Fully coupled thermal-stress analysis

Automatic incrementation controlled by a maximum allowable temperature change

The time increments can be selected automatically based on a user-prescribed maximum allowable nodal temperature change in an increment, $\mathrm{\Delta }{\theta }_{max}$. Abaqus/Standard will restrict the time increments to ensure that this value is not exceeded at any node (except nodes with boundary conditions) during any increment of the analysis (see Time integration accuracy in transient problems).

COUPLED TEMPERATURE-DISPLACEMENT, DELTMX=$\mathrm{\Delta }{\theta }_{max}$

Step module: Create Step: General: Coupled temp-displacement: Basic: Response: Transient; Incrementation: Type: Automatic, Max. allowable temperature change per increment: $\mathrm{\Delta }{\theta }_{max}$

Fixed incrementation

If you do not specify $\mathrm{\Delta }{\theta }_{max}$, fixed time increments equal to the user-specified initial time increment, $\mathrm{\Delta }{t}_0$, 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.

COUPLED TEMPERATURE-DISPLACEMENT
$\mathrm{\Delta }{t}_0$

Step module: Create Step: General: Coupled temp-displacement: Basic: Response: Transient; Incrementation: Type: Fixed: Increment size: $\mathrm{\Delta }{t}_0$

Spurious oscillations due to small time increments

In transient analysis with second-order elements there is a relationship between the minimum usable time increment and the element size. A simple guideline is

where $\mathrm{\Delta }t$ is the time increment, $\rho$ is the density, c is the specific heat, k is the thermal conductivity, and $\mathrm{\Delta }\mathrm{\ell }$ is a typical element dimension (such as the length of a side of an element). If time increments smaller than this value are used in a mesh of second-order elements, spurious oscillations can appear in the solution, in particular in the vicinity of boundaries with rapid temperature changes. These oscillations are nonphysical and may cause problems if temperature-dependent material properties are present. In transient analyses using first-order elements the heat capacity terms are lumped, which eliminates such oscillations but can lead to locally inaccurate solutions for small time increments. If smaller time increments are required, a finer mesh should be used in regions where the temperature changes rapidly.

There is no upper limit on the time increment size (the integration procedure is unconditionally stable) unless nonlinearities cause convergence problems.

Automatic incrementation controlled by the creep response

The accuracy of the integration of time-dependent (creep) material behavior is governed by the user-specified accuracy tolerance parameter, $tolerance\ge \left(\dot{\overline{\epsilon }}^{cr}{}_{t+\mathrm{\Delta }t}-\dot{\overline{\epsilon }}^{cr}{}_t\right)\mathrm{\Delta }t$. This parameter is used to prescribe the maximum strain rate change allowed at any point during an increment, as described in Rate-dependent plasticity: creep and swelling. The accuracy tolerance parameter can be specified together with the maximum allowable nodal temperature change in an increment, $\mathrm{\Delta }{\theta }_{max}$ (described above); however, specifying the accuracy tolerance parameter activates automatic incrementation even if $\mathrm{\Delta }{\theta }_{max}$ is not specified.

COUPLED TEMPERATURE-DISPLACEMENT, DELTMX=$\mathrm{\Delta }{\theta }_{max}$, 
CETOL=tolerance

Step module: Create Step: General: Coupled temp-displacement: Basic: Response: Transient, Include creep/swelling/viscoelastic behavior; Incrementation: Type: Automatic, Max. allowable temperature change per increment: $\mathrm{\Delta }{\theta }_{max}$, Creep/swelling/viscoelastic strain error tolerance: tolerance

Selecting explicit creep integration

Nonlinear 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 as long as no other nonlinearities are present. 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 most coupled thermal-stress analyses, however, the unconditional stability of the backward difference operator (implicit method) is desirable. In such cases the implicit integration scheme may be invoked automatically by Abaqus/Standard.

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.

COUPLED TEMPERATURE-DISPLACEMENT, CETOL=tolerance, CREEP=EXPLICIT 

Step module: Create Step: General: Coupled temp-displacement: Basic: Response: Transient, Include creep/swelling/viscoelastic behavior; Incrementation: Type: Automatic, Creep/swelling/viscoelastic strain error tolerance: tolerance, Creep/swelling/viscoelastic integration: Explicit

Excluding creep and viscoelastic response

You can specify that no creep or viscoelastic response will occur during a step even if creep or viscoelastic material properties have been defined.

COUPLED TEMPERATURE-DISPLACEMENT, DELTMX=$\mathrm{\Delta }{\theta }_{max}$, CREEP=NONE 

Step module: Create Step: General: Coupled temp-displacement: Basic: Response: Transient, toggle off Include creep/swelling/viscoelastic behavior

Unstable problems

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 a method of stabilizing 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.

Estimating the time increment size

An approximation to the stability limit for the forward-difference operator in the thermal solution response is given by

where $L_{min}$ is the smallest element dimension in the mesh and $\alpha =\frac{k}{\rho c}$ is the thermal diffusivity of the material. The parameters k, $\rho$, and c represent the material's thermal conductivity, density, and specific heat, respectively.

In most applications of explicit analysis the mechanical response will govern the stability limit. The thermal response may govern the stability limit when material parameter values are non-physical or a very large amount of mass scaling is used. The calculation of the time increment size for the mechanical solution response is discussed in Explicit dynamic analysis.

Stable time increment report

Abaqus/Explicit writes a report to the status (.sta) file during the data check phase of the analysis that contains an estimate of the minimum stable time increment and a listing of the elements with the smallest stable time increments and their values. The initial minimum stable time increment accounts for the stability requirements of both the thermal and mechanical solution responses. The initial stable time increments listed do not include damping (bulk viscosity), mass scaling, or penalty contact effects in the mechanical solution response.

This listing is provided because often a few elements have much smaller stability limits than the rest of the elements in the mesh. The stable time increment can be increased by modifying the mesh to increase the size of the controlling element or by using appropriate mass scaling.

Scaling the time increment

To reduce the chance of a solution going unstable, the stable time increment computed by Abaqus/Explicit can be adjusted by a constant scaling factor. This factor can be used to scale the default global time estimate, the element-by-element estimate, or the fixed time increment based on the initial element-by-element estimate; it cannot be used to scale a fixed time increment that you specified directly.

DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT, SCALE FACTOR=f
DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT, 
ELEMENT BY ELEMENT, SCALE FACTOR=f
DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT, 
FIXED TIME INCREMENTATION, SCALE FACTOR=f

Step module: Create Step: General: Dynamic, Temp-disp, Explicit: Incrementation: Time scaling factor: f

Automatic time incrementation

The default time incrementation scheme in Abaqus/Explicit is fully automatic and requires no user intervention. Two types of estimates are used to determine the stability limit: element-by-element for both the thermal and mechanical solution responses and global for the mechanical solution response. An analysis always starts by using the element-by-element estimation method and may switch to the global estimation method under certain circumstances, as explained in Explicit dynamic analysis.

In an analysis Abaqus/Explicit initially uses a stability limit based on the thermal and mechanical solution responses in the whole model. This element-by-element estimate is determined using the smallest time increment size due to the thermal and mechanical solution responses in each element.

The element-by-element estimate is conservative; it will give a smaller stable time increment than the true stability limit, which is based upon the maximum frequency of the entire model. In general, constraints such as boundary conditions and kinematic contact have the effect of compressing the eigenvalue spectrum, and the element-by-element estimates do not take this into account (see Explicit dynamic analysis)

The stable time increment size due to the mechanical solution response will be determined by the global estimator as the step proceeds unless the element-by-element estimator is chosen, fixed time incrementation is specified, or one of the conditions explained in Explicit dynamic analysis prevents the use of global estimation. The stable time increment size due to the thermal solution response will always be determined by using an element-by-element estimation method. The switch to the global estimation method in mechanical solution response occurs once the algorithm determines that the accuracy of the global estimation method is acceptable. For details, see Explicit dynamic analysis

For three-dimensional continuum elements and elements with plane stress formulations (shell, membrane, and two-dimensional plane stress elements) an improved estimate of the element characteristic length is used by default. This improved method usually results in a larger element stable time increment than a more traditional method. For analyses using variable mass scaling, the total mass added to achieve a given stable time increment will be less with the improved estimate.

DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT, ELEMENT BY ELEMENT

DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT, IMPROVED DT METHOD=YES

DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT, IMPROVED DT METHOD=NO

Step module: Create Step: General: Dynamic, Temp-disp, Explicit: Incrementation: Type: Automatic, Stable increment estimator: Element-by-element

Step module: Create Step: General: Dynamic, Temp-disp, Explicit: Incrementation: Type: Automatic: toggle on Improved Dt Method

Step module: Create Step: General: Dynamic, Temp-disp, Explicit: Incrementation: Type: Automatic: toggle off Improved Dt Method

Fixed time incrementation

A fixed time incrementation scheme is also available in Abaqus/Explicit. The fixed time increment size is determined either by the initial element-by-element stability estimate for the step or by a user-specified time increment.

Fixed time incrementation may be useful when a more accurate representation of the higher mode response of a problem is required. In this case a time increment size smaller than the element-by-element estimates may be used. The element-by-element estimate can be obtained simply by running a data check analysis (see Abaqus/Standard and Abaqus/Explicit execution).

When fixed time incrementation is used, Abaqus/Explicit will not check that the computed response is stable during the step. You should ensure that a valid response has been obtained by carefully checking the energy history and other response variables.

If you choose to use time increments the size of the initial element-by-element stability limit throughout a step, the dilatational wave speed and the thermal diffusivity in each element at the beginning of the step are used to compute the fixed time increment size. To reduce the chance of a solution going unstable, the initial stable time increment that Abaqus/Explicit computes can be adjusted by a constant scaling factor, as described above in Scaling the time increment. Alternatively, you can specify a time increment size directly.

DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT, 
FIXED TIME INCREMENTATION

DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT, DIRECT USER CONTROL
$\mathrm{\Delta }t$

Step module: Create Step: General: Dynamic, Temp-disp, Explicit: Incrementation: Type: Fixed, Use element-by-element time increment estimator or User-defined time increment: $\mathrm{\Delta }t$