Thermal Conductivity, Density, and Specific Heat must be defined for a transient thermal analysis. Thermal Conductivity can be isotropic or orthotropic. All properties can be constant or temperature-dependent.

There are no special considerations for a transient thermal analysis.

Mechanical does not support Rigid Bodies in thermal analyses. For more information, see the Stiffness Behavior documentation for Rigid Bodies.

You can define a Thermal Point Mass for this analysis type.

In a thermal analysis only contact is valid. Any joints or springs are ignored.

With contact the initial status is maintained throughout the thermal analysis, that is, any closed contact faces will remain closed and any open contact faces will remain open for the duration of the thermal analysis. Heat conduction across a closed contact face is set to a sufficiently high enough value (based on the thermal conductivities and the model size) to model perfect contact with minimal thermal resistance. If needed, you can model imperfect contact by manually inputting a Thermal Conductance value.

By default, Contact Results (accessible through User Defined Results via CONTSTAT or CONTFLUX – see the User Defined Results for the Mechanical APDL Solver section.) are not written to the result file in a thermal analysis.

There are no specific considerations for transient thermal analysis itself. However if the temperatures from this analysis are to be used in a subsequent structural analysis the mesh must be identical. Therefore in this case you may want to make sure the mesh is fine enough for a structural analysis.

For a Transient Thermal analysis, the basic Analysis Settings controls include:

Step Controls for Static and Transient Analyses

Step Controls are used to: i) specify the end time of the transient analysis, ii) control the time step size, and iii) create multiple steps when needed.

The rate of loading could be important in a transient thermal analysis if the material properties vary rapidly with temperature. When such nonlinearities are present it may be necessary to apply the loads in small increments and perform solutions at these intermediate loads to achieve convergence. Multiple steps are needed if you want to change the solution settings, for example, the time step size or the solution output frequency over specific time spans in the transient analysis.

Output Controls

Solver Controls enable you to specify the time points at which results should be available for postprocessing. A transient analysis involves calculating solutions at several time points in the load history. However: i) you may not be interested in all the intermediate results and ii) writing all the results can make the results file size unwieldy. In this case you can restrict the amount of output by requesting results only at certain time points.

Nonlinear Controls

Nonlinear Controls enable you to modify convergence criteria and other specialized solution controls. Typically you will not need to change the default values for this control.

Analysis Data Management

Analysis Data Management settings enable you to save specific solution files from the transient thermal analysis for use in other analyses.

A transient thermal analysis involves loads that are functions of time. The first step in applying transient thermal loads is to establish initial temperature distribution at Time = 0.

The default initial condition for a transient thermal analysis is a uniform temperature of 22°C or 71.6°F. You can change this to an appropriate value for your analysis. An example might be modeling the cooling of an object taken out of a furnace and plunged into water.

You can also use the temperature results from a steady-state analysis of the same model for the initial temperature distribution. A casting solidification study might start with different initial temperatures for the mold and the metal. In this case a steady-state analysis of the hot molten metal inside the mold can serve as the starting point for the solidification analysis.

In the first iteration of a transient thermal analysis, this initial temperature is used as the starting temperature value for the model except where temperatures are explicitly specified. In addition this temperature is also used to evaluate temperature-dependent material property values for the first iteration.

If the Initial Temperature field is set to Non-Uniform Temperature, a Time field is displayed where you can specify a time at which the temperature result of the steady-state thermal analysis (selected in Initial Condition Environment field) will be used as the initial temperature in the transient analysis. A zero value will be translated as the end time (of the steady-state thermal analysis) and this value can not be greater than the end time.

The following loads are supported in a transient thermal analysis:

Temperature Convection Radiation Heat Flow Perfectly Insulated Heat Flux

Internal Heat Generation Imported Heat Generation Imported Temperature Imported Convection Coefficient System Coupling Region

In this analysis, the load's magnitude could be a constant value or could vary with time as defined in a table or via a function. Details of how to apply a tabular or function load are described in Specifying Boundary Condition Magnitude. In addition, for more information about time stepping and ramped loads, see the Applying Stepped and Ramped Loads section.

The Solution Information object provides some tools to monitor solution progress.

Solution Output continuously updates any listing output from the solver and provides valuable information on the behavior of the structure during the analysis. Any convergence data output in this printout can be graphically displayed as explained in the Solution Information section.

You can also insert a Result Tracker object under Solution Information. This tool enables you to monitor temperature at a vertex as the solution progresses. Result Tracker is not available to the Samcef or ABAQUS solver.

Applicable results are all thermal result types.

Once a solution is available you can contour the results or animate the results to review the response of the structure.

As a result of a nonlinear analysis you may have a solution at several time points. You can use probes to display the variation of a result item over the load history. Also of interest is the ability to plot one result quantity (for example, maximum temperature on a face) against another results item (for example, applied heat generation rate). You can use the Charts feature to develop such charts.

Note that Charts are also useful to compare results between two analyses of the same model.