김경종
13 KiB
• a misalignment of the bounding box local orientation;
• a mismatch between the shape of the mesh boundary and the bounding box (i.e., the Eulerian mesh is not a rectangular box); or
• an inadequately sized or positioned initial Eulerian mesh.
Input File Usage: *EULERIAN MESH MOTION, SURFACE=name
Abaqus/CAE Usage: Load module: Eulerian mesh motion editor: Object to Follow: name
Constraining Eulerian mesh motion
Once the motion of the bounding box is computed, the translations and scaling factors are applied directly to the Eulerian mesh. Several types of constraints are available to restrict these motions. Conflicts between competing constraints are resolved in the following order of precedence:
- constraining the center and faces of the mesh bounding box,
- limiting the rate of mesh motion,
- turning off mesh contraction,
- centering the mesh bounding box on the target’s center of mass or bounding box center,
- preventing mesh expansion or contraction outside the scale factor limits,
- limiting aspect ratio changes, and
- maintaining a buffer between the mesh and target.
Constraining mesh expansion and contraction
By default, the Eulerian mesh may expand or contract by an unlimited amount in each direction, as necessary to contain the target object. This can be undesirable: expansion creates large Eulerian elements that crudely approximate the shape of Eulerian objects, while contraction leads to decreased stable time increment sizes.
You can apply constraints to limit the expansion and contraction independently in each local direction by specifying lower and/or upper limits on the bounding box size scale factors. For example, a maximum scale factor of 1.0 constrains the box dimension to be no larger than 1.0 times the initial box dimension, effectively prohibiting any expansion, while a minimum scale factor of 0.5 limits the box dimension to be no smaller than half its initial dimension.
Input File Usage: *EULERIAN MESH MOTION
scaling factor limits
Abaqus/CAE Usage: Load module: Eulerian mesh motion editor: Axis n:
Expansion ratio, Contraction ratio
Preventing mesh contraction
An additional control is available to prevent incremental contraction. If specified, the box dimensions may increase, but at no point during the simulation may they decrease below their current values. This option prevents oscillations in mesh size during simulations where the mesh is nominally expanding.
Input File Usage: *EULERIAN MESH MOTION, CONTRACT=NO
Abaqus/CAE Usage: Load module: Eulerian mesh motion editor: Controls: toggle off Allow mesh contraction
Constraining mesh translation
You can specify the motion of the center of the bounding box to be either free (default) or fixed in each of the local directions. You can also independently specify free (default) or fixed normal motion of the positive and negative box faces in the local coordinate directions.
Input File Usage: *EULERIAN MESH MOTION
，face constraintscenter constraints
Abaqus/CAE Usage: Load module: Eulerian mesh motion editor: Axis n: Center position, Positive plane position, Negative plane position
Centering the mesh bounding box
If the motion of the mesh bounding box is unconstrained, the center of the bounding box is aligned with the center of a box enclosing the target surface. If the target surface fragments or “emits” low density material, aligning the center of the bounding box with the center of mass of the target may be advantageous.
Input File Usage: Use the following option to center the mesh bounding box on the center of mass of the target object:
*EULERIAN MESH MOTION, CENTER=MASS
Use the following option to center the mesh bounding box on the center of the target object’s bounding box:
*EULERIAN MESH MOTION, CENTER=BOUNDING BOX
Abaqus/CAE Usage: The center of the mesh bounding box cannot be changed in Abaqus/CAE; the center of the mesh bounding box corresponds to the center of the target object’s bounding box.
Controlling the mesh buffer around the target object
The mesh moves to maintain a buffer of Eulerian elements between the target object and the bounding box. By default, this buffer is equal to twice the maximum Eulerian element size in the mesh. You can specify the buffer size as a multiple of the maximum Eulerian element size. You can also specify that the initial spacing between the target object and the mesh (set to zero where the target initially extends outside of the mesh) is used to compute the buffer size.
Input File Usage: Use the following option to use a buffer equal to the initial spacing between the target object and the mesh:
*EULERIAN MESH MOTION, BUFFER=INITIAL
Use the following option to specify a buffer as a multiple of the maximum Eulerian element size:
*EULERIAN MESH MOTION, BUFFER= value
Abaqus/CAE Usage: Load module: Eulerian mesh motion editor: Controls: Buffer size: Initial or Specify
Limiting aspect ratio changes
Excessive mesh motion in a single direction can produce badly shaped Eulerian elements. An optional parameter is available to limit the change in maximum aspect ratio of the bounding box. By default, this limit is 10. When the aspect ratio limit is reached, motion in one local direction will induce motion in the other directions to preserve the box aspect ratio. This aspect ratio limit applies to the bounding box dimensions, not the underlying Eulerian element dimensions.
Input File Usage: *EULERIAN MESH MOTION, ASPECT RATIO MAX= value
Abaqus/CAE Usage: Load module: Eulerian mesh motion editor: Controls: Aspect ratio limit: value
Limiting the rate of mesh motion
The Eulerian mesh must not be allowed to move abruptly. A hard limit on its motion is given by the advective Courant condition, which prohibits mesh velocity larger than the material wave speed. In addition you can limit the mesh velocity to a multiple of the maximum velocity in the target object. By default, this limit is set to 1.01.
Input File Usage: *EULERIAN MESH MOTION, VMAX FACTOR= value
Abaqus/CAE Usage: Load module: Eulerian mesh motion editor: Controls: Mesh velocity factor: value
Ignoring fragments of Eulerian material
When the target object is an Eulerian material, tiny fragments can drive excessive mesh motion. You can specify a minimum Eulerian volume fraction below which Eulerian material is ignored during the mesh motion calculation. This can be particularly useful for impact calculations, where tiny fragments of an impacting, splattering projectile may be allowed to leave the Eulerian domain. The default minimum volume fraction is 0.5.
Input File Usage: *EULERIAN MESH MOTION, VOLFRAC MIN= value
Abaqus/CAE Usage: Load module: Eulerian mesh motion editor: Controls: Volume fraction threshold: value
Limitations
An Eulerian mesh can move only according to the available Eulerian mesh motion options. You cannot apply prescribed displacement boundary conditions to Eulerian nodes.
14.1.4 DEFINING ADAPTIVE MESH REFINEMENT IN THE EULERIAN DOMAIN
Product: Abaqus/Explicit
References
• “Eulerian analysis,” Section 14.1.1
• *ADAPTIVE MESH REFINEMENT
• *EULERIAN SECTION
• *EULERIAN MESH MOTION
• *CONTACT CONTROLS ASSIGNMENT
Overview
The adaptive mesh refinement feature:
• can refine elements locally inside an Eulerian mesh;
• allows the user to define various criteria for refinement;
• can remove the refinement automatically once the refinement criteria are no longer met; and
• is available for Eulerian element type EC3D8R only.
Adaptive mesh refinement
In a traditional Eulerian analysis the topology of the Eulerian mesh does not change during the analysis. Although the Eulerian mesh motion feature allows the Eulerian mesh to move in space to cover areas of interest, its ability to create a nonuniformly refined mesh that changes with time is limited. The adaptive mesh refinement feature can locally refine the mesh by subdividing elements identified by user-defined criteria. This refinement can be removed automatically during the analysis once the criteria are no longer satisfied. This feature offers great savings in computational cost compared to a uniformly refined mesh. See “Impact of a copper rod,” Section 1.3.10 of the Abaqus Benchmarks Guide, for an example of using the adaptive mesh refinement feature.
Activating adaptive mesh refinement
You can independently activate adaptive mesh refinement for each Eulerian section in a model. The feature applies to all the elements specified in the element set; all the elements in the element set have to be in the same Eulerian section.
Input File Usage: *ADAPTIVE MESH REFINEMENT, ELSET=name
Setting the refinement limit
When adaptive mesh refinement occurs, elements are added to the Eulerian mesh. You can limit how many elements can be created by specifying an upper bound ratio of added elements to original elements. The default value of this upper bound ratio is 8.0.
Input File Usage: *ADAPTIVE MESH REFINEMENT, RATIO=maximum increase in number of elements/original number of elements
Setting the refinement level
With one level of refinement, each time a user-defined Eulerian element is refined, it is equally divided into eight subelements. These subelements can subsequently be divided again if two levels of refinement are allowed. You can set a limit on the maximum number of levels of refinement. The default maximum level is one.
Input File Usage: *ADAPTIVE MESH REFINEMENT, LEVEL=maximum level of refinement
Deactivateing coarsening
You can specify whether refinement can be removed when the refinement criteria are no longer met.
Input File Usage: Use the following option to specify that refinement can be removed once the refinement criteria are no longer met:
*ADAPTIVE MESH REFINEMENT, COARSENING=YES (default)
Use the following option to specify that refinement cannot be removed even when the refinement criteria are no longer met:
*ADAPTIVE MESH REFINEMENT, COARSENING=NO
Defining refinement criteria
You must specify at least one refinement criterion. An element will be selected for refinement if any of the criteria is met. To reduce the numerical artifacts at the mesh transition boundaries (where a fine mesh meets a coarse mesh), the elements adjacent to the selected elements are also refined. The elements are coarsened once the refinement criteria are no longer met. Each selected element can be refined or coarsened by only one level in every increment. Table 14.1.4–1 lists all the refinement criteria available in Abaqus/Explicit.
Table 14.1.4–1 Refinement criteria.
| Refinement criterion description | Refinement criterion label | User-specified values |
| Refine elements containing material interfaces | VF | N/A |
| Refine elements that are in contact with Lagrangian bodies | CONT | You can specify the value ALL to refine all elements intersecting the Lagrangian surfaces even if contact has not occurred; using this option avoids frequent refining and coarsening with chattering contact. You can also specify the value MAT to refine only elements containing materials that are in contact with the Lagrangian surfaces. If no values are specified, MAT will be used except for materials with Mie-Grüneisen equations of state. |
| Refine elements in which significant plastic deformation occurs. Not supported for the critical state (clay) plasticity model. | PEEQ | Critical value of the equivalent plastic strain |
| Refine elements near a sharp density gradient | DENSITY | You can specify two values for this criterion. The first value is the critical value of the density gradient, computed as the ratio between the change of density across element faces and the density of the material inside the element; the second value is the critical density. For an element to be selected, both the density and the density gradient must exceed the critical value. |
| Refine elements near a sharp pressure gradient | PRESS | You can specify two values for this criterion. The first value is the critical value of the pressure gradient, computed as the ratio between the change of pressure across element faces and the pressure of the material inside the element; the second value is the critical pressure. For an element to be selected, both the pressure and the pressure gradient must exceed the critical value. |
Input File Usage:
*ADAPTIVE MESH REFINEMENT, refinement criteria label, value of the criteria
Contact
When adaptive mesh refinement is specified in an Eulerian section that is involved in general contact, dynamic seeding is activated by default. Dynamic seeding allows more seeds to be created once the Eulerian elements near a Lagrangian face are refined; these seeds will be deleted once these Eulerian elements are coarsened.
Dynamic seeding can also be useful for Eulerian analyses with no adaptive mesh refinement.
Input File Usage:
*CONTACT CONTROLS ASSIGNMENT, SEEDING=DYNAMIC
15. Particle Methods
Discrete element method 15.1
Continuum particle analyses 15.2
Particle generator 15.3