Implicit Dynamic Analysis Using Direct Integration

General Dynamic Analysis

General nonlinear dynamic analysis in Abaqus/Standard uses implicit time integration to calculate the transient dynamic or quasi-static response of a system. The procedure can be applied to a broad range of applications calling for varying numerical solution strategies, such as the amount of numerical damping required to obtain convergence and the way in which the automatic time incrementation algorithm proceeds through the solution. Typical dynamic applications fall into three categories:

Transient fidelity applications, such as an analysis of satellite systems, require minimal energy dissipation. In these applications small time increments are taken to accurately resolve the vibrational response of the structure, and numerical energy dissipation is kept at a minimum. These stringent requirements tend to degrade convergence behavior for simulations involving contact or nonlinearities.
Moderate dissipation applications encompass a more general range of dynamic events in which a moderate amount of energy is dissipated by plasticity, viscous damping, or other effects. Typical applications include various insertion, impact, and forming analyses. The response of these structures can be either monotonic or nonmonotonic. Accurate resolution of high-frequency vibrations is usually not of interest in these applications. Some numerical energy dissipation tends to reduce solution noise and improve convergence behavior in these applications without significantly degrading solution accuracy.
Quasi-static applications are primarily interested in determining a final static response. These problems typically show monotonic behavior, and inertia effects are introduced primarily to regularize unstable behavior. For example, the statically unstable behavior may be due to temporarily unconstrained rigid body modes or “snap-through” phenomena. Large time increments are taken when possible to obtain the final solution at minimal computational cost. Considerable numerical dissipation may be required to obtain convergence during certain stages of the loading history.

An example of a transient fidelity application is available in Modeling of an automobile suspension. An analysis that includes both a moderate dissipation step and a quasi-static step is described in Impact analysis of a pawl-ratchet device.

Specifying the Application Type

Based on the classifications listed above, you should indicate the type of application you are studying when performing a general dynamic analysis. Abaqus/Standard assigns numerical settings based on your classification of the application type, and this classification can significantly affect a simulation. In some cases accurate results can be obtained with more than one application-type setting, in which case analysis efficiency should be considered. A general trend is that—among the three classifications—the high-dissipation quasi-static classification tends to result in the best convergence behavior and the low-dissipation transient fidelity classification tends to have the highest likelihood of convergence difficulty.

Input File Usage

Use the following option for transient fidelity applications:

DYNAMIC, APPLICATION=TRANSIENT FIDELITY (default for models without contact)

Use the following option for moderate dissipation applications:

DYNAMIC, APPLICATION=MODERATE DISSIPATION (default for models with contact)

Use the following option for quasi-static applications:

DYNAMIC, APPLICATION=QUASI-STATIC

Abaqus/CAE Usage

Step module: Create Step: General: Dynamic, Implicit

The application type is specified in the Edit Step dialog box:

Basic: Application: Transient fidelity, Moderate dissipation, Quasi-static, or Analysis product default

Diagnostics for Modeling Errors Associated with Mass Properties

Accurate representation of inertia properties is necessary for accurate dynamic analyses. In some cases Abaqus/Standard provides diagnostic messages when it detects likely modeling errors associated with the specification of inertia properties. The most common way of specifying inertia properties is with material densities. Abaqus/Standard issues a warning message to the data (.dat) file if a material density is omitted in a dynamic analysis (this warning is not issued if the density is zero only for certain values of temperature or field variables). Other methods of specifying inertia properties include:

point mass and rotary inertia definitions, and
constraining nodes without inertia themselves to nodes having inertia properties defined.

In some circumstances Abaqus/Standard attempts to solve systems of equations involving effective inversion of the global mass matrix to directly adjust velocities and accelerations during a general dynamic analysis as described in Initial Conditions and Intermittent Contact/Impact below. These additional velocity and acceleration adjustments occur by default only for transient fidelity application types as defined above. If the global mass matrix is found to be singular, Abaqus/Standard issues an error message by default, because singular mass is an indication that the mass properties are not realistic due to a modeling error.

Diagnostic feedback specific to the global mass matrix being singular is typically not provided for quasi-static and moderate dissipation application types, although warnings typically are issued regarding the lack of material density. Singular mass is not necessarily detrimental to a quasi-static analysis. For example, it would be reasonable to only define inertia properties (such as density) in components or regions with temporary static instabilities (such as initially unconstrained rigid body modes that become constrained once contact occurs) in a quasi-static analysis.

You can control the course of action Abaqus/Standard takes on detecting a singular global mass matrix.

Input File Usage

Use the following default option to issue an error message and stop execution if a singular global mass matrix is detected when calculating velocity and acceleration adjustments:

DYNAMIC, SINGULAR MASS=ERROR

Use the following option to issue a warning message and avoid velocity and acceleration adjustments (that is., continue time integration using current velocities and accelerations) if a singular global mass matrix is detected:

DYNAMIC, SINGULAR MASS=WARNING

Use the following option to adjust velocities and accelerations even if a singular mass matrix is detected. This setting can result in large, non-physical velocity and/or acceleration adjustments, which can, in turn, cause poor time integration solutions and artificial convergence difficulties. This approach is not generally recommended; it should be used only in special cases when the analyst has a thorough understanding of how to interpret results obtained in this way.

DYNAMIC, SINGULAR MASS=MAKE ADJUSTMENTS

Abaqus/CAE Usage

The default singular mass setting cannot be modified in Abaqus/CAE.

Numerical Details

The effect of the application-type classification on numerical aspects of general dynamic analyses is described below. In most cases the settings determined by the application type are sufficient to successfully perform an analysis. However, detailed user controls are provided to override settings on an individual basis.

Time Integration Methods

Abaqus/Standard uses the Hilber-Hughes-Taylor time integration by default unless you specify that the application type is quasi-static. The Hilber-Hughes-Taylor operator is an extension of the Newmark $β$ -method. Numerical parameters associated with the Hilber-Hughes-Taylor operator are tuned differently for moderate dissipation and transient fidelity applications (as discussed later in this section). The backward Euler operator is used by default if the application classification is quasi-static.

These time integration operators are implicit, which means that the operator matrix must be inverted and a set of simultaneous nonlinear dynamic equilibrium equations must be solved at each time increment. This solution is done iteratively using Newton's method. The principal advantage of these operators is that they are unconditionally stable for linear systems; there is no mathematical limit on the size of the time increment that can be used to integrate a linear system. An unconditionally stable integration operator is of great value when studying structural systems because a conditionally stable integration operator (such as that used in the explicit method) can lead to impractically small time steps and, therefore, a computationally expensive analysis.

Marching through a simulation with a finite time increment size generally introduces some degree of numerical damping. This damping differs from the material damping discussed in Material Damping (and in many cases these two forms of damping work well together). The amount of damping associated with the time integration varies among the operator types (for example, the backward Euler operator tends to be more dissipative than the Hilber-Hughes-Taylor operator) and in many cases (such as with the Hilber-Hughes-Taylor operator) depends on settings of numerical parameters associated with the operator. The ability of the operator to effectively treat contact conditions is often of considerable importance with respect to their usefulness. For example, some changes in contact conditions can result in “negative damping” (nonphysical energy source) for many time integrators, which can be very undesirable.

It is possible to override the time integrator implied by the application-type classification; for example, you can perform a moderate dissipation dynamic analysis using the backward Euler integrator. Changing the default integrator is not generally recommended but may be useful in special cases.

Input File Usage

Use the following option to use the Hilber-Hughes-Taylor integrator with default integrator parameter settings corresponding to those for transient fidelity applications:

DYNAMIC, TIME INTEGRATOR=HHT-TF

Use the following option to use the Hilber-Hughes-Taylor integrator with default integrator parameter settings corresponding to those for moderate dissipation applications:

DYNAMIC, TIME INTEGRATOR=HHT-MD

Use the following option to use the backward Euler integrator:

DYNAMIC, TIME INTEGRATOR=BWE

Abaqus/CAE Usage

The default time integrator cannot be modified in Abaqus/CAE.

Additional Control over Integrator Parameters

Additional user controls enable modifications to settings of numerical parameters associated with the Hilber-Hughes-Taylor operator (see Hilber, Hughes, and Taylor (1977) for descriptions of the numerical parameters). The default parameter settings depend on the specified application type, as indicated in Table 1 (see Czekanski, El-Abbasi, and Meguid (2001) for the basis of these settings).

Table 1. Default parameters for the Hilber-Hughes-Taylor integrator.
Parameter	Application
Parameter	Transient Fidelity	Moderate Dissipation
$α$	–0.05	–0.41421
$β$	0.275625	0.5
$γ$	0.55	0.91421

These parameters can be adjusted or modified individually if the Hilber-Hughes-Taylor operator is being used. If the default settings of these parameters correspond to the transient fidelity settings shown in Table 1 and you explicitly modify the $α$ parameter alone, the other parameters are adjusted automatically to $β = 1 / 4 \cdot {(1 - α)}^{2}$ and $γ = 1 / 2 - α$ . This relation provides control of the numerical damping associated with the time integrator while preserving desirable characteristics of the integrator. The numerical damping grows with the ratio of the time increment to the period of vibration of a mode. Negative values of $α$ provide damping; whereas $α = 0$ results in no damping (energy preserving) and is exactly the trapezoidal rule (sometimes called the Newmark $β$ -method, with $β = 1 / 4$ and $γ = 1 / 2$ ). The setting $α = - 1 / 3$ provides the maximum numerical damping. It gives a damping ratio of about 6% when the time increment is 40% of the period of oscillation of the mode being studied. Allowable values of $α$ , $β$ , and $γ$ are: $- \frac{1}{2} \leq α \leq 0$ , $β > 0$ , $γ \geq \frac{1}{2}$ .

Input File Usage

DYNAMIC, ALPHA= $α$ , BETA= $β$ , GAMMA= $γ$

Abaqus/CAE Usage

Only the $α$ parameter can be modified in Abaqus/CAE:

Step module: Create Step: General: Dynamic, Implicit: Other: Alpha: Specify:  $α$

Default Incrementation Schemes

Automatic time incrementation is used by default for nonlinear dynamic procedures. The main factors used to control adjustments to the time increment size for an implicit dynamic procedure are the convergence behavior of the Newton iterations and the accuracy of the time integration. The time increment size may vary considerably during an analysis. Details of the time increment control algorithm depend on the type of dynamic application you are studying.

The following factors are considered by default in the time increment control algorithm if you specify a quasi-static–type application (the same factors control the time increment size for purely static analyses):

The time increment size is reduced if an increment appears to be diverging or if the convergence rate is slow.
The time increment size is fairly aggressively increased if rapid convergence occurs in previous increments.

Analyses for moderate dissipation-type applications also use these same factors, as well as a default upper bound on the time increment size equal to one-tenth of the step duration.

The following factors are considered by default in the time increment control algorithm if you specify a transient fidelity–type application:

The time increment size is reduced if an increment appears to be diverging or if the convergence rate is slow.
The time increment size is reduced if changes in contact status are detected during the first attempt of processing an increment. The new increment size is set such that the end of the increment corresponds to the average time of the contact status changes that were detected with the previous increment size. (In such cases an additional very small time increment is used to enforce compatibility of velocities and accelerations across active contact interfaces.)
The time increment size is reduced if the half-increment residual (out-of-balance force) halfway through a time increment exceeds the half-increment residual tolerance, which is 10,000 times the time average force for a contact analysis or 1000 times the time average force for an analysis without contact.
The time increment is gradually increased if rapid convergence occurs in previous increments.
The upper bound for the time increment size is equal to 1/100 of the step duration.

Intermittent Contact/Impact

The second and third factors described in the preceding list often result in very small time increment sizes for contact simulations that are performed as a transient fidelity application (and the time increment size tends to remain small due to the fourth factor). This problem can be avoided by specifying a different application type or by using more detailed user controls, as discussed below.

General Settings for the Time Increment Controls

A high-level user control over which factors are considered by the time increment control algorithm can be used to override the defaults implied by the specified application type for the analysis. Regardless of the application type you have specified, you can enforce time increment controls associated with either quasi-static applications or transient fidelity applications.

Input File Usage

Use the following option to obtain the aggressive time increment control settings associated with quasi-static applications:

DYNAMIC, INCREMENTATION=AGGRESSIVE

Use the following option to obtain the more conservative time increment control settings associated with transient fidelity applications:

DYNAMIC, INCREMENTATION=CONSERVATIVE

Abaqus/CAE Usage

The default time incrementation control settings cannot be modified in Abaqus/CAE.

Controlling the Half-Increment Residual

Controls associated with the half-increment residual tolerance are provided for tuning the time incrementation. These controls are intended for advanced users and typically do not need to be modified.

Input File Usage

Use the following option to specify that no check of the half-increment residual should be performed:

DYNAMIC, NOHAF

Use the following option to specify the half-increment residual tolerance as a scale factor of the time average force (moment):

DYNAMIC, HALFINC SCALE FACTOR=scale factor

Use the following option to directly specify the half-increment residual force tolerance (the half-increment residual moment tolerance is the half-increment residual force tolerance times the characteristic element length automatically calculated):

DYNAMIC, HAFTOL=tolerance

Abaqus/CAE Usage

Use the following option to specify that no check of the half-increment residual should be performed:

Step module: Create Step: General: Dynamic, Implicit: Incrementation: toggle on Suppress half-increment residual calculation

Use the following option to specify the half-increment residual tolerance as a scale factor of the time average force (moment):

Step module: Create Step: General: Dynamic, Implicit: Incrementation: Half-increment Residual: Specify scale factor: scale factor

Use the following option to specify the half-increment residual force tolerance directly:

Step module: Create Step: General: Dynamic, Implicit: Incrementation: Half-increment Residual: Specify value: tolerance

Controlling Incrementation Involving Contact

By default, specifying a transient fidelity application typically results in reduced time increment sizes on changes in contact status. An extra time increment with a very small size is subsequently performed to enforce compatibility of velocities and accelerations across active contact interfaces. Direct user control over these incrementation aspects is available.

Input File Usage

Use the following option to avoid automatically cutting back the increment size and enforcing velocity and acceleration compatibility in the contact region on changes in contact status:

DYNAMIC, IMPACT=NO

Use the following option to automatically cut back the increment size and enforce velocity and acceleration compatibility in the contact region on changes in contact status:

DYNAMIC, IMPACT=AVERAGE TIME

Use the following option to enforce velocity and acceleration compatibility in the contact region without automatically cutting back the increment size on changes in contact status:

DYNAMIC, IMPACT=CURRENT TIME

Abaqus/CAE Usage

The default contact incrementation scheme cannot be modified in Abaqus/CAE.

Direct Time Incrementation

You may directly specify the time increment size to be used. This approach is not generally recommended but may be useful in special cases. The analysis ends if convergence tolerances are not satisfied within the maximum number of iterations allowed.

It is possible to ignore convergence tolerances: the solution to an increment is accepted after the specified maximum number of iterations allowed even if convergence tolerances are not satisfied. Ignoring convergence tolerances can result in highly nonphysical results and is not recommended except by analysts with a thorough understanding of how to interpret results obtained this way.

Input File Usage

Use the following option to directly specify the time increment:

DYNAMIC, DIRECT

Use the following option to ignore convergence tolerances after the maximum number of iterations is reached:

DYNAMIC, DIRECT=NO STOP

Abaqus/CAE Usage

Use the following option to specify the time increment directly:

Step module: Create Step: General: Dynamic, Implicit: Incrementation: Fixed

Use the following option to ignore convergence tolerances after the maximum number of iterations is reached:

Step module: Create Step: General: Dynamic, Implicit: Other: Accept solution after reaching maximum number of iterations

Default Amplitude for Loads

Loads such as applied forces or pressures are ramped on by default if you have selected the quasi-static application classification; such ramping tends to enhance robustness because the load increment size is proportional to the time increment size. For example, if the Newton iterations are unable to converge for a particular time increment size, the automatic time incrementation algorithm reduces the time increment size and restart the Newton iterations with a smaller load increment considered.

For the other application classifications the dynamic procedure applies loads with a step function by default such that the full load is applied in the first increment of the step (regardless of the time increment size) and the load magnitude remains constant over each step. Thus, if the first increment is unable to converge with the original time increment size, reducing the time increment does not reduce the load increment by default. In some cases the convergence behavior still improves on reducing the time increment because the regularizing effect of inertia on the integration operators is inversely proportional to the square of the time increment size. See Defining an Analysis for more information on default amplitude types for the various procedures and how to override the default.

The “Subspace Projection” Method

The alternative approach provided in Abaqus/Standard for nonlinear dynamic problems is the “subspace projection” method. See Subspace dynamics for the theory behind this method. In this method the modes of the linear system are extracted in an eigenfrequency extraction step (Natural Frequency Extraction) prior to the dynamic analysis and are used as a small set of global basis vectors to develop the solution. These modes include eigenmodes and, if activated in the eigenfrequency extraction step, residual modes. The method works well when the system exhibits mildly nonlinear behavior, such as small regions of plastic yielding or rotations that are not small but not too large.

This method can be very effective. As with the other direct integration methods, it is more expensive in terms of computer time than the modal methods of purely linear dynamic analysis, but it is often significantly less expensive than the direct integration of all of the equations of motion of the model. However, since the subspace projection method is based on the modes of the system, it is not accurate if there is extreme nonlinear response that cannot be modeled well by the modes that form the basis of the solution.

Input File Usage

DYNAMIC, SUBSPACE

Abaqus/CAE Usage

Step module: Create Step: General: Dynamic, Subspace

Selecting the Modes on Which to Project

You can select the modes of the system on which the subspace projection is performed. The mode numbers can be listed individually, or they can be generated automatically. If you choose not to select the modes, all modes extracted in the prior frequency extraction step, including residual modes if they were activated, are used in the subspace projection.

Input File Usage

Use one of the following options:

SELECT EIGENMODES
SELECT EIGENMODES, GENERATE

Abaqus/CAE Usage

Step module: Create Step: General: Dynamic, Subspace: Basic: Number of modes to use: All or Specify

Numerical Implementation

The subspace projection method is implemented in Abaqus/Standard using the explicit (central difference) operator to integrate the equations of motion written in terms of the modes of the linear system. This integration method is particularly effective here because the modes are orthogonal with respect to the mass matrix so that the projected system always has a diagonal mass matrix.

A fixed time increment is used: this increment is the smaller of the time increment that you specify or 80% of the stable time increment, which is $2 / ω_{\max}$ for the linear system, where $ω_{\max}$ is the highest circular frequency of the modes that are used as the basis of the solution. The 80% factor is intended as a safety factor so that any increase in this highest frequency caused by nonlinear effects is less likely to cause the integration to become unstable. The 80% is rather arbitrary; in some cases it may be nonconservative. You must monitor the response—for example, the energy balance—to ensure that the time increment is not causing instability. Instability is a concern if the nonlinearities can stiffen the system significantly, although in many practical cases such stiffening effects are more prominent in increasing the lower frequencies of the system than in affecting the highest frequencies that are likely to be retained to represent the dynamic behavior accurately.

Accuracy of the Subspace Projection Method

The effectiveness of the subspace projection method depends on the value of the modes of the linear system as a set of global interpolation functions for the problem, which is a matter of judgment on your part—the same sort of judgment as required when deciding if a particular mesh of finite elements is sufficient. The method is valuable for mildly nonlinear systems and for cases where it is easy to extract enough modes that you can be confident that they describe the system adequately.

If nonlinear geometric effects are considered in the subspace dynamics step, it is possible to perform a dynamic simulation for some time, reextract the modes on the current stressed geometry by using another frequency extraction step, and then continue the analysis with the new modes as the subspace basis system. This procedure can improve the accuracy of the method in some cases.

Material Damping

You can introduce Rayleigh damping, as explained in Material Damping. This damping acts in addition to numerical damping associated with the time integrator (discussed previously).

Input File Usage

DAMPING, ALPHA= $α_{R}$ , BETA= $β_{R}$

Abaqus/CAE Usage

Property module: material editor: MechanicalDamping: Alpha and Beta

Initial Conditions

Initial Conditions describes all of the available initial conditions. Initial velocities must be defined in global directions regardless of the use of nodal transformations (see Transformed Coordinate Systems).

If initial velocities are specified at nodes for which displacement boundary conditions are also specified, the initial velocities are ignored at these nodes. However, if a displacement boundary condition refers to an amplitude curve with an analytically defined time variation (that is, excluding the piecewise linear tabular and equally spaced definitions), Abaqus/Standard computes the initial velocity for the nodes involved in the boundary condition as the time derivative (evaluated at time zero) of the analytic variation.

When initial velocities are specified for dynamic analysis, they should be consistent with all of the constraints on the model, especially time-dependent boundary conditions. Abaqus/Standard ensures that initial velocities are consistent with boundary conditions and with multi-point and equation constraints but does not check for consistency with internal constraints such as incompressibility of the material. In case of a conflict, boundary conditions and multi-point constraints take precedence over initial conditions.

Specified initial velocities are used in a dynamic step only if it is the first dynamic step in an analysis. If a dynamic step is not the first dynamic step and there is an immediately preceding dynamic step, the velocities from the end of the preceding step are used as the initial velocities for the current step. If a dynamic step is not the first dynamic step and the immediately preceding step is not a dynamic step, zero initial velocities are assumed for the current step.

Controlling Calculation of Accelerations at the Beginning of a Dynamic Step

By default, Abaqus/Standard calculates accelerations at the beginning of the dynamic step for transient fidelity applications. You can choose to bypass these acceleration calculations, in which case Abaqus/Standard assumes that initial accelerations for the current step are zero unless there is an immediately preceding dynamic step. If the immediately preceding step is also a dynamic step, bypassing the acceleration calculations causes Abaqus/Standard to use the accelerations from the end of the previous step to continue the new step. It is appropriate to bypass the acceleration calculations if the loading has not changed suddenly at the start of the dynamic step, but it is not correct if the loading at the beginning of the first increment is significantly different from that at the end of the previous step. In cases where large loads are applied suddenly, high-frequency noise due to the bypass of the acceleration calculations may greatly increase the half-increment residual.

Input File Usage

DYNAMIC, INITIAL=NO

Abaqus/CAE Usage

Step module: Create Step: General: Dynamic, Implicit: Other: Initial acceleration calculations at beginning of step: Bypass

Boundary Conditions

Boundary conditions can be applied to any of the displacement or rotation degrees of freedom (1–6), to warping degree of freedom 7 in open-section beam elements, to fluid pressure degree of freedom 8 for hydrostatic fluid elements, or to acoustic pressure degree of freedom 8 for acoustic elements (Boundary Conditions).

Amplitude references can be used to prescribe time-varying boundary conditions in a direct-integration dynamic step. Default amplitude variations are described in Defining an Analysis.

In direct time integration dynamic analysis, when a node with a prescribed motion is used in an equation constraint or a multi-point constraint to control the motion of another node, the equation or multi-point constraint is imposed correctly for the displacement and velocity of the dependent node. However, the acceleration is not rigorously transmitted to the dependent node, which may cause some high-frequency noise.

In the subspace projection method it is not currently possible to specify nonzero boundary conditions directly. Instead, acceleration boundary conditions can be approximated by using appropriate combinations of large point masses and concentrated loads. At the node where such a boundary condition is desired, attach a large point mass that is approximately 10⁵–10⁶ times larger than the mass of the original model. In addition, a concentrated load of magnitude equal to the product between the large point mass and the desired acceleration must be specified in the direction of the approximated boundary condition. Since the point mass is significantly larger than the mass of the model, the big mass–concentrated load combination approximates the desired acceleration in the specified direction accurately. Boundary conditions other than accelerations must be converted into acceleration histories before they can be approximated.

Loads

The following loads can be prescribed in a dynamic analysis:

Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see Concentrated Loads.
Distributed pressure forces or body forces can be applied; see Distributed Loads. The distributed load types available with particular elements are described in Abaqus Elements Guide.
Distributed pressure or volumetric accelerations (on acoustic elements) can be applied; these are described in Acoustic, Shock, and Coupled Acoustic-Structural Analysis.

Predefined Fields

The following predefined fields can be specified in a dynamic analysis, as described in Predefined Fields:

Although temperature is not a degree of freedom in stress/displacement elements, nodal temperatures can be specified as a predefined field. 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 only affect field-variable-dependent material properties, if any.

Material Options

Most material models that describe mechanical behavior are available for use in a dynamic analysis. The following material properties are not active during a dynamic analysis: thermal properties (except for thermal expansion), mass diffusion properties, electrical conductivity properties, and pore fluid flow properties.

Rate-dependent material properties (Time Domain Viscoelasticity, Hysteresis in Elastomers, Rate-Dependent Yield, and Two-Layer Viscoplasticity) can be included in a dynamic analysis.

Rate-Dependent Yield and Friction in Quasi-Static Response

You can control whether to consider or ignore the strain rate–dependence of the yield stress and the slip rate–dependence of the friction coefficient within the step in a quasi-static response.

Input File Usage

Use the following option to consider rate dependence within the step:

DYNAMIC, APPLICATION=QUASI-STATIC, RATE DEPENDENCE=ON (default)

Use the following option to ignore rate dependence within the step:

DYNAMIC, APPLICATION=QUASI-STATIC, RATE DEPENDENCE=OFF

Abaqus/CAE Usage

Abaqus/CAE always considers the strain rate–dependence of the yield stress and the slip rate–dependence of the friction coefficient.

Elements

Other than generalized axisymmetric elements with twist, any of the stress/displacement elements in Abaqus/Standard (including those with temperature, pressure, and electrical potential degrees of freedom) can be used in a dynamic analysis. Inertia effects are ignored in hydrostatic fluid elements, and the inertia of the fluid in pore pressure elements is not taken into account.

Output

In addition to the usual output variables available in Abaqus/Standard (see Abaqus/Standard Output Variable Identifiers), the following variables are provided specifically for implicit dynamic analysis:

Variables for a specified element set or for the entire model:

XC: Current coordinates of the center of mass.
XCn: Coordinate n of the center of mass ( $n = 1, 2, 3$ ).
UC: Displacement of the center of mass.
UCn: Displacement component n of the center of mass ( $n = 1, 2, 3$ ).
URCn: Rotation component n of the center of mass.
VC: Equivalent rigid body velocity components.
VCn: Component n of the equivalent rigid body velocity ( $n = 1, 2, 3$ ).
VRCn: Component n of the equivalent rigid body angular velocity ( $n = 1, 2, 3$ ).
HC: Angular momentum about the center of mass.
HCn: Component n of the angular momentum about the center of mass ( $n = 1, 2, 3$ ).
HO: Angular momentum about the origin.
HOn: Component n of the angular momentum about the origin ( $n = 1, 2, 3$ ).
RI: Rotary inertia about the origin.
RIij: $i j$ -component of the rotary inertia about the origin ( $i \leq j \leq 3$ ).
MASS: Mass.
VOL: Current volume.

Input File Template

HEADING
…
BOUNDARY
Data lines to specify zero-valued boundary conditions
INITIAL CONDITIONS
Data lines to specify initial conditions
AMPLITUDE, NAME=name
Data lines to define amplitude variations
**
STEP (,NLGEOM)
Once NLGEOM is specified, it will be active in all subsequent steps.
DYNAMIC
Data line to control automatic time incrementation
BOUNDARY
Data lines to describe zero-valued or nonzero boundary conditions
CLOAD and/or DLOAD and/or INCIDENT WAVE
Data lines to specify loads
TEMPERATURE and/or FIELD
Data lines to prescribe predefined fields
CECHARGE and/or DECHARGE (if electrical potential degrees of
freedom are active)
Data lines to specify charges 
END STEP

References

Czekanski, A., N. El-Abbasi, and S. A. Meguid, “Optimal Time Integration Parameters for Elastodynamic Contact Problems,” Communications in Numerical Methods in Engineering, vol. 17, pp. 379–384, 2001.
Hilber, H. M., T. J. R. Hughes, and R. L. Taylor, “Improved Numerical Dissipation for Time Integration Algorithms in Structural Dynamics,” Earthquake Engineering and Structural Dynamics, vol. 5, pp. 283–292, 1977.