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 $$ \Delta t \leq \min \left(L _ {e} \sqrt {\frac {\rho}{\hat {\lambda} + 2 \hat {\mu}}}\right), $$ where the minimum is taken over all elements in the mesh, $L _ { e }$ is a characteristic length associated with an element (see “Explicit dynamic analysis,” Section 2.4.5 of the Abaqus Theory Guide), $\rho$ is the density of the material in the element, and $\hat { \lambda }$ and $\hat { \mu }$ are the effective Lamé’s constants for the material in the element (defined above). The time increment from the global stability estimate may 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 $n ~ = ~ T / \Delta t { \mathrm { ~ i f ~ } } \Delta t$ remains constant, where $\pmb { T }$ is the time period of the event being simulated. (Even the element-by-element approximation of $\Delta t$ will not remain constant in general, since element distortion will change $L _ { e }$ and nonlinear material response will change the effective Lamé constants. But the assumption is sufficiently accurate for the purposes of this discussion.) Thus, $$ n \approx T \max \left(\frac {1}{L _ {e}} \sqrt {\frac {\hat {\lambda} + 2 \hat {\mu}}{\rho}}\right). $$ 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—may 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 $f ^ { 2 }$ reduces n to $n / f ,$ , just like decreasing $\mathbf { \nabla } T$ to $T / f .$ 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,” Section 11.6.1). 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 may be reduced significantly. Selective subcycling can be invoked by defining the subcycling zones. See “Selective subcycling,” Section 11.7.1 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 $b _ { 1 }$ and $b _ { 2 }$ 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,” Section 27.1.4).

Input File Usage:

Use the following option to define bulk viscosity for the entire model:*BULK VISCOSITYUse the following options to define bulk viscosity for an individual element set:*BULK VISCOSITY*SECTION CONTROLS

Abaqus/CAE Usage:

Use the following option to define bulk viscosity for the entire model:Step module:Create Step:General:Dynamic,Explicit:Other:Linear bulk viscosity parameterandQuadratic bulk viscosity parameterDefining 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 $$ p _ {b v 1} = b _ {1} \rho c _ {d} L _ {e} \dot {\epsilon} _ {v o l}, $$ where $b _ { 1 }$ is a damping coefficient (default=.06), $\rho$ is the current material density, $c _ { d }$ is the current dilatational wave speed, $L _ { e }$ is an element characteristic length, and $\dot { \epsilon } _ { v o l }$ 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,” Section 2.9.1 of the Abaqus Theory Guide) as $$ p _ {b v 1} = - \frac {b _ {1} L _ {e}}{c} \dot {p}, $$ where $\dot { p }$ 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 $$ p _ {b v 2} = \rho (b _ {2} L _ {e} \dot {\epsilon} _ {v o l}) ^ {2}, $$ where $b _ { 2 }$ 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 $$ \xi = b _ {1} - b _ {2} ^ {2} \frac {L _ {e}}{c _ {d}} \mathrm{min} (0, \dot {\epsilon} _ {v o l}). $$ # 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 $$ m = b _ {1} \frac {h _ {0} ^ {2}}{1 2} \rho c _ {d} L \dot {\kappa}, $$ where $b _ { 1 }$ is a damping coefficient (default = 0.06), $h _ { 0 }$ is the original thickness, $\rho$ is the mass density, $c _ { d }$ 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,” Section 3.6.5 of the Abaqus Theory Guide), and $\dot { \kappa } = \dot { \kappa } _ { 1 1 } + \dot { \kappa } _ { 2 2 }$ is twice the mean curvature strain rate. The resultant pressure moment $m h _ { ; }$ , 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,” Section 26.1.1). Adding damping to a model, especially stiffness proportional damping, $\beta _ { R }$ , may significantly reduce the stable time increment. $\mathrm { l n p u t \ F i l e \ U s a g e : } \qquad \ast \mathrm { D A M P I N G } , \mathrm { A L P H A } = \alpha _ { R } , \mathrm { B E T A } = \beta _ { R }$ Abaqus/CAE Usage: Property module: material editor: Mechanical→Damping: 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. Input File Usage: \*DIAGNOSTICS, CRITICAL ELEMENTS=value Abaqus/CAE Usage: 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, $L _ { e }$ . 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 may 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 “Output,” Section 4.1.1, 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. Input File Usage: \*DIAGNOSTICS, WARNING RATIO=ratio Abaqus/CAE Usage: 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 check for this cutoff ratio is not applied to any model that has an equation of state material (see “Equation of state,” Section 25.2.1) or a user-defined material (see “User-defined mechanical material behavior,” Section 26.7.1). Input File Usage: \*DIAGNOSTICS, CUTOFF RATIO=ratio Abaqus/CAE Usage: 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. Input File Usage: \*DIAGNOSTICS, DEFORMATION SPEED CHECK=SUMMARY Abaqus/CAE Usage: 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. Input File Usage: \*DIAGNOSTICS, DEFORMATION SPEED CHECK=DETAIL Abaqus/CAE Usage: You cannot output detailed diagnostic information about the deformation speed in Abaqus/CAE. # Disabling deformation speed checks You can choose to completely bypass the checks for large deformation speed. Input File Usage: \*DIAGNOSTICS, DEFORMATION SPEED CHECK=OFF Abaqus/CAE Usage: 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 may 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,” Section 4.2.2.

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*EXTREME ELEMENT VALUE, ELSET=element_set_name*EXTREME NODE VALUE, NSET=nset_set_nameThe *EXTREME VALUE option can be repeated in the same step, and the*EXTREME ELEMENT VALUE and *EXTREME NODE VALUE options can be repeated as many times as necessary.

Abaqus/CAE Usage: 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.

Input File Usage:

Use the following options:*EXTREME VALUE, HALT=YES*EXTREME ELEMENT VALUE and/or *EXTREME NODE VALUE

Abaqus/CAE Usage: 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 ELEMENT VALUE, ELSET=element_set_name, OUTPUT=YES

*EXTREME NODE VALUE, NSET=node_set_name, OUTPUT=YES

Abaqus/CAE Usage: 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 You can stop monitoring variables in a new step. Input File Usage: Use the \*EXTREME VALUE option without the \*EXTREME ELEMENT VALUE and \*EXTREME NODE VALUE options. Abaqus/CAE Usage: Extreme value output monitoring is not supported in Abaqus/CAE. # Initial conditions “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1, 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 in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1. Boundary conditions applied during an explicit dynamic response step should use appropriate amplitude references (“Amplitude curves,” Section 34.1.2). 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 “Applying loads: overview,” Section 34.4.1. 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 Part VI, “Elements.” As with boundary conditions, loads applied during a dynamic response step should use appropriate amplitude references (“Amplitude curves,” Section 34.1.2). 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,” Section 34.6.1: • Although temperature is not a degree of freedom in explicit dynamic analysis, nodal temperatures can be specified. Any difference between the applied and initial temperatures will cause thermal strain if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2). 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-variabledependent material properties, if any. # Material options Any of the material models in Abaqus/Explicit can be used in a general explicit dynamic analysis (see “Combining material behaviors,” Section 21.1.3). # Elements All of the elements available in Abaqus/Explicit can be used in an explicit dynamic analysis. The elements are listed in Part VI, “Elements.” 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 of the output variable identifiers are outlined in “Abaqus/Explicit output variable identifiers,” Section 4.2.2. The types of output available are described in “Output,” Section 4.1.1. 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 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 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 ```txt *HEADING ... *MATERIAL, NAME=name *ELASTIC ... ``` \*DENSITY Data lines to define density \*DAMPING, ALPHA = , BETA= Data lines to define Rayleigh damping \*BOUNDARY Data lines to specify zero-valued boundary conditions \*INITIAL CONDITIONS, TYPE=type Data lines to specify initial conditions \*AMPLITUDE, NAME=name Data lines to define amplitude variations \*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\* \*STEP \*DYNAMIC, EXPLICIT Data line to specify the time period of the step \*DIAGNOSTICS, DEFORMATION SPEED CHECK=SUMMARY \*BOUNDARY, AMPLITUDE=name Data lines to describe zero-valued or nonzero boundary conditions \*CLOAD and/or \*DLOAD Data lines to specify loading \*TEMPERATURE and/or \*FIELD Data lines to specify predefined fields \*FILE OUTPUT, NUMBER INTERVAL=n \*EL FILE Data line specifying element output variables \*NODE FILE Data line specifying node output variables \*ENERGY FILE \*OUTPUT, FIELD, NUMBER INTERVAL=n \*ELEMENT OUTPUT Data line specifying element output variables \*NODE OUTPUT Data line specifying node output variables \*OUTPUT, HISTORY, TIME INTERVAL=t \*ELEMENT OUTPUT, ELSET=element set name Data line specifying element output variables \*NODE OUTPUT, NSET=node set name Data line specifying node output variables \*ENERGY OUTPUT Data line specifying energy output variables \*END STEP \*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*\*