<!-- source-page: 81 -->

fully encompasses the domain through which the model moves; otherwise, you will lose tracking of the particle.

<table><tr><td>Input File Usage:</td><td>Use the following option to specify a fixed size for the particle tracking box in a DEM analysis:*SECTION CONTROLSblank lineblank lineX, Y, and Z-coordinates (lower box corner) and X, Y, and Z-coordinates (upper box corner)Use the following option to specify a fixed size for the particle tracking box in an SPH analysis:*SECTION CONTROLSfirst data linesecond data lineX, Y, and Z-coordinates (lower box corner) and X, Y, and Z-coordinates (upper box corner), 0</td></tr><tr><td>Abaqus/CAE Usage:</td><td>In Abaqus/CAE you can only specify section controls for SPH parameters in Abaqus/Explicit analyses involving the conversion of continuum elements to SPH particles.</td></tr></table>

# Using section controls for smoothed particle hydrodynamics (SPH)

In addition to controlling the size of the particle tracking box, you can control other aspects of the smoothed particle hydrodynamic (SPH) formulation implemented in Abaqus/Explicit.

# Using section controls for specifying the SPH kernel

For a smoothed particle hydrodynamic analysis, you can choose the order of the kernel used for interpolation. For a list of references that discuss the various kernels that can be used, see “Smoothed particle hydrodynamics,” Section 15.2.1.

Input File Usage: Use one of the following options:

\*SECTION CONTROLS, KERNEL=CUBIC

\*SECTION CONTROLS, KERNEL=QUADRATIC

\*SECTION CONTROLS, KERNEL=QUINTIC

Abaqus/CAE Usage: In Abaqus/CAE you can choose the order of the kernel used for interpolation only in Abaqus/Explicit analyses involving the conversion of continuum elements to SPH particles.

Mesh module: Mesh→Element Type: Conversion to particles:

Kernel: Cubic, Quadratic, or Quintic

<!-- source-page: 82 -->

# Using section controls for specifying the SPH formulation

By default, the SPH kernels satisfy the zero-order completeness requirement. A first-order complete corrected (normalized) kernel is also available, which is sometimes referred in the literature as the normalized SPH (NSPH) method. In high-deformation solid mechanics analyses the use of the NSPH method may lead to more accurate results.

In the SPH methods, a mean velocity filtering coefficient can be used for the modified coordinate updates for particles. A nonzero value for this coefficient leads to the XSPH method, as discussed in “Smoothed particle hydrodynamics,” Section 15.2.1.

Input File Usage: Use one of the following options to specify the SPH formulation:

\*SECTION CONTROLS, SPH FORMULATION=CLASSICAL (default)   
\*SECTION CONTROLS, SPH FORMULATION=NSPH   
\*SECTION CONTROLS, SPH FORMULATION=XSPH

Abaqus/CAE Usage: In Abaqus/CAE you can only specify section controls for SPH parameters in Abaqus/Explicit analyses involving the conversion of continuum elements to SPH particles.

# Using section controls for specifying SPH parameters

You can control the way the smoothing length is computed (see “Smoothed particle hydrodynamics,” Section 15.2.1). You can specify the smoothing length (units of length) for precise control of the radius of influence associated with a given particle. Alternatively, you can scale the default smoothing length by specifying a dimensionless smoothing length factor. By default, the smoothing length is kept constant throughout the analysis. You can specify a variable smoothing length that will increase or decrease during the analysis depending on the divergence of the velocity field, which is a measure of compressive or expansive behavior.

You can also specify the minimum number of particles within the sphere of influence for the given particle. If the total number of particles within the sphere of influence for the given particle is less than the specified minimum number of particles, the deformation gradient for this given particle is frozen, that is, unchanged between the previous and current time increment. In solid mechanics it means that the strain associated with this element will not be changed during the current time increment.

You can specify a mean velocity filtering coefficient that is used for the modified coordinate updates for particles using the XSPH method.

Input File Usage: Use the following option to specify SPH parameters:

\*SECTION CONTROLS

first data line

smoothing length, smoothing length factor,

min number of neighboring particles, , mean velocity filtering coefficient

<!-- source-page: 83 -->

Use one of the following options to define the smoothing length:

\*SECTION CONTROLS, SPH SMOOTHING

LENGTH=CONSTANT (default)

\*SECTION CONTROLS, SPH SMOOTHING LENGTH=VARIABLE

Abaqus/CAE Usage: In Abaqus/CAE you can only specify section controls for SPH parameters in Abaqus/Explicit analyses involving the conversion of continuum elements to SPH particles.

# Using section controls to convert continuum elements to particles

Reduced-integration continuum elements can convert to particles if a certain criterion is met, as discussed in “Finite element conversion to SPH particles,” Section 15.2.2. You can specify the number of particles per parent element to be generated. Several criteria to trigger the conversion are available.

Input File Usage: Use the following option to prevent finite elements from converting to particles:

\*SECTION CONTROLS, ELEMENT CONVERSION=NO (default)

Use the following option to trigger the conversion of finite elements to particles:

\*SECTION CONTROLS, ELEMENT CONVERSION=YES

Use the following option to trigger the conversion of finite elements to particles based on a uniform background grid:

\*SECTION CONTROLS, ELEMENT CONVERSION=BACKGROUND GRID

Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Conversion to particles: No or Yes

Generating particles based on a uniform background grid is not supported in Abaqus/CAE.

# Specifying the number of particles generated

You specify the number of particles to be generated per isoparametric direction. The number of particles can range from 1 to 7.

Input File Usage: \*SECTION CONTROLS, ELEMENT CONVERSION=YES

first data line

second data line

third data line

number of particles to be generated per isoparametric direction

Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Conversion to particles: Yes,

PPD: number of particles to be generated per isoparametric direction

# Specifying the background grid

You specify the spacing of the background grid and the name of an orientation definition to define a local coordinate system for the background grid.

<!-- source-page: 84 -->

<table><tr><td>Input File Usage:</td><td>*SECTION CONTROLS, ELEMENT CONVERSION=BACKGROUND GRIDfirst data linesecond data linethird data linespacing of the background grid, name of an orientation definition</td></tr></table>

<table><tr><td>Abaqus/CAE Usage:</td><td>Generating particles based on a uniform background grid is not supported in Abaqus/CAE.</td></tr></table>

# Specifying the thickness of generated particles

The thickness of the particles is primarily used in resolving initial overclosures between the particles and the surfaces in the general contact. When particles are generated based on the uniform background method, you can specify the thickness of the generated particles to be either variable or uniform.

<table><tr><td>Input File Usage:</td><td>Use one of the following options to define the thickness of the generated particles:</td></tr><tr><td></td><td>*SECTION CONTROLS, PARTICLE THICKNESS=VARIABLE (default)</td></tr><tr><td></td><td>*SECTION CONTROLS, PARTICLE THICKNESS=UNIFORM</td></tr></table>

<table><tr><td>Abaqus/CAE Usage:</td><td>Generating particles based on a uniform background grid is not supported in Abaqus/CAE.</td></tr></table>

# Specifying a time-based criterion

The time-based criterion is primarily intended as a modeling tool to allow all particles to convert from the defined finite element mesh at the same time.

<table><tr><td>Input File Usage:</td><td>*SECTION CONTROLS, ELEMENT CONVERSION=YES, CONVERSION CRITERION=TIME (default)first data linesecond data linethird data line, time of conversion</td></tr></table>

<table><tr><td>Abaqus/CAE Usage:</td><td>Mesh module: Mesh→Element Type: Conversion to particles: Yes, Criterion: Time</td></tr></table>

# Specifying a strain-based criterion

The strain-based criterion is primarily intended for cases in which you want to use a progressive conversion approach. You specify the maximum principle strain (absolute value) when continuum elements are to convert to SPH particles.

<table><tr><td>Input File Usage:</td><td>*SECTION CONTROLS, ELEMENT CONVERSION=YES, CONVERSION CRITERION=STRAINfirst data linesecond data line</td></tr></table>

<!-- source-page: 85 -->

third data line

, maximum principle strain (absolute value)

Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Conversion to particles:

Yes, Criterion: Strain

Specifying a stress-based criterion

Similar to the strain-based criterion, the stress-based criterion is primarily intended for cases in which you want to use a progressive conversion approach. You specify the maximum principle stress (absolute value) when continuum elements are to convert to SPH particles.

Input File Usage: \*SECTION CONTROLS, ELEMENT CONVERSION=YES, CONVERSION CRITERION=STRESS

first data line

second data line

third data line

, maximum principle stress (absolute value)

Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Conversion to particles:

Yes, Criterion: Stress

Specifying a user subroutine–based criterion

The user subroutine–based criterion allows you to implement a user-defined conversion criterion. You can control element conversion 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.

Input File Usage: Use the following option to trigger a user subroutine–based conversion criterion:

\*SECTION CONTROLS, ELEMENT CONVERSION=YES, CONVERSION CRITERION=USER

(no data lines)

Abaqus/CAE Usage: Specifying a user subroutine–based criterion for element conversion is not supported in Abaqus/CAE.

<!-- source-page: 86 -->

<!-- source-page: 87 -->

# 28. Continuum Elements

General-purpose continuum elements 28.1

Fluid continuum elements 28.2

Infinite elements 28.3

Warping elements 28.4

<!-- source-page: 88 -->

<!-- source-page: 89 -->

# 28.1 General-purpose continuum elements

• “Solid (continuum) elements,” Section 28.1.1   
• “One-dimensional solid (link) element library,” Section 28.1.2   
• “Two-dimensional solid element library,” Section 28.1.3   
• “Three-dimensional solid element library,” Section 28.1.4   
• “Cylindrical solid element library,” Section 28.1.5   
• “Axisymmetric solid element library,” Section 28.1.6   
• “Axisymmetric solid elements with nonlinear, asymmetric deformation,” Section 28.1.7

<!-- source-page: 90 -->
