Finite element conversion to SPH particles

By default, one particle is generated per parent element. You can control the number of particles generated per element by specifying the number of particles to be generated per parent element isoparametric direction. The total number of particles generated per element depends on the element type that is being converted. For example, if you specify 3 particles to be generated per isoparametric direction, upon conversion 27 particles would be generated from a C3D8R element, 18 from a C3D6 element, and 10 from a C3D4 element, as illustrated in Figure 1. A maximum value of seven particles per direction can be specified. The particles are evenly spaced inside the parent element such that they fill the volume as uniformly as possible. For example, if cubic parent elements are stacked in the user-defined mesh, the particles would be evenly spaced throughout the part.

Figure 1. Internally generated particles per parent element illustrated for three particles per isoparametric direction.

You can control the number of particles generated per isoparametric direction as discussed in Using section controls to convert continuum elements to particles.

You can specify the time when the conversion of all the elements in the affected element set is to take place regardless of the deformation levels. This option is intended for applications where the SPH functionality is the preferred modeling method, such as fluid sloshing in a tank or a synthetic bird strike on an aircraft. If the conversion time is specified as zero, the conversion takes place at the beginning of the analysis. For example, fluid sloshing is a good candidate for using a time-based criterion if sloshing is expected to start at the beginning of the analysis. You can specify a later time at which the conversion takes place if extreme deformations do not occur until later in the analysis. A bird strike analysis is a potential candidate as the bird might travel for some time without any deformation prior to hitting the intended target.

You can control the time when the conversion is to occur as discussed in Using section controls to convert continuum elements to particles.

You can specify the absolute value of the maximum principal strain when the conversion of a given element is to take place. As elements deform, if the absolute value of the maximum principal strain is greater than the specified threshold, the parent elements will convert progressively to SPH particles. This option is intended for applications where the finite element method is the preferred modeling method but severe deformations could occur in certain regions. Examples include blast applications and crushing.

You can control the strain-based threshold upon which conversion is to occur as discussed in Using section controls to convert continuum elements to particles.

You can specify the absolute value of the maximum principal stress value at which the conversion of a given element takes place. As elements deform, if the absolute value of the maximum principal stress is greater than the specified threshold, the parent elements will convert progressively to SPH particles. This option is intended for the same candidate applications as those discussed for the strain-based criterion.

You can control the stress-based threshold upon which conversion is to occur as discussed in Using section controls to convert continuum elements to particles.

The user subroutine–based criterion provides the flexibility of a user subroutine implementation that allows you to implement your own conversion criterion. Element conversion can be controlled during the course of an Abaqus/Explicit analysis through any of the user subroutines that can actively modify state variables associated with a material point, such as VUSDFLD and VUMAT. You specify the state variable number controlling the element conversion flag. For example, specifying a state variable number of two indicates that the second state variable is the conversion flag in the user subroutine. The conversion state variable should be set to a value of one or zero. A value of one indicates that the element is active, while a value of zero indicates that Abaqus/Explicit should convert the element to particles. Since user subroutines have access via arguments (or in the case of the VUSDFLD subroutine via utility routines) to material point state data, the functionality provides a comprehensive means to define the conversion state variable.

SECTION CONTROLS, ELEMENT CONVERSION=YES,
CONVERSION CRITERION=USER
...
MATERIAL
DEPVAR, CONVERT=variable number

When using the conversion technique of generating particles per parent element, particles are generated internally at the beginning of the preprocessing phase of the analysis, and they are placed in an inactive or dormant state. The particles are attached to the parent elements in a similar fashion as the nodes of embedded elements are attached (see Embedded Elements), and they follow the motion of the parent element nodes in an average sense. The inertial properties of the particles in this inactive state (while the parent finite elements are active) are disregarded automatically to avoid doubling the momentum at a given location. Similar to SPH particles defined directly as PC3D elements, particles generated from parent element sets associated with different section definitions will not interact with each other.

Upon conversion a number of internally generated particles per parent element are activated, as illustrated for various element types in Figure 1. The computational cost of the analysis can increase significantly after conversion takes place if a large number of particles are generated per element since a larger number of active elements needs to be processed. In addition, the computational cost increases because the stable time increment associated with the internally generated particles decreases as the particle density increases.

Upon conversion the state information (such as stress or equivalent plastic strain) associated with the element being converted is transferred to the generated particles to ensure the smoothest possible transition. The activated particles interact via the SPH formalism with both the previously activated particles and the neighboring inactive particles that are still embedded in active parent elements.

The thickness of the particles is primarily used for resolving initial overclosures between the particles and the surfaces in the general contact domain. By default, Abaqus/Explicit determines the particle thickness such that no initial overclosures exist, as illustrated in Figure 2(b). You can specify a uniform thickness, although the particle thickness can expand beyond the original surface of the finite element mesh, as illustrated in Figure 2(a), which could lead to initial overclosures. The thickness of the particles does not affect the particle’s volume and mass.

You can specify the thickness of the generated particles to be either variable or uniform as discussed in Using section controls to convert continuum elements to particles.

Figure 2. Internally generated particles based on a uniform background.