14.1.1 Eulerian analysis
Products: Abaqus/Explicit Abaqus/CAE
References
Overview
In a traditional Lagrangian analysis nodes are fixed within the material, and elements deform as the material deforms. Lagrangian elements are always 100% full of a single material, so the material boundary coincides with an element boundary.
By contrast, in an Eulerian analysis nodes are fixed in space, and material flows through elements that do not deform. Eulerian elements may not always be 100% full of material—many may be partially or completely void. The Eulerian material boundary must, therefore, be computed during each time increment and generally does not correspond to an element boundary. The Eulerian mesh is typically a simple rectangular grid of elements constructed to extend well beyond the Eulerian material boundaries, giving the material space in which to move and deform. If any Eulerian material moves outside the Eulerian mesh, it is lost from the simulation.
Eulerian material can interact with Lagrangian elements through Eulerian-Lagrangian contact; simulations that include this type of contact are often referred to as coupled Eulerian-Lagrangian (CEL) analyses. This powerful, easy-to-use feature of Abaqus/Explicit general contact enables fully coupled multi-physics simulation such as fluid-structure interaction.
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,” Section 2.3.1 of the Abaqus Example Problems Guide; using coupled Eulerian-Lagrangian contact for a fluid-structure interaction application is illustrated in “Impact of a water-filled bottle,” Section 2.3.2 of the Abaqus Example Problems Guide.
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. Abaqus/CAE can apply a nodal averaging algorithm to estimate a more realistic, continuous surface during visualization. For more information on visualizing the material interfaces in an Eulerian model, see “Viewing output from Eulerian analyses,” Section 28.7 of the Abaqus/CAE User's Guide.
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.
| Input File Usage: | *EULERIAN SECTION, ADVECTION=SECOND ORDER |
| Abaqus/CAE Usage: | The second-order advection method is used by default in Abaqus/CAE. |
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.
| Input File Usage: | *EULERIAN SECTION, ADVECTION=FIRST ORDER |
| Abaqus/CAE Usage: | The first-order advection method cannot be specified in Abaqus/CAE. |
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.
| Input File Usage: | *EULERIAN SECTION, FLUX LIMIT RATIO=maximum ratio |
| Abaqus/CAE Usage: | The flux limit ratio cannot be modified in Abaqus/CAE. |
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.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=VOLUME FRACTION |
| Abaqus/CAE Usage: | Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Material Assignment for the Types for Selected Step |
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,” Section 14.1.2.
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,” Section 25.2.1). 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,” Section 22.9.1) 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,” Section 27.1.4).
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 “Mechanical contact properties: overview,” Section 37.1.1). 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,” Section 2.3.5) to create material-specific interactions or to exclude contact between particular Lagrangian surfaces and Eulerian materials.
| Input File Usage: | Use both of the following options to define contact between all Lagrangian bodies and all Eulerian materials: |
*CONTACT *CONTACT INCLUSIONS, ALL EXTERIOR Use the following options to include or exclude contact between particular Lagrangian surfaces and Eulerian materials: *CONTACT *CONTACT INCLUSIONS Lagrangian_surface, Eulerian_surface *CONTACT EXCLUSIONS Lagrangian_surface, Eulerian_surface |
| Abaqus/CAE Usage: | Use the following option to define contact between all Lagrangian bodies and all Eulerian materials: |
Interaction module: Create Interaction: General contact (Explicit): Included surface pairs: All* with self Use the following options to include contact between particular Lagrangian surfaces and Eulerian materials: Interaction module: Create Interaction: General contact (Explicit): Included surface pairs: Selected surface pairs: Edit, select the Lagrangian surface in the left column and the Eulerian material instance in the right column, then click the arrows to transfer them to the list of included pairs Use the following options to exclude contact between particular Lagrangian surfaces and Eulerian materials: Interaction module: Create Interaction: General contact (Explicit): Excluded surface pairs: Edit, select the Lagrangian surface in the left column and the Eulerian material instance in the right column, then click the arrows to transfer them to the list of excluded pairs |
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” in “Defining general contact interactions in Abaqus/Explicit,” Section 36.4.1).
Eulerian-Lagrangian contact constraints are enforced using a penalty method, where the default penalty stiffness parameter is automatically maximized subject to stability limits.
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,” Section 4.2.2, 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.
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 or adding a fillet to the Lagrangian mesh with radius equal to the local Eulerian element size.
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
Additional 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.