Products: ABAQUS/Standard ABAQUS/CAE
A quasi-static stress analysis in ABAQUS/Standard:
is used to analyze problems with time-dependent material response (creep, swelling, viscoelasticity, and two-layer viscoplasticity);
is used when inertia effects can be neglected; and
can be linear or nonlinear.
You can control the time incrementation in a quasi-static analysis directly, or it can be controlled automatically by ABAQUS/Standard. Automatic incrementation is preferred in almost all cases.
If you specify the time increments in a quasi-static analysis directly, fixed time increments equal to the specified initial time increment will be used throughout the analysis.
|Input File Usage:|
Step module: Create Step: General: Visco
If you select automatic incrementation, the size of the time increment is limited by the accuracy of the integration. The user-specified accuracy tolerance parameter limits the maximum inelastic strain rate change allowed over an increment:
|Input File Usage:|
Step module: Create Step: General: Visco: Incrementation: Creep/swelling/viscoelastic strain error tolerance: tolerance
Nonlinear creep problems (Rate-dependent plasticity: creep and swelling, Section 18.2.4) that exhibit no other nonlinearities can be solved efficiently by forward-difference integration of the inelastic strains if the inelastic strain increments are smaller than the elastic strains. This explicit method is efficient computationally because, unlike implicit methods, iteration is not required. Although this method is only conditionally stable, the numerical stability limit of the explicit operator is in many cases sufficiently large to allow the solution to be developed in a reasonable number of time increments.
For creep at very low stress levels, however, the unconditional stability of the backward difference operator (implicit method) is desirable. In such cases ABAQUS/Standard will invoke the implicit integration scheme automatically.
Explicit integration can be less expensive computationally and simplifies implementation of user-defined creep laws in user subroutine CREEP; you can restrict ABAQUS/Standard to using this method for creep problems (with or without geometric nonlinearity included). See Rate-dependent plasticity: creep and swelling, Section 18.2.4, for further details.
|Input File Usage:|
*VISCO, CETOL=tolerance, CREEP=EXPLICIT
Step module: Create Step: General: Visco: Incrementation: Creep/swelling/viscoelastic strain error tolerance: tolerance and Creep/swelling/viscoelastic integration: Explicit
Problems including Time domain viscoelasticity, Section 17.7.1, are always integrated with an unconditionally stable operator. The time step in these problems is limited only by the accuracy tolerance parameter defined above.
Problems including Rate-dependent yield, Section 18.2.3, are always integrated using an implicit, unconditionally stable method. The accuracy tolerance parameter does not limit the inelastic strain rate change and can be set equal to any nonzero value to activate automatic time incrementation.
Some types of analyses may develop local instabilities, such as surface wrinkling, material instability, or local buckling. In such cases it may not be possible to obtain a quasi-static solution, even with the aid of automatic incrementation. ABAQUS/Standard offers the ability 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:
*VISCO, STABILIZE=dissipated energy fraction
Use the following option to specify the damping factor directly:
*VISCO, STABILIZE, FACTOR=damping factor
Step module: Create Step: General: Visco: toggle on Use stabilization with, and select dissipated energy fraction or damping factor
Initial values of stresses, temperatures, field variables, solution-dependent state variables, etc. can be specified, as described in Initial conditions, Section 27.2.1.
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 ABAQUS handles finite rotations. See Boundary conditions, Section 27.3.1.
The following types of loading can be prescribed in a quasi-static analysis:
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see Concentrated loads, Section 27.4.2.
Distributed pressure forces or body forces can be applied; see Distributed loads, Section 27.4.3. The distributed load types available with particular elements are described in Part VI, Elements.”
The following predefined fields can be specified in a quasi-static analysis, as described in Predefined fields, Section 27.6.1:
Although temperature is not a degree of freedom in quasi-static 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 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 affect only field-variable-dependent material properties, if any.
The quasi-static procedure in ABAQUS/Standard is generally used to analyze quasi-static creep and swelling problems, which occur over fairly long time periods (Rate-dependent plasticity: creep and swelling, Section 18.2.4). This procedure can also be used to analyze viscoelastic materials (Time domain viscoelasticity, Section 17.7.1) and two-layer viscoplastic materials (Two-layer viscoplasticity, Section 18.2.11). In addition, all material models that are valid in a static analysis procedure can be used.
Any of the stress/displacement elements in ABAQUS/Standard (including those with temperature or pressure degrees of freedom) can be used in a quasi-static stress analysis—see Choosing the appropriate element for an analysis type, Section 21.1.3.
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 creep problems:
Equivalent creep strain, .
Magnitude of the swelling strain.
Magnitude of the creep strain, .
Principal creep strains.
Output of all of the creep strain components and CEEQ, CESW, and CEMAG.
*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) *VISCO, CETOL=tolerance Data line to define time incrementation and a “real” time scale *BOUNDARY Data lines to describe nonzero boundary conditions *CLOAD and/or *DLOAD and/or *TEMPERATURE and/or *FIELD Data lines to specify loading *END STEP