When user-defined adaptive mesh domains are split by ABAQUS/Explicit, the elements that compose the new subdivided domains are printed to the data (.dat) file.

New element sets are created and written to the output database (.odb) for all adaptive mesh domains. The name of the element set created for each domain is the user-defined name, plus the number of the subdivision (1 if no subdivisions were created), plus the step number. For example, if the user-defined adaptive mesh domain specified for the element set domain_name spanned three disjoint parts, ABAQUS/Explicit would subdivide the user-defined domain into three domains and create three element sets in the output database (.odb) for the first step: domain_name-1-1, domain_name-2-1, and domain_name-3-1.

ABAQUS/CAE can be used to verify the creation of the subdivided domains.

ABAQUS/Explicit automatically forms Lagrangian edges and corners and identifies nonadaptive nodes based on the topology of the adaptive mesh domains, connections to nonadaptive domains, and user-specified boundary regions. Furthermore, geometric edges and corners are formed automatically based on the initial geometry and the value of the initial feature angle. See “Defining ALE adaptive mesh domains in ABAQUS/Explicit,” Section 12.2.2. Lagrangian edges, geometric edges and corners, and nonadaptive nodes (including Lagrangian corners) are output to the data (.dat) file for each adaptive mesh domain. This information can be obtained by requesting a history definition summary printout to the data file (see “Model and history definition summaries” in “Output,” Section 4.1.1) or by monitoring the progress of the adaptive meshing (see “Monitoring the progress of ALE adaptive meshing” below).

In addition, up to three node sets are created in the output database (.odb) for each adaptive mesh domain in each step. The names of the node sets are created by concatenating the following information:

Since boundary regions are separated by corners, not edges, in two dimensions, node sets will not be created for Lagrangian edges in two-dimensional adaptive mesh domains. The Lagrangian corners are included in the nonadaptive (NA) node set, as for three-dimensional domains.

ABAQUS/CAE can be used to verify the creation of Lagrangian edges and corners, geometric edges and corners, and nonadaptive nodes.

When adaptive meshing is performed, a material point that is coincident with a node at the beginning of the step may not remain coincident with that node throughout the step. Values of displacement and current coordinates represent the motion of the node, not necessarily the motion of the material. All other nodal variables—including velocity, acceleration, and reaction forces—represent the value of the variable for the material particle at the current location of the node. Contour or vector plots of these variables will show their correct spatial distribution and are, therefore, meaningful. However, time histories of nodal variables for nodes that undergo adaptive meshing are generally not meaningful. In steady-state problems, though, a velocity or acceleration time history based at a fixed spatial location rather than at a specific material point may be useful.

Similarly, when adaptive meshing is performed, a material particle that is coincident with an element integration point at the beginning of a step may not remain so throughout the step. Therefore, element integration point variables do not necessarily represent values at the same material point throughout the step. Contour or vector plots of element integration point variables are meaningful for the same reasons described for nodal variables. However, time histories are based at the spatial location of the element integration point and not at a specific material point.

Whole element variables have a similar interpretation.

In most adaptive meshing simulations using Lagrangian domains, the nodes and elements in the domain correspond neither to a specific spatial location nor to a specific material point or volume. Thus, time histories of variables at nodes and at element integration points are often physically meaningless in a Lagrangian adaptive mesh domain. Tracer particles should be defined to view time history information. Tracer particles can also be used to visualize the motion of the material.

The initial location of a tracer particle is defined to be coincident with a node, termed the parent node. Tracer particles are defined in sets by defining multiple parent nodes or node sets. You indicate the nodes whose current locations correspond to the initial location of the tracer particles and assign a name to the tracer particle set to identify it for use in output requests. Tracer particles are released from their parent nodes repeatedly at specified intervals during the step in which they are defined. The particles follow material points for the remainder of that step and in all subsequent steps.

Tracer particles are typically defined only on adaptive mesh domains, although they can be defined on nodes connected to any low-order solid element in the model. For analyses in which adaptive meshing is not performed until later steps, tracer particles can be defined on nonadaptive domains at the beginning of an analysis and will be tracked continuously as the domain becomes adaptive. Similarly, tracer particles will be tracked from domain to domain if adaptive mesh domain topologies change from step to step.

*TRACER PARTICLE, TRACER SET=tracer_set_name
list of tracer particle parent nodes

Time histories at nodes and element integration points in an Eulerian domain may have physical meaning at points where spatial adaptive mesh constraints are applied. For example, the time variation of equivalent plastic strain in elements along an outflow Eulerian boundary acts as a spatial time history of that variable and can be used to evaluate whether the process has reached a steady-state solution.

Tracer particles can be defined to evaluate the material time history of variables at a material point as it flows through the Eulerian domain. Tracer particles can also be used to evaluate the trajectory and path of material points as they pass through the domain.

Tracer particles can be assigned to any parent node in an Eulerian adaptive mesh domain. If a tracer particle reaches an outflow boundary and material continues to flow out, the tracer particle will no longer be tracked and all output history variables associated with the tracer particle will be zero after deactivation.

When material flow through the mesh domain is significant, sets of tracer particles can be released from the current locations of the parent nodes at multiple times during the step. Each release of tracer particles is referred to as particle birth. After particle birth the tracer particles follow the motion of the material regardless of the motion of the mesh. You can indicate the number of particle birth stages in a step. These stages will be evenly spaced throughout the time period of the step.

For example, a tracer particle set can be defined such that all nodes along an inflow Eulerian boundary are parent nodes. Multiple birth stages can be specified so that a set of tracer particles is released from the mesh at the inflow boundary periodically during the step. If enough birth stages are defined, the domain will eventually be spanned with tracer particles as material flows from the inflow boundary to the outflow boundary.

*TRACER PARTICLE, TRACER SET=tracer_set_name, PARTICLE BIRTH STAGES=n
list of tracer particle parent nodes

By default, a summary of adaptive meshing information for each adaptive mesh domain will be written to the message (.msg) file at the end of each step. This summary information includes:

*DIAGNOSTICS, ADAPTIVE MESH=STEP SUMMARY

In addition to the step summary information, the following diagnostics can be obtained for each adaptive mesh domain at every adaptive mesh increment:

*DIAGNOSTICS, ADAPTIVE MESH=SUMMARY

The following detailed diagnostic information can also be written to the message (.msg) file to track the accuracy of the advection:

*DIAGNOSTICS, ADAPTIVE MESH=DETAIL

You can suppress output of all adaptive mesh diagnostic information.

*DIAGNOSTICS, ADAPTIVE MESH=OFF