is computationally efficient for the analysis of large models with relatively short
dynamic response times and for the analysis of extremely discontinuous events or
processes;
uses a consistent, large-deformation theory—models can undergo large rotations and large
deformation;
can use a geometrically linear deformation theory—strains and rotations are assumed to be
small (see Defining an Analysis);
can be used to perform an adiabatic stress analysis if inelastic dissipation is expected
to generate heat in the material (see Adiabatic Analysis);
can be used to perform quasi-static analyses with complicated contact conditions; and
allows for either automatic or fixed time incrementation to be used—by default, Abaqus/Explicit uses automatic time incrementation with the global time estimator.
The explicit dynamics procedure performs a large number of small time increments
efficiently. An explicit central-difference time integration rule is used; each increment is
relatively inexpensive (compared to the direct-integration dynamic analysis procedure
available in Abaqus/Standard) because there is no solution for a set of simultaneous equations. The explicit
central-difference operator satisfies the dynamic equilibrium equations at the beginning of
the increment, t; the accelerations calculated at time
t are used to advance the velocity solution to time and the displacement solution to time .
Central-Difference Time Integration with Implicit Corrections
The explicit dynamic analysis procedure is based on the implementation of an explicit
integration rule together with the use of diagonal (“lumped”) element mass matrices. A
correction phase is used to implicitly treat connectors and constraints.
Predicted nodal accelerations, , at the beginning of increment number i of an
explicit dynamic step are computed by:
where is the mass matrix, is the applied load vector, and is the explicit internal force vector. A lumped mass matrix is used
because its inverse is simple to compute and because the vector multiplication of the mass
inverse by the inertial force requires only n operations, where
n is the number of degrees of freedom in the model. The
internal force vector, , is assembled from contributions from the individual elements such that a
global stiffness matrix need not be formed.
The equations of motion for the body are integrated using the explicit central-difference
integration rule to compute predicted mid-increment nodal velocity (or angular velocity), , and predicted end-of-increment displacement (or rotation), as follows:
The central-difference integration operator is explicit in the sense that the predicted
kinematic state is advanced using known values of and from the previous increment.
However, the predicted kinematic quantities do not account for implicitly treated
connections and constraints. To account for these entities, implicit forces are computed
considering the predicted configuration. Calculation of the implicit force vector, , often requires solution of nonlinear systems of equations each increment,
which is typically efficient but can degrade performance for situations with overlapping
constraints, as discussed in Constraint Enforcement and Overlapping Constraints. These implicit
forces cause nodal acceleration corrections at increment i:
Acceleration corrections are applied to determine corrected kinematic quantities that
satisfy connection and constraint behavior as follows:
Sometimes it is necessary to enforce the constraints implicitly, especially if there are
multiple constraints applied at a node. The implicit enforcement of constraints can lead to
a performance degradation (see Computational Cost for Constraint Solution in Abaqus/Explicit).
Nodal Mass and Inertia
The explicit integration scheme in Abaqus/Explicit requires nodal mass or inertia to exist at all activated degrees of freedom (see Conventions) unless
constraints are applied using boundary conditions. More precisely, a nonzero nodal mass must
exist unless all activated translational degrees of freedom are constrained and nonzero
rotary inertia must exist unless all activated rotational degrees of freedom are
constrained. Nodes that are part of a rigid body do not require mass, but the entire rigid
body must possess mass and inertia unless constraints are used. Nodes that belong to
Eulerian elements also do not require mass, since the surrounding Eulerian elements might be
void at some time during the simulation.
When degrees of freedom at a node are activated by elements with a nonzero mass density
(for example, solid, shell, beam) or mass and inertia elements, a nonzero nodal mass or
inertia occurs naturally from the assemblage of lumped mass contributions.
When degrees of freedom at a node are activated by elements with no mass (for example,
spring, dashpot, or connector elements), care must be taken either to constrain the node or
to add mass and inertia as appropriate.
Stability
The explicit procedure integrates through time by using many small time increments. The
central-difference operator is conditionally stable, and the stability limit for the
operator (with no damping) is given in terms of the highest frequency of the system as
With damping, the stable time increment is given by
where is the fraction of critical damping in the mode with the highest
frequency. Contrary to our usual engineering intuition, introducing damping to the solution
reduces the stable time increment. In Abaqus/Explicit a small amount of damping is introduced in the form of bulk viscosity to control high
frequency oscillations. Physical forms of damping, such as dashpots or material damping, can
also be introduced. Bulk viscosity and material damping are discussed below.
Estimating the Stable Time Increment Size
An approximation to the stability limit is often written as the smallest transit time of
a dilatational wave across any of the elements in the mesh
where is the smallest element dimension in the mesh and is the dilatational wave speed in terms of and , defined below.
In general, for beams, conventional shells, and membranes the element thickness or
cross-sectional dimensions are not considered in determining the smallest element
dimension; the stability limit is based on the midplane or membrane dimensions only. When
the transverse shear stiffness is defined for shell elements (see Shell Section Behavior), the stable
time increment will also be based on the transverse shear behavior.
This estimate for is only approximate and in most cases is not a conservative (safe)
estimate. In general, the actual stable time increment chosen by Abaqus/Explicit will be less than this estimate by a factor between and 1 in a two-dimensional model and between and 1 in a three-dimensional model. The time increment chosen by Abaqus/Explicit also accounts for any stiffness behavior in a model associated with penalty contact.
For further discussion, see Computational Cost below.
Stable Time Increment Report
Abaqus/Explicit writes a report to the status (.sta) file during the data check
phase of the analysis that contains an estimate of the minimum stable time increment and a
listing of the elements with the smallest stable time increments and their values. The
initial stable time increments listed do not include damping (bulk viscosity), mass
scaling, or penalty contact effects.
This listing is provided because often a few elements have much smaller stability limits
than the rest of the elements in the mesh. The stable time increment can be increased by
modifying the mesh to increase the size of the controlling element or by using appropriate
mass scaling.
Dilatational Wave Speed
The current dilatational wave speed, , is determined in Abaqus/Explicit by calculating the effective hypoelastic material moduli from the material's constitutive
response. Effective Lamé's constants, and , are determined in the following manner. Define as the increment in the mean stress, as the increment in the deviatoric stress, as the increment of volumetric strain, and as the deviatoric strain increment. We assume a hypoelastic stress-strain
rule of the form
The effective moduli can then be computed as
For shell elements defined by a shell cross-section that requires numerical integration
(see Using a Shell Section Integrated during the Analysis to Define the Section Behavior), the effective
moduli for the section are computed by integrating the effective moduli at the section
points through the thickness. These effective moduli represent the element stiffness and
determine the current dilatational wave speed in the element as
where is the density of the material.
In an isotropic, elastic material the effective Lamé's constants can be defined in terms of
Young's modulus, E, and Poisson's ratio, , by
and
Time Incrementation
The time increment used in an analysis must be smaller than the stability limit of the
central-difference operator. Failure to use a small enough time increment will result in an
unstable solution. When the solution becomes unstable, the time history response of solution
variables such as displacements will usually oscillate with increasing amplitudes. The total
energy balance will also change significantly.
If the model contains only one material type, the initial time increment is directly
proportional to the size of the smallest element in the mesh. If the mesh contains uniform
size elements but contains multiple material descriptions, the element with the highest wave
speed will determine the initial time increment.
In nonlinear problems—those with large deformations and/or nonlinear material response—the
highest frequency of the model will continually change, which consequently changes the
stability limit. Abaqus/Explicit has two strategies for time incrementation control: fully automatic time incrementation
(where the code accounts for changes in the stability limit) and fixed time incrementation.
Scaling the Time Increment
To reduce the chance of a solution going unstable, you can adjust the stable time
increment computed by Abaqus/Explicit by a constant scaling factor. This factor can be used to scale the default global time
estimate, the element-by-element estimate, or the fixed time increment based on the
initial element-by-element estimate; it cannot be used to scale a fixed time increment
specified directly by you.
Input File Usage
Use the following option to scale the stable time increment based on the global time
estimate:
Use the following option to scale the stable time increment based on the
element-by-element estimate:
DYNAMIC, EXPLICIT, ELEMENT BY ELEMENT, SCALE FACTOR=f
Use the following option to scale the stable time increment based on the fixed time
increment on the initial element-by-element estimate:
DYNAMIC, EXPLICIT, FIXED TIME INCREMENTATION, SCALE FACTOR=f
Abaqus/CAE Usage
Step module: Create Step: General: Dynamic, Explicit: Incrementation: Time scaling factor: f
Automatic Time Incrementation
The default time incrementation scheme in Abaqus/Explicit is fully automatic and requires no user intervention. Two types of estimates are used
to determine the stability limit: element by element and global. An analysis always starts
by using the element-by-element estimation method and might switch to the global
estimation method under certain circumstances, as explained below.
Element-by-Element Estimation
In an analysis Abaqus/Explicit initially uses a stability limit based on the highest element frequency in the whole
model. This element-by-element estimate is determined using the current dilatational
wave speed in each element.
The element-by-element estimate is conservative; it will give a smaller stable time
increment than the true stability limit that is based upon the maximum frequency of the
entire model. In general, constraints such as boundary conditions and kinematic contact
have the effect of compressing the eigenvalue spectrum, and the element-by-element
estimates do not take this into account.
The concept of the stable time increment as the time required to propagate a
dilatational wave across the smallest element dimension is useful for interpreting how
the explicit procedure chooses the time increment when element-by-element stability
estimation controls the time increment. As the step proceeds, the global stability
estimate, if used, makes the time increment less sensitive to element size.
The stability limit will be determined by the global estimator as the step proceeds
unless the element-by-element estimation method is specified, fixed time incrementation
is specified, or one of the conditions explained below prevents the use of global
estimation. The switch to the global estimation method occurs once the algorithm
determines that the accuracy of the global estimation method is acceptable.
The adaptive, global estimation algorithm determines the maximum frequency of the
entire model using the current dilatational wave speed. This algorithm continuously
updates the estimate for the maximum frequency. The global estimator will usually allow
time increments that exceed the element-by-element values.
Abaqus/Explicit monitors the effectiveness of the global estimation algorithm. If the cost for
computing the global time estimate is more than its benefit, the code will turn off the
global estimation algorithm and simply use the element-by-element estimates to save
computation time.
Conditions That Will Prevent the Use of the Global Time Estimator
The global estimation algorithm will not be used when any of the following capabilities
are included in the model:
Fluid elements
Infinite elements
Dashpots
Thick shells (thickness to characteristic length ratio larger than 0.92)
Thick beams (thickness to length ratio larger than 1.0)
The JWL equation of state
Material damping
Nonisotropic elastic materials with temperature and field variable dependency
Distortion control
Adaptive meshing
Subcycling
Improved Stable Time Increment for Three-Dimensional Continuum
Elements and Elements with Plane Stress Formulations
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. For analyses using variable mass scaling, the
total mass added to achieve a given stable time increment will be less with the improved
estimate.
Input File Usage
Use the following option to activate the improved element time
estimation method:
A fixed time incrementation scheme is also available in Abaqus/Explicit. The fixed time increment size is determined either by the initial element-by-element
stability estimate for the step or by a user-specified time increment.
Fixed time incrementation might be useful when a more accurate representation of the
higher mode response of a problem is required. In this case a time increment size smaller
than the element-by-element estimates might be used. The element-by-element estimate can
be obtained simply by running a data check analysis (see Abaqus/Standard and Abaqus/Explicit Execution).
When fixed time incrementation is used, Abaqus/Explicit will not check that the computed response is stable during the step. You should ensure
that a valid response has been obtained by carefully checking the energy history and other
response variables.
Basing the Fixed Time Increment Size on the Initial Element-by-Element Stability
Limit
You can use time increments the size of the initial element-by-element stability limit
throughout a step. The dilatational wave speed in each element at the beginning of the
step is used to compute the fixed time increment size.
The use of small increments (dictated by the stability limit) is advantageous because it
allows the solution to proceed without iterations and without requiring tangent stiffness
matrices to be formed. It also simplifies the treatment of contact.
The explicit dynamics procedure is ideally suited for analyzing high-speed dynamic events,
but many of the advantages of the explicit procedure also apply to the analysis of slower
(quasi-static) processes. A good example is sheet metal forming, where contact dominates the
solution and local instabilities might form due to wrinkling of the sheet.
The results in an explicit dynamics analysis are not automatically checked for accuracy as
they are in Abaqus/Standard (Abaqus/Standard uses the half-increment residual). In most cases this is not of concern because the
stability condition imposes a small time increment such that the solution changes only
slightly in any one time increment, which simplifies the incremental calculations. While the
analysis might take an extremely large number of increments, each increment is relatively
inexpensive, often resulting in an economical solution. It is not uncommon for Abaqus/Explicit to take over 105 increments for an analysis. The method is, therefore,
computationally attractive for problems where the total dynamic response time that must be
modeled is only a few orders of magnitude longer than the stability limit; for example, wave
propagation studies or some “event and response” applications.
Computational Cost
The computer time involved in running a simulation using explicit time integration with a
given mesh is proportional to the time period of the event. The time increment based on the
element-by-element stability estimate can be rewritten (ignoring damping) in the form
where the minimum is taken over all elements in the mesh, is a characteristic length associated with an element (see Explicit dynamic analysis), is the density of the material in the element, and and are the effective Lamé's constants for the material in the element
(defined above).
The time increment from the global stability estimate might be somewhat larger, but for
this discussion we will assume that the above inequality always holds (when the inequality
does not hold, the solution time will be somewhat faster).
For linear, nonisotropic elastic materials this stability limit is further scaled down by
the square root of the ratio of the effective material stiffness to the maximum material
stiffness in one particular direction. Since this effectively means that the time increment
can be no larger than the time required to propagate a stress wave across an element, the
computer time involved in running a quasi-static analysis can be very large: the cost of the
simulation is directly proportional to the number of time increments required.
The number of increments, n, required is if remains constant, where T is the time period of the
event being simulated. (Even the element-by-element approximation of will not remain constant in general, since element distortion will change and nonlinear material response will change the effective Lamé constants.
But the assumption is sufficiently accurate for the purposes of this discussion.) Thus,
In a two-dimensional analysis refining the mesh by a factor of two in each direction will
increase the run time in the explicit procedure by a factor of eight—four times as many
elements and half the original time increment size. Similarly, in a three-dimensional
analysis refining the mesh by a factor of two in each direction will increase the run time
by a factor of sixteen.
In a quasi-static analysis it is expedient to reduce the computational cost by either
speeding up the simulation or by scaling the mass. In either case the kinetic energy should
be monitored to ensure that the ratio of kinetic energy to internal energy does not get too
large—typically less than 10%.
Reducing the Computational Cost by Speeding Up the Simulation
To reduce the number of increments required, n, we can speed up the
simulation compared to the time of the actual process—that is, we can artificially reduce
the time period of the event, T. This will introduce two possible
errors. If the simulation speed is increased too much, the increased inertia forces will
change the predicted response (in an extreme case the problem will exhibit wave
propagation response). The only way to avoid this error is to choose a speed-up that is
not too large.
The other error is that some aspects of the problem other than inertia forces—for
example, material behavior—might also be rate dependent. In this case the actual time
period of the event being modeled cannot be changed.
Reducing the Computational Cost by Using Mass Scaling
Artificially increasing the material density, , by a factor reduces n to , just like decreasing T to . This concept, called “mass scaling,” reduces the ratio of the event
time to the time for wave propagation across an element while leaving the event time
fixed, which allows rate-dependent behavior to be included in the analysis. Mass scaling
has exactly the same effect on inertia forces as speeding up the time of simulation.
Mass scaling is attractive because it can be used in rate-dependent problems, but it must
be used with care to ensure that the inertia forces do not dominate and change the
solution. Either fixed or variable mass scaling can be invoked (see Mass Scaling).
Mass scaling can also be accomplished by altering the density; however, the fixed and
variable mass scaling capabilities provide more versatile methods of scaling the mass of
the entire model or specific element sets in the model.
Reducing the Computational Cost by Using Selective Subcycling
One disadvantage in an explicit dynamic analysis is that a few very small elements will
force the entire model to be integrated with a small time increment. You can use mixed
time integration or “subcycling” methods to reduce this problem. In these methods the
equations of motion for the body are still integrated using the explicit
central-difference integration rule as shown above, but the different time increments are
allowed for different groups of nodes in the finite element model. If most nodes are
integrated with a large stable time increment and only a few nodes are integrated with a
small time increment, the computational cost might be reduced significantly.
Selective subcycling can be invoked by defining the subcycling zones. See Selective Subcycling for details.
Bulk Viscosity
Bulk viscosity introduces damping associated with volumetric straining. Its purpose is to
improve the modeling of high-speed dynamic events (see Stability above for a discussion of
the effect of damping on the stable time increment). Abaqus/Explicit contains two forms of bulk viscosity: linear and quadratic. Linear bulk viscosity is
included by default in an Abaqus/Explicit analysis.
The bulk viscosity parameters and defined below can be redefined and can be changed from step to step. If
the default values are changed in a step, the new values will be used in subsequent steps
until they are redefined. Bulk viscosities defined this way apply to the whole model. For an
individual element set the linear and quadratic bulk viscosities can be scaled by a factor
by defining section controls (see Section Controls).
Input File Usage
Use the following option to define bulk viscosity for the entire model:
Use the following option to define bulk viscosity for the entire model:
Step module: Create Step: General: Dynamic, Explicit: Other: Linear bulk viscosity parameter and Quadratic bulk viscosity parameter
Defining bulk viscosity for an individual element set is not supported in Abaqus/CAE.
Linear Bulk Viscosity
Linear bulk viscosity is found in all elements and is introduced to damp “ringing” in the
highest element frequency. This damping is sometimes referred to as truncation frequency
damping. It generates a bulk viscosity pressure that is linear in the volumetric strain
rate
where is a damping coefficient (default=.06), is the current material density, is the current dilatational wave speed, is an element characteristic length, and is the volumetric strain rate.
For acoustic elements, the bulk viscosity pressure can be obtained from the above
equation by using the relationship of the fluid particle velocity and the pressure rate
(see Coupled acoustic-structural medium analysis) as
where and c are the pressure rate and the speed of sound
in the fluid, respectively.
Quadratic Bulk Viscosity
The second form of bulk viscosity pressure is found only in solid continuum elements
(except the plane stress element CPS4R).
This form is quadratic in the volumetric strain rate
where is a damping coefficient (default=1.2) and all other quantities are as
defined for the linear bulk viscosity. Quadratic bulk viscosity is applied only if the
volumetric strain rate is compressive.
The quadratic bulk viscosity pressure will smear a shock front across several elements
and is introduced to prevent elements from collapsing under extremely high velocity
gradients. Consider a simple one-element problem in which the nodes on one side of the
element are fixed and the nodes on the other side have an initial velocity in the
direction of the fixed nodes. If the initial velocity is equal to the dilatational wave
speed of the material, without the quadratic bulk viscosity, the element would collapse to
zero volume in one time increment (because the stable time increment size is precisely the
transit time of a dilatational wave across the element). The quadratic bulk viscosity
pressure will introduce a resisting pressure that will prevent the element from
collapsing.
Fraction of Critical Damping due to Bulk Viscosity
The bulk viscosity pressure is not included in the material point stresses because it is
intended as a numerical effect only—it is not considered part of the material's
constitutive response. The bulk viscosity pressures are based upon the dilatational mode
of each element. The fraction of critical damping in the dilatational mode of each element
is given by
Rotational Bulk Viscosity for Shell Elements
For the displacement degrees of freedom, bulk viscosity introduces damping associated
with volumetric straining. Linear bulk viscosity or truncation frequency damping is used
to damp the high frequency ringing that leads to unwanted noise in the solution or
spurious overshoot in the response amplitude. For the same reason, in shells the high
frequency ringing in the rotational degrees of freedom is damped with linear bulk
viscosity acting on the mean curvature strain rate. This damping generates a bulk
viscosity “pressure moment,” m, which is linear in the mean curvature
strain rate
where is a damping coefficient (default = 0.06), is the original thickness, is the mass density, is the current dilatational wave speed, L is the
characteristic length used for rotary inertia and transverse shear stiffness scaling (see
Finite-strain shell element formulation), and is twice the mean curvature strain rate. The resultant pressure moment , where h is the current thickness, is added to the
direct components of the moment resultant.
Material Damping
Defining inelastic material behavior, dashpots, etc. will introduce energy dissipation into
a model. In addition to these mechanisms, general (“Rayleigh”) material damping can be
introduced (see Material Damping). Adding damping
to a model, especially stiffness proportional damping, , might significantly reduce the stable time increment.
Property module: material editor: MechanicalDamping: Alpha and Beta
Obtaining Diagnostic Information about Critical Elements
Abaqus/Explicit writes critical elements (elements with the smallest stable time increments) and their
stable time increment values to the output database at each summary increment for visualization in Abaqus/CAE. By default, the number of critical elements written to the output database is 10.
The ability to control the number of critical elements written to the output database
is not supported in Abaqus/CAE.
Obtaining Diagnostic Information about the Deformation Speed
The deformation speed in an element is defined as the largest absolute value of all the
deformation rate components of an element times the element characteristic length, . You can request diagnostic information about the deformation speed within
a step definition, as described below. In a multistep analysis diagnostic requests remain in
effect until they are explicitly redefined.
Deformation Speed Warnings
By default, Abaqus/Explicit will check for a relatively large deformation speed in all the elements since too high
a value might cause the element to deform or collapse unrealistically. A warning message
is issued if the ratio of deformation speed versus dilatational wave speed in an element
reaches the value specified for the “warning ratio.” By default, the warning ratio is 0.3.
You can redefine this limit.
The first occurrence of the warning message is written to the status
(.sta) file; subsequent occurrences are written to the message
(.msg) file. See About Output for a
description of these output files.
Generally when the ratio of deformation speed to dilatational wave speed is greater than
0.3, it is an indication that the purely mechanical material constitutive relationship is
no longer valid and that a thermomechanical equation of state material is required.
The ability to redefine the warning ratio limit is not supported in Abaqus/CAE.
Deformation Speed Errors
An error message is issued and the analysis is terminated when the maximum ratio of
deformation speed versus current dilatational wave speed for any element is greater than
the “cutoff ratio.” By default, the cutoff ratio is 1.0. You can redefine this limit.
The ability to redefine the cutoff ratio limit is not supported in Abaqus/CAE.
Obtaining a Summary of the Deformation Speed Information
You can request summary diagnostic information to obtain warning and error messages for
only the element with the largest ratio of deformation speed to dilatational wave speed.
A summary of the deformation speed diagnostic information is output by default in
Abaqus/CAE.
Obtaining Detailed Deformation Speed Information
You can request detailed diagnostic information to obtain warning and error messages for
all elements with large deformation speed to dilatational wave speed ratios.
You cannot disable the deformation speed checks in Abaqus/CAE.
Monitoring Output Variables for Extreme Values
There are some analyses in which it is useful to monitor the value of a variable at every
increment. For example, in a force-driven analysis such as hydro-forming, the simulation
time that is sufficient to model the completion of the physical process might depend on the
magnitude of the displacement of a node or a group of nodes in the model. Another example is
a drop test simulation where the postfailure response is not of interest. Monitoring the
values of critical variables and halting the analysis when those variables exceed a given
criterion can reduce computational expense and turnaround time.
For such problems Abaqus/Explicit allows output variables to be monitored during an analysis to verify whether or not their
values have exceeded or fallen below user-specified values in specified element or node
sets. Comparisons of specified element integration point variables, element section
variables, or nodal variables with user-specified values are performed at every increment.
At the first occurrence of a variable exceeding the user-specified bounds, the variable
name, the associated element or node number, and the increment number are written to the
status (.sta) file. In addition, you can request that the
analysis be stopped and/or the output state be written in the increment following the one in
which the variable has exceeded the user-specified bound. At the end of each step in which
variables are monitored, the maximum, minimum, or absolute maximum value that each variable
attains during the course of the analysis, along with the number of the element or node
where the extreme value occurred, will be written to the status file.
Defining the Element and Nodal Variables to Be Monitored
The element output variables that can be monitored include all the element integration
point variables and element section point variables that are available for history-type
output to the output database. Similarly, the nodal output variables that can be monitored
include all the nodal variables that are available for history output to the output
database. The keys identifying the output variables are defined in Abaqus/Explicit Output Variable Identifiers.
Input File Usage
Use the first option with one or both of the following options in the history
portion of the input file:
Extreme value output monitoring is not supported in Abaqus/CAE.
Halting the Analysis When the Extreme Value Criterion Is Met
You can choose to halt the analysis when the extreme value criterion is met. The analysis
will stop at the end of the increment following the one in which any of the specified
element or nodal variables exceeded the prescribed bounds.
Extreme value output monitoring is not supported in Abaqus/CAE.
Obtaining Output When the Extreme Value Criterion Is Met
You can obtain field-type output to the output database and an additional restart state
when any of the selected variables fall outside the specified bounds for the first time
during the analysis. The output will be written in the increment following the one in
which such an occurrence took place. Since output is automatically written when the
analysis terminates, this request has an effect only if you have not chosen to halt the
analysis when the extreme value criterion is met as described above.
Input File Usage
Use either or both of the following options in conjunction with the EXTREME VALUE option:
Extreme value output monitoring is not supported in Abaqus/CAE.
Monitoring Variables in a Multistep Analysis
In a multistep analysis the monitoring requests you specify remain in effect until they
are redefined. You must redefine all requests to add or change any variables, element or
node sets, or maxima or minima.
Stopping the Monitoring of Variables in a New Step
Extreme value output monitoring is not supported in Abaqus/CAE.
Controlling Material Rate Dependence
You can control whether to consider or ignore material rate dependence within the step in
an explicit dynamic response. A step that ignores material rate dependence should not follow
a step or analysis that considers material rate dependence.
The fully relaxed long-term elastic response is used for viscoelastic materials when the
step ignores material rate dependence. The rate dependence of the material response defined
via user subroutines VUCREEPNETWORK, VUHARD, and VUMAT can be ignored when the step
ignores material rate dependence.
Input File Usage
Use the following option to consider material rate dependence within the step
(default):
Abaqus/CAE always considers material rate dependence.
Initial Conditions
Initial Conditions describes all of
the initial conditions that are available for an explicit dynamic analysis.
Boundary Conditions
Boundary conditions can be defined as explained in Boundary Conditions. Boundary
conditions applied during an explicit dynamic response step should use appropriate amplitude
references (Amplitude Curves). If boundary
conditions are specified for the step without amplitude references, they are applied
instantaneously at the beginning of the step. Since Abaqus/Explicit does not admit jumps in displacement, the value of a nonzero displacement boundary
condition that is specified without an amplitude reference will be ignored, and a zero
velocity boundary condition will be enforced.
Loads
The loading types available for an explicit dynamic analysis are explained in About Loads. Concentrated
nodal forces or moments can be applied to the displacement or rotation degrees of freedom
(1–6). Distributed pressure forces or body forces can also be applied; the distributed load
types available with particular elements are described in Abaqus Elements Guide.
As with boundary conditions, loads applied during a dynamic response step should use
appropriate amplitude references (Amplitude Curves). If loads are
specified for the step without amplitude references, they are applied instantaneously at the
beginning of the step.
Predefined Fields
The following predefined fields can be specified, as described in Predefined Fields:
Although temperature is not a degree of freedom in explicit dynamic analysis, you can
specify nodal temperatures. Any difference between the applied and initial temperatures
causes thermal strain if a thermal expansion coefficient is given for the material
(Thermal Expansion). The
specified temperature also affects temperature-dependent material properties, if any.
The values of user-defined field variables can be specified. These values affect only
field-variable-dependent material properties, if any.
Although pore fluid pressure is not a degree of freedom in an explicit dynamic
analysis, you can specify nodal pore fluid pressure as a predefined field variable (see
Pore Fluid Pressure). The total
stress is computed as the sum of the effective stress and the pore fluid pressure. It is
assumed that the solid grains are incompressible (the effective strain is equal to the
total strain).
Material Options
Any of the material models in Abaqus/Explicit can be used in a general explicit dynamic analysis (see Combining Material Behaviors).
Elements
All of the elements available in Abaqus/Explicit can be used in an explicit dynamic analysis. The elements are listed in Abaqus Elements Guide.
If coupled temperature-displacement elements are used in an explicit dynamic analysis, the
temperature degrees of freedom will be ignored.
Output
The element output available for a dynamic analysis includes stress; strain; energies; and
the values of state, field, and user-defined variables. The nodal output available includes
displacements, velocities, accelerations, reaction forces, and coordinates. All the output
variable identifiers are outlined in Abaqus/Explicit Output Variable Identifiers. The types of
output available are described in About Output.
When an Abaqus/Explicit analysis encounters a fatal error, the preselected variables applicable to the current
procedure are added automatically to the output database as field data for the last
increment.
Energy output is particularly important in checking the accuracy of the solution in an
explicit dynamic analysis. In general, the total energy
(ETOTAL) should be a constant or close to
a constant; the “artificial” energies, such as the artificial strain energy
(ALLAE), the damping dissipation
(ALLVD), and the mass scaling work
(ALLMW) should be negligible compared to
“real” energies such as the recoverable strain energy
(ALLSE) and the kinetic energy
(ALLKE).
In a quasi-static analysis the value of the kinetic energy
(ALLKE) should not exceed a small fraction
of the value of the total strain energy
(ALLIE).
It is a good practice to output the constraint penalty work
(ALLCW) and the contact penalty work
(ALLPW) in analyses involving constraints
(such as ties and fasteners) and contact. The value of these energies should be close to
zero.
Input File Template
HEADING
…
MATERIAL, NAME=nameELASTIC
…
DENSITYData lines to define densityDAMPING, ALPHA=, BETA=
Data lines to define Rayleigh damping
…
BOUNDARYData lines to specify zero-valued boundary conditionsINITIAL CONDITIONS, TYPE=typeData lines to specify initial conditionsAMPLITUDE, NAME=nameData lines to define amplitude variations
*************************
STEPDYNAMIC, EXPLICITData line to specify the time period of the stepDIAGNOSTICS, DEFORMATION SPEED CHECK=SUMMARYBOUNDARY, AMPLITUDE=nameData lines to describe zero-valued or nonzero boundary conditionsCLOAD and/or DLOADData lines to specify loadingTEMPERATURE and/or FIELDData lines to specify predefined fieldsFILE OUTPUT, NUMBER INTERVAL=nEL FILEData line specifying element output variablesNODE FILEData line specifying node output variablesENERGY FILEOUTPUT, FIELD, NUMBER INTERVAL=nELEMENT OUTPUTData line specifying element output variablesNODE OUTPUTData line specifying node output variablesOUTPUT, HISTORY, TIME INTERVAL=tELEMENT OUTPUT, ELSET=element set nameData line specifying element output variablesNODE OUTPUT, NSET=node set nameData line specifying node output variablesENERGY OUTPUTData line specifying energy output variablesEND STEP
*************************
STEPDYNAMIC, EXPLICIT, ELEMENT BY ELEMENT
…
BULK VISCOSITYData line to define linear and/or quadratic bulk viscosity in this step
…
END STEP