Defining ALE adaptive mesh domains in Abaqus/Explicit

By default, all adaptive mesh domains defined in the previous analysis step remain unchanged in the subsequent step. You define the adaptive mesh domains in effect for a given step relative to the preexisting adaptive mesh domains. At each new step the existing adaptive mesh domains can be modified and additional adaptive mesh domains can be specified (except in Abaqus/CAE, where only one adaptive mesh domain can be in effect for a given step).

ADAPTIVE MESH, ELSET=name
ADAPTIVE MESH, ELSET=name, OP=MOD

Step module: OtherALE Adaptive Mesh DomainEdit

If you choose to remove any adaptive mesh domain in a step, no adaptive mesh domains will be propagated from the previous step. Therefore, all adaptive mesh domains that are in effect during this step must be respecified.

ADAPTIVE MESH, ELSET=name, OP=NEW

Step module: OtherALE Adaptive Mesh DomainEdit: toggle on No adaptive mesh domain for this step

User-defined adaptive mesh domains are examined by Abaqus/Explicit. The user-defined domain will be modeled using a single adaptive mesh if the domain:

• consists of a single element type;

• consists of a single connected region;

• consists of a single material;

• is subject to a uniform body force (including zero body force); and

• has identical section controls.

The user-defined domain will be split into multiple adaptive mesh domains, separated by boundary regions, if the domain:

• consists of multiple element types;

• spans part instances;

• consists of multiple regions (including regions that are connected by less than a single element face, only by contact conditions, or only by connectors such as MPCs);

• consists of multiple materials;

• is subject to multiple body force definitions; or

• is subject to multiple section control definitions.

In this documentation the term “adaptive mesh domain” refers to a single domain after splitting by Abaqus/Explicit. On the rare occasion that a reference is made to an adaptive mesh domain prior to the automatic splitting, it is referred to as a “user-defined adaptive mesh domain.” Since adaptive mesh domains are split across element types, degenerate elements should be used for mixed domains that include both triangles and quadrilaterals (or tetrahedron and bricks). For example, when defining a mixed plane strain domain with quadrilateral and triangular elements, the CPE4R element type should be used to define both quadrilaterals and degenerated quadrilaterals. Using the CPE3 element will result in split domains, which is generally not desirable.

Two types of boundary region edges can exist: Lagrangian and sliding. Lagrangian edges are always associated with a material line. Material can never flow past a Lagrangian edge, and nodes can move only along a Lagrangian edge (like beads on a string). Sliding edges are associated only with the mesh. Material can flow past a sliding edge (that is, sliding edges are free to slide over the underlying material).

Lagrangian edges can be viewed with Abaqus/CAE; see Output and diagnostics for ALE adaptive meshing in Abaqus/Explicit.

Lagrangian boundary regions are the most common boundary regions in structural finite element analysis; therefore, with the exception of contact surfaces, they are always the default in Abaqus/Explicit. A Lagrangian boundary region has the most constraints of all the boundary region types. The mesh is constrained to move with the material in the direction normal to the surface of the boundary region and in the directions perpendicular to the boundary region edges.

Lagrangian boundary regions have Lagrangian edges: the edges follow the material. On the interior of a Lagrangian boundary region, the mesh can move independently of the material in the surface of the boundary region. Thus, a Lagrangian boundary region can be thought of as a “mesh patch” that follows the material. Nodes are free to move within and along the edges of the patch but cannot leave the patch.

A sliding boundary region is the same as a Lagrangian boundary region except that it has a sliding edge. Sliding boundary regions are created by default when you define a surface on the boundary of an adaptive mesh domain (see About surfaces).

The mesh is constrained to move with the material in the direction normal to the boundary region, but it is completely unconstrained in the directions tangential to the boundary region. Thus, a sliding boundary region can be thought of as a “mesh patch” that moves independently of the underlying material.

Sliding boundary regions can be created by defining a surface, boundary condition, or load on the boundary of an adaptive mesh domain (as explained later in this section). Since the mesh is totally unconstrained in the directions tangential to a sliding boundary region, the location of an applied boundary condition or load may not be physically meaningful as the mesh moves over the material. Therefore, to retain the spatial meaning of an applied boundary condition or load, spatial mesh constraints (described in Mesh constraints, presented later in this section) are usually applied tangential to sliding boundary regions.

Eulerian boundary regions can be defined on the exterior of a model where it makes physical sense to let material flow across the boundary (for example, at the inlet and outlet of a steady-state extrusion or rolling problem). This flow across the boundary distinguishes Eulerian boundary regions from Lagrangian or sliding boundary regions.

Eulerian boundary regions have sliding edges and must lie completely on an exterior surface of a model. It makes no physical sense to allow material flow to originate on an interior surface. You must explicitly define Eulerian boundary regions since, by default, Abaqus/Explicit assumes that no material flows into or out of an adaptive mesh domain.

Eulerian boundary regions are created by defining a surface, a boundary condition, or a load on the boundary of an adaptive mesh domain. On Eulerian boundary regions the mesh motion usually should be constrained in the direction normal to the material motion; therefore, the surface mesh should be fixed in space using spatial mesh constraints (described in Mesh constraints, presented later in this section). Applying these constraints normal to an Eulerian boundary region allows material to flow into or out of the mesh, as in a fluid flow problem, while allowing adaptive meshing to occur on the surface of the boundary region to maximize mesh quality.

The material flowing into an Eulerian boundary region is assumed to have the same properties as the material that is inside the adaptive mesh domain.

Techniques for modeling Eulerian domains are presented in Modeling techniques for Eulerian adaptive mesh domains in Abaqus/Explicit.

Abaqus/Explicit will create adaptive mesh boundary regions automatically on

• the exterior of a model,

• the boundary between different adaptive mesh domains, or

• the boundary between an adaptive mesh domain and a nonadaptive domain.

By default, a boundary region on the exterior of a model will be Lagrangian, so that the boundary region follows the material, and loads, boundary conditions, etc. will retain their Lagrangian interpretation. A boundary region between different adaptive mesh domains is always Lagrangian: no material can flow through such a boundary region. An additional constraint is applied when the model contains multiple parallel domains (see Parallel execution in Abaqus/Explicit). In this case the boundary region is nonadaptive: no material can flow through the boundary region, and the nodes on this boundary are constrained to move exactly with the underlying material in all directions. A boundary region between an adaptive mesh domain and a nonadaptive domain is always nonadaptive. The only exception to this occurs if an Eulerian boundary region is defined on the boundary between an adaptive mesh domain and a nonadaptive domain that comprises displacement-based infinite elements. In this case the nodes on the boundary behave as in Eulerian boundary regions (see the description under Eulerian boundary regions, presented earlier in this section), and the mesh motion at the boundary nodes can be constrained using spatial mesh constraints.

The boundary between two different materials can never “flow” through the mesh; such a physical boundary is always associated with a Lagrangian boundary region or a nonadaptive mesh boundary.

Figure 1 shows some boundary regions that will be created automatically by Abaqus/Explicit. In the model shown in this figure Abaqus/Explicit splits the user-defined adaptive mesh domain into two adaptive mesh domains because the original domain is composed of two different materials.

Figure 1. Automatic splitting of mesh domains and creation of boundary regions.

In addition to the boundary regions created automatically by Abaqus/Explicit, Lagrangian, sliding, and Eulerian boundary regions can be created by the definition of surfaces, boundary conditions, and loads, as described later in this section.

Geometric features are identified initially as edges on boundary regions where the angle between the normals on adjacent element faces is greater than the initial geometric feature angle, ${\theta }_I$ ($0^{\circ }\le {\theta }_I\le {180}^{\circ }$). See Figure 3. The default value for the initial geometric feature angle is ${\theta }_I={30}^{\circ }$.

Figure 3. Detection and deactivation of geometric features.

You can change the value of the angle that will be used to recognize geometric features. Setting ${\theta }_I={180}^{\circ }$ will ensure that no geometric edges or corners are formed on the boundary of the adaptive mesh domain.

ADAPTIVE MESH CONTROLS, NAME=name, 
INITIAL FEATURE ANGLE=${\theta }_I$

Step module: OtherALE Adaptive Mesh ControlsCreate: Name: name, Initial feature angle: ${\theta }_I$

Geometric features affect only Lagrangian and sliding boundary regions, where they act as temporary Lagrangian edges. During each mesh sweep in an adaptive mesh increment, nodes along a geometric edge are positioned by applying the basic smoothing methods (see ALE adaptive meshing and remapping in Abaqus/Explicit). The nodes are constrained to lie along the discrete geometric edge unless the angle forming the geometric edge becomes less than the transition geometric feature angle, ${\theta }_T$ ($0^{\circ }\le {\theta }_T\le {180}^{\circ }$). The default value for the transition feature angle is ${\theta }_T={30}^{\circ }$. If the angle across the geometric edge becomes less than ${\theta }_T$, the boundary surface is considered to be flattened sufficiently for the feature to be deactivated, and the mesh is allowed to slide freely over the material (unconstrained by the deactivated geometric edge). Geometric corners are allowed to flatten in a similar fashion. This logic allows great flexibility in mesh adaptation while preserving geometric features in the model.

You can change the transition feature angle. Setting ${\theta }_T=0^{\circ }$ will ensure that no geometric edges or corners are ever deactivated.

ADAPTIVE MESH CONTROLS, NAME=name, 
TRANSITION FEATURE ANGLE=${\theta }_T$

Step module: OtherALE Adaptive Mesh ControlsCreate: Name: name, Transition feature angle: ${\theta }_T$

Use a spatial mesh constraint (the default) to prescribe spatial mesh motion that is independent of the material motion. You specify the nodes to which the constraint is applied, the directions of the prescribed motion, and the amplitude of the prescribed motion. You can prescribe either a displacement or a velocity for the spatial mesh motion.

ADAPTIVE MESH CONSTRAINT, CONSTRAINT TYPE=SPATIAL, 
TYPE=DISPLACEMENT or VELOCITY

Step module: OtherALE Adaptive Mesh ConstraintCreate: Types for selected step: Displacement/Rotation or Velocity/Angular velocity: select region: Motion: Independent of underlying material

Rules for applying spatial mesh constraints

Spatial mesh constraints can be applied without restriction to nodes on an Eulerian boundary region or in the interior of an adaptive mesh domain.

In both two and three dimensions nodes at Lagrangian and active geometric corners are fully constrained to move with the underlying material. No mesh constraints can be applied at such corners.

Adaptive mesh constraints must not conflict with other mesh constraints inherent to Lagrangian and sliding boundary regions; therefore, adaptive mesh constraints can be applied only tangentially to a Lagrangian or sliding boundary region. This restriction implies that adaptive mesh constraints can be applied only in two directions in a three-dimensional boundary region, in one direction in a two-dimensional boundary region, or in one direction on a Lagrangian or active geometric edge. It may not always be feasible to adhere to this rule, particularly if the boundary experiences finite rotation. Therefore, if the normal to a boundary region is not perpendicular to a prescribed mesh constraint at a node, it is always moved along the current surface of the boundary region so that the projection of the mesh motion in the direction of the prescribed constraint is correct (see Figure 4).

Figure 4. Enforcing a spatial mesh constraint.

If the normal to the boundary region approaches the direction of the applied mesh constraint, large mesh motions will be required to satisfy the constraint. By default, an analysis is terminated if the angle between the normal to the boundary region and the direction of the prescribed constraint becomes less than ${\theta }_C$. This cutoff angle is referred to as the mesh constraint angle, and its default value is 60°.

The mesh constraint angle, ${\theta }_C$, is also used when adaptive mesh constraints are applied to nodes along a Lagrangian or active geometric edge. Since independent mesh motion cannot be prescribed perpendicular to these edges, an analysis is terminated if the angle between the prescribed constraint and the plane perpendicular to the edge falls below the specified mesh constraint angle.

You can change the value of the mesh constraint angle ($5^{\circ }\le {\theta }_C\le {85}^{\circ }$). Setting ${\theta }_C<{45}^{\circ }$ is not recommended because it may cause errors in determining the free surface geometry, especially for curved surfaces.

Input File Usage

ADAPTIVE MESH CONTROLS, MESH CONSTRAINT ANGLE=${\theta }_C$

Abaqus/CAE Usage

Step module: OtherALE Adaptive Mesh ControlsCreate: Mesh constraint angle: ${\theta }_C$

AMPLITUDE, NAME=name
ADAPTIVE MESH CONSTRAINT, AMPLITUDE=name

Step module: OtherALE Adaptive Mesh ConstraintCreate: Types for selected step: Displacement/Rotation or Velocity/Angular velocity: select region: Motion: Independent of underlying material: Amplitude: amplitude

Spatial mesh constraints are applied in local directions if a local coordinate system is defined at a node (see Transformed coordinate systems); otherwise, they are applied in global directions.

Lagrangian mesh constraints on a node are used to indicate that mesh smoothing should not be applied; i.e., the node must follow the material.

ADAPTIVE MESH CONSTRAINT,
CONSTRAINT TYPE=LAGRANGIAN

Step module: OtherALE Adaptive Mesh ConstraintCreate: Types for selected step: Displacement/Rotation or Velocity/Angular velocity: select region: Motion: Follow underlying material

By default, all adaptive mesh constraints defined in the previous analysis step remain unchanged in the subsequent step. You define the adaptive mesh constraints in effect for a given step relative to the preexisting adaptive mesh constraints. At each new step the existing adaptive mesh constraints can be modified and additional adaptive mesh constraints can be specified.

ADAPTIVE MESH CONSTRAINT,
ADAPTIVE MESH CONSTRAINT, OP=MOD

Step module: OtherALE Adaptive Mesh ConstraintManager: select the desired step and mesh constraint: Edit

If you choose to remove any adaptive mesh constraint in a step, no adaptive mesh constraints will be propagated from the previous step. Therefore, all adaptive mesh constraints that are in effect during this step must be respecified.

ADAPTIVE MESH CONSTRAINT, OP=NEW

Step module: OtherALE Adaptive Mesh ConstraintManager: select the desired step and mesh constraint: Deactivate

By default, the boundary region created by a surface definition will be sliding (the surface edge will slide freely over the material).

SURFACE, REGION TYPE=SLIDING

To force the surface edge to follow the material, create a Lagrangian boundary region.

SURFACE, REGION TYPE=LAGRANGIAN

To decouple the surface from the material motion, create an Eulerian boundary region and apply spatial mesh constraints normal to the surface. If no mesh constraints are applied, the surface will behave like a sliding boundary region (no material will flow through the surface).

As an example, it is often assumed that there is no normal or shear stress in the material at the outflow boundary of an Eulerian domain. This condition can be modeled by defining an Eulerian boundary region using a surface and applying spatial mesh constraints perpendicular to the surface, as shown in Figure 5.

SURFACE, REGION TYPE=EULERIAN

Figure 5. Modeling the outflow boundary of an Eulerian adaptive mesh domain.

Lagrangian and sliding boundary regions created using surfaces can be used in contact pairs; they have the same meaning as surfaces defined on nonadaptive regions. Since contact generally involves relative sliding between bodies, sliding boundary regions are typically appropriate for contact surfaces.

Surfaces defined on Eulerian boundary regions cannot be used in contact pairs.

If the small-sliding formulation is used for a contact pair, all the nodes on both surfaces are nonadaptive (see About contact pairs in Abaqus/Explicit and Contact formulations for contact pairs in Abaqus/Explicit). The nodes of an element-based surface in a no-separation contact pair are nonadaptive (see Contact pressure-overclosure relationships). All nodes in a general contact domain are nonadaptive (see About general contact in Abaqus/Explicit). Similarly, the nodes at which spot welds are defined are nonadaptive (see Breakable bonds.)

By default, the boundary region created to coincide with a pressure load will be Lagrangian. Pressure loads applied to Lagrangian regions are identical to pressure loads applied to nonadaptive regions, except that the mesh can move inside the boundary region.

DLOAD, REGION TYPE=LAGRANGIAN

A pressure load can be applied to a sliding boundary region to simulate a load that is fixed in space while material moves past it (see Figure 7). A sliding edge is unconstrained in the direction tangential to the boundary region; therefore, unless adaptive mesh constraints are applied, the area of the load application will move according to the adaptive meshing algorithm, which is probably not physically meaningful.

To allow a pressure load to slide over the material, create a sliding boundary region.

DLOAD, REGION TYPE=SLIDING

Figure 7. Applying a sliding distributed pressure load to an adaptive mesh domain.

To decouple the area of pressure application from the material motion, create an Eulerian boundary region and apply spatial mesh constraints normal to the surface. If no mesh constraints are applied, the mesh will behave like a sliding boundary region (no material will flow through the surface).

As an example, it is often assumed that a uniform ambient pressure exists at the outflow boundary of an Eulerian domain. This condition can be modeled by defining the pressure at an Eulerian boundary region using a distributed load and applying spatial mesh constraints perpendicular to the surface, as shown in Figure 8.

DLOAD, REGION TYPE=EULERIAN

Figure 8. Modeling an ambient pressure at the outflow boundary of an Eulerian adaptive mesh domain.

By default, the boundary region created by a concentrated load will be Lagrangian. Each one-node Lagrangian boundary region will follow the material in every direction (the nodes will be nonadaptive).

CLOAD, REGION TYPE=LAGRANGIAN

A concentrated load can be applied to a sliding boundary region to simulate a load that is fixed in space while material moves past it (see Figure 9).

Figure 9. Applying a concentrated sliding load to an adaptive mesh domain.

A sliding node is unconstrained in the direction tangential to the boundary region; therefore, unless adaptive mesh constraints are applied, the point of load application will move according to the adaptive meshing algorithm, which is probably not physically meaningful.

To allow the concentrated load to slide freely over the material, create a sliding boundary region.

CLOAD, REGION TYPE=SLIDING

To decouple the concentrated load from the material motion, create an Eulerian boundary region and apply spatial mesh constraints normal to the surface. If no mesh constraints are applied, each one-node boundary region will behave like a sliding boundary region.

CLOAD, REGION TYPE=EULERIAN

By default, the boundary region created by a kinematic boundary condition will be Lagrangian. Abaqus/Explicit will recognize surface-type and point or edge constraints automatically and will create an appropriate Lagrangian boundary region for each type, as explained in the following subsections.

BOUNDARY, REGION TYPE=LAGRANGIAN

A sliding boundary region associated with a boundary condition can move according to the adaptive meshing algorithm. Since this behavior is probably not physically meaningful, the edges of a sliding boundary region are usually fixed in the direction tangential to the surface using adaptive mesh constraints. This approach can be used, for example, to simulate frictionless contact between a rigid punch and a deformable body, as shown in Figure 10.

Figure 10. Contact simulation using a sliding boundary region.

In this example the punch is replaced by a sliding boundary region with a constant velocity boundary condition applied in the area of “contact.” A tangential mesh constraint is applied to the edge of the boundary region at node N (the other edge is constrained by the Lagrangian boundary region created automatically on the symmetry plane). This problem definition allows material to flow radially underneath the “punch” while retaining the original size and location of the “contact” area.

Abaqus/Explicit makes no distinction between surface-type constraints and point or edge constraints for sliding boundary regions.

To allow the boundary condition to slide freely over the material, create a sliding boundary region.

BOUNDARY, REGION TYPE=SLIDING

To decouple the boundary region from the material motion, create an Eulerian boundary region and apply spatial mesh constraints normal to the surface. If no mesh constraints are applied, the mesh will behave like a sliding boundary region (no material will flow through the surface).

As an example, the mass flow rate at an Eulerian inflow boundary can be prescribed by defining an Eulerian boundary region using a boundary condition.

Abaqus/Explicit makes no distinction between surface-type constraints and point or edge constraints for Eulerian boundary regions.

BOUNDARY, REGION TYPE=EULERIAN

Edges shared by different types of boundary regions are subject to the following rules:

• An edge shared between a Lagrangian and a sliding boundary region will be Lagrangian.

• An edge shared between a Lagrangian and an Eulerian boundary region will be sliding.

• An edge shared between a Lagrangian and a nonadaptive boundary region will be nonadaptive.

• An edge shared between a sliding and a nonadaptive boundary region will be nonadaptive.

• An edge of an Eulerian boundary region can never be coincident with an edge of a nonadaptive region.