Introduction
You can use a steady-state thermal analysis to determine temperatures, thermal gradients, heat flow rates, and heat fluxes in an object that are caused by thermal loads that do not vary over time. A steady-state thermal analysis calculates the effects of steady thermal loads on a system or component. Engineers often perform a steady-state analysis before performing a transient thermal analysis, to help establish initial conditions. A steady-state analysis also can be the last step of a transient thermal analysis, performed after all transient effects have diminished. A steady-state thermal analysis can be performed using the Mechanical APDL, Samcef, or ABAQUS solver.
Important: By default, the application does not write thermal gradient results to the result file. To have these results written to the results file, use a Command object and insert the command OUTRES,ERASE.
Point to Remember
A steady-state thermal analysis may be either linear, with constant material properties; or nonlinear, with material properties that depend on temperature. The thermal properties of most material do vary with temperature, so the analysis usually is nonlinear. Including radiation effects or temperature dependent convection coefficient also makes the analysis nonlinear.
Preparing the Analysis
Create Analysis System
Basic general information about this topic
... for this analysis type:
From the Toolbox, drag a Steady-State Thermal, Steady-State Thermal (Samcef), or Steady-State Thermal (ABAQUS) template to the Project Schematic.
Define Engineering Data
Basic general information about this topic
... for this analysis type:
Thermal Conductivity must be defined for a steady-state thermal analysis. Thermal Conductivity can be isotropic or orthotropic, and constant or temperature-dependent.
Attach Geometry
Basic general information about this topic
... for this analysis type:
There are no specific considerations for a steady-state thermal analysis.
Define Part Behavior
Basic general information about this topic
... for this analysis type:
Mechanical does not support Rigid Bodies in thermal analyses. For more information, see the Stiffness Behavior documentation for Rigid Bodies.
Define Connections
Basic general information about this topic
... 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.
Apply Mesh Controls/Preview Mesh
Basic general information about this topic
... for this analysis type:
There are no specific considerations for steady-state 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 structural analysis.
Establish Analysis Settings
Basic general information about this topic
... for this analysis type:
For a steady-state thermal analyses you typically do not need to change these settings. The basic Analysis Settings include:
- Step Controls for Static and Transient Analyses
Step Controls enable you to control the rate of loading which could be important in a steady-state 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. You may wish to use multiple steps if you a) want to analyze several different loading scenarios within the same analysis or b) if you want to change the analysis settings such as the time step size or the solution output frequency over specific time ranges.
- Output Controls
Output Controls enable you to specify the time points at which results should be available for postprocessing. In a nonlinear analysis it may be necessary to perform many solutions at intermediate load values. 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.
Nonlinear Controls are exposed for the Mechanical APDL solver only.
- Analysis Data Management
Analysis Data Management settings enable you to save specific solution files from the steady-state thermal analysis for use in other analyses.
Define Initial Conditions
Basic general information about this topic
... for this analysis type:
For a steady-state thermal analysis you can specify an initial temperature value. This uniform temperature is used during the first iteration of a solution as follows:
To evaluate temperature-dependent material properties.
As the starting temperature value for constant temperature loads.
Apply Boundary Conditions
Basic general information about this topic
... for this analysis type:
The following loads are supported in a steady-state thermal analysis:
Loads and supports vary as a function of time even in a static analysis as explained in the Role of Time in Role of Time in Tracking. In a static 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.
Fluid Solid Interface is not available for the Samcef or ABAQUS solver.
Solve
Basic general information about this topic
... for this analysis type:
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.
Review Results
Basic general information about this topic
... for this analysis type:
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.