Products: ABAQUS/Standard ABAQUS/CAE
A static stress analysis:
is used when inertia effects can be neglected;
can be linear or nonlinear; and
ignores time-dependent material effects (creep, swelling, viscoelasticity) but takes rate-dependent plasticity and hysteretic behavior for hyperelastic materials into account.
During a static step you assign a time period to the analysis. This is necessary for cross-references to the amplitude options, which can be used to determine the variation of loads and other externally prescribed parameters during a step (see Amplitude curves, Section 27.1.2). In some cases this time scale is quite real—for example, the response may be caused by temperatures varying with time based on a previous transient heat transfer run; or the material response may be rate dependent (rate-dependent plasticity), so that a natural time scale exists. Other cases do not have such a natural time scale; for example, when a vessel is pressurized up to limit load with rate-independent material response. If you do not specify a time period, ABAQUS/Standard defaults to a time period in which “time” varies from 0.0 to 1.0 over the step. The “time” increments are then simply fractions of the total period of the step.
Linear static analysis involves the specification of load cases and appropriate boundary conditions. If all or part of a problem has linear response, substructuring is a powerful capability for reducing the computational cost of large analyses (see Using substructures, Section 10.1.1).
Nonlinearities can arise from large-displacement effects, material nonlinearity, and/or boundary nonlinearities such as contact and friction (see General and linear perturbation procedures, Section 6.1.2) and must be accounted for. If geometrically nonlinear behavior is expected in a step, the large-displacement formulation should be used. In most nonlinear analyses the loading variations over the step follow a prescribed history such as a temperature transient or a prescribed displacement.
|Input File Usage:||Use the following option to specify that a large-displacement formulation should be used for a static step:|
Step module: Create Step: General: Static, General: Basic: Nlgeom: On (to activate the large-displacement formulation)
Some static problems can be naturally unstable, for a variety of reasons.
In some geometrically nonlinear analyses, buckling or collapse may occur. In these cases a quasi-static solution can be obtained only if the magnitude of the load does not follow a prescribed history; it must be part of the solution. When the loading can be considered proportional (the loading over the complete structure can be scaled with a single parameter), a special approach—called the “modified Riks method”—can be used, as described in Unstable collapse and postbuckling analysis, Section 6.2.4.
|Input File Usage:|
Step module: Create Step: General: Static, Riks
In other unstable analyses the instabilities are local (e.g., surface wrinkling, material instability, or local buckling), in which case global load control methods such as the Riks method are not appropriate. ABAQUS/Standard offers the option to stabilize this class of problems by applying damping throughout the model in such a way that the viscous forces introduced are sufficiently large to prevent instantaneous buckling or collapse but small enough not to affect the behavior significantly while the problem is stable. ABAQUS/Standard generates an artificial damping matrix by using the mass matrix with a unit density together with a mass-proportional damping factor, as described in Solving nonlinear problems, Section 7.1.1. Whenever possible, the damping factor is chosen such that, based on extrapolation of the results obtained during the first increment, the dissipated energy during the step is a small fraction of the change in strain energy during the step. You control the value of this dissipated energy fraction; the default value is 2.0 × 104. If the problem is either unstable or contains rigid body motions during the first increment, an alternative method is used to determine the damping factor; this method is based on making an averaged damping stiffness equal to the dissipated energy fraction times an averaged material stiffness.
|Input File Usage:||Use the following option to activate automatic stabilization with the default dissipated energy fraction:|
Use the following option to specify a nondefault dissipated energy fraction:
*STATIC, STABILIZE=dissipated energy fraction
Use the following option to specify the damping factor directly:
*STATIC, STABILIZE, FACTOR=damping factor
Step module: Create Step: General: Static, General: Basic: toggle on Use stabilization with, and select dissipated energy fraction or damping factor
ABAQUS/Standard uses Newton's method to solve the nonlinear equilibrium equations. Many problems involve history-dependent response; therefore, the solution usually is obtained as a series of increments, with iterations to obtain equilibrium within each increment. Increments must sometimes be kept small (in the sense that rotation and strain increments must be small) to ensure correct modeling of history-dependent effects. Most commonly the choice of increment size is a matter of computational efficiency: if the increments are too large, more iterations will be required. Furthermore, Newton's method has a finite radius of convergence; too large an increment can prevent any solution from being obtained because the initial state is too far away from the equilibrium state that is being sought—it is outside the radius of convergence. Thus, there is an algorithmic restriction on the increment size.
In most cases the default automatic incrementation scheme is preferred because it will select increment sizes based on computational efficiency.
|Input File Usage:|
Step module: Create Step: General: Static, General: Incrementation: Type: Automatic (default)
Direct user control of the increment size is also provided because if you have considerable experience with a particular problem, you may be able to select a more economical approach.
|Input File Usage:|
Step module: Create Step: General: Static, General: Incrementation: Type: Fixed
With direct user control, the solution to an increment can be accepted after the maximum number of iterations allowed has been completed (as defined in Commonly used control parameters, Section 7.2.2), even if the equilibrium tolerances are not satisfied. This approach is not recommended; it should be used only in special cases when you have a thorough understanding of how to interpret results obtained in this way. Very small increments and a minimum of two iterations are usually necessary if this option is used.
|Input File Usage:|
*STATIC, DIRECT=NO STOP
Step module: Create Step: General: Static, General: Other: Accept solution after reaching maximum number of iterations
In a static analysis procedure you can model steady-state frictional sliding between two deformable bodies or between a deformable and a rigid body that are moving with different velocities by specifying the motions of the bodies as predefined fields. In this case it is assumed that the slip velocity follows from the difference in the user-specified velocities and is independent of the nodal displacements, as described in Coulomb friction, Section 5.2.3 of the ABAQUS Theory Manual.
Since this frictional behavior is different from the frictional behavior used without steady-state frictional sliding, discontinuities may arise in the solutions between an analysis step in which relative velocity is determined from predefined motions and prior steps. An example is the discontinuity that occurs between the initial preloading of the disc pads in a disc brake system and the subsequent braking analysis where the disc spins with a prescribed rotation. To ensure a smooth transition in the solution, it is recommended that all analysis steps prior to the analysis step in which predefined motion is specified use a zero coefficient of friction. You can then modify the friction properties in the steady-state analysis to use the desired friction coefficient (see Changing friction properties during an ABAQUS/Standard analysis” in “Frictional behavior, Section 30.1.5).
|Input File Usage:|
|ABAQUS/CAE Usage:||Predefined motion fields are not supported in ABAQUS/CAE.|
Initial values of stresses, temperatures, field variables, solution-dependent state variables, etc. can be specified. Initial conditions, Section 27.2.1, describes all of the available initial 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; or, if hydrostatic fluid elements are included in the model, to fluid pressure degree of freedom 8. If boundary conditions are applied to rotation degrees of freedom, you must understand how finite rotations are handled by ABAQUS (see Boundary conditions, Section 27.3.1). During the analysis prescribed boundary conditions can be varied using an amplitude definition (see Amplitude curves, Section 27.1.2).
The following loads can be prescribed in a static stress analysis:
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see Concentrated loads, Section 27.4.2.
The following predefined fields can be specified in a static stress analysis, as described in Predefined fields, Section 27.6.1:
Although temperature is not a degree of freedom in a static stress analysis, 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.
Most material models that describe mechanical behavior are available for use in a static stress analysis. The following material properties are not active during a static stress analysis: acoustic properties, thermal properties (except for thermal expansion), mass diffusion properties, electrical conductivity properties, and pore fluid flow properties.
Rate-dependent yield (Rate-dependent yield, Section 18.2.3), hysteresis (Hysteresis in elastomers, Section 17.8.1), and two-layer viscoplasticity (Two-layer viscoplasticity, Section 18.2.11) are the only time-dependent material responses that are active during a static analysis. The rate-dependent yield response is often important in rapid processes such as metal-working problems. The hysteresis model is useful in modeling the large-strain, rate-dependent response of elastomers that exhibit a pronounced hysteresis under cyclic loading. The two-layer viscoplasticity model is useful in situations where a significant time-dependent behavior as well as plasticity is observed, which for metals typically occurs at elevated temperatures. An appropriate time scale must be specified so that ABAQUS/Standard can treat the rate dependence of the material responses correctly.
Static creep and swelling problems and time-domain viscoelastic models are analyzed by the quasi-static procedure (Quasi-static analysis, Section 6.2.5). When any of these time-dependent material models are used in a static analysis, a rate-independent elastic solution is obtained and the chosen time scale does not have an effect on the material response. For creep and swelling behavior this implies that the loading is applied instantaneously compared with the natural time scale over which creep effects take place.
The same concept of instantaneous load application applies to time-domain viscoelastic behavior. You can also obtain the fully relaxed long-term viscoelastic solution directly in a static procedure without having to perform a transient analysis; this choice is meaningful only when time-domain viscoelastic material properties are defined. If the long-term viscoelastic solution is requested, the internal stresses associated with each of the Prony series terms are increased gradually from their values at the beginning of the step to their long-term values at the end of the step.
For the two-layer viscoplastic material model, you can obtain the long-term response of the elastic-plastic network alone.
When frequency-domain viscoelastic material properties are defined (see Frequency domain viscoelasticity, Section 17.7.2), the corresponding elastic moduli must be specified as long-term elastic moduli. This implies that the response corresponds to the long-term elastic solution, regardless of the time period specified for the step.
|Input File Usage:||Use the following option to obtain the fully relaxed long-term elastic solution with time-domain viscoelasticity or the long-term elastic-plastic solution for two-layer viscoplasticity:|
*STATIC, LONG TERM
Step module: Create Step: General: Static, General or Static, Riks: Other: Obtain long-term solution with time-domain material properties
Any of the stress/displacement elements in ABAQUS/Standard can be used in a static stress analysis (see Choosing the appropriate element for an analysis type, Section 21.1.3). Although velocities are not available in a static stress analysis, dashpots can still be used (they can be useful in stabilizing an unstable problem). The relative velocity will be calculated as described in Dashpots, Section 26.2.1.
Acoustic elements are not active in a static step. Consequently, if an acoustic-solid analysis includes a static step, only the solid elements will deform. If the deformations are large, the acoustic and solid meshes may not conform, and subsequent acoustic-structural analysis steps may produce misleading results. See ALE adaptive meshing: overview, Section 12.2.1, for information on using the adaptive meshing technique to deform the acoustic mesh.
The element output available for a static stress analysis includes stress; strain; energies; the values of state, field, and user-defined variables; and composite failure measures. The nodal output available includes displacements, reaction forces, and coordinates. All of the output variable identifiers are outlined in ABAQUS/Standard output variable identifiers, Section 4.2.1.
*HEADING … *BOUNDARY Data lines to specify zero-valued boundary conditions *INITIAL CONDITIONS Data lines to specify initial conditions *AMPLITUDE Data lines to define amplitude variations ** *STEP (,NLGEOM) Once NLGEOM is specified, it will be active in all subsequent steps *STATIC, DIRECT Data line to define direct time incrementation *BOUNDARY Data lines to prescribe zero-valued or nonzero boundary conditions *CLOAD and/or *DLOAD Data lines to specify loads *TEMPERATURE and/or *FIELD Data lines to specify values of predefined fields *END STEP ** *STEP *STATIC Data line to control automatic time incrementation *BOUNDARY, OP=MOD Data lines to modify or add zero-valued or nonzero boundary conditions *CLOAD, OP=NEW Data lines to specify new concentrated loads; all previous concentrated loads will be removed *DLOAD, OP=MOD Data lines to specify additional or modified distributed loads *TEMPERATURE and/or *FIELD Data lines to specify additional or modified values of predefined fields *END STEP