If you choose to allow Abaqus/CAE to remesh your model iteratively, the adaptivity process in the Job module controls the adaptive remeshing for you. You need only define the remeshing rule in the Mesh module and apply the rule to the regions in your model that you want to be remeshed.

Conversely, you can manually apply modified remeshing rules and view the impact of your modifications on the generated mesh. When you are satisfied that your remeshing rule is producing the desired mesh, you can use the rule to drive a sequence of iterative remeshing and analysis operations that is controlled by Abaqus/CAE. Select AdaptivityManual Adaptive Remesh from the main menu bar to apply the adaptive remesh rules manually. For more information, see “Manually resizing and remeshing,” Section 17.21.6.

When you apply manual adaptive remeshing, you must enter the name of the output database file that was generated by a previous analysis of your model. This output database contains the error indicator output variables that Abaqus/CAE uses to calculate the mesh sizing functions. The error indicator output variables stored in the output database limit the changes that you can make to a remeshing rule. For example, if your original rule specified energy density in a certain region, you will not be able to switch the rule to use error in equivalent plastic strain without first rerunning the analysis. You can modify the sizing method and the element size constraints in the remeshing rule and still use the output database from a previous analysis. However, the output database cannot be used if you modify the step, the region, or the error indicator output variables.