ProductsAbaqus/StandardAbaqus/CAE IncrementationYou 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. Fixed incrementationIf 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, except when the explicit creep integration scheme is used. In this case Abaqus/Standard might decrease the time increment if the stability limit is exceeded. Input File Usage VISCO Abaqus/CAE Usage Step module: Create Step: General: Visco Automatic incrementationIf 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: where t is the time at the beginning of the increment, is the time increment (so that is the time at the end of the increment), and is the equivalent creep strain rate. To achieve accuracy, the value chosen for the accuracy tolerance parameter should be on the order of for creep problems, where is an acceptable level of error in the stress and E is a typical elastic modulus, or on the order of the elastic strains for viscoelasticity problems. Input File Usage VISCO, CETOL=tolerance Abaqus/CAE Usage Step module: Create Step: General: Visco: Incrementation: Creep/swelling/viscoelastic strain error tolerance: tolerance Selecting explicit creep integrationNonlinear creep problems (Rate-dependent plasticity: creep and swelling) 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 for further details. Input File Usage VISCO, CETOL=tolerance, CREEP=EXPLICIT Abaqus/CAE Usage Step module: Create Step: General: Visco: Incrementation: Creep/swelling/viscoelastic strain error tolerance: tolerance and Creep/swelling/viscoelastic integration: Explicit Integration scheme for viscoelasticity and rate-dependent yieldProblems including Time domain viscoelasticity 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 and Parallel rheological framework 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. Unstable problemsSome 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. The available automatic stabilization schemes are described in detail in Automatic stabilization of unstable problems. Initial conditionsInitial values of stresses, temperatures, field variables, solution-dependent state variables, etc. can be specified, as described in Initial conditions in Abaqus/Standard and Abaqus/Explicit. Boundary conditionsBoundary 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 in Abaqus/Standard and Abaqus/Explicit. LoadsThe following types of loading can be prescribed in a quasi-static analysis:
Predefined fieldsThe following predefined fields can be specified in a quasi-static analysis, as described in Predefined Fields:
Material optionsThe 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). This procedure can also be used to analyze viscoelastic materials (Time domain viscoelasticity and Parallel rheological framework) and two-layer viscoplastic materials (Two-layer viscoplasticity). In addition, all material models that are valid in a static analysis procedure can be used. ElementsAny 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. OutputIn addition to the usual output variables available in Abaqus/Standard (see Abaqus/Standard output variable identifiers), the following variables are provided specifically for creep problems: Element integration point variables:
Input file templateHEADING … 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 |