6.3.2 Implicit dynamic analysis using direct integration

Products: ABAQUS/Standard  ABAQUS/CAE  



A direct-integration dynamic analysis in ABAQUS/Standard:

  • must be used when nonlinear dynamic response is being studied; and

  • can be fully nonlinear (general dynamic analysis) or can be based on the modes of the linear system (subspace projection method).

General dynamic analysis

General linear or nonlinear dynamic analysis in ABAQUS/Standard uses implicit time integration to calculate the transient dynamic response of a system. See Implicit dynamic analysis, Section 2.4.1 of the ABAQUS Theory Manual, for details on implicit dynamic analysis.

Input File Usage:           


Step module: Create Step: General: Dynamic, Implicit

Numerical implementation

The general direct-integration method provided in ABAQUS/Standard, called the Hilber-Hughes-Taylor operator, is an extension of the trapezoidal rule. The Hilber-Hughes-Taylor operator is implicit: the integration 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.

This nonlinear equation solving process is expensive; and if the equations are very nonlinear, it may be difficult to obtain a solution. However, nonlinearities are usually more simply accounted for in dynamic situations than in static situations because the inertia terms provide mathematical stability to the system; thus, the method is successful in all but the most extreme cases.

The principal advantage of the Hilber-Hughes-Taylor operator is that it is 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. (It is very difficult to establish stability results for integration operators in the context of nonlinear equations, but for practical purposes the linear stability results provide an adequate indication of the integration method's properties for nonlinear systems.) 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.

Automatic time incrementation

An automatic incrementation scheme is provided for use with the general implicit dynamic integration method. The scheme uses a half-step residual control to ensure an accurate dynamic solution. The half-step residual is the equilibrium residual error (out-of-balance forces) halfway through a time increment; for a continuum solution the equilibrium residual should be moderately small compared to significant forces in the problem. This half-step residual check is the basis of the adaptive time incrementation scheme. If the half-step residual is small, it indicates that the accuracy of the solution is high and that the time step can be increased safely; conversely, if the half-step residual is large, the time step used in the solution should be reduced—see Time integration accuracy in transient problems, Section 7.2.4.

The automatic incrementation scheme is especially effective in cases where a sudden event initiates the dynamic problem (a vehicle crash, a pipe break, a bird strike, etc.) and the structural response involves very large amounts of energy being dissipated—by plasticity effects, for example, or by viscous damping such as a fluid might provide. In such studies small time increments are required immediately after the sudden event (and there may be several such occasions in the total history of the problem—for example, repeated severe impacts). At later times the response can be modeled accurately with large time increments because most of the high frequency content of the solution has been damped out by the dissipation mechanisms present in the model.

In structural problems implicit integration schemes usually give acceptable solutions with time steps typically one or two orders of magnitude larger than the stability limit of simple explicit schemes, but the response prediction will deteriorate as the time step size, , increases relative to the period, T, of typical modes of response. See, for example, Hilber, Hughes, and Taylor (1978) for a discussion of such errors. Three factors should be considered when selecting the maximum allowable time step size: the rate of variation of the applied loading, the complexity of the nonlinear damping and stiffness properties, and the typical period of vibration of the structure. In general, a maximum increment versus period ratio 1/10 is a good rule of thumb for obtaining reliable results.

Controlling the accuracy of the solution

You can specify the acceptable half-step residual tolerance, , to be used with the automatic time incrementation scheme. The half-step residual tolerance has dimensions of force and is usually chosen by comparison with typical actual force values, P, such as applied forces or expected reaction forces. The following guidelines can be used for choosing the value of the half-step residual tolerance:

  • If , the solution will generally be highly accurate for elastic cases with little damping. In problems where considerable plasticity or other dissipation is expected to damp out the high frequency response, a tolerance this restrictive is not necessary.

  • If , the solution is moderately accurate for elastic cases with little damping and highly accurate for problems including plasticity or other damping mechanisms.

  • If , the solution is coarse for elastic problems with little damping but still quite good for problems with dissipative effects. Even values of will give useful results for primary effects such as overall deformation.

The half-step residual moment tolerance is the half-step residual tolerance times the characteristic element length calculated for a problem.

Automatic incrementation is recommended for most cases, especially when the dynamic response can be expected to change significantly during the solution.

You must specify the half-step residual tolerance; otherwise, ABAQUS/Standard will use a fixed time increment.

Input File Usage:           
*DYNAMIC, HAFTOL=tolerance


Step module: Create Step: General: Dynamic, Implicit: Incrementation: Half-step residual tolerance: tolerance

Direct time incrementation

You may choose to control the incrementation directly through a step. This approach is not generally recommended; it should be used only in special cases when you have a thorough understanding of how to interpret results obtained in this way. Impact events are particularly difficult to solve using fixed time increments. Small increments and a minimum of two iterations are usually necessary if direct user control is selected.

Input File Usage:           


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

Suppressing the half-step residual

If fixed time incrementation is used, it is possible to suppress calculation of the half-step residual to reduce the solution cost.

Input File Usage:           


Step module: Create Step: General: Dynamic, Implicit: Incrementation: Fixed and Suppress half-step residual calculation

Artificial damping

You can introduce and control artificial damping through the numerical damping control parameter, . This damping is purely numerical and is different from the material damping discussed in Material damping, Section 20.1.1.

Artificial damping grows with the ratio of the time increment to the period of vibration of a mode. Negative values of provide damping. can range from , which gives no artificial damping (energy preserving) and is exactly the trapezoidal rule (sometimes called the Newmark -method, with and ), to , which provides the maximum artificial damping available from this operator. At the maximum level gives a damping ratio of about 6% when the time increment is 40% of the period of oscillation of the mode being studied and smaller if the oscillation period increases. Therefore, this artificial damping is never very substantial for realistic time increments.

A value of is used by default because it introduces just enough artificial damping in the system to allow the automatic time stepping procedure to work smoothly.

Input File Usage:           


Step module: Create Step: General: Dynamic, Implicit: Other: Numerical damping control parameter:

The “subspace projection” method

The alternative approach provided in ABAQUS/Standard for nonlinear dynamic problems is the “subspace projection” method. See Subspace dynamics, Section 2.4.3 of the ABAQUS Theory Manual, 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, Section 6.3.5) prior to the dynamic analysis and are used as a small set of global basis vectors to develop the solution. These modes will 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 will not be 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:           


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 will be 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:


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 for the linear system, where 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.


You can introduce Rayleigh damping, as explained in Material damping, Section 20.1.1.

Input File Usage:           


Property module: material editor: MechanicalDamping: Alpha and Beta

Initial conditions

Initial conditions, Section 27.2.1, 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, Section 2.1.5).

If initial velocities are specified at nodes for which displacement boundary conditions are also specified, the initial velocities will be ignored at these nodes. However, if a displacement boundary condition refers to an amplitude curve with an analytically defined time variation (i.e., excluding the piecewise linear tabular and equally spaced definitions), ABAQUS/Standard will compute 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 will ensure that initial velocities are consistent with boundary conditions and with multi-point and equation constraints but will 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 will calculate accelerations at the beginning of the dynamic step. You can choose to bypass these acceleration calculations, in which case ABAQUS/Standard will assume 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 will cause 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-step residual.

Input File Usage:           


Step module: Create Step: General: Dynamic, Implicit: Other: Bypass calculations of initial accelerations at beginning of step

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, Section 27.3.1).

Amplitude references can be used to prescribe time-varying boundary conditions in a direct-integration dynamic step. Default amplitude variations are described in Procedures: overview, Section 6.1.1.

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 will be imposed correctly for the displacement and velocity of the dependent node. However, the acceleration will not be 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 approximatively 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 will approximate the desired acceleration in the specified direction accurately. Boundary conditions other than accelerations must be converted into acceleration histories before they can be approximated.

Intermittent contact/impact

When “hard,” augmented Lagrangian or penalty contact conditions (Contact pressure-overclosure relationships, Section 30.1.2) change state from open to closed, ABAQUS/Standard performs the following sequence of increments:

  1. An increment is analyzed ignoring contact changes during the increment.

  2. If contact changes occur during the increment, the solution is then returned to the beginning of the increment and is again stepped forward using a new time increment estimated from the average time of impact (assuming constant velocity) of all points that have changed contact state. Again, no contact is assumed to occur.

  3. Next, a solution to the impulse equation is obtained using a time increment that is equal to 10–6 times the original time increment prior to impact (the size of the time increment used in Step 1). Any geometric incompatibilities (overclosure or underclosure) associated with points that had been predicted to close are calculated and maintained constant so long as such points remain closed.

  4. The analysis is then resumed, with the new contact constraints added. For automatic time incrementation the next time increment is equal to the time increment prior to impact. For fixed time incrementation the next time increment is equal to the fixed time increment minus the impact time increment.

In many cases high-frequency noise generated by the impact greatly increases the half-step residual. Therefore, with automatic time incrementation ABAQUS/Standard may reduce the time increment immediately after impact until the half-step residual tolerance is satisfied. See Intermittent contact/impact, Section 2.4.2 of the ABAQUS Theory Manual, for details.

When impact is preceded by large relative motion between the contact surfaces, multiple points may change state within a single increment. Because the increment is repeated to satisfy the closure in an average sense, some nodes remain overclosed, while others are fixed at a distance away from the contact surface. Such geometric incompatibilities are most commonly caused by rigid body motion of one or both of the bodies before impact. In such cases the incompatibilities can be eliminated by generating the model with the bodies in contact and applying the appropriate initial conditions. If this is not feasible, the error can be minimized by limiting the maximum allowable time increment.

Solution of impulse equations upon impact is not necessary when softened contact is chosen with the exponential, linear, or tabular pressure-overclosure relationship. If the soft contact constraint compatibility is not satisfied within the given tolerance, however, a severe discontinuity iteration is forced (see Convergence criteria for nonlinear problems, Section 7.2.3).


The following loads can be prescribed in a dynamic analysis:

Predefined fields

The following predefined fields can be specified in a dynamic analysis, as described in Predefined fields, Section 27.6.1:

  • 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 will cause thermal strain if a thermal expansion coefficient is given for the material (Thermal expansion, Section 20.1.2). The specified temperature also affects temperature-dependent material properties, if any.

  • The values of user-defined field variables can be specified. These values 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, Section 17.7.1; Hysteresis in elastomers, Section 17.8.1; Rate-dependent yield, Section 18.2.3; and Two-layer viscoplasticity, Section 18.2.11) can be included in a dynamic analysis.


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.


In addition to the usual output variables available in ABAQUS/Standard (see ABAQUS/Standard output variable identifiers, Section 4.2.1), the following variables are provided specifically for implicit dynamic analysis:

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

Current coordinates of the center of mass.


Coordinate n of the center of mass ().


Displacement of the center of mass.


Displacement component n of the center of mass ().


Rotation component n of the center of mass.


Equivalent rigid body velocity components.


Component n of the equivalent rigid body velocity ().


Component n of the equivalent rigid body angular velocity ().


Angular momentum about the center of mass.


Component n of the angular momentum about the center of mass ().


Angular momentum about the origin.


Component n of the angular momentum about the origin ().


Rotary inertia about the origin.


-component of the rotary inertia about the origin ().




Current volume.

Input file template

Data lines to specify zero-valued boundary conditions
Data lines to specify initial conditions
Data lines to define amplitude variations
Once NLGEOM is specified, it will be active in all subsequent steps.
*DYNAMIC, HAFTOL=tolerance
Data line to control automatic time incrementation
Data lines to describe zero-valued or nonzero boundary conditions
Data lines to specify loads
Data lines to prescribe predefined fields
*CECHARGE and/or *DECHARGE (if electrical potential degrees of
freedom are active)
Data lines to specify charges