김경종
303 lines
21 KiB
Markdown
303 lines
21 KiB
Markdown
<!-- source-page: 1141 -->
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
node set BACK
|
||
flow
|
||
element set LOAD
|
||
node set BOTTOM
|
||
z
|
||
y
|
||
x
|
||
z
|
||
sliding edge
|
||
lagrangian edge
|
||
geometric edge
|
||
zero-displacement adaptive mesh constraint
|
||
applied to node set LOADEDGE in direction 3
|
||
sliding boundary region defined by a pressure load
|
||
applied to element set LOAD in direction 1
|
||
lagrangian boundary region defined by symmetry
|
||
boundary conditions applied to node set BACK
|
||
about the x-direction and node set BOTTOM about
|
||
the y-direction
|
||
</details>
|
||
|
||
Figure 12.2.4–5 Applying a spatial pressure load to a portion of the surface along the length of an Eulerian control volume.
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
sliding edge
|
||
sliding boundary region defined
|
||
by a boundary condition
|
||
adaptive mesh constraint
|
||
flow
|
||
</details>
|
||
|
||
Figure 12.2.4–6 Applying a boundary condition along the entire length of the Eulerian control volume.
|
||
|
||
outflow boundary and act in a Lagrangian manner transversely to the flow. In three dimensions, symmetry conditions should typically act in a Lagrangian manner transverse to the flow direction. In many cases geometric edges will prevent material from flowing off the symmetry plane and
|
||
|
||
<!-- source-page: 1142 -->
|
||
|
||
onto the free surface. However, since geometric edges can be deactivated as surfaces flatten, Lagrangian boundary regions should be used to define the symmetry planes for these types of problems. In Figure 12.2.4–5 quarter-symmetry is assumed, and the symmetry planes are defined using Lagrangian boundary regions. The resulting Lagrangian edges that run from one Eulerian boundary to the other separate the symmetry planes from the free surface.
|
||
|
||
• Boundary conditions or loads that act on only a specific portion of the material between the inflow and outflow boundaries cannot usually be modeled for problems utilizing Eulerian control volumes. Since the mesh underneath the load or boundary condition must follow the material, it will eventually be restricted by the Eulerian boundary. This treatment of loads and boundary conditions is not usually consistent with a steady-state model and should not arise in practical simulations using Eulerian adaptive mesh domains.
|
||
|
||
<!-- source-page: 1143 -->
|
||
|
||
# 12.2.5 OUTPUT AND DIAGNOSTICS FOR ALE ADAPTIVE MESHING IN Abaqus/Explicit
|
||
|
||
Products: Abaqus/Explicit Abaqus/CAE
|
||
|
||
# References
|
||
|
||
• “Output to the output database,” Section 4.1.3
|
||
• “ALE adaptive meshing: overview,” Section 12.2.1
|
||
• “Defining ALE adaptive mesh domains in Abaqus/Explicit,” Section 12.2.2
|
||
• \*ADAPTIVE MESH
|
||
• \*ADAPTIVE MESH CONTROLS
|
||
• \*DIAGNOSTICS
|
||
• \*TRACER PARTICLE
|
||
• Chapter 78, “Using display groups to display subsets of your model,” of the Abaqus/CAE User’s Guide
|
||
|
||
# Overview
|
||
|
||
Output for ALE adaptive meshing:
|
||
|
||
• can be used to verify the automatic splitting of user-defined domains, the formation of Lagrangian edges and corners, the formation of geometric edges and corners, and the determination of nonadaptive nodes;
|
||
• must be interpreted carefully, since the values of output variables at specific locations in the mesh are no longer linked to values at particular material points;
|
||
• can include the definition of tracer particles, which follow material points and allow you to examine the trajectory of those points and plot material time histories of all element and nodal variables at those points; and
|
||
• can include diagnostic information on the efficiency of adaptive meshing and the accuracy of advection.
|
||
|
||
# Verifying the model
|
||
|
||
Output that can be used to verify adaptive meshing models is available in the data (.dat) file and in the output database (.odb) (see “Output,” Section 4.1.1, for details on these files).
|
||
|
||
# Element sets
|
||
|
||
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
|
||
|
||
<!-- source-page: 1144 -->
|
||
|
||
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.
|
||
|
||
# Edges and nonadaptive nodes
|
||
|
||
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:
|
||
|
||
• the domain element set name;
|
||
• the number of the subdivision (1 if no subdivisions were created);
|
||
• the letters LE for Lagrangian edge, GE for geometric edge or corner, or NA for nonadaptive nodes (including Lagrangian corners); and
|
||
• the step number.
|
||
|
||
For example, if a user-defined three-dimensional adaptive mesh domain specified for element set domain\_name is subdivided automatically into two adaptive mesh domains, Abaqus/Explicit will generate up to six node sets in the output database for the first step: domain\_name-1-LE-1, domain\_name-1-GE-1, domain\_name-1-NA-1, domain\_name-2-LE-1, domain\_name-2-GE-1, and domain\_name-2-NA-1.
|
||
|
||
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.
|
||
|
||
# Interpreting results
|
||
|
||
When adaptive meshing is not performed, the finite element mesh follows the material, which enables a straightforward interpretation of analysis results. You can visualize deformation and material motion by studying the motion of the mesh. Each nodal and element output variable corresponds to a specific material location, because the mesh is fixed to the same material point throughout time.
|
||
|
||
<!-- source-page: 1145 -->
|
||
|
||
Once adaptive meshing takes place, the locations of mesh and material points deviate, and analysis results must be interpreted accordingly. The motion of the mesh on the interior of an adaptive mesh domain represents the composite effects of the material motion and adaptive meshing. The motion of the mesh and the motion of the material on Lagrangian and sliding boundary regions is identical in the direction normal to the boundary but not in the direction tangential to it.
|
||
|
||
# Nodal variables
|
||
|
||
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.
|
||
|
||
# Element variables
|
||
|
||
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.
|
||
|
||
# Tracking nodal or element variables at material points
|
||
|
||
Tracer particles can be defined to track material points in an adaptive mesh domain. These particles can also be used to obtain time histories of nodal or element integration point variables that correspond to the time variation of the variable at a specific material point. Tracer particles are defined as described below (see “Output to the output database,” Section 4.1.3, for more information). Node and element variable output can be requested for tracer particle sets to examine the trajectory of material particles or to obtain material time histories. Output for tracer particles can be written only to the output database (.odb).
|
||
|
||
# Using tracer particles in Lagrangian domains
|
||
|
||
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.
|
||
|
||
<!-- source-page: 1146 -->
|
||
|
||
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.
|
||
|
||
Input File Usage: Use the following option to define a tracer particle set:
|
||
|
||
\*TRACER PARTICLE, TRACER SET=tracer\_set\_name list of tracer particle parent nodes
|
||
|
||
Abaqus/CAE Usage: Tracer particles are not supported in Abaqus/CAE.
|
||
|
||
# Using tracer particles in Eulerian domains
|
||
|
||
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.
|
||
|
||
<!-- source-page: 1147 -->
|
||
|
||
Input File Usage: Use the following option to define a tracer particle set with multiple birth stages:
|
||
|
||
\*TRACER PARTICLE, TRACER SET=tracer\_set\_name, PARTICLE BIRTH STAGES=n list of tracer particle parent nodes
|
||
|
||
Abaqus/CAE Usage: Tracer particles are not supported in Abaqus/CAE.
|
||
|
||
# Monitoring the progress of ALE adaptive meshing
|
||
|
||
Diagnostic information can be written to the message (.msg) file to track the efficiency and accuracy of adaptive meshing. You can select the level of diagnostic output that is written.
|
||
|
||
# Obtaining a summary at the end of a step
|
||
|
||
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:
|
||
|
||
• the average percentage of nodes moved,
|
||
• the maximum percentage of nodes moved,
|
||
• the minimum percentage of nodes moved, and
|
||
• the average number of advection sweeps.
|
||
|
||
Each value is calculated for a single adaptive mesh domain over all adaptive mesh increments. The cost of advection is approximately proportional to the percentage of nodes moved, since variables are not advected for elements that have not been relocated during adaptive meshing.
|
||
|
||
Input File Usage: Use the following option to request a summary for each adaptive mesh domain at the end of each step:
|
||
|
||
\*DIAGNOSTICS, ADAPTIVE MESH=STEP SUMMARY
|
||
|
||
Abaqus/CAE Usage: Adaptive mesh diagnostics are not supported in Abaqus/CAE.
|
||
|
||
# Obtaining a summary for every ALE adaptive mesh increment
|
||
|
||
In addition to the step summary information, the following diagnostics can be obtained for each adaptive mesh domain at every adaptive mesh increment:
|
||
|
||
• the percentage of nodes moved, and
|
||
• the number of advection sweeps.
|
||
|
||
Input File Usage: Use the following option to obtain summary information at the end of the step and at every adaptive mesh increment:
|
||
|
||
\*DIAGNOSTICS, ADAPTIVE MESH=SUMMARY
|
||
|
||
Abaqus/CAE Usage: Adaptive mesh diagnostics are not supported in Abaqus/CAE.
|
||
|
||
# Obtaining details of advection accuracy for every ALE adaptive mesh increment
|
||
|
||
The following detailed diagnostic information can also be written to the message (.msg) file to track the accuracy of the advection:
|
||
|
||
<!-- source-page: 1148 -->
|
||
|
||
• mass and momentum before and after advection, and
|
||
• percentage volume change.
|
||
|
||
Input File Usage: Use the following option to request the most detailed diagnostics, which include advection accuracy measures and summary information for each adaptive mesh domain, reported at every adaptive mesh increment:
|
||
|
||
\*DIAGNOSTICS, ADAPTIVE MESH=DETAIL
|
||
|
||
Abaqus/CAE Usage: Adaptive mesh diagnostics are not supported in Abaqus/CAE.
|
||
|
||
# Suppressing ALE adaptive mesh diagnostics
|
||
|
||
You can suppress output of all adaptive mesh diagnostic information.
|
||
|
||
Input File Usage: \*DIAGNOSTICS, ADAPTIVE MESH=OFF
|
||
|
||
Abaqus/CAE Usage: Adaptive mesh diagnostics are not supported in Abaqus/CAE.
|
||
|
||
<!-- source-page: 1149 -->
|
||
|
||
# 12.2.6 DEFINING ALE ADAPTIVE MESH DOMAINS IN Abaqus/Standard
|
||
|
||
Products: Abaqus/Standard Abaqus/CAE
|
||
|
||
# References
|
||
|
||
• “ALE adaptive meshing: overview,” Section 12.2.1
|
||
• “ALE adaptive meshing and remapping in Abaqus/Standard,” Section 12.2.7
|
||
• \*ADAPTIVE MESH
|
||
• \*ADAPTIVE MESH CONSTRAINT
|
||
• \*ADAPTIVE MESH CONTROLS
|
||
• “Customizing ALE adaptive meshing,” Section 14.14 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
|
||
# Overview
|
||
|
||
ALE adaptive meshing in Abaqus/Standard:
|
||
|
||
• maintains a topologically similar mesh;
|
||
• can be used to solve Lagrangian problems (in which no material leaves the mesh) and to model effects of ablation, or wear (in which material is eroded at the boundary);
|
||
• can be used in static stress/displacement analysis, steady-state transport analysis, coupled pore fluid flow and stress analysis, and coupled temperature-displacement analysis;
|
||
• can be used only in geometrically nonlinear general analysis steps; and
|
||
• is available only for acoustic elements and a subset of the solid elements.
|
||
|
||
# Defining an ALE adaptive mesh domain
|
||
|
||
You can apply ALE adaptive mesh smoothing to an entire model or to individual parts of the model as a step-dependent feature. Adaptive meshing for solid elements in Abaqus/Standard uses a subset of the adaptive meshing functionality available in Abaqus/Explicit.
|
||
|
||
You must specify the portion of the original mesh that will be subject to adaptive meshing.
|
||
|
||
Input File Usage: \*ADAPTIVE MESH, ELSET=name
|
||
|
||
Multiple adaptive mesh domains can be defined in a step by reusing the \*ADAPTIVE MESH option, but each element set must refer to a unique set of elements.
|
||
|
||
Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Domain→Edit: toggle on Use the ALE adaptive mesh domain below, and click Edit to select the region
|
||
|
||
Only one adaptive mesh domain can be defined in Abaqus/CAE for any particular step.
|
||
|
||
<!-- source-page: 1150 -->
|
||
|
||
# Modifying an ALE adaptive mesh domain
|
||
|
||
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).
|
||
|
||
Input File Usage: Use either of the following options to modify an existing adaptive mesh domain or to specify an additional adaptive mesh domain:
|
||
|
||
\*ADAPTIVE MESH, ELSET=name
|
||
|
||
\*ADAPTIVE MESH, ELSET=name, OP=MOD
|
||
|
||
Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Domain→Edit
|
||
|
||
# Removing an ALE adaptive mesh domain
|
||
|
||
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.
|
||
|
||
Input File Usage: Use the following option to remove all previously defined adaptive mesh domains and to specify new adaptive mesh domains:
|
||
|
||
\*ADAPTIVE MESH, ELSET=name, OP=NEW
|
||
|
||
If the OP=NEW parameter is used on any \*ADAPTIVE MESH option within a step, it must be used on all \*ADAPTIVE MESH options in the step.
|
||
|
||
Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Domain→Edit: toggle on No ALE adaptive mesh domain for this step
|
||
|
||
# Splitting ALE adaptive mesh domains
|
||
|
||
Abaqus/Standard may subdivide each adaptive mesh domain that you specify such that
|
||
|
||
• all elements in an adaptive domain refer to one element property definition; and
|
||
• all elements in an adaptive domain are of similar type (such as hybrid elements with linear pressure).
|
||
|
||
If Abaqus/Standard subdivides the adaptive mesh domains that you specified, each of the adaptive mesh domain subdivisions will have a new name, which will be used for output and diagnostic purposes. The new names will be formed by concatenating the name of the user-specified element set, a number identifying the subdivision, and the step number. Each of the subdivisions will be further examined to ensure that all the elements in a subdivision are subjected to the same body forces. You may be asked to modify the definition of the adaptive mesh domain to satisfy this requirement.
|
||
|
||
# ALE adaptive mesh regions
|
||
|
||
Each adaptive mesh domain has an interior region and a boundary region. The boundary region may include distinct kinks that take the form of geometric edges or corners. The nodes on the boundary region
|