 CONVERSION CRITERION

This parameter applies only to
Abaqus/Explicit
analyses involving the conversion of continuum elements to
SPH particles and is valid only when ELEMENT CONVERSION=YES.
Set CONVERSION CRITERION=TIME (default) to specify the time when continuum elements are to
convert to SPH particles.
Set CONVERSION CRITERION=STRAIN to specify the maximum principal strain (absolute value) when
continuum elements are to convert to SPH
particles.
Set CONVERSION CRITERION=STRESS to specify the maximum principal stress (absolute value) when
continuum elements are to convert to SPH
particles.
Set CONVERSION CRITERION=USER to specify a useddefined criterion when continuum elements
are to convert to SPH particles.
 DISTORTION CONTROL

This parameter applies to
Abaqus/Explicit
analyses and to solid sections in
Abaqus/Standard
analyses containing C3D10HS elements.
Set DISTORTION CONTROL=YES to activate a constraint that acts to prevent negative element
volumes or other excessive distortion for crushable materials. This is the
default value for elements with hyperelastic or hyperfoam materials. The DISTORTION CONTROL parameter is not relevant for linear kinematics and cannot
prevent elements from being distorted due to temporal instabilities, hourglass
instabilities, or physically unrealistic deformation.
Set DISTORTION CONTROL=NO to deactivate a constraint that acts to prevent negative
element volumes or other excessive distortion for crushable materials. This
value is the default except for elements with hyperelastic or hyperfoam
materials.
 DRILL STIFFNESS

This parameter applies only to the smallstrain shell elements S3RS and S4RS.
Set DRILL STIFFNESS=ON (default) to activate the constraint against the drill mode in
S3RS and S4RS elements.
Set DRILL STIFFNESS=OFF to deactivate the constraint against the drill mode.
Deactivating the drill constraint can result in large values for the rotation
degrees of freedom at the nodes of these elements.
The drill constraint is always active for finitestrain conventional shell
elements such as S4R.
 ELEMENT CONVERSION

This parameter applies only to
Abaqus/Explicit
analyses involving the conversion of continuum elements to
SPH particles.
Set ELEMENT CONVERSION=NO (default) to prevent continuum elements from converting to
SPH particles.
Set ELEMENT CONVERSION=YES to allow continuum elements to convert to
SPH particles.
Set ELEMENT CONVERSION=BACKGROUND GRID to allow continuum elements to convert to
SPH particles that are uniformly distributed
in an equally spaced background grid.
 ELEMENT DELETION

This parameter applies to all elements with progressive damage behavior,
except connector elements in
Abaqus/Explicit.
Set ELEMENT DELETION=YES to allow element deletion when the element has completely
damaged. This value is the default for all elements with a damage evolution
model. However, this value is not applicable to pore pressure cohesive
elements.
Set ELEMENT DELETION=NO to allow fully damaged elements to remain in the computations.
The element retains a residual stiffness given by the specified value of MAX DEGRADATION. In addition, elements with threedimensional stress states
(including generalized plane strain elements) can sustain hydrostatic
compressive stresses, and elements with onedimensional stress states can
sustain compressive stresses. This value is the default for pore pressure
cohesive elements and is not available for beam elements.
 HOURGLASS

Set HOURGLASS=COMBINED to define the viscousstiffness form of hourglass control for
solid and membrane elements with reduced integration in
Abaqus/Explicit.
Set HOURGLASS=ENHANCED (default for elements with hyperelastic and hyperfoam
materials in
Abaqus/Standard
and
Abaqus/Explicit;
default in
Abaqus/Standard
and only option in
Abaqus/Explicit
for modified tetrahedral or triangular elements) to define hourglass control
that is based on the assumed enhanced strain method for solid, membrane,
finitestrain shell elements with reduced integration and modified tetrahedral
or triangular elements in
Abaqus/Standard
and
Abaqus/Explicit.
Any data given on the data line will be ignored for this case.
Set HOURGLASS=RELAX STIFFNESS (default for
Abaqus/Explicit,
except for elements with hyperelastic and hyperfoam materials) to use the
integral viscoelastic form of hourglass control for all elements with reduced
integration in
Abaqus/Explicit.
This value is not supported for Eulerian EC3D8R elements.
Set HOURGLASS=STIFFNESS (default for
Abaqus/Standard,
except for elements with hyperelastic and hyperfoam materials and modified
tetrahedral or triangular elements) to define hourglass control that is
strictly elastic for all elements with reduced integration in
Abaqus/Standard
and
Abaqus/Explicit
and modified tetrahedral or triangular elements in
Abaqus/Standard.
Set HOURGLASS=VISCOUS (default for Eulerian EC3D8R elements) to define the hourglass damping used to control the
hourglass modes for solid and membrane elements with reduced integration in
Abaqus/Explicit.
 IMPROVED DT METHOD

Include this parameter to activate the "improved" element time estimation
method for threedimensional continuum elements and elements with plane stress
formulations in
Abaqus/Explicit.
Set IMPROVED DT METHOD=GLOBAL (default) to match the setting of the "improved" element time
estimation method defined globally for the whole model.
Set IMPROVED DT METHOD=YES to activate the "improved" element time estimation method.
Set IMPROVED DT METHOD=NO to deactivate the "improved" element time estimation method.
 INITIAL GAP OPENING

This parameter applies only to
Abaqus/Standard
analyses using pore pressure cohesive elements.
Set this parameter equal to the value of the initial gap opening used in the
tangential flow continuity equation for pore pressure cohesive elements. The
default value is 0.002.
 KERNEL

This parameter applies only to
Abaqus/Explicit
analyses involving smoothed particle hydrodynamics
(SPH).
Set KERNEL=CUBIC (default) to use a cubic spline interpolator for the
SPH formalism.
Set KERNEL=QUADRATIC to use a quadratic interpolator for the
SPH formalism.
Set KERNEL=QUINTIC to use a quintic interpolator for the
SPH formalism.
 KINEMATIC SPLIT

Include this parameter to change the kinematic formulation for 8node brick
elements only.
Set KINEMATIC SPLIT=AVERAGE STRAIN (default in
Abaqus/Explicit)
to use the uniform strain formulation and the hourglass shape vectors in the
hourglass control. This is the only option available for
Abaqus/Standard.
Set KINEMATIC SPLIT=CENTROID to use the centroid strain formulation and the hourglass base
vectors in the hourglass control in
Abaqus/Explicit.
Set KINEMATIC SPLIT=ORTHOGONAL to use the centroid strain formulation and the hourglass shape
vectors in the hourglass control in
Abaqus/Explicit.
If SECOND ORDER ACCURACY=YES, the KINEMATIC SPLIT parameter will be reset to AVERAGE STRAIN in
Abaqus/Explicit.
 LENGTH RATIO

This parameter applies only to
Abaqus/Explicit
analyses and is valid only when the DISTORTION CONTROL parameter is used.
Set this parameter equal to $r$
($0.0<r\le 1.0$)
to define the length ratio when using distortion control for crushable
materials. The default value is $r=0.1$.
 MAX DEGRADATION

This parameter applies to all elements with progressive damage behavior,
except connector elements in
Abaqus/Explicit.
Set this parameter equal to the value of the damage variable at or above
which a material point will be assumed to be completely damaged. This parameter
also determines the amount of residual stiffness that will be retained by
elements for which the ELEMENT DELETION parameter is set to NO. For elements other than cohesive elements, connector
elements, and elements with plane stress formulations the default value is 1.0
if the element is deleted from the mesh and 0.99 otherwise. For cohesive
elements, connector elements, and elements with plane stress formulations the
default value is always 1.0.
 PARTICLE THICKNESS

This parameter applies only to
Abaqus/Explicit
analyses and is valid only when ELEMENT CONVERSION=BACKGROUND GRID.
Set PARTICLE THICKNESS=VARIABLE (default) to define the nonuniform thickness of the particles.
Set PARTICLE THICKNESS=UNIFORM to define the uniform thickness of the particles.
 PERTURBATION

This parameter applies only to
Abaqus/Standard
analyses.
Set this parameter equal to a small perturbation to be applied to the second
orientation for the FLEXIONTORSION connectors.
 RAMP INITIAL STRESS

This parameter applies to membrane elements in
Abaqus/Explicit
analyses.
Set this parameter equal to the name of a total timebased amplitude defined
to go from an initial value of zero to a final value of one. When this
parameter is specified, the element stiffness is controlled until the amplitude
value reaches its final value of one, so that the initial stresses are
introduced gradually and not abruptly.
 SECOND ORDER ACCURACY

This parameter applies only to
Abaqus/Explicit
analyses; the element formulation is always secondorder accurate in
Abaqus/Standard.
Set SECOND ORDER ACCURACY=YES to use a secondorder accurate formulation for solid or shell
elements suitable for problems undergoing a large number of revolutions (>
5).
Set SECOND ORDER ACCURACY=NO (default) to use the firstorder accurate solid or shell
elements.
The SECOND ORDER ACCURACY parameter is not relevant for linear kinematics.
 SPH FORMULATION

This parameter applies only to
Abaqus/Explicit
analyses involving smoothed particle hydrodynamics
(SPH).
Set SPH FORMULATION=CLASSICAL (default) to use the classical
SPH method.
Set SPH FORMULATION=NSPH to use the normalized SPH
method.
Set SPH FORMULATION=XSPH to use the XSPH method.
 SPH SMOOTHING LENGTH

This parameter applies only to
Abaqus/Explicit
analyses involving smoothed particle hydrodynamics
(SPH).
Set SPH SMOOTHING LENGTH=CONSTANT (default) to use the constant smoothing length.
Set SPH SMOOTHING LENGTH=VARIABLE to use the variable smoothing length.
 SPH TENSILE INSTABILITY CONTROL

This parameter applies only to
Abaqus/Explicit
analyses and is valid only when ELEMENT CONVERSION=BACKGROUND GRID or when SPH particles are
initially in a uniform distribution.
Set SPH TENSILE INSTABILITY CONTROL=NO (default) to not use the SPH
tensile instability control.
Set SPH TENSILE INSTABILITY CONTROL=YES to use the SPH tensile
instability control.
 VISCOSITY

This parameter applies to cohesive elements, connector elements, and
elements with plane stress formulations (plane stress, shell, continuum shell,
and membrane elements) in
Abaqus/Standard
analyses.
Set this parameter equal to the value of the viscosity coefficient used in
the viscous regularization scheme for cohesive elements or connector elements
or equal to the value of the damping coefficient used in connector failure
modeling. When this parameter is used to specify the viscosity coefficients for
the damage model for fiberreinforced materials, the specified value is applied
to all the damage modes. The default value is 0.0.
 WEIGHT FACTOR

This parameter applies only to
Abaqus/Explicit
analyses.
Set this parameter equal to $\alpha $
($0.0\le \alpha \le 1.0$)
to scale the contributions from the constant hourglass stiffness term and the
hourglass damping term to the hourglass control formulation. Setting
$\alpha =0.0$
or $\alpha =1.0$
corresponds to pure constant stiffness hourglass control and pure damping
hourglass control, respectively. The default is $\alpha =0.5$.
This option is used only for solid and membrane elements when the HOURGLASS parameter is set equal to COMBINED.