김경종
339 lines
18 KiB
Markdown
339 lines
18 KiB
Markdown
<!-- source-page: 1111 -->
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
F
|
||
t = t₀
|
||
N
|
||
flow
|
||
y
|
||
x
|
||
t = t₁
|
||
F
|
||
N
|
||
flow
|
||
Lagrangian
|
||
interpretation
|
||
t = t₁
|
||
F
|
||
N
|
||
material slides past this node
|
||
flow
|
||
zero-displacement adaptive mesh
|
||
constraint applied to node N in
|
||
direction 1
|
||
Sliding
|
||
interpretation
|
||
</details>
|
||
|
||
Figure 12.2.2–9 Applying a concentrated sliding load to an adaptive mesh domain.
|
||
|
||
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.
|
||
|
||
Input File Usage: \*CLOAD, REGION TYPE=SLIDING
|
||
|
||
Abaqus/CAE Usage: Boundary regions defined using concentrated loads are not supported in Abaqus/CAE.
|
||
|
||
# Defining an Eulerian boundary region with a concentrated load
|
||
|
||
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.
|
||
|
||
Input File Usage: \*CLOAD, REGION TYPE=EULERIAN
|
||
|
||
<!-- source-page: 1112 -->
|
||
|
||
Abaqus/CAE Usage: Boundary regions defined using concentrated loads are not supported in Abaqus/CAE.
|
||
|
||
# Concentrated fluxes and thermal conditions
|
||
|
||
In coupled thermal-stress analysis Abaqus/Explicit also creates boundary regions for concentrated heat fluxes, film conditions, and radiation conditions. The rules governing boundary regions for these loads are identical to those discussed for concentrated loads. The ability to specify the boundary region type is also the same.
|
||
|
||
# Boundary conditions
|
||
|
||
Lagrangian, sliding, and Eulerian boundary regions can be created by applying kinematic constraints to the boundary of an adaptive mesh domain. If kinematic boundary conditions are applied to nodes in the interior of an adaptive mesh domain, those nodes will move with the material in all directions (i.e., they will be nonadaptive), regardless of the specified boundary region type.
|
||
|
||
# Defining a Lagrangian boundary region using a boundary condition
|
||
|
||
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.
|
||
|
||
Input File Usage: \*BOUNDARY, REGION TYPE=LAGRANGIAN
|
||
|
||
Abaqus/CAE Usage: Boundary regions defined using boundary conditions are not supported in Abaqus/CAE.
|
||
|
||
# Surface-type constraints applied using boundary conditions
|
||
|
||
Although boundary conditions are always applied to individual nodes in Abaqus/Explicit, they often represent physical constraints on surfaces. For example, symmetry conditions, where nodes are constrained to move in a plane, are actually surface constraints. A fully clamped (ENCASTRE) condition along a boundary can also be considered a surface constraint. (During adaptive meshing it is meaningful to allow nodes to move along a fully clamped edge.)
|
||
|
||
Abaqus/Explicit will examine an adaptive mesh boundary and try to create regions that are coincident with the applied boundary conditions. Currently, Abaqus/Explicit can create boundary regions for surface-based constraints on:
|
||
|
||
• symmetry planes,
|
||
• fully clamped planes, and
|
||
• planes on which a uniform motion is prescribed.
|
||
|
||
Figure 12.2.2–2 shows an example in which boundary regions are created by applying surface-type boundary conditions. This figure shows a block of material with a crack and three symmetry planes (therefore, three Lagrangian boundary regions). Material will not flow across any symmetry plane, yet
|
||
|
||
<!-- source-page: 1113 -->
|
||
|
||
adaptive meshing can be performed within each Lagrangian boundary region. This flexibility is often helpful in problems that have significant deformation.
|
||
|
||
Point or edge constraints applied using boundary conditions
|
||
|
||
Some boundary conditions represent point or edge constraints. For example, a displacement can be prescribed at a node. The boundary regions associated with such nodes are exactly the same as those created by concentrated loads.
|
||
|
||
# Defining a sliding boundary region using a boundary condition
|
||
|
||
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 12.2.2–10.
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
zero-displacement adaptive mesh constraint applied to node N in direction 1
|
||
sliding boundary region created by velocity-type boundary condition applied to node set CONTACT
|
||
node set CONTACT
|
||
symmetry
|
||
(a) effect of punch modeled with contact
|
||
x
|
||
y
|
||
(b) effect of punch modeled with boundary conditions applied to sliding boundary region
|
||
</details>
|
||
|
||
Figure 12.2.2–10 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.
|
||
|
||
<!-- source-page: 1114 -->
|
||
|
||
Input File Usage: \*BOUNDARY, REGION TYPE=SLIDING
|
||
|
||
Abaqus/CAE Usage: Boundary regions defined using boundary conditions are not supported in Abaqus/CAE.
|
||
|
||
# Defining an Eulerian boundary region using a boundary condition
|
||
|
||
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.
|
||
|
||
Input File Usage: \*BOUNDARY, REGION TYPE=EULERIAN
|
||
|
||
Abaqus/CAE Usage: Boundary regions defined using boundary conditions are not supported in Abaqus/CAE.
|
||
|
||
# Overlapping boundary regions
|
||
|
||
A Lagrangian boundary region can overlap any number of other Lagrangian or sliding boundary regions (see Figure 12.2.2–11). If two boundary regions partially overlap, three regions are formed: the overlapping region and the two initial regions minus the overlapping region. A sliding boundary region is formed when a Lagrangian and a sliding boundary region overlap.
|
||
|
||
An Eulerian boundary region can never overlap a Lagrangian or sliding boundary region. Furthermore, an Eulerian boundary region can never share a boundary with or overlap a nonadaptive region. Because infinite elements are nonadaptive, this latter restriction implies that infinite elements cannot be used to simulate ambient conditions at an outflow boundary.
|
||
|
||
# Coincident edges
|
||
|
||
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.
|
||
|
||
# Predefined fields
|
||
|
||
There are no restrictions on applying prescribed temperatures or field variables in an adaptive mesh domain, but these nodal values are not remapped when adaptive meshing is performed. Therefore, predefined fields that are not spatially uniform may not be meaningful within an adaptive mesh domain.
|
||
|
||
<!-- source-page: 1115 -->
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
L
|
||
L
|
||
L
|
||
S
|
||
S
|
||
S
|
||
L
|
||
E
|
||
</details>
|
||
|
||
Lagrangian edge L = Lagrangian boundary region Sliding edge S = Sliding boundary region Lagrangian corner E = Eulerian boundary region
|
||
|
||
Figure 12.2.2–11 Overlapping boundary regions.
|
||
|
||
(Time-varying, spatially uniform predefined fields are acceptable, since adaptive meshing is applied at discrete instances in time.) However, if temperature or field variable data are collected from a spatial frame of reference, it may make physical sense to apply a spatially varying field for an Eulerian domain in which the mesh does not move. Abaqus/Explicit does not perform any checks or calculations on predefined fields for adaptive meshing; you must ensure that the predefined fields are meaningful.
|
||
|
||
# Materials
|
||
|
||
All material models and behaviors, except brittle cracking (“Cracking model for concrete,” Section 23.6.2), fabric (“Fabric material behavior,” Section 23.4.1), and low-density foam (“Low-density foams,” Section 22.9.1) materials, can be used in an adaptive mesh domain.
|
||
|
||
For domains modeled with hyperelastic or hyperfoam materials the usefulness of adaptive meshing is limited. The recommended enhanced hourglass method (“Section controls,” Section 27.1.4), which will generally predict a much better return to the original configuration for these materials when loading is removed, cannot be used in an adaptive mesh domain. Therefore, for hyperelastic or hyperfoam materials it is recommended that the analysis be run without adaptive meshing but with enhanced hourglass control.
|
||
|
||
If the porous failure model (“Failure criteria in Abaqus/Explicit” in “Porous metal plasticity,” Section 23.2.9), shear failure model (“Shear failure model” in “Dynamic failure models,” Section 23.2.8), tensile failure model (“Tensile failure model” in “Dynamic failure models,” Section 23.2.8), or one of the progressive damage models (Chapter 24, “Progressive Damage and Failure”) is specified within an adaptive mesh domain, Abaqus/Explicit will continuously monitor the status of elements while performing adaptive meshing. When elements within the domain fail, the nodes along the interface
|
||
|
||
<!-- source-page: 1116 -->
|
||
|
||
between the failed and unfailed elements will become nonadaptive. This has the effect of creating a material boundary between the failed and unfailed zones.
|
||
|
||
When failure occurs in elements that use the shear failure, the tensile failure, or the progressive damage models without element deletion, elements in the failure zone will not be deleted; they can carry some states of stress. Adaptive meshing will occur within the failure zone but not along the interface with the unfailed material.
|
||
|
||
# Elements
|
||
|
||
An adaptive mesh domain can contain only first-order, reduced-integration, solid elements. All elements within an adaptive mesh domain must have the same geometry (all two-dimensional, three-dimensional, axisymmetric, or plane strain, etc.). 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). All elements other than first-order, reduced-integration, solid elements—including mass, rotary inertia, and infinite elements—are nonadaptive. These elements can be connected to an adaptive mesh domain, but their nodes are nonadaptive. All nodes and elements on a rigid body are nonadaptive. Rebar are not supported within an adaptive mesh domain.
|
||
|
||
# Multi-point constraints and equations
|
||
|
||
As with boundary conditions, multi-point constraints (“General multi-point constraints,” Section 35.2.2) and equations (“Linear constraint equations,” Section 35.2.1) are always applied to nodes but sometimes represent constraints on surfaces. Abaqus/Explicit will recognize surface-type constraints when the following conditions are satisfied:
|
||
|
||
• an equation, PIN MPC, or TIE MPC ties a node set to a single node; and
|
||
• all the nodes involved in the MPC or equation are coplanar and lie within the boundary region.
|
||
|
||
If these conditions are satisfied, a boundary region will be associated with the node set in the MPC or equation. If the MPC is applied within a Lagrangian or sliding boundary region, a Lagrangian edge will be created. If the MPC is applied within an Eulerian boundary region, no edge will be created. If the above conditions are not satisfied, all nodes connected to the MPC or equation will be nonadaptive.
|
||
|
||
As an example, a constraint can be applied to force a plane section to remain plane in a Lagrangian adaptive mesh domain, as shown in Figure 12.2.2–12(a). In this case all nodes are constrained by an equation to lie in the same plane throughout the analysis, but adaptive meshing is allowed within the plane.
|
||
|
||
As another example, consider the outflow boundary of an Eulerian domain, as shown in Figure 12.2.2–12(b). The outflow boundary of an Eulerian domain is often assumed to be far enough downstream that the velocity is uniform but unknown. To model this condition, an Eulerian boundary region is created at the outflow boundary using a surface. An adaptive mesh constraint is used to fix the mesh perpendicular to the boundary, and all nodes on the plane are constrained by an equation to have the same velocity orthogonal to the plane.
|
||
|
||
For surface-based tie constraints (see “Mesh tie constraints,” Section 35.3.1), all nodes on the tied surfaces will be nonadaptive.
|
||
|
||
<!-- source-page: 1117 -->
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
symmetry
|
||
+
|
||
node set PLANE
|
||
1
|
||
</details>
|
||
|
||
Linear constraint equation
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
+
|
||
Lagrangian
|
||
boundary
|
||
region
|
||
</details>
|
||
|
||
|
||
|
||
(a) Using an equation to force a plane section to remain a plane.
|
||
|
||
|
||
<details>
|
||
<summary>flowchart</summary>
|
||
|
||
```mermaid
|
||
graph LR
|
||
A["material flow"] --> B["element set OUTFLOW"]
|
||
B --> C["node set OUTFLOW"]
|
||
C --> D["zero-displacement applied to right in direction"]
|
||
style A fill:#f9f,stroke:#333
|
||
style B fill:#ccf,stroke:#333
|
||
style C fill:#cfc,stroke:#333
|
||
style D fill:#fcc,stroke:#333
|
||
```
|
||
</details>
|
||
|
||
Linear constraint equation
|
||
acement adaptive mesh constraints node 1 and to node set OUTFLOW 1
|
||
|
||
|
||
Eulerian boundary region created using a surface defined on the S4 faces of element set OUTFLOW
|
||
(b) Using an equation to prescribe a uniform velocity outflow condition.
|
||
Figure 12.2.2–12 Using equations with adaptive meshing.
|
||
|
||
# Procedures
|
||
|
||
During an adiabatic analysis temperatures will be remapped properly in adaptive mesh domains. Adaptive meshing is not used during annealing procedures or during geometrically linear analyses.
|
||
|
||
<!-- source-page: 1118 -->
|
||
|
||
The definitions of adaptive mesh domains, boundary regions, mesh constraints, and controls (as explained in “ALE adaptive meshing and remapping in Abaqus/Explicit,” Section 12.2.3) will propagate from step to step.
|
||
|
||
# User subroutines
|
||
|
||
Solution-dependent state variables defined in user subroutine VUMAT will be remapped to the new mesh when adaptive meshing is performed.
|
||
|
||
Solution-dependent state variables that are defined on a slave surface in user subroutines VFRIC, VUINTER, VFRICTION, and VUINTERACTION will not be remapped to the new mesh when adaptive meshing is performed. Therefore, to ensure physically meaningful results, a Lagrangian adaptive mesh constraint should be used for nodes on the contact slave surfaces with solution-dependent state variables where the contact constraint is defined using these user subroutines.
|
||
|
||
# Output
|
||
|
||
Since the mesh is no longer constrained to the material when adaptive meshing is performed, output at elements and nodes must be interpreted differently than in a pure Lagrangian problem. See “Output and diagnostics for ALE adaptive meshing in Abaqus/Explicit,” Section 12.2.5, for details.
|
||
|
||
# Input file template
|
||
|
||
To create a Lagrangian adaptive mesh domain:
|
||
|
||
```txt
|
||
*HEADING
|
||
...
|
||
*ELSET, ELSET=ADAPT
|
||
**************************
|
||
*STEP
|
||
*DYNAMIC, EXPLICIT
|
||
Data line to specify the time period of the step
|
||
*ADAPTIVE MESH, ELSET=ADAPT
|
||
...
|
||
*END STEP
|
||
```
|
||
|
||
To create an Eulerian adaptive mesh domain with a prescribed velocity inflow condition and a prescribed pressure outflow condition (both in the global x-direction):
|
||
|
||
```prolog
|
||
*HEADING...
|
||
*ELSET, ELSET=ADAPT
|
||
...
|
||
*ELSET, ELSET=OUT
|
||
...
|
||
*NSET, NSET=INFLOW
|
||
...
|
||
```
|
||
|
||
<!-- source-page: 1119 -->
|
||
|
||
```txt
|
||
*NSET, NSET=OUTFLOW
|
||
...
|
||
*SURFACE, NAME=INSURF, REGION TYPE=EULERIAN
|
||
Data lines to define the surface
|
||
*SURFACE, NAME=OUTSURF, REGION TYPE=EULERIAN
|
||
Data lines to define the surface
|
||
...
|
||
*EQUATION
|
||
Data lines specifying uniform velocity at the inflow
|
||
**************************
|
||
*STEP
|
||
*DYNAMIC, EXPLICIT
|
||
Data line to specify the time period of the step
|
||
*ADAPTIVE MESH, ELSET=ADAPT
|
||
*ADAPTIVE MESH CONSTRAINT
|
||
INFLOW, 1, 1, 0
|
||
OUTFLOW, 1, 1, 0
|
||
*BOUNDARY, TYPE=VELOCITY, REGION TYPE=EULERIAN
|
||
INFLOW, 1, 1, 10.0
|
||
*DLOAD, REGION TYPE=EULERIAN
|
||
OUT, P2, 15.0
|
||
...
|
||
*END STEP
|
||
```
|
||
|
||
<!-- source-page: 1120 -->
|