixed targets, Abaqus/CAE displays the maximum and/or minimum base solution targets. Abaqus/CAE displays a dash if you selected Default methods and parameters or Auto if you selected Automatic target reduction.

    • The sizing method used by the rule.

  3. If desired, click Display Error.

    Abaqus/CAE displays the percentage Error Indicator Result and the Element Count for each error indicator output variable. The element count is the number of elements in the region to which the remeshing rule is applied.

  4. Click Manual Adaptive Remesh.

    Abaqus/CAE remeshes the model. All of the active (not suppressed) remeshing rules contribute to the remeshing of the model. If you applied more than one remeshing rule to the same region, the rule that results in the finest mesh takes precedence.

  5. If desired, you can select AdaptivityRemeshing RuleEditrule name from the main menu and modify the parameters that define the rule. You can then return to the Manual Adaptive Remesh dialog box and view the effect of the modified rule on the error estimate and the resulting mesh.

    Note:

    When you edit a remeshing rule, you can modify parameters such as the remeshing rule sizing method and constraints on the element size and view the effect of your changes on the resulting mesh. However, if you change the step or the error indicator output variables, you must run the analysis again.

  6. You can modify the remeshing rules and remesh your model manually until you are satisfied with the resulting mesh. You can then use the same rules to drive a sequence of iterative remeshing operations that are controlled by Abaqus/CAE. For more information, see Creating, editing, and manipulating adaptivity processes.