|
Applications
Eulerian analyses are effective for applications involving extreme
deformation, up to and including fluid flow. In these applications, traditional
Lagrangian elements become highly distorted and lose accuracy. Liquid sloshing,
gas flow, and penetration problems can all be handled effectively using
Eulerian analysis. Eulerian-Lagrangian contact allows the Eulerian materials to
be combined with traditional nonlinear Lagrangian analyses.
An example of using Eulerian analysis for a severe deformation analysis is
discussed in
Rivet forming;
using coupled Eulerian-Lagrangian contact for a fluid-structure interaction
application is illustrated in
Impact of a water-filled bottle.
Eulerian Volume Fraction
The Eulerian implementation in
Abaqus/Explicit
is based on the volume-of-fluid method. In this method, material is tracked as
it flows through the mesh by computing its Eulerian volume fraction
(EVF) within each element. By definition, if a
material completely fills an element, its volume fraction is one; if no
material is present in an element, its volume fraction is zero.
Eulerian elements may simultaneously contain more than one material. If the
sum of all material volume fractions in an element is less than one, the
remainder of the element is automatically filled with “void” material. Void
material has neither mass nor strength.
Material Interfaces
Volume fraction data are computed for each Eulerian material in an element.
Within each time increment, the boundaries of each Eulerian material are
reconstructed using these data. The interface reconstruction algorithm
approximates the material boundaries within an element as simple planar facets
(the Eulerian method is implemented only for three-dimensional elements). This
assumption produces a simple, approximate material surface that may be
discontinuous between neighboring elements. Therefore, accurate determination
of a material's location within an element is possible only for simple
geometries, and fine grid resolution is required in most Eulerian analyses.
The discontinuities in an Eulerian material surface can lead to physically
unrealistic configurations when visualizing the results of an Eulerian
analysis.
Eulerian Section Definition
An Eulerian section definition lists all of the materials that may appear
within an Eulerian element. Void material is automatically included in this
list.
The material list supports an optional material instance name. Material
instance names are required to uniquely identify materials that you use more
than once. Repeated materials are useful, for example, in mixing simulations
where the motion of a material interface is to be computed: the water in a tank
could be divided by creating water material instances named “water_left” and
“water_right,” and the evolution of the interface between these materials could
be simulated.
By default, all Eulerian elements are initially filled with void material,
regardless of the section assignment. You must introduce nonvoid material into
your Eulerian mesh using an initial condition (see
Initial Conditions
below).
Eulerian Mesh Deformation
The Eulerian time incrementation algorithm is based on an operator split of
the governing equations, resulting in a traditional Lagrangian phase followed
by an Eulerian, or transport, phase. This formulation is known as
“Lagrange-plus-remap.” During the Lagrangian phase of the time increment nodes
are assumed to be temporarily fixed within the material, and elements deform
with the material. During the Eulerian phase of the time increment deformation
is suspended, elements with significant deformation are automatically remeshed,
and the corresponding material flow between neighboring elements is computed.
At the end of the Lagrangian phase of each time increment, a tolerance is
used to determine which elements are significantly deformed. This test improves
performance by allowing those elements with little or no deformation to remain
inactive during the Eulerian phase. The inactive elements typically have no
impact on the visualization of an Eulerian analysis; however, plotting an
Eulerian mesh using a very large deformation scale factor may reveal slight
deformations for elements within the deformation tolerance.
Eulerian Material Advection
As material flows through an Eulerian mesh, state variables are transferred
between elements by advection. The variables are assumed to be linear or
constant in each old element, then these values are integrated over the new
elements after remeshing. The new value of the variable is found by dividing
the value of each integral by the material volume or mass in the new element.
Second-Order Advection
Second-order advection assumes a linear distribution of the variable in each
old element. To construct the linear distribution, a quadratic interpolation is
constructed from the constant values at the integration points of the middle
element and its adjacent elements. A trial linear distribution is found by
differentiating the quadratic function to find the slope at the integration
point of the middle element. The trial linear distribution in the middle
element is limited by reducing its slope until its minimum and maximum values
are within the range of the original constant values in the adjacent elements.
This process is referred to as flux limiting and is essential to ensure that
the advection is monotonic.
Second-order advection is used by default, and it is recommended for all
problems, ranging from quasi-static to transient dynamic shock.
First-Order Advection
First-order advection assumes a constant value of the variable in each old
element. This method is simple and computationally efficient; however, it tends
to diffuse sharp gradients over time. Therefore, this technique should be used
only as a computationally efficient alternative for quasi-static simulations.
Reducing the Stable Time Increment Based on the Advection Speed
The stable time increment size is adjusted automatically to prevent material
from flowing across more than one element in each increment. When the material
velocity approaches the speed of sound (for example, in simulations involving
blast and shocks), further restrictions on the time increment size may be
needed to maintain accuracy and stability. You can specify a flux limit ratio
to restrict the stable time increment size such that material can flow across
only a fraction of an element in each increment. The default flux limit ratio
is 1.0, and recommended values range from 0.1 to 1.0.
Initial Conditions
You can apply initial conditions to Eulerian nodes and elements in the same
way that they are used for Lagrangian nodes and elements. Initial stress,
temperature, and velocity are common examples. In addition, most Eulerian
analyses require the initialization of Eulerian material.
By default, all Eulerian elements are initially void. You can use initial
conditions to fill Eulerian elements with one or more of the materials listed
in the Eulerian section definition. By selectively filling elements, you can
create the initial shape of each Eulerian material.
To fill an Eulerian element, you must define an initial volume fraction for
each available material instance. Material is filled until a volume fraction of
1.0 is reached; any excess material is ignored. The initial conditions apply
only at the beginning of an analysis; during the analysis the materials deform
according to the applied loads, and the volume fractions are recalculated
accordingly.
Boundary Conditions
By default, Eulerian material can flow freely into and out of the Eulerian
domain through mesh boundaries. You can constrain degrees of freedom at
Eulerian nodes to restrict material flow. For example, you can define typical
fluid “stick” or “sliding” walls using constraints normal and/or tangential to
the boundary. Since Eulerian nodes are automatically repositioned during the
Eulerian transport phase, you cannot apply prescribed displacement boundary
conditions to them.
You can use prescribed velocity or acceleration conditions on Eulerian nodes
to control material flow. Prescribed velocity or acceleration is implemented in
an Eulerian frame, so material velocity will reach the prescribed value as the
material passes the Eulerian node. If velocity is directed outward at an
Eulerian mesh boundary, either by prescribed condition or naturally as a result
of dynamic equilibrium, material may flow out of the Eulerian domain. This
material is lost from the simulation, and corresponding decreases in total mass
and energy will occur.
Similarly, if velocity is directed inward at a boundary, inflow of material
into the Eulerian domain will occur. When materials flow into an element
through a boundary face, the material content and the state of each inflowing
material are equal to that which presently exists within the element. For
example, if a boundary element contains 60% hot water and 40% cold air and the
interface normal is parallel to the boundary face, inflow velocity will
introduce a mixture of 60% hot water and 40% cold air. In this case
corresponding increases in total mass and energy will occur.
You can also define inflow and outflow conditions at an Eulerian domain
boundary, as described in
Defining Eulerian Boundaries.
Loads
You can apply loads to Eulerian nodes, elements, and faces in the same way
as to their Lagrangian counterparts. Eulerian loads act in an Eulerian frame:
they affect Eulerian material as it passes the point of load application.
Material Options
You can define material properties for Eulerian analysis in the same way as
for Lagrangian analysis. Liquids and gases can be modeled using equation of
state materials (see
Equation of State).
Brittle cracking is not supported because the number of cracks is not a
continous quantity and cannot be easily remapped. Hyperelastic materials can be
used in an Eulerian analysis, but due to inaccuracies introduced to the
deformation gradient during material transport, these materials might not fully
recover their original configuration after loads are removed; the same
inaccuracies also affect user-defined materials. The low-density foam material
model (Low-Density Foams)
is not supported.
Eulerian analysis allows materials to undergo extreme strain without the
mesh distortion limitations of Lagrangian analysis. Therefore, it is especially
important to define your material behavior through the entire strain range,
which often requires definition of a failure behavior.
Isotropic material failure is supported using a damage variable to
characterize the failure level. Element deletion is suppressed for Eulerian
sections because undamaged material may flow into “failed” elements. Shear
failure models are not supported.
Rayleigh mass proportional damping is not supported.
Elements
The Eulerian method is implemented in the multi-material element type EC3D8R and the multi-material thermally coupled element type EC3D8RT. The underlying mechanical response formulation of these elements
is based on the Lagrangian C3D8R element with extensions to allow multiple materials and to
support the Eulerian transport phase. The formulation applies the same strain
to each material in the element, then allows the stress and other state data to
evolve independently within each material. These stresses are combined using
volume fraction data to create element averaged values, which are integrated to
obtain nodal forces. Similarly, the thermal response formulation for the
thermally coupled element is based on the Lagrangian element C3D8RT with the extension to allow multiple materials with different
thermal properties and to support temperature advection. All the materials have
the same temperature, and the thermal properties (such as thermal conductivity
and thermal capacitance) are volume averaged before being used in solving one
single heat transfer equation for the multi-material model.
Element averaged values of other state data are computed similarly for
output purposes.
The Eulerian EC3D8R and EC3D8RT elements require eight nodes. Degenerate elements are not
supported. The Eulerian method is not implemented for two-dimensional elements.
Axisymmetry can be simulated using a wedge-shaped mesh and symmetry boundary
conditions.
By default, the Eulerian elements use viscous hourglass control. Hourglass
control is disabled by default for incompressible liquids modeled using
equation of state material types. These choices can be modified using section
controls (see
Section Controls).
Constraints
Since Eulerian nodes are automatically repositioned during the Eulerian
transport phase, you cannot use Eulerian nodes in Lagrangian modeling features
such as elements, connectors, and constraints. However, constraints between
Eulerian materials and Lagrangian parts can be modeled using tied contact
interfaces.
Interactions
Eulerian material instances interact with each other with a sticky behavior.
This sticking occurs because of the kinematic assumption that a single strain
field is applied to all materials within an element. Tensile stress can be
transmitted across an interface between two Eulerian materials, and no slip
occurs at these interfaces. This Eulerian-to-Eulerian contact behavior can be
reasonable in some situations, such as in a simulation of a lead bullet
penetrating a steel plate. Ablation of the bullet surface against the steel is
captured by the sticky behavior within the Eulerian elements at the
bullet-steel interface. Relative motion along this interface will occur only
due to shearing of the lead material.
Eulerian-to-Eulerian contact occurs by default in an Eulerian analysis; you
do not need to define contact interactions between Eulerian materials.
More complex contact interactions can be simulated when one of the
contacting bodies is modeled using Lagrangian elements. This powerful
capability supports applications such as fluid-structure interaction, where an
Eulerian fluid contacts a Lagrangian structure.
The implementation of Eulerian-Lagrangian contact is an extension of general
contact in
Abaqus/Explicit.
The general contact property models and defaults apply to Eulerian-Lagrangian
contact (see
About Mechanical Contact Properties).
For example, by default, tensile stresses are not transmitted across an
Eulerian-Lagrangian contact interface, and the interface friction coefficient
is zero. Specifying automatic contact for an entire Eulerian-Lagrangian model
allows for interactions between all Lagrangian structures and all Eulerian
materials in the model. You can also use Eulerian surfaces (see
Eulerian Surface Definition)
to create material-specific interactions or to exclude contact between
particular Lagrangian surfaces and Eulerian materials.
Formulation of Eulerian-Lagrangian Contact
The Eulerian-Lagrangian contact formulation is based on an enhanced immersed
boundary method. In this method the Lagrangian structure occupies void regions
inside the Eulerian mesh. The contact algorithm automatically computes and
tracks the interface between the Lagrangian structure and the Eulerian
materials. A great benefit of this method is that there is no need to generate
a conforming mesh for the Eulerian domain. In fact, a simple regular grid of
Eulerian elements often yields the best accuracy.
If the Lagrangian body is initially positioned inside the Eulerian mesh, you
must make sure that the underlying Eulerian elements contain void after
material initialization. During the analysis the Lagrangian body pushes
material out of the Eulerian elements that it passes through, and they become
filled with void. Similarly, Eulerian material flowing toward the Lagrangian
body is prevented from entering the underlying Eulerian elements. This
formulation ensures that two materials never occupy the same physical space.
If the Lagrangian body is initially positioned outside the Eulerian mesh, at
least one layer of void Eulerian elements must be present at the Eulerian mesh
boundary. This creates a free surface on the Eulerian material inside the
Eulerian mesh boundary and provides a source for void material to replace
Eulerian material that is driven out of interior elements. Several layers of
void elements are typically used above free surfaces to allow simulation of
crater formation and backsplashing before this material leaves the Eulerian
domain.
Eulerian-Lagrangian contact also supports failure and erosion in the
Lagrangian body. Lagrangian element failure can open holes in a surface through
which Eulerian material may flow. When modeling erosion of a solid Lagrangian
body, the interior faces of the solid body must be included in the contact
surface definition (see
Modeling Surface Erosion).
Eulerian-Lagrangian contact constraints are enforced using a penalty method,
where the default penalty stiffness parameter is automatically maximized
subject to stability limits.
The default contact formulation is effective for modeling solid materials but may exhibit leakage
when modeling liquids or gases. An enhanced Eulerian-Lagrangian contact formulation is
available to prevent the leakage of liquids or gases through the Lagrangian surface. It is
more computationally expensive and should be activated only when required.
Eulerian-Lagrangian contact supports thermal interactions when using coupled
temperature-displacement Eulerian element EC3D8RT in a dynamic coupled thermal-stress analysis. However, gap
radiation and gap conductance as a function of clearance are not supported.
Output
The set of element output variables EVF gives the Eulerian volume fraction for each material in the
Eulerian section definition, including void. It is important to request output
for EVF in all Eulerian analyses because visualization of Eulerian
material boundaries is based on the material volume fractions.
Material-specific Eulerian field output variables are distinguished by
appending material names to the base field name. For example, if you request
output variable S (stress components) in an Eulerian analysis involving material
instances named “steel” and “tin,” you will see results for individual material
stresses named “S_steel” and “S_tin.”
Several volume fraction averaged field data are also available for output.
For example, output variable SVAVG gives a single value of stress for each element computed as a
volume fraction average of stress over all materials present in the element.
Use of these volume fraction averaged output data has the advantage of
substantially reducing the size of the output database for the case where
several materials are defined in the Eulerian section. See
Abaqus/Explicit Output Variable Identifiers
for a complete list of Eulerian-specific output variables.
Output variables EVF and SVAVG are included in the PRESELECT variable list when Eulerian elements appear in the model.
You can also request integrated volume (VOLEUL) and integrated mass (MASSEUL) over a particular Eulerian element set. These output variables
are material specific and are distingushed by having the material names
appended to the variable name.
Limitations
Eulerian analyses are subject to the following limitations:
-
Boundary conditions: You cannot apply prescribed nonzero displacement
boundary conditions to Eulerian nodes.
-
Lagrangian attachments: You cannot attach Lagrangian elements to
Eulerian nodes. Use tied contact interfaces instead.
-
Constraints: You cannot apply Lagrangian constraints
(MPCs, etc.) to Eulerian nodes. Use tied
contact interfaces instead.
-
Materials: Brittle cracking and shear failure models are also not
supported. Rayleigh mass proportional damping is not supported.
-
Elements: The Eulerian formulation is implemented only for EC3D8R and EC3D8RT elements.
-
Element import: Eulerian elements are not available for import.
-
Double-sided contact: Penetration of Eulerian material through the contact interface can occur
in some cases involving Eulerian material contacting Lagrangian shell or membrane
elements. This type of contact introduces complexity because the sign of the outward
normal direction must be determined on the fly as material approaches the Lagrangian
element; contact with either side of the element is potentially allowable. You should
simplify the contact problem wherever possible by using Lagrangian solid elements
instead of shell or membrane elements, since the outward normal direction at solid
element faces is unique. For example, if a model involves Eulerian material flowing
around a rigid Lagrangian obstacle, mesh the obstacle with solid elements rather than
shell elements and activate the enhanced contact formulation to reduce the leakage.
-
Contact penetration: In some cases Eulerian material may penetrate through the Lagrangian
contact surface near corners. This penetration should be limited to an area equal to the
local Eulerian element size. Penetration can be minimized by refining the Eulerian mesh
(manually or through adaptive mesh refinement) or by adding a fillet to the Lagrangian
mesh with radius equal to the local Eulerian element size. Alternatively, you can
activate the enhanced contact formulation to reduce or eliminate the leakage.
-
When the enhanced contact formulation through adaptive mesh refinement is activated,
you should simplify the Lagrangian contact surface wherever possible by avoiding
double-sided, folded, and T-section surfaces. If more than one surface cuts through a
single Eulerian element, the enhanced contact formulation is turned off, and the default
formulation is used. For thin structures modeled with solid elements, refining the
Eulerian element size to avoid this behavior is recommended.
-
Contact types: Eulerian-Lagrangian contact does not support Lagrangian
beam elements, Lagrangian pipe elements, Lagrangian truss elements, or
analytical rigid surfaces.
-
Contact import: Import of the Eulerian-Lagrangian contact states is not
supported.
-
Thermal contact: Gap radiation and gap conductance as a function of
clearance are not supported.
-
Contact output: Contact variables are output only for the Lagrangian
side of Eulerian-Lagrangian interfaces.
-
Surface loads: You cannot use the Eulerian material surface type for
general surface loading. However, distributed loads such as pressure can be
applied to surfaces defined on Eulerian element faces.
-
Mass scaling: You cannot apply mass scaling to Eulerian elements.
-
Heat transfer: Use coupled temperature-displacement EC3D8RT Eulerian elements to model a fully coupled thermal-stress
analysis. Adiabatic conditions are assumed in Eulerian materials when EC3D8R elements are used.
-
Output: Total strain (LE) is not available for Eulerian elements in field or history
output, but it can be accessed via the utility routine VGETVRM.
-
Subcycling: You cannot include Eulerian elements in subcycling zones.
Input File Template
The following example illustrates a coupled Eulerian-Lagrangian analysis
of a Lagrangian boat floating on Eulerian water. A conforming mesh is assumed,
so Eulerian material initialization is achieved by whole element filling.
Material-specific interactions between the Lagragian body and the Eulerian
materials are implemented: a contact interaction is defined between the boat
and water, but contact between the boat and air is ignored. Output is requested
for Eulerian volume fractions, Eulerian element-averaged stress, and material
stress. HEADING
…
ELEMENT, TYPE=C3D8R, ELSET=BOAT_ELSET
element definitions for Lagrangian boat
ELEMENT, TYPE=EC3D8R, ELSET=ALL_EULERIAN
element definitions for whole Eulerian mesh
ELSET, NAME=AIR_ELSET
data lines giving Eulerian elements that are initially filled with air
ELSET, NAME=WATER_ELSET
data lines giving Eulerian elements that are initially filled with water
**
MATERIAL, NAME=AIR
material definition for air
MATERIAL, NAME=WATER
material definition for water
**
EULERIAN SECTION, ELSET=ALL_EULERIAN
AIR
WATER
**
INITIAL CONDITIONS, TYPE=VOLUME FRACTION
AIR_ELSET, AIR, 1.0
WATER_ELSET, WATER, 1.0
INITIAL CONDITIONS, TYPE=STRESS, GEOSTATIC
data lines to define water pressure due to gravity
**
SURFACE, NAME=WATER_SURFACE, TYPE=EULERIAN MATERIAL
WATER
SURFACE, NAME=BOAT_SURFACE
BOAT_ELSET
**
STEP
DYNAMIC, EXPLICIT
DLOAD
data lines to define gravity load
**
CONTACT
CONTACT INCLUSIONS
BOAT_SURFACE, WATER_SURFACE
**
OUTPUT, FIELD
ELEMENT OUTPUT
EVF, SVAVG, PEEQVAVG
END STEP
References
- Benson, D. J., “Computational
Methods in Lagrangian and Eulerian Hydrocodes,” Computer Methods in Applied Mechanics and
Engineering, vol. 99, pp. 235–394, 1992.
- Benson, D. J., “Contact in a
Multi-Material Eulerian Finite Element Formulation,” Computer Methods in Applied Mechanics and
Engineering, vol. 193, pp. 4277–4298, 2004.
- Peery, J. S., and D. E. Carroll, “Multi-Material ALE
methods in Unstructured Grids,” Computer
Methods in Applied Mechanics and Engineering, vol. 187, pp. 591–619, 2000.
|