Thermal Analysis Steps

An analysis case is a template (a set of objects sets) for defining environmental actions on a given system. A Thermal Analysis case consists of a Simulation History, which can contain one or more steps. Each step represents a period of time in the simulation history and is associated with a specific analysis procedure. In the Thermal Analysis workbench you can define the following type of step:

Inserting a New Heat Transfer Step: Generates a Heat Transfer step in a Thermal case. A Heat Transfer step is included by default when you create a Thermal case.

Inserting a New Heat Transfer Step

Inserting a heat transfer step within the Simulation History indicates that a heat transfer solution procedure should be used for the computation of the system response to applied thermal loads under given constraints. You can create environmental specifications (for example, boundary conditions and loads) within the step. Heat transfer steps are available only in the Thermal Analysis workbench. They can be defined in new analysis cases or in analysis cases that contain other heat transfer steps; they cannot be defined in structural cases. See Step Sequence Restrictions for more information. Thermal Analysis creates a Heat Transfer step by default for a new Thermal case.

In a pure heat transfer analysis the temperature field is calculated without knowledge of the stress/deformation state in the bodies being studied. Pure heat transfer analyses can be transient or steady state and linear or nonlinear. See Inserting a New General Static Step for information on sequentially coupled thermal-stress analyses.

The thermal conductivity and density of the materials in a heat transfer analysis must be defined. The specific heat must also be defined for transient heat transfer problems. Thermal expansion coefficients are not meaningful in a pure (uncoupled) heat transfer analysis since deformation of the structure is not considered.

This task shows you how to insert a new Heat Transfer step in a Thermal case.

  1. Select Start>Analysis & Simulation>Thermal Analysis from the menu bar to enter the Thermal Analysis workbench.

  2. If necessary, set an empty Thermal case or an Thermal case that contains thermal analysis procedures to be the current case.

    Thermal Analysis creates a Heat Transfer step by default for a new Thermal case.

  3. To create an additional Heat Transfer step, do either of the following:

    • To append a new Heat Transfer step to the end of the Simulation History, click the Heat Transfer Step icon .

      Tip: Alternatively, you can select Insert>Heat Transfer Step from the menu bar.

    • To insert a new Heat Transfer step between two existing steps in the Simulation History, right-click the step object in the specification tree after which you want to create the new step, then select Insert Heat Transfer Step Below from the menu that appears.

    The Heat Transfer Step dialog box appears, and a new Heat Transfer Step objects set appears in the specification tree under the Simulation History objects set for the current Thermal case.

  4. You can change the step identifier by editing the Step name field. This name will be used in the specification tree.

  5. Enter a description for the step in the Step description field.

  6. If necessary, edit the Step time field to specify a value for the total time period of the step.

  7. If necessary, do the following to modify the Incrementation Controls:

    1. Select the Incrementation type: Automatic or Fixed. Automatic incrementation means that the solver will select increment sizes based on the user-specified maximum allowable nodal temperature change per increment. Fixed incrementation means that you specify a fixed increment size.

    2. Enter a value for the Maximum number of increments. The default number of increments for a step is 100; if significant nonlinearity is present in the simulation, the analysis may require many more increments. If the solver needs more increments than the specified upper limit to complete the step, it will terminate the analysis with an error message.

    3. Enter a value for the Initial increment size. This value will be modified as required if automatic incrementation is used or will be used as the constant time increment if fixed time incrementation is used.

    4. Enter a value for the Minimum increment size. This value is used only for automatic time incrementation. Abaqus will terminate an analysis if excessive cutbacks caused by convergence problems reduce the increment size below the minimum value. If a value is given, the solver will use the minimum of the given value and 0.8 times the initial time increment. If no value is given, the solver sets the minimum increment to the minimum of 0.8 times the initial time increment and 1 × 10–5 times the total time period.

    5. Enter a value for the Maximum increment size. This value is used only for automatic time incrementation. By default, there is no upper limit on the increment size, other than the total step time.

  8. If necessary, do the following to modify the Heat Transfer Data:

    1. Select the Thermal response: Steady-state or Transient. Transient heat transfer analyses consider the internal thermal energy in the structure and, as a result, have a physically meaningful time scale. Steady-state heat transfer analyses omit consideration of internal energy, resulting in a long-time or steady-state solution that has no intrinsic physically meaningful time scale. However, you can assign a “time” scale to a steady-state analysis step; for example, to efficiently ramp on thermal loading that results in nonlinear material behavior.

    2. Toggle on End step when temperature change is less than, and enter a value for the temperature change rate (temperature per time) used to define steady state. When all nodal temperatures are changing at less than this rate, the step solution terminates. If this option is not selected, the step solution terminates when the total time period of the step has been completed. This option is available only for transient heat transfer steps.

    3. Enter a value for the Maximum temperature change allowed per increment. The solver will restrict the time step to ensure that this value will not be exceeded at any node (except nodes whose temperature degree of freedom is constrained via boundary conditions) during any increment of the step. This option is available only for transient heat transfer steps with automatic incrementation.

  9. Click OK when you have finished defining the step.

    The Heat Transfer Step objects set contains a default Field Output Request object in a Field Output Requests objects set. See Requesting Results for more information.