1.6.4 Quenching of an infinite plate

Products: ABAQUS/Standard  ABAQUS/Explicit  

This example is an illustration of uncoupled heat transfer and subsequent thermal-stress analysis. A semi-analytic solution is available for the case (see Landau et al., 1960), so the problem provides verification of this type of analysis in ABAQUS. The purpose of the analysis is to predict the residual stresses caused by the quenching of a large homogeneous plate in regions away from the edges of the plate so that it can be treated as a plate of infinite extent in all but the thickness direction. The plate is made of an elastic, perfectly plastic material, with a yield stress that drops linearly with temperature above 121°C (250°F). The problem is one-dimensional since the plate is assumed to be of infinite extent: the only gradients occur through the thickness. The plate is initially at a uniform temperature, near its melting point (when its yield stress is small). It is assumed to be stress-free in this condition. The surface is then quenched in a medium at room temperature. Cooling is allowed to continue until all of the plate reaches room temperature.

The analyses performed in ABAQUS/Standard consist of both sequential thermal-stress and fully coupled solution procedures. In the sequential analyses the transient heat transfer analysis is followed by the thermal stress analysis. During the heat transfer analysis the temperature distributions are recorded in the ABAQUS results file. This temperature-time history is then used as input to the thermal stress analysis. The transient stresses are large enough to cause significant plastic flow, so residual stresses will remain after the plate reaches room temperature. In the fully coupled procedures the sequentially coupled problems are simulated by setting the fraction of inelastic dissipation that is converted into heat to zero. In this problem this uncouples the thermal response from the mechanical response.

A fully coupled solution procedure is used in ABAQUS/Explicit; the sequentially coupled problem described above is again simulated by setting the fraction of inelastic dissipation that is converted into heat to zero. For completeness, another analysis is performed in ABAQUS/Explicit, this time using the VUMAT user subroutine to define the material response and assuming that a 0.2 fraction of the inelastic dissipation is converted into heat. This last analysis illustrates the use of the VUMAT user subroutine in conjunction with the *INELASTIC HEAT FRACTION, *SPECIFIC HEAT, and *CONDUCTIVITY options; the heat flux due to inelastic energy dissipation is calculated automatically by ABAQUS/Explicit.

Problem description

Analysis sequence

The ABAQUS/Standard sequential thermal-stress simulation consists of a transient heat transfer analysis, followed by a thermal-stress analysis in which the temperatures predicted by the heat transfer analysis are used as the loading of the problem. ABAQUS makes it very simple to transfer temperature data in this way. The *NODE FILE option is used in the heat transfer analysis to write the temperatures at the nodes to a file. Then, in the stress analysis the FILE parameter on the *TEMPERATURE option is used to read these temperatures back into the stress model. This mode of transferring the temperatures is based on node numbers: the temperature at node N on the *NODE FILE output from the heat transfer analysis is applied at node N in the stress mesh. Thus, the node numbers must remain the same from the heat transfer model to the stress model. ABAQUS does not check that the nodes are in the same location. In some cases nonstructural components (such as insulation) are modeled in the heat transfer analysis but not in the stress analysis. This situation does not present a problem; if the *NODE FILE output includes temperatures at nodes that do not exist in the stress analysis model, those temperatures are ignored when the *TEMPERATURE option reads the data.

In the ABAQUS/Standard and ABAQUS/Explicit fully coupled analyses the thermal and mechanical responses of the plate are determined simultaneously.

Controls

The following discussion is relevant only for the ABAQUS/Standard simulations.

The DELTMX parameter limits the maximum temperature change that may occur in an increment and, thus, determines the accuracy with which the transient temperature solution is integrated in time. It also implies the use of automatic time incrementation, which is desirable in a case such as this where we wish to carry the analysis through to steady-state conditions, so that large time increments are used toward the end of the solution. In this example DELTMX is set to 5.56°C (10°F). This choice should provide sufficient accuracy in the heat transfer solution to define the residual stresses correctly.

The initial time increment is suggested to be 20 seconds, and the time period is suggested to be 4 × 106 seconds. Since the solution is to reach steady state, the time period specification is rather arbitrary: it has to be long enough to reach steady state. The END=SS parameter is used on the *HEAT TRANSFER option, which indicates that the analysis should terminate when steady-state conditions are reached. Steady-state conditions are defined for the purpose of this parameter by the time rate of change of temperature at all nodes falling below the value given on the data line. In this analysis this value is set to 0.556 × 10–6°C per second (10–6°F per second). When END=SS is used, the step terminates either when steady-state conditions have been reached or when the time period specified for the step has been completed, whichever comes first. Therefore, a very large time period is generally used in such cases.

It is usually desirable to specify a minimum time increment (the third data item on the data line following the *HEAT TRANSFER option) to cover the possibility that a data error or unforeseen event in the solution causes the automatic time increment scheme to choose very small increments. In this case a value of 0.5 seconds is used for this purpose. Uncoupled heat transfer analysis, Section 6.5.2 of the ABAQUS Analysis User's Manual, recommends a minimum time increment for transient heat transfer analysis when there is a rapid change in temperature of

In this case is 0.9 in, so this formula suggests a minimum time increment of at least 6.9 sec. In the case where the surface temperature is changed suddenly, time increments that are smaller than this can cause initial oscillations in the solution. However, the physics of this problem do not produce sufficiently large temperature gradients to cause such oscillations with the time increment that satisfies the maximum temperature change specified with the DELTMX parameter.

Results and discussion

Input files

Reference

Figures

Figure 1.6.4–1 Infinite plate quenching problem and finite element mesh.

Figure 1.6.4–2 Residual stresses through the half-plate (ABAQUS/Standard).

Figure 1.6.4–3 Stress history for the plate surface and center.