14.1.4 Defining adaptive mesh refinement in the Eulerian domain
Product: Abaqus/Explicit
References
Overview
The adaptive mesh refinement feature:
can refine elements locally inside an Eulerian mesh;
allows the user to define various criteria for refinement;
can remove the refinement automatically once the refinement criteria are no longer met; and
is available for Eulerian element type EC3D8R only.
Adaptive mesh refinement
In a traditional Eulerian analysis the topology of the Eulerian mesh does not change during the analysis. Although the Eulerian mesh motion feature allows the Eulerian mesh to move in space to cover areas of interest, its ability to create a nonuniformly refined mesh that changes with time is limited. The adaptive mesh refinement feature can locally refine the mesh by subdividing elements identified by user-defined criteria. This refinement can be removed automatically during the analysis once the criteria are no longer satisfied. This feature offers great savings in computational cost compared to a uniformly refined mesh. See “Impact of a copper rod,” Section 1.3.10 of the Abaqus Benchmarks Guide, for an example of using the adaptive mesh refinement feature.
Activating adaptive mesh refinement
You can independently activate adaptive mesh refinement for each Eulerian section in a model. The feature applies to all the elements specified in the element set; all the elements in the element set have to be in the same Eulerian section.
| Input File Usage: | *ADAPTIVE MESH REFINEMENT, ELSET=name |
Setting the refinement limit
When adaptive mesh refinement occurs, elements are added to the Eulerian mesh. You can limit how many elements can be created by specifying an upper bound ratio of added elements to original elements. The default value of this upper bound ratio is 8.0.
| Input File Usage: | *ADAPTIVE MESH REFINEMENT, RATIO=maximum increase in number of elements/original number of elements |
Setting the refinement level
With one level of refinement, each time a user-defined Eulerian element is refined, it is equally divided into eight subelements. These subelements can subsequently be divided again if two levels of refinement are allowed. You can set a limit on the maximum number of levels of refinement. The default maximum level is one.
| Input File Usage: | *ADAPTIVE MESH REFINEMENT, LEVEL=maximum level of refinement |
Deactivateing coarsening
You can specify whether refinement can be removed when the refinement criteria are no longer met.
| Input File Usage: | Use the following option to specify that refinement can be removed once the refinement criteria are no longer met: *ADAPTIVE MESH REFINEMENT, COARSENING=YES (default) Use the following option to specify that refinement cannot be removed even when the refinement criteria are no longer met: *ADAPTIVE MESH REFINEMENT, COARSENING=NO |
Defining refinement criteria
You must specify at least one refinement criterion. An element will be selected for refinement if any of the criteria is met. To reduce the numerical artifacts at the mesh transition boundaries (where a fine mesh meets a coarse mesh), the elements adjacent to the selected elements are also refined. The elements are coarsened once the refinement criteria are no longer met. Each selected element can be refined or coarsened by only one level in every increment. Table 14.1.4–1 lists all the refinement criteria available in Abaqus/Explicit.
Table 14.1.4–1 Refinement criteria.
| Refinement criterion description | Refinement criterion label | User-specified values |
|---|---|---|
| Refine elements containing material interfaces | VF | N/A |
| Refine elements that are in contact with Lagrangian bodies | CONT | You can specify the value ALL to refine all elements intersecting the Lagrangian surfaces even if contact has not occurred; using this option avoids frequent refining and coarsening with chattering contact. You can also specify the value MAT to refine only elements containing materials that are in contact with the Lagrangian surfaces. If no values are specified, MAT will be used except for materials with Mie-Grüneisen equations of state. |
| Refine elements in which significant plastic deformation occurs. Not supported for the critical state (clay) plasticity model. | PEEQ | Critical value of the equivalent plastic strain |
| Refine elements near a sharp density gradient | DENSITY | You can specify two values for this criterion. The first value is the critical value of the density gradient, computed as the ratio between the change of density across element faces and the density of the material inside the element; the second value is the critical density. For an element to be selected, both the density and the density gradient must exceed the critical value. |
| Refine elements near a sharp pressure gradient | PRESS | You can specify two values for this criterion. The first value is the critical value of the pressure gradient, computed as the ratio between the change of pressure across element faces and the pressure of the material inside the element; the second value is the critical pressure. For an element to be selected, both the pressure and the pressure gradient must exceed the critical value. |
| Input File Usage: | *ADAPTIVE MESH REFINEMENT, refinement criteria label, value of the criteria |
Contact
When adaptive mesh refinement is specified in an Eulerian section that is involved in general contact, dynamic seeding is activated by default. Dynamic seeding allows more seeds to be created once the Eulerian elements near a Lagrangian face are refined; these seeds will be deleted once these Eulerian elements are coarsened.
Dynamic seeding can also be useful for Eulerian analyses with no adaptive mesh refinement.
| Input File Usage: | *CONTACT CONTROLS ASSIGNMENT, SEEDING=DYNAMIC |