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). In some cases
this time scale is quite real—for example, the response might be caused by temperatures
varying with time based on a previous transient heat transfer run; or the material response
might 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 fractions of the total period of the step.
Linear Static Analysis
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).
Nonlinear Static Analysis
Nonlinearities can arise from large-displacement effects, material nonlinearity, and/or
boundary nonlinearities such as contact and friction (see General and Perturbation Procedures) 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 is used for
a static step:
Step module: Create Step: General: Static, General: Basic: Nlgeom: On (to activate the large-displacement formulation)
Unstable Problems
Some static problems can be naturally unstable, for a variety of reasons.
Buckling or Collapse
In some geometrically nonlinear analyses, buckling or collapse might 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.
In other unstable analyses the instabilities are local (for example, 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. The available automatic stabilization schemes
are described in detail in Automatic Stabilization of Unstable Problems.
Incrementation
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 are 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.
Automatic Incrementation
In most cases the default automatic incrementation scheme is preferred because it
selects increment sizes based on computational efficiency.
Direct user control of the increment size is also provided because if you have
considerable experience with a particular problem, you might be able to select a more
economical approach.
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), 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.
Step module: Create Step: General: Static, General: Other: Accept solution after reaching maximum number of iterations
Steady-State Frictional Sliding
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.
Since this frictional behavior is different from the frictional behavior used without
steady-state frictional sliding, discontinuities might 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).
Predefined motion fields are not supported in Abaqus/CAE.
Rate-Dependent Yield and Friction
Rate-dependent yield (Rate-Dependent Yield) is active
during a static analysis. 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.
Input File Usage
Use the following option to consider rate dependence within the step (default):
Abaqus/CAE always considers the strain rate–dependence of the yield stress and the slip
rate–dependence of the friction coefficient.
Initial Conditions
Initial values of stresses, temperatures, field variables, solution-dependent state
variables, etc. can be specified. Initial Conditions describes all
the available initial conditions.
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; 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). During the
analysis prescribed boundary conditions can be varied using an amplitude definition (see
Amplitude Curves).
Loads
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.
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.
Predefined Fields
The following predefined fields can be specified in a static stress analysis, as described
in Predefined Fields:
Although temperature is not a degree of freedom in a static stress analysis, you can
specify nodal temperatures 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.
Although pore fluid pressure is not a degree of freedom in a static stress analysis,
you can specify nodal pore fluid pressure as a predefined field variable (see Pore Fluid Pressure). The total
stress is computed as the sum of the effective stress and the pore fluid pressure. When
the solid grains are compressible (finite bulk modulus), the effective strain is
computed as the total strain minus the volumetric strain caused by the pore pressure
acting on the solid grain.
Material Options
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, hysteresis
(Hysteresis in Elastomers), and two-layer
viscoplasticity (Two-Layer Viscoplasticity) are the only
time-dependent material responses that are active during a static analysis. 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). When you use any of these
time-dependent material models in a static analysis, Abaqus/Standard obtains a rate-independent elastic solution and the chosen time scale does not affect the
material response. For creep and swelling behavior this indicates 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 you define time-domain viscoelastic material properties. If you request the
long-term viscoelastic solution, Abaqus/Standard ramps the internal stresses associated with each of the Prony series terms 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), you must
specify the corresponding elastic moduli 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:
Step module: Create Step: General: Static, General or Static, Riks: Other: Obtain long-term solution with time-domain material properties
Elements
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). 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 is calculated as
described in Dashpots.
Acoustic elements are not active in a static step. Consequently, if an acoustic-solid
analysis includes a static step, only the solid elements deform. If the deformations are
large, the acoustic and solid meshes might not conform, and subsequent acoustic-structural
analysis steps might produce misleading results. See About ALE Adaptive Meshing
for information on using the adaptive meshing technique to deform the acoustic mesh.
Output
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 the output variable identifiers are outlined in Abaqus/Standard Output Variable Identifiers.
Input File Template
HEADING
…
BOUNDARYData lines to specify zero-valued boundary conditionsINITIAL CONDITIONSData lines to specify initial conditionsAMPLITUDEData lines to define amplitude variations
**
STEP (,NLGEOM)
Once NLGEOM is specified, it will be active in all subsequent stepsSTATIC, DIRECTData line to define direct time incrementationBOUNDARYData lines to prescribe zero-valued or nonzero boundary conditionsCLOAD and/or DLOADData lines to specify loadsTEMPERATURE and/or FIELDData lines to specify values of predefined fieldsEND STEP
**
STEPSTATICData line to control automatic time incrementationBOUNDARY, OP=MODData lines to modify or add zero-valued or nonzero boundary conditionsCLOAD, OP=NEWData lines to specify new concentrated loads; all previous concentrated
loads will be removedDLOAD, OP=MODData lines to specify additional or modified distributed loadsTEMPERATURE and/or FIELDData lines to specify additional or modified values of predefined fieldsEND STEP