Using Section Controls
In Abaqus/Standard section controls are used to select the enhanced hourglass control formulation for solid,
shell, and membrane elements. This formulation provides improved coarse mesh accuracy with
slightly higher computational cost and performs better for nonlinear material response at
high strain levels when compared with the default total stiffness formulation. Section
controls can also be used to select some element formulations that might be relevant for a
subsequent Abaqus/Explicit analysis.
In
Abaqus/Explicit
the default formulations for solid, shell, and membrane elements have been
chosen to perform satisfactorily on a wide class of quasi-static and explicit
dynamic simulations. However, certain formulations give rise to some trade-off
between accuracy and performance.
Abaqus/Explicit
provides section controls to modify these element formulations so that you can
optimize these objectives for a specific application. Section controls can also
be used in
Abaqus/Explicit
to specify scale factors for linear and quadratic bulk viscosity parameters.
You can also control the initial stresses in membrane elements for applications
such as airbags in crash simulations and introduce the initial stresses
gradually based on an amplitude definition.
In addition, section controls are used to specify the maximum stiffness degradation and to choose
the behavior on complete failure of an element, once the material stiffness is fully
degraded, including the removal of failed elements from the mesh. This functionality applies
only to elements with a material definition that includes progressive damage (see About Progressive Damage and Failure, Connector Damage Behavior, and Defining the Constitutive Response of Cohesive Elements Using a Traction-Separation Description). In Abaqus/Standard this functionality is limited to
-
cohesive elements with a traction-separation constitutive response that
includes damage evolution,
-
any element with a plane stress formulation that can be used with the
damage evolution model for fiber-reinforced composites,
-
any element that can be used with the damage evolution models for
ductile metals,
-
any element that can be used with the damage evolution law in a low-cycle fatigue analysis, and
-
connector elements with a constitutive response that includes damage
evolution.
Methods for Suppressing Hourglass Modes
The formulation for reduced-integration elements considers only the linearly
varying part of the incremental displacement field in the element for the
calculation of the increment of physical strain. The remaining part of the
nodal incremental displacement field is the hourglass field and can be
expressed in terms of hourglass modes.
Excitation of these modes might lead to severe mesh distortion, with no stresses resisting the
deformation. Similarly, the formulation for element type
C3D4H considers in the constraint equations
only the constant part of the incremental pressure Lagrange multiplier field. The remaining
part of the nodal incremental pressure Lagrange multiplier interpolation is comprised of
hourglass modes.
Hourglass control attempts to minimize these problems without introducing
excessive constraints on the element's physical response.
Several methods are available in
Abaqus
for suppressing the hourglass modes, as described below.
Integral Viscoelastic Approach in Abaqus/Explicit
The integral viscoelastic approach available in
Abaqus/Explicit
generates more resistance to hourglass forces early in the analysis step where
sudden dynamic loading is more probable.
Let q be an hourglass mode magnitude and
Q be the force (or moment) conjugate to
q. The integral viscoelastic approach is defined as
where K is the hourglass stiffness selected by
Abaqus/Explicit,
and s is one of up to three scaling factors
,
,
and
that you can define (by default, ).
The scale factors are dimensionless and relate to specific displacement degrees
of freedom. For solid elements
scales all hourglass stiffnesses. For membrane elements
scales the hourglass stiffnesses related to the in-plane displacement degrees
of freedom, and
scales the out-of-plane displacement degrees of freedom. For shell elements
scales the hourglass stiffnesses related to the in-plane displacement degrees
of freedom, and
scales the hourglass stiffnesses related to the rotational degrees of freedom.
In addition,
scales the hourglass stiffness related to the transverse displacement for
small-strain shell elements.
The integral viscoelastic form of hourglass control is available for all
reduced-integration elements and is the default form in
Abaqus/Explicit,
except for elements modeled with hyperelastic, hyperfoam, and low-density foam
materials and for Eulerian EC3D8R elements. It is the most computationally intensive hourglass
control method. It is not supported for Eulerian EC3D8R elements.
Kelvin Viscoelastic Approach in Abaqus/Explicit
The Kelvin-type viscoelastic approach available in
Abaqus/Explicit
is defined as
where K is the linear stiffness and
C is the linear viscous coefficient. This general form has
pure stiffness and pure viscous hourglass control as limiting cases. When the
combination is used, the stiffness term acts to maintain a nominal resistance
to hourglassing throughout the simulation and the viscous term generates
additional resistance to hourglassing under dynamic loading conditions.
Three approaches are provided in
Abaqus/Explicit
for specifying Kelvin viscoelastic hourglass control.
Specifying the Pure Stiffness Approach
The pure stiffness form of hourglass control is available for all
reduced-integration elements and is recommended for both quasi-static and
transient dynamic simulations.
Specifying the Pure Viscous Approach
The pure viscous form of hourglass control is available only for solid and membrane elements
with reduced integration and is the default form in Abaqus/Explicit for Eulerian EC3D8R elements. It is the
most computationally efficient form of hourglass control and has been shown to be
effective for high-rate dynamic simulations. However, the pure viscous method is not
recommended for low frequency dynamic or quasi-static problems since continuous (static)
loading in hourglass modes results in excessive hourglass deformation due to the lack of
any nominal stiffness.
Specifying a Combination of Stiffness and Viscous Hourglass Control
A linear combination of stiffness and viscous hourglass control is
available only for solid and membrane elements with reduced integration. You
can specify the blending weight factor
()
to scale the stiffness and viscous contributions. Specifying a weight factor
equal to 0.0 or 1.0 results in the limiting cases of pure stiffness and pure
viscous hourglass control, respectively. The default weight factor is 0.5.
Total Stiffness Approach in Abaqus/Standard
The total stiffness approach available in
Abaqus/Standard
is the default hourglass control approach for all first-order,
reduced-integration elements in
Abaqus/Standard,
except for elements modeled with hyperelastic, hyperfoam, or hysteresis
materials. It is the only hourglass control approach available in
Abaqus/Standard
for S8R5, S9R5, and M3D9R elements and the only hourglass control approach available for
the pressure Lagrange multiplier interpolation for C3D4H elements. Hourglass stiffness factors for first-order,
reduced-integration elements depend on the shear modulus, while factors for C3D4H elements depend on the bulk modulus. A scale factor can be
applied to these stiffness factors to increase or decrease the hourglass
stiffness.
Let q be an hourglass mode magnitude and
Q be the force (moment, pressure, or volumetric flux)
conjugate to q. The total stiffness approach for hourglass
control in membrane or solid elements or membrane hourglass control in shell
elements is defined as
where
is a dimensionless scale factor (by default, );
is an hourglass stiffness factor with units of stress;
is the gradient interpolator used to define constant gradients in the element
(
where the superscript P refers to an element node, the
subscript
refers to a direction, and
is a material coordinate); and V is the element volume.
Similarly, the hourglass control for the pressure Lagrange multiplier
interpolation for C3D4H elements is defined as
where
is a dimensionless scale factor (by default, );
is a volumetric gradient operator; and
is an hourglass stiffness factor with units of stress for compressible
hyperelastic and hyperfoam materials and units of stress compliance for all
other materials. The total stiffness approach for bending hourglass control in
shell elements is defined as
where
is the scale factor (by default, ),
is the hourglass stiffness factor, t is the thickness of
the shell element, and A is the area of the shell element.
Default Hourglass Stiffness Values
Normally the hourglass control stiffness is defined from the elasticity associated with the
material. In most cases, the control stiffness of first-order, reduced-integration
elements is based on a typical value of the initial shear modulus of the material, which
might, for example, be given as part of the elastic material definition (Linear Elastic Behavior). Similarly,
hourglass control stiffness of the reduced-integration pressure and volumetric Lagrange
multiplier interpolations of C3D4H
elements is based on a typical value of the initial bulk modulus. For an isotropic
elastic or hyperelastic material G is the shear modulus. For a
nonisotropic elastic material average moduli are used to calculate the hourglass
stiffness: for orthotropic elasticity defined by specifying the terms in the elastic
stiffness matrix or for anisotropic elasticity
and for orthotropic elasticity defined by specifying the engineering
constants or for orthotropic elasticity in plane stress
If the elastic moduli are dependent on temperature or field variables, the
first value in the table is used. The default values for the stiffness factors
are defined below.
For membrane or solid elements
For membrane hourglass control in a shell
For control of bending hourglass modes in a shell
For a general shell section defined by specifying the equivalent section
properties directly, t is defined as
and an effective shear modulus for the section is used to calculate the
hourglass stiffness:
where
is the section stiffness matrix.
User-Defined Hourglass Stiffness
When the initial shear modulus is not defined, you must define the
hourglass stiffness parameters; an example is when user subroutine
UMAT is used to describe the material behavior of elements with
hourglassing modes. In some cases the default value provided for the hourglass
control stiffness may not be suitable and you should define the value.
In some coupled pore fluid diffusion and stress analyses the prevailing
pore pressure in the medium may approach the magnitude of the stiffness of the
material skeleton, as measured by constitutive parameters such as the elastic
modulus. These cases are expected in some partial saturation evaluations of the
wetting of relatively compliant materials such as tissues or cloth. When
reduced-integration or modified tetrahedral or triangular elements are used in
such analyses, the default choice of the hourglass control stiffness parameter,
which is based on a scaling of skeleton material constitutive parameters, may
not be adequate to control hourglassing in the presence of large pore pressure
fields. An appropriate hourglass control stiffness in these cases should scale
with the expected magnitude of pore pressure changes over an element.
Enhanced Hourglass Control Approach in Abaqus/Standard and Abaqus/Explicit
The enhanced hourglass control approach available in both
Abaqus/Standard
and
Abaqus/Explicit
represents a refinement of the pure stiffness method in which the stiffness
coefficients are based on the enhanced assumed strain method; no scale factor
is required. It is the default hourglass control approach for hyperelastic,
hyperfoam, and low-density foam materials in
Abaqus/Explicit
and for hyperelastic, hyperfoam, and hysteresis materials in
Abaqus/Standard.
This method gives more accurate displacement solutions for coarse meshes with
linear elastic materials as compared to other hourglass control methods. It
also provides increased resistance to hourglassing for nonlinear materials.
Although generally beneficial, this may give overly stiff response in problems
displaying plastic yielding under bending. In
Abaqus/Explicit
the enhanced hourglass method will generally predict a much better return to
the original configuration for hyperelastic or hyperfoam materials when loading
is removed.
The enhanced hourglass control approach is compatible between
Abaqus/Standard
and
Abaqus/Explicit.
It is recommended that enhanced hourglass control be used for both
Abaqus/Standard
and
Abaqus/Explicit
for all import analyses. See
Transferring Results between Abaqus/Explicit and Abaqus/Standard.
The enhanced hourglass method is not supported for enriched elements (see
Modeling Discontinuities as an Enriched Feature Using the Extended Finite Element Method).
Specifying the Enhanced Hourglass Control Approach
The enhanced hourglass control method is available for first-order solid,
membrane, and finite-strain shell elements with reduced integration. In
Abaqus/Explicit
it cannot be used for a hyperelastic or hyperfoam material when adaptive
meshing is used on that domain (see the discussion below).
Special Considerations for Hyperelastic and Hyperfoam Materials in an Adaptive Mesh Domain in Abaqus/Explicit
The enhanced hourglass method cannot be used with elements modeled with
hyperelastic or hyperfoam materials that are included in an adaptive mesh
domain. Thus, if you decide to use hyperelastic or hyperfoam materials in an
adaptive mesh domain, you must specify section controls to choose a different
hourglass control approach. The use of adaptive meshing in domains modeled with
finite-strain elastic materials is not recommended since better results are
generally predicted using the enhanced hourglass method and, for solid
elements, element distortion control (discussed below). Therefore, for these
materials it is recommended that the analysis be run without adaptive meshing
but with enhanced hourglass control.
Use in Coupled Pore Pressure Analysis
When first-order, reduced-integration, or modified tetrahedral or
triangular elements are used in coupled pore fluid diffusion and stress
analyses or coupled temperature–pore pressure analyses with enhanced hourglass
control, the hourglass control stiffness, which is based on skeleton material
constitutive parameters, may not be adequate to control hourglassing in the
presence of large pore pressure fields. Since enhanced hourglass control does
not allow you to change the hourglass control stiffness, it is recommended that
total stiffness hourglass control be used in these cases with an appropriate
hourglass control stiffness scaled with the expected magnitude of pore pressure
changes over an element.
Controlling Element Distortion for Crushable Materials in Abaqus/Explicit
Many analyses with volumetrically compacting materials such as crushable
foams see large compressive and shear deformations, especially when the
crushable materials are used as energy absorbers between stiff or heavy
components. The material behavior for crushable materials usually stiffens
significantly under high compression. When a finer mesh is used, the stiffening
behavior of the material model is enough to prevent negative element volumes or
other excessive distortion from occurring under high compressive loads.
However, analyses may fail prematurely when the mesh is coarse relative to
strain gradients and the amount of compression.
Abaqus/Explicit
offers distortion control to prevent solid elements from inverting or
distorting excessively for these cases. The constraint method used in
Abaqus/Explicit
prevents each node on an element from punching inward toward the center of the
element past a point where the element would become non-convex. Constraints are
enforced by using a penalty approach, and you can control the associated
distortion length ratio.
Distortion control is available only for solid elements and cannot be used
when the elements are included in an adaptive mesh domain. Distortion control
is activated by default for elements modeled with hyperelastic, hyperfoam,
crushable foam, or low-density foam materials when the default hourglass
control method is used. If you decide to use any of these materials with solid
elements included in an adaptive mesh domain, you must specify section controls
to deactivate distortion control. Using adaptive meshing in a domain modeled
with hyperelastic or hyperfoam materials is not recommended since better
results are generally predicted using the enhanced hourglass method in
combination with element distortion control.
When element distortion control is used in combination with the enhanced
hourglass method (default behavior for hyperelastic and hyperfoam materials), a
small amount of viscous damping is added to the element formulation and the
associated viscous energy dissipation is included in the output of artificial
strain energy (ALLAE).
If distortion control is used, the energy dissipated by distortion control
can be output upon request (see
Abaqus/Explicit Output Variable Identifiers
for details). Although developed for analyses of energy absorbing,
volumetrically compacting materials, distortion control can be used with any
material model. However, care must be used in interpreting results since the
distortion control constraints may inhibit legitimate deformation modes and
lock up the mesh. Distortion control cannot prevent elements from being
distorted due to temporal instabilities, hourglass instabilities, or physically
unrealistic deformation.
Controlling the Distortion Length Ratio
By default, the constraint penalty forces are applied when the node moves to a point a small
offset distance away from the actual plane of constraint. This appears to improve the
robustness of the method and limits the reduction of time increment due to severe
shortening of the element characteristic length. This offset distance is determined by the
distortion length ratio times the initial element characteristic length. The default value
of the distortion length ratio, r, is 0.1. You can change the
distortion length ratio by specifying a value for r,
.
For C3D10 elements, instead of the
distortion length ratio, the distortion volume ratio (the current volume over the original
volume at each integration point) is used. The default threshold value of the distortion
volume ratio, r, is also 0.1. You can change the distortion volume
ratio by specifying a value for r,
.
Selecting a Scale Factor for the Drill Stiffness in Abaqus/Explicit
A drill constraint acts to keep the element nodal rotations in the direction
of the shell normal consistent with the average in-plane rotation of the
element. Lack of such a constraint can lead to large rotations at these element
nodes. Section controls can be used to select a scale factor for the default
drill stiffness of an individual element set.
Drill Constraint in Small Strain Shell Elements S3RS and S4RS in Abaqus/Explicit
The formulation of small strain shell elements S3RS and S4RS includes a drill constraint and does so by default.
Alternatively, you can deactivate the drill constraint for these elements. The
drill constraint is always active for the finite strain conventional shell
elements such as S4R, but the default value of the drill stiffness can be scaled as
mentioned above.
Ramping of Initial Stresses in Membrane Elements in Abaqus/Explicit
For applications such as airbags in crash simulations the initial strains
(hence, the initial stresses) are introduced into the model through a reference
configuration that is different from the initial configuration. Often the
components that confine the airbag in the initial configuration are excluded
from the numerical model causing motion of the airbag under initial stresses at
the beginning of the analysis.
Abaqus/Explicit
provides a technique to introduce the initial stresses in the membrane elements
gradually based on an amplitude definition. This amplitude must be defined with
its value starting from zero and reaching a final value of one. The initial
stresses will not be applied for the duration that the amplitude stays at zero.
Defining the Kinematic Formulation for Hexahedron Solid Elements
The default kinematic formulation for reduced-integration solid elements in
Abaqus
(and the only kinematic formulation available in
Abaqus/Standard)
is based on the uniform strain operator and the hourglass shape vectors.
Details can be found in
Solid isoparametric quadrilaterals and hexahedra.
These kinematic assumptions result in elements that pass the constant strain
patch test for a general configuration and give zero strain under large rigid
body rotation. However, the formulation is relatively expensive, especially in
three dimensions.
Abaqus/Explicit
offers two alternative kinematic formulations for the C3D8R solid element that can reduce the computational cost. The
performance for each kinematic formulation on the patch test and under large
rigid body rotation for various element configurations is summarized in
Table 1.
Suitable applications for each kinematic formulation are summarized in
Table 2.
You can specify the kinematic formulation for 8-node brick elements.
Default Formulation
The default average strain formulation of uniform strain and hourglass shape
vectors is the only formulation available in
Abaqus/Standard.
This formulation is recommended for all problems and is particularly well
suited for applications exhibiting high confinement, such as closed-die forming
and bushing analyses.
Orthogonal Formulation in Abaqus/Explicit
A noticeable reduction in computational cost can be obtained by using the
orthogonal formulation available in
Abaqus/Explicit.
This formulation is based on the centroidal strain operator and a slight
modification to the hourglass shape vectors. The centroidal strain operator
requires three times fewer floating point operations than the uniform strain
operator. Elements formulated with an orthogonal kinematic split pass the patch
test only for rectangular or parallelepiped element configurations. However,
numerical experience has shown that the element converges on the exact solution
for general element configurations as the mesh is refined. It also performs
well for large rigid body motions.
This formulation provides a good balance between computational speed and
accuracy. It is recommended for all analyses except those involving highly
distorted elements, very coarse meshes, or high confinement. Suitable
applications for this formulation include elastic drop testing.
Centroid Formulation in Abaqus/Explicit
The fastest formulation available in
Abaqus/Explicit
is specified by selecting the centroid formulation. The centroid formulation is
based on the centroidal strain operator and the hourglass base vectors. Using
the hourglass base vectors instead of the hourglass shape vectors reduces
hourglass mode computations by a factor of three. However, the hourglass base
vectors are not orthogonal to rigid body rotation for general element
configurations, so that hourglass strain may be generated with large rigid body
rotations with this formulation.
This formulation should be used only to improve computational performance on problems that have
reasonable mesh refinement and no significant amount of rigid body rotation (for example,
transient flat rolling simulation).
Choosing the Order of Accuracy in Solid and Shell Element Formulations
Abaqus/Standard
offers only a second-order accurate formulation for all elements.
Abaqus/Explicit
offers both first- and second-order accurate formulations for solid and shell
elements. First-order accuracy is the default and yields sufficient accuracy
for nearly all
Abaqus/Explicit
problems because of the inherently small time increment size. Second-order
accuracy is usually required for analyses with components undergoing a large
number of revolutions (>5). For three-dimensional solids the second-order
accuracy formulation is available only with the default average strain
kinematic formulation.
First-Order Accuracy
In
Abaqus/Explicit
the first-order accurate formulation for solid and shell elements is the
default. This formulation is not available in
Abaqus/Standard.
Second-Order Accuracy
The second-order accurate element formulation is appropriate for problems
with a large number of revolutions (>5). This is the only formulation
available in
Abaqus/Standard.
Simulation of propeller rotation
illustrates the performance of second-order accurate shell and solid elements
in
Abaqus/Explicit
as they undergo about 100 revolutions.
Selecting Scale Factors for Bulk Viscosity in Abaqus/Explicit
Bulk viscosity introduces damping associated with volumetric straining. Its
purpose is to improve the modeling of high-speed dynamic events.
Abaqus/Explicit
contains two forms of bulk viscosity, linear and quadratic, which can be
defined for the whole model at each step of the analysis, as discussed in
Bulk Viscosity.
Section controls can be used to select scale factors for the linear and
quadratic bulk viscosities of an individual element set.
The pressure term generated by bulk viscosity might introduce unexpected results in the
volumetric response of highly compressible materials; therefore, it is recommended to
suppress bulk viscosity for these materials by specifying scale factors equal to zero.
Controlling the Activation of the "Improved" Element Time Estimation Method in Abaqus/Explicit
For three-dimensional continuum elements and elements with plane stress
formulations (shell, membrane, and two-dimensional plane stress elements) an
"improved" estimate of the element characteristic length is used by default.
This "improved" method usually results in a larger element stable time
increment than a more traditional method. The activation of the "improved"
element time estimation method can be defined globally for the whole model at
each step of the analysis, as discussed in
Time Incrementation.
Alternatively, you can selectively control the activation of the "improved"
element time estimation method for each individual element set.
Controlling Element Deletion and Maximum Degradation for Materials with Damage Evolution
Abaqus offers a general capability for modeling progressive damage and failure of materials
(About Progressive Damage and Failure). In Abaqus/Standard this capability is available only for cohesive elements, connector elements, elements
with plane stress formulations (plane stress, shell, continuum shell, and membrane
elements), any element that can be used with the damage evolution models for ductile metals,
and any element that can be used with the damage evolution law in a low-cycle fatigue
analysis. In Abaqus/Explicit this capability is available for all elements with progressive damage behavior except
connector elements. Section controls are provided to specify the value of the maximum
stiffness degradation,
, for material failure and whether element deletion occurs when the
degradation reaches this level. By default, an element is deleted on material failure.
Details for element deletion driven by material failure are described in Material Failure and Element Deletion. The choice of element deletion also affects how the damage
is applied; details can be found in the following sections:
Controlling Shell Element Deletion Based on Integration Point Status in Abaqus/Explicit
In
Abaqus/Explicit
you can delete shell elements based on the number of active or failed
integration points through the shell section. By default, when only one
integration point through the shell section is active, the shell element is
deleted. You can specify either the number of active integration points or the
number of failed integration points through the shell section at which the
shell element is deleted. The number you specify must not exceed the total
number of integration points through the shell section. Alternatively, you can
specify that a shell element is deleted when all of the integration points
through the shell section are failed.
Controlling Distortion-Based Element Deletion in Abaqus/Explicit
In
Abaqus/Explicit
you can control element deletion for deformable elements (except cohesive
elements) based on distortion. An inherent limit exists as to how much
deformation a Lagrangian element can accommodate to obtain accurate simulation
results. By default, elements are deleted only when material failure is defined
and failure occurs. In rare cases, an element can become excessively distorted
before material failure occurs and cause the simulation to stop prematurely. In
addition, when an element gets distorted, the element stable time increment can
drop dramatically, causing a performance issue. You can activate
distortion-based element deletion to delete the distorted elements and allow
the simulation to continue.
You can control the deletion of distorted elements using the following measures: current element
stable time increment, volume or area, or characteristic length. The element stable time
increment used does not include damping (bulk viscosity), mass scaling, or penalty contact
effects. The element is removed once the measure falls below the specified value. The
deletion criteria can be based on a ratio of the deletion measure over the original value;
for example, the ratio of the element volume over the original element volume at which the
element is deleted. Alternatively, you can specify a value for the deletion measure; for
example, the element volume at which the element is deleted.
Distortion-based element deletion is intended for experienced users and
should be used with caution. Setting improper values for the deletion criteria
can lead to unphysical or misleading results.
Using Linear Kinematic Conversion in Abaqus/Explicit
When elements are subject to large compressive forces, they can reach a point when negative
volumes are calculated. The negative volumes cause a fatal error if nonlinear geometric
effects are considered. One method to avoid the fatal error is to convert the element from
nonlinear kinematics to linear kinematics when it reaches a certain level of compression
(volume reduction).
Linear kinematic conversion is activated only when distortion control is also activated.
The element is converted when distortion control forces become active. For
C3D10 elements, linear kinematic conversion
does not require the use of distortion control. For
C3D10 elements, linear kinematic conversion
occurs when the ratio of the element characteristic length over the original characteristic
length reaches a critical value.
Linear kinematic conversion allows the simulation to continue subject to approximation of
linear kinematics for the highly distorted elements. Linear kinematic conversion can be used
as an alternative to distortion-based element deletion (see ).
The linear kinematic conversion is mainly developed to improve element robustness. The
element computation results will not be exactly accurate for the elements that have been
converted to linear kinematics. Therefore, linear kinematic conversion should be used with
caution to avoid unphysical or misleading results.
Using Viscous Regularization with Cohesive Elements, Connector Elements, and Elements That Can Be Used with the Damage Evolution Models for Ductile Metals and Fiber-Reinforced Composites in Abaqus/Standard
Material models exhibiting softening behavior and stiffness degradation
often lead to severe convergence difficulties in implicit analysis programs,
such as
Abaqus/Standard.
A common technique to overcome some of these convergence difficulties is the
use of viscous regularization of the constitutive equations, which causes the
tangent stiffness matrix of the softening material to be positive for
sufficiently small time increments.
The traction-separation laws used to describe the constitutive behavior of
cohesive elements can be regularized in
Abaqus/Standard
using viscosity, by permitting stresses to be outside the limits defined by the
traction-separation law. The details of the regularization procedure are
discussed in
Viscous Regularization in Abaqus/Standard.
The same technique is also used to regularize the following:
You specify the amount of viscosity to be used for the regularization
procedure. By default, no viscosity is included so that no viscous
regularization is performed.
Using Viscous Damping with Connector Elements in Abaqus/Standard
Material failure in connector elements often causes convergence problems in
Abaqus/Standard.
To avoid such convergence problems, you can introduce viscous damping into the
connector components by specifying the value of the damping coefficient as
discussed in
Connector Failure Behavior.
By default, no damping is included.
Using Section Controls in an Import Analysis
The recommended procedure for doing import analysis is to specify the
enhanced hourglass control formulation in the original analysis. Once the
section controls have been specified in the original analysis, they cannot be
modified in subsequent import analyses. This ensures that the enhanced
hourglass control formulation is used in the original as well as import
analyses. The default values for other section controls are usually appropriate
and should not be changed. For further details on using section controls in an
import analysis, see
Transferring Results between Abaqus/Explicit and Abaqus/Standard.
Using Section Controls for Flexion-Torsion Type Connector
When the third axes of the two local coordinate systems for a
flexion-torsion type connector are exactly aligned, a numerical singularity
occurs that may lead to convergence difficulties. To avoid this, a small
perturbation can be applied to the local coordinate system defined at the
second connector node.
Using Section Controls to Define the Particle Tracking Box for DEM and SPH Particles
For discrete element method (DEM) analyses,
a particle tracking box is established at the beginning of the analysis to
define the rectangular region within which the particle search (finding all
neighbors for all particles) is performed. A region that is 10% larger in all
directions than the overall model initial dimensions and is centered at the
geometric center of the model is used.
For smoothed particle hydrodynamic (SPH)
analyses, all particles are tracked as the analysis progresses by default. For
DEM analyses, particle tracking is based on
the initially established tracking box by default. Alternatively, you can
define a particle tracking box to define the region within which the particle
search is performed.
You define a fixed size for the particle tracking box by specifying the
coordinates of two opposite corners (lower left and upper right) of this box.
As the analysis progresses, if a particle is outside this tracking box, it
behaves like a free-flying point mass and does not contribute to the
DEM or SPH
calculations. If the particle reenters the box at a later stage, it is once
again included in the calculations. If you want to track all of the particles
during the analysis, you must ensure that the particle tracking box fully
encompasses the domain through which the model moves; otherwise, you will lose
tracking of the particle.
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.
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.
Using Section Controls for Specifying SPH Parameters
You can control the way the smoothing length is computed (see Smoothed Particle Hydrodynamics). 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 increases or decreases 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.
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.
You can specify the number of particles per parent element to be generated.
Several criteria to trigger the conversion are available.
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.
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.
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.
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.
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.
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.
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.
|