김경종
27 KiB
text_image
y z-symmetry crack front x-symmetry z y-symmetry x y z geometric corner Lagrangian corner plus geometric corner geometric edge Lagrangian edge
Figure 12.2.2–2 Geometric features formed on a solid block with a crack.
text_image
θ > θ₁ n n
Initial mesh with a geometric feature: no mesh flow is permitted past the corner.
text_image
n n θ θ ≤ θ_T
The geometric feature is deactivated during simulation.
Figure 12.2.2–3 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 } = 1 8 0 ^ { \circ } will ensure that no geometric edges or corners are formed on the boundary of the adaptive mesh domain.
Input File Usage: *ADAPTIVE MESH CONTROLS, NAME=name, INITIAL FEATURE ANGLE=
Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, Initial feature angle: \theta _ { I }
Controlling the deactivation of geometric edges and corners
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,” Section 12.2.3). 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 } ~ \leq ~ \theta _ { T } ~ \leq ~ 1 8 0 ^ { \circ } ) . The default value for the transition feature angle is \theta _ { T } = 3 0 ^ { \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.
Input File Usage: *ADAPTIVE MESH CONTROLS, NAME=name, TRANSITION FEATURE ANGLE=
Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, Transition feature angle: \theta _ { T }
Mesh constraints
In most adaptive mesh problems the motion of nodes in the mesh is determined by the meshing algorithm, with constraints imposed by the domain boundary and the boundary region edges. However, there are cases when you must explicitly define the motion of the nodes. As explained earlier, Eulerian and sliding boundary regions generally require mesh constraints for the regions to be physically meaningful. In some problems you may wish to keep certain nodes fixed, to move nodes in a particular direction, or to force certain nodes to move with the material. In other problems you may desire a node or particular set of nodes to follow the material motion. Adaptive mesh constraints allow full control over the mesh movement and act independently of any boundary conditions or loads applied to the underlying material.
Applying spatial mesh constraints
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.
Input File Usage: Use the following option to define the mesh constraints explicitly: *ADAPTIVE MESH CONSTRAINT, CONSTRAINT TYPE=SPATIAL, TYPE=DISPLACEMENT or VELOCITY
Abaqus/CAE Usage: To define the mesh constraints explicitly:
Step module: Other→ALE Adaptive Mesh Constraint→Create: 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 twodimensional 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 12.2.2–4).
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 } \leq \theta _ { C } \leq 8 5 ^ { \circ } ) . Setting \theta _ { C } < 4 5 ^ { \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=
Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Mesh constraint angle: \theta _ { C }
Defining mesh constraints that vary with time
The prescribed magnitude of a nonzero mesh constraint can vary with time during a step according to an amplitude definition (see “Amplitude curves,” Section 34.1.2).
Input File Usage: Use both of the following options:
*AMPLITUDE, NAME=name *ADAPTIVE MESH CONSTRAINT, AMPLITUDE=name
text_image
zero-displacement adaptive mesh constraint applied at node 3 in direction 1 direction of applied constraint Θ < Θc, analysis is terminated movement of node 3 without mesh constraint motion of node 3 along surface to satisfy constraint boundary region t = t0 t = t1 y n 3 4 5 n 3 4 5 x projection of mesh motion in prescribed direction
Figure 12.2.2–4 Enforcing a spatial mesh constraint.
Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Constraint→Create: Types for selected step: Displacement/Rotation or Velocity/Angular velocity: select region: Motion: Independent of underlying material: Amplitude: amplitude
Applying spatial mesh constraints in local directions
Spatial mesh constraints are applied in local directions if a local coordinate system is defined at a node (see “Transformed coordinate systems,” Section 2.1.5); otherwise, they are applied in global directions.
Applying Lagrangian mesh constraints
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.
Input File Usage: *ADAPTIVE MESH CONSTRAINT, CONSTRAINT TYPE=LAGRANGIAN
Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Constraint→Create: Types for selected step: Displacement/Rotation or Velocity/Angular velocity: select region: Motion: Follow underlying material
Modifying ALE adaptive mesh constraints
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.
Input File Usage: Use either of the following options to modify an existing adaptive mesh constraint or to specify an additional adaptive mesh constraint:
*ADAPTIVE MESH CONSTRAINT, *ADAPTIVE MESH CONSTRAINT, OP=MOD
Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Constraint→Manager: select the desired step and mesh constraint: Edit
Removing ALE adaptive mesh constraints
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.
Input File Usage: Use the following option to remove all previously defined adaptive mesh constraints and to specify new adaptive mesh constraints:
*ADAPTIVE MESH CONSTRAINT, OP=NEW
If the OP=NEW parameter is used on any *ADAPTIVE MESH CONSTRAINT option within a step, it must be used on all *ADAPTIVE MESH CONSTRAINT options in the step.
Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Constraint→Manager: select the desired step and mesh constraint: Deactivate
Initial conditions
There are no initial conditions specific to adaptive meshing; initial conditions can be defined in the same way as in nonadaptive problems. If initial mesh sweeps are performed to smooth the mesh at the beginning of a step (see “ALE adaptive meshing and remapping in Abaqus/Explicit,” Section 12.2.3), all initial conditions (except temperatures and field variables, which are discussed in “Predefined fields,” presented later in this section) are remapped to the new mesh. Initial temperatures are remapped during adaptive meshing in an adiabatic analysis.
Initial conditions prescribed near an inflow Eulerian boundary region will affect the state of the material flowing into the domain throughout the analysis. See “Modeling techniques for Eulerian adaptive mesh domains in Abaqus/Explicit,” Section 12.2.4, for a discussion of the proper treatment of inflow boundaries.
Defining surfaces on ALE adaptive mesh boundaries
When you define a surface on the boundary of an adaptive mesh domain (see “Surfaces: overview,” Section 2.3.1), Abaqus creates a boundary region coinciding with the surface. By default, a sliding boundary region is created. You can choose to create a Lagrangian or Eulerian boundary region instead.
A surface defined in the interior of an adaptive mesh domain will move independently of the material (unless constrained by mesh constraints).
Defining a sliding boundary region using a surface
By default, the boundary region created by a surface definition will be sliding (the surface edge will slide freely over the material).
Input File Usage: *SURFACE, REGION TYPE=SLIDING
Abaqus/CAE Usage: Boundary regions defined using surfaces are not supported in Abaqus/CAE.
Defining a Lagrangian boundary region using a surface
To force the surface edge to follow the material, create a Lagrangian boundary region.
Input File Usage: *SURFACE, REGION TYPE=LAGRANGIAN
Abaqus/CAE Usage: Boundary regions defined using surfaces are not supported in Abaqus/CAE.
Defining an Eulerian boundary region using a surface
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 12.2.2–5.
Input File Usage: *SURFACE, REGION TYPE=EULERIAN
Abaqus/CAE Usage: Boundary regions defined using surfaces are not supported in Abaqus/CAE.
Contact
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.
flowchart
graph TD
A["free surface"] --> B["Lagrangian boundary region (automatic)"]
B --> C["node set OUT"]
C --> D["Eulerian boundary region (defined using a surface)"]
D --> E["symmetry"]
E --> F["Lagrangian boundary region (automatic)"]
F --> G["zero-displacement adaptive mesh constraint applied to node set OUT in direction 1"]
Figure 12.2.2–5 Modeling the outflow boundary of an Eulerian adaptive mesh domain.
If the small-sliding formulation is used for a contact pair, all the nodes on both surfaces are nonadaptive (see “Defining contact pairs in Abaqus/Explicit,” Section 36.5.1, and “Contact formulations for contact pairs in Abaqus/Explicit,” Section 38.2.2). The nodes of an element-based surface in a no-separation contact pair are nonadaptive (see “Contact pressure-overclosure relationships,” Section 37.1.2). All nodes in a general contact domain are nonadaptive (see “Defining general contact interactions in Abaqus/Explicit,” Section 36.4.1). Similarly, the nodes at which spot welds are defined are nonadaptive (see “Breakable bonds,” Section 37.1.9.)
Distributed loads
When a distributed pressure load is applied to the boundary of an adaptive mesh domain, Abaqus/Explicit creates a boundary region that coincides with the area of the load application. The characteristics of boundary regions created in this way are identical to those of boundary regions created by defining surfaces. If a pressure load is applied to a surface in the interior of an adaptive mesh domain, the nodes on the surface will move with the material in all directions (i.e., they will be nonadaptive).
Boundary regions created by different pressure loads may overlap. If pressure loads with the same magnitude and amplitude definition are applied to adjacent regions, the regions will be merged into a single boundary region to minimize the number of Lagrangian edges and corners formed (see Figure 12.2.2–6).
If a nonuniform pressure is applied (for example, a pressure that varies linearly over a surface) or if a pressure load is defined in user subroutine VDLOAD, each element face or edge becomes a separate Lagrangian boundary region. Since Lagrangian corners are formed where Lagrangian edges meet, all
flowchart
graph TD
A["If these distributed loads have identical magnitudes and amplitude definitions, they will be combined into one Lagrangian boundary region."] --> B["Overlapping distributed loads result in three Lagrangian boundary regions."]
B --> C["This node is adaptive because the sliding boundary region does not create a Lagrangian corner."]
style A fill:#f9f,stroke:#333
style B fill:#ccf,stroke:#333
style C fill:#cfc,stroke:#333
L = Lagrangian boundary region created by pressure load
S = Sliding boundary region created by pressure load
= Lagrangian corner
Figure 12.2.2–6 Applying distributed pressure loads to an adaptive mesh domain.
nodes will follow the material in every direction, and each region becomes nonadaptive. Likewise, if a nonuniform body force is applied to an adaptive mesh domain, the domain is split into multiple domains, each with a uniform body force. If this splitting results in one-element domains, the region becomes nonadaptive.
Defining a Lagrangian boundary region with a pressure load
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.
Input File Usage: *DLOAD, REGION TYPE=LAGRANGIAN
Abaqus/CAE Usage: Boundary regions defined using pressure loads are not supported in Abaqus/CAE.
Defining a sliding boundary region with a pressure load
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 12.2.2–7). 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.
Input File Usage: *DLOAD, REGION TYPE=SLIDING
Abaqus/CAE Usage: Boundary regions defined using pressure loads are not supported in Abaqus/CAE.
flowchart
graph TD
A["t = t₀"] --> B["Flow"]
B --> C["Timepoint 1"]
C --> D["Flow"]
D --> E["Timepoint 4"]
E --> F["Flow"]
F --> G["Timepoint 1"]
G --> H["Timepoint 4"]
H --> I["Timepoint 1"]
I --> J["Timepoint 4"]
J --> K["Timepoint 1"]
K --> L["Timepoint 4"]
L --> M["Timepoint 1"]
M --> N["Timepoint 4"]
N --> O["Timepoint 1"]
O --> P["Timepoint 4"]
P --> Q["Timepoint 1"]
Q --> R["Timepoint 4"]
R --> S["Timepoint 1"]
S --> T["Timepoint 4"]
T --> U["Timepoint 1"]
U --> V["Timepoint 4"]
V --> W["Timepoint 1"]
W --> X["Timepoint 4"]
X --> Y["Timepoint 1"]
Y --> Z["Timepoint 4"]
Z --> AA["Timepoint 1"]
AA --> AB["Timepoint 4"]
AB --> AC["Timepoint 1"]
AC --> AD["Timepoint 4"]
AD --> AE["Timepoint 1"]
AE --> AF["Timepoint 4"]
AF --> AG["Timepoint 1"]
AG --> AH["Timepoint 4"]
AH --> AI["Timepoint 1"]
AI --> AJ["Timepoint 4"]
AJ --> AK["Timepoint 1"]
AK --> AL["Timepoint 4"]
AL --> AM["Timepoint 1"]
AM --> AN["Timepoint 4"]
AN --> AO["Timepoint 1"]
AO --> AP["Timepoint 4"]
AP --> AQ["Timepoint 1"]
AQ --> AR["Timepoint 4"]
AR --> AS["Timepoint 1"]
AS --> AT["Timepoint 4"]
AT --> AU["Timepoint 1"]
AU --> AV["Timepoint 4"]
AV --> AW["Timepoint 1"]
AW --> AX["Timepoint 4"]
AX --> AY["Timepoint 1"]
AY --> AZ["Timepoint 4"]
AZ --> BA["Timepoint 1"]
BA --> BB["Timepoint 4"]
BB --> BC["Timepoint 1"]
BC --> BD["Timepoint 4"]
BD --> BE["Timepoint 1"]
BE --> BF["Timepoint 4"]
BF --> BG["Timepoint 1"]
BG --> BH["Timepoint 4"]
BH --> BI["Timepoint 1"]
BI --> BJ["Timepoint 4"]
BJ --> BK["Timepoint 1"]
BK --> BL["Timepoint 4"]
BL --> BM["Timepoint 1"]
BM --> BN["Timepoint 4"]
BN --> BO["Timepoint 1"]
BO --> BP["Timepoint 4"]
BP --> BQ["Timepoint 1"]
BQ --> BR["Timepoint 4"]
BR --> BS["Timepoint 1"]
BS --> BT["Timepoint 4"]
BT --> BU["Timepoint 1"]
BU --> BV["Timepoint 4"]
BV --> BW["Timepoint 1"]
BW --> BX["Timepoint 4"]
BX --> BY["Timepoint 1"]
BX --> BZ["Timepoint 4"]
BZ --> CA["Timepoint 1"]
CA --> CB["Timepoint 4"]
CB --> CC["Timepoint 1"]
CC --> CD["Timepoint 4"]
CD --> CE["Timepoint 1"]
CE --> CF["Timepoint 4"]
CF --> CG["Timepoint 1"]
CG --> CH["Timepoint 4"]
CH --> CI["Timepoint 1"]
CI --> CJ["Timepoint 4"]
CJ --> CK["Timepoint 1"]
CK --> CR["Timepoint 4"]
CR --> CS["Timepoint 1"]
CS --> CT["Timepoint 4"]
CT --> CU["Timepoint 1"]
CU --> CV["Timepoint 4"]
CV --> CW["Timepoint 1"]
CW --> CX["Timepoint 4"]
CX --> CY["Timepoint 1"]
CY --> CZ["Timepoint 4"]
CZ --> DA["Timepoint 1"]
DA --> DB["Timepoint 4"]
DB --> DC["Timepoint 1"]
DC --> DD["Timepoint 4"]
DD --> DE["Timepoint 1"]
DE --> DF["Timepoint 4"]
DF --> DG["Timepoint 1"]
DG --> DH["Timepoint 4"]
DH --> DI["Timepoint 1"]
DI --> DJ["Timepoint 4"]
DJ --> DK["Timepoint 1"]
DK --> DL["Timepoint 4"]
DL --> DJ["Timepoint 1"]
DJ --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
D --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
DK --> DK
style DK fill:#f9f,stroke:#333,stroke-width:2px
style DK fill:#ccf,stroke:#333,stroke-width:2px
style DK fill:#cfc,stroke:#333,stroke-width:2px
style DK fill:#fcc,stroke:#333,stroke-width:2px
style DK fill:#cff,stroke:#333,stroke-width:2px
style DK fill:#ffc,stroke:#333,stroke-width:2px
style DK fill:#cfc,stroke:#333,stroke-width:2px
style DK fill:#fcc,stroke:#333,stroke-width:2px
style DK fill:#ffc,stroke:#333,stroke-width:2px
style DK fill:#cfc,stroke:#333,stroke-width:2px
style DK fill:#fcc,stroke:#333,stroke-width:2px
style DK fill:#ffc,stroke:#333,stroke-width:2px
style DK fill:#cfc,stroke-width:2px
style DK fill:#fcc,stroke-width:2px
style DK fill:#ffc,stroke-width:2px
style DK fill:#cfc,stroke-width:2px
style DK fill:#fcc,stroke-width:2px
style DK fill:#ffc,stroke-width:2px
style DK fill:#cfc,stroke-width:2px
style DK fill:#fcc,stroke-width:2px
style DK fill:#ffc,stroke-width:2px
style DK fill:#cfc,stroke-width:2 px
style DK fill:#fcc,stroke-width:2 px
style DK fill:#ffc,stroke-width:2 px
style DK fill:#cfc,stroke-width:2 px
style DK fill:#fcc,stroke-width:2 px
style DK fill:#ffc,stroke-width:2 px
style DK fill:#cfc,stroke-width:2 px
style DK fill:#fcc,stroke-width:2 px
style DK fill:#ffc,stroke-width:2 px
style DK fill:#cfc,stroke-width:2 px
style DK fill = sliding boundary region created by pressure load
style DK fill = zero-displacement adaptive mesh constraints applied to nodes 1 and 4 in direction 1
Figure 12.2.2–7 Applying a sliding distributed pressure load to an adaptive mesh domain.
Defining an Eulerian boundary region with a pressure load
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 12.2.2–8.
Input File Usage: *DLOAD, REGION TYPE=EULERIAN
Abaqus/CAE Usage: Boundary regions defined using pressure loads are not supported in Abaqus/CAE.
Distributed surface fluxes and thermal conditions
In coupled thermal-stress analysis Abaqus/Explicit also creates boundary regions for distributed surface fluxes, convective film conditions, and radiation conditions. The rules governing boundary regions for
text_image
free surface flow node set OUT symmetry y x = Eulerian boundary region created by pressure load = zero-displacement adaptive mesh constraint applied to node set OUT in direction 1
Figure 12.2.2–8 Modeling an ambient pressure at the outflow boundary of an Eulerian adaptive mesh domain.
these loads are identical to those discussed for distributed loads. The ability to specify the boundary region type is also the same.
Concentrated loads
When a concentrated load is applied to the boundary of an adaptive mesh domain, Abaqus/Explicit creates a boundary region to coincide with the load. Every node to which a concentrated load is applied will be considered its own boundary region because it is not possible to identify a surface area associated with a concentrated load. However, you can control the behavior of each one-node region.
If concentrated loads 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).
Defining a Lagrangian boundary region with a concentrated load
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).
Input File Usage: *CLOAD, REGION TYPE=LAGRANGIAN
Abaqus/CAE Usage: Boundary regions defined using concentrated loads are not supported in Abaqus/CAE.
Defining a sliding boundary region with a concentrated load
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 12.2.2–9). A sliding node is unconstrained in the direction