김경종
19 KiB
Steady-state rolling example
This example shows how adaptive meshing can be used in a steady-state simulation to allow the flow of material through Eulerian boundaries on the problem domain. A steel plate is passed through a symmetric roll stand to reduce its height by 50%. This simulation is run until it reaches steady-state conditions.
Figure 12.2.1–5 and Figure 12.2.1–6 show the initial and final (steady-state) configurations in a purely Lagrangian model of this problem.
text_image
rigid roller plane of symmetry
Figure 12.2.1–5 The initial configuration of the roller and the undeformed blank in the pure Lagrangian model.
natural_image
Pure curved line diagram without any text, numbers, or symbols
Figure 12.2.1–6 The final steady-state configuration in the pure Lagrangian model.
Figure 12.2.1–7 shows this problem modeled using an Eulerian adaptive mesh domain, where material flows through the mesh. Only the region near the roller is modeled. The exact location of the free surface does not need to be known to set up the problem: it is created in a likely location, and the final steady-state position is found as part of the solution. Although not shown, a focused mesh can be
text_image
free surface 100 INFLOW OUTFLOW
Figure 12.2.1–7 The initial Eulerian adaptive mesh domain.
used to capture steep strain gradients directly beneath the roller. The Eulerian domain reaches the same steady-state solution as obtained with the Lagrangian approach.
The Eulerian adaptive mesh domain is created by defining an inflow and an outflow boundary on the adaptive mesh domain. Adaptive mesh constraints are applied normal to these boundaries so that material will flow through the mesh (see “Defining ALE adaptive mesh domains in Abaqus/Explicit,” Section 12.2.2). Frictional contact between the roller and the blank pulls material through the adaptive mesh domain.
The problem is set up by making the following modifications to the input file for the pure Lagrangian analysis:
*HEADING
...
*ELSET, ELSET=BILLET
...
*ELSET, ELSET=INFLOW
...
*ELSET, ELSET=OUTFLOW
...
*NSET, NSET=INFLOW
...
*NSET, NSET=OUTFLOW
...
*SURFACE, NAME=INFLOW, REGION TYPE=EULERIAN INFLOW, S1
*SURFACE, NAME=OUTFLOW, REGION TYPE=EULERIAN OUTFLOW, S2
**************************
*STEP
*DYNAMIC, EXPLICIT
Data line to specify the time period of the step
...
*ADAPTIVE MESH, ELSET=BILLET, CONTROLS=ADAPT
*ADAPTIVE MESH CONTROLS, NAME=ADAPT
*ADAPTIVE MESH CONSTRAINT, TYPE=DISPLACEMENT
INFLOW, 1, 1, 0.0
100, 2, 2, 0.0
OUTFLOW, 1, 1, 0.0
...
*END STEP
Adaptive mesh controls were not required to solve this problem; they were included for illustrative purposes (see “ALE adaptive meshing and remapping in Abaqus/Explicit,” Section 12.2.3, for details).
12.2.2 DEFINING ALE ADAPTIVE MESH DOMAINS IN Abaqus/Explicit
Products: Abaqus/Explicit Abaqus/CAE
References
• “ALE adaptive meshing: overview,” Section 12.2.1
• “ALE adaptive meshing and remapping in Abaqus/Explicit,” Section 12.2.3
• *ADAPTIVE MESH
• “Understanding ALE adaptive meshing,” Section 14.6 of the Abaqus/CAE User’s Guide
Overview
Arbitrary Lagrangian-Eulerian (ALE) adaptive mesh domains:
• define the portions of a finite element model where mesh movement is independent of material deformation;
• can be used to analyze Lagrangian or Eulerian problems;
• can contain only first-order, reduced-integration, solid elements (4-node quadrilaterals, 3-node triangles, 8-node hexahedra, 6-node wedges, and 4-node tetrahedra);
• can be used in planar, axisymmetric, and three-dimensional geometries;
• have boundary regions where loads, boundary conditions, and surfaces can be defined; and
• are active only for geometrically nonlinear steps.
Defining an ALE adaptive mesh domain
ALE adaptive meshing is performed in adaptive mesh domains, which can be either Lagrangian or Eulerian. Within either type of adaptive mesh domain the mesh will move independently of the material. Lagrangian adaptive mesh domains are usually used to analyze transient problems with large deformations. On the boundary of a Lagrangian domain the mesh will follow the material in the direction normal to the boundary, so that the mesh covers the same material domain at all times. Eulerian adaptive mesh domains are usually used to analyze steady-state processes involving material flow. On certain user-defined boundaries of an Eulerian domain, material can flow into or out of the mesh. By default, the mesh is not fixed spatially on these boundaries; mesh constraints must be applied to prevent the mesh from moving with the material, as described in “Mesh constraints,” presented later in this section. There can never be any “empty” elements; all elements in the domain must be filled completely with material at all times.
You must specify the region 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 (for example, to prevent material from flowing
from one domain to another or to apply adaptive meshing to unconnected domains). The element sets used to create adaptive mesh domains cannot overlap.
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.
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 adaptive mesh domain for this step
Splitting ALE adaptive mesh domains
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.
ALE adaptive mesh boundary regions
Each ALE adaptive mesh domain has a boundary, which can consist of one or more regions. (Regions, in this context, are surfaces in three-dimensional models or lines in two-dimensional or axisymmetric models.) A boundary region can be either Lagrangian, sliding, or Eulerian. Some boundary regions are created automatically by Abaqus/Explicit; others can be created by defining boundary conditions, loads, and surfaces. Adaptive mesh boundary regions are separated by edges in three dimensions and by corners in two dimensions. Both edges and corners are referred to as “boundary region edges” throughout this documentation.
Boundary region edges
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,” Section 12.2.5.
Lagrangian boundary regions
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.
Lagrangian corners
A Lagrangian corner is formed where two Lagrangian edges meet. The node at a Lagrangian corner is constrained to move with the material in all directions; it is nonadaptive.
Sliding boundary regions
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 “Surfaces: overview,” Section 2.3.1).
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
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,” Section 12.2.4.
Creation of boundary regions
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,” Section 3.5.3). 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 12.2.2–1 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.
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
Many models include distinct geometric kinks that take the form of geometric edges or corners. It is usually not desirable to perform adaptive meshing across such geometric features unless they flatten.
text_image
adaptive mesh domain nonadaptive domain material 1 adaptive mesh domain material 2 nonadaptive boundary region Lagrangian boundary region user-defined adaptive mesh domain: right half of box
Figure 12.2.2–1 Automatic splitting of mesh domains and creation of boundary regions.
Once a geometric feature does flatten, it is usually best if the feature is deactivated so that adaptive meshing will occur across it. This is especially true when adaptive mesh domains are subject to large deformation.
The adaptive meshing algorithm in Abaqus/Explicit will respect geometric features on Lagrangian and sliding boundaries. In three dimensions geometric features consist of edges and corners (see Figure 12.2.2–2), while in two dimensions they consist of only corners. If a geometric edge coincides with the edge of a Lagrangian boundary region, the presence of the geometric feature has no effect on the treatment of the edge: material cannot flow perpendicular to a Lagrangian edge.
Geometric features are not detected or tracked on Eulerian boundary regions because they generally are not physically meaningful.
Output options are available for viewing the formation of geometric edges and corners—see “Output and diagnostics for ALE adaptive meshing in Abaqus/Explicit,” Section 12.2.5.
Controlling the detection of geometric edges and corners
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 } \ \leq \ \theta _ { I } \ \leq ). See Figure 12.2.2–3. The default value for the initial geometric feature angle is \theta _ { I } = 3 0 ^ { \circ } .