Temperatures

Note: The information in this section applies to all linear and nonlinear structural analyses for which temperatures are applicable and to electrostatic analyses.

Temperatures are also applicable to heat transfer analyses but are significantly different within that context. For more information, please refer to the following pages in the, Setting Up and Performing the Analysis: Analysis-Specific Information: Thermal Analyses: Loads and Constraints section of the Help:

• Initial Temperature
• Controlled Temperature

A temperature can be applied to nodes, surfaces, or parts in a linear or nonlinear structural analysis model and to nodes or surfaces in an electrostatic analysis model.

What Does a Temperature Do?

• A surface temperature applies nodal temperatures to each node on the surface, and a part temperature applies nodal temperatures to each node in the part.
• In linear and nonlinear structural models, temperatures are used for thermal stress analysis. Temperatures cause thermal expansion of any materials with non-zero coefficients of thermal expansion.
• The nodes to which a temperature is applied are kept at the value specified in the Magnitude field. This temperature is only applied to the selected nodes and does not conduct through the material. (A thermal analysis is required to calculate heat conduction or heat flow via convection or radiation.)
• The stress caused by the temperature is calculated from the difference between the nodal temperature and the Stress Free Reference Temperature, which is specified within the Element Definition dialog box. The effect of this temperature difference depends on the Thermal Coefficient of Expansion defined in the Material Specification dialog box.
• For the manually-applied temperatures to be accounted for in a linear or nonlinear structural analysis, you must select the Model file option in the Source of temperature drop-down box in the Thermal tab of the Analysis Parameters dialog box.
• For a linear analysis, you must also assign a Thermal multiplier in the Multipliers tab of the Analysis Parameters dialog box.
• For a nonlinear analysis, select the load curve that will control the magnitudes of the temperatures as a function of time in the Nodal temperature load curve index field within the Thermal tab of the Analysis Parameters dialog box. A load curve must have been previously defined for its number to appear in this drop-down menu. The load curve can be used to vary temperatures from a steady-state heat transfer analysis over time. For example, you can gradually increase the applied temperature from zero to the input temperature values by varying the load curve multiplier from zero to 1.
  Important: For nonlinear stress analyses using transient heat transfer results, the temperature as a function of time in the stress analysis is the same as the temperature versus time from the thermal analysis. The duration of the thermal simulation event must be equal to or greater than the duration of the stress analysis event. In this case, the load curve will typically have a constant value of 1 (applied temperature equals input temperature from the thermal analysis throughout the event). This is discussed further in the Use Load Curves to Control Temperature versus Time in Nonlinear Analyses section at the bottom of this page.
• For linear, nonlinear, and electrostatic analyses, temperatures affect the material properties when temperature-dependent material models are specified within the Element Definition dialog box.

Apply Temperatures

If you have nodes, surfaces, or parts selected, you can right-click in the display area and select the Add pull-out menu. Select the Nodal Temperatures or Surface Temperatures or Part Temperatures command, respectively. You can also access this command via the ribbon (Setup Loads Temperature).

Specify the magnitude of the temperature that is applied to each selected object in the Magnitude field.

Note: If different temperatures are applied to the same node, the last temperature is used for the node. For example, if parts 1 and 2 are bonded together, and if part 1 is assigned a temperature of 100 degrees, then part 2 is assigned a temperature of 75 degrees, the nodes in common will have an initial temperature of 75 degrees.

Apply Constant Temperatures to Entire Models

If you simply want to determine the thermal stress in a model due to a uniform temperature change, it is not necessary to add nodal temperatures to the entire model. Instead, right-click the Thermal heading under the Analysis Type heading in the browser and choose Edit. Note that this heading may be gray before a temperature has been defined, but the command is still available. Perform the following two steps:

• Choose the Loads from FEA Editor option from the Source of Temperature drop-down menu.
• Type the desired temperature value in the Default Temperature field. Any node in the model that does not have a nodal temperature applied is set to this value. Any applied temperature overrides the default value.

Apply Temperature Profiles from Thermal Analyses

In some cases, the temperature profiles for a model have already been calculated using either a steady-state or transient heat transfer analysis. If the geometry of the structural model is identical to the thermal model, the thermal results can be used for the temperature profile. There are two methods to do this.

Method 1:

1. For a linear or nonlinear stress analysis, right-click the Thermal heading under the Analysis Type heading in the browser and select the Edit command. For a natural frequency (modal) with load stiffening or critical buckling load analysis, right-click the Analysis Type heading, select the Edit Analysis Parameters command and go to the Thermal tab.
2. Then, select the type of heat transfer analysis that was previously performed on this model in the Source of Temperature drop-down menu. The choices are as follows:
   • Another Design Scenario in loaded file.
   • Another Simulation Mechanical file.
   • Simulation CFD file. Please refer to the Using Autodesk® Simulation CFD Temperature Results as Thermal Loads page for more information concerning this option.
3. If using another Simulation Mechanical file or a Simulation CFD model, press the Browse button next to the Filename and Design Scenario heading. Then, navigate to and select the desired thermal analysis model file. Specify which design scenario of the thermal source model to use from the drop-down menu below the filename field.
   If you are using a different design scenario within the same model file, specify which one to use from the Use temperature from design scenario pull-down menu.

   Note: This menu will only list design scenarios for which the analysis type is either steady-state or transient heat transfer. If a heat transfer analysis was completed but the analysis type later changed to a non-thermal type, the design scenario will not appear in the Use temperature from design scenario pull-down menu, even though the thermal results file is still present in the folder.
4. If you are using the results from a transient heat transfer analysis as a load in a linear static stress analysis, specify which thermal analysis time step to use as the source of temperatures for the stress analysis. Do this using the Which step to use pull-down menu. The default is to use the last time step.

Note: Method 1 permits the meshes to be different between the thermal model and the stress model. See the paragraph Requirements for Different Meshes on the page Multiphysics for details.

Method 2:

1. With nothing selected, right-click in the display area of the FEA Editor. Select the Loads from File command.
2. Press the Browse button in the Results File column. A dialog box appears so you can select the results file. Use the Files of type: pull-down to select Thermal Results File (*.to, *.tto).
3. Select the file with the temperature results and click Open.
4. Only the temperatures from a single load case or time step in the selected file can be applied to the stress model. Select the load case or time step in the Load Case from File column.
5. The temperatures are placed in load case 1 regardless of what number is entered in the Structural Load Case field.
6. If you want the temperatures to be multiplied by a constant value before being applied to the model, specify the constant value in the Multiplier column.
7. Press the OK button.

Attention: Unlike other types of loads which can be applied to the model using the Loads from File method, only one temperature can be applied to a given node. You cannot specify multiple result files (or the same file multiple times) and have the temperatures added together at the same node. Nor can you apply different thermal results files to the same nodes for different load cases. Only the last temperature applied to a node will be retained. You can use multiple temperature results files only if each file pertains to a different portion of the stress model.

Note: Method 2 requires the meshes to be identical between the thermal model and the stress model because it transfers the temperatures by coordinates in the overall model (not on a per-part basis). See the paragraph Requirements for Same Meshes on the page Multiphysics for details.

Use Temperatures to Model Initial Strain Conditions in a Linear Analysis

The easiest way to model an initial strain in a part is to use a temperature. If you know the amount of existing strain and the properties of the material, you can apply the correct temperature difference using the following procedure.

1. Using the basic equation for expansion, we know that the strain is equal to the product of the temperature difference and the coefficient of thermal expansion, α:

   

2. Solving this equation for the temperature difference we get:

   

Using this process we can now calculate the temperature difference that we have to apply to the model to simulate a prestrain condition based on the known strain and the material properties.

Use Load Curves to Control Temperature versus Time in Nonlinear Analyses

All temperatures are multiplied by the assigned load curve multiplier where the load curve is set with the Nodal temperature load curve index drop-down. For a uniform rod, the expansion due to the temperatures would be...

L = L*α*(LCM*T - Tref)

where

• ΔL is the change in length
• L is the length
• α is the coefficient of thermal expansion, which is based on the temperature T, not LCM*T
• LCM is the load curve multiplier
• T is the temperature at each node, either from temperatures explicitly assigned to the nodes, or the default nodal temperature, or the results from a steady state analysis
• Tref is the stress free reference temperature.

Since a transient heat transfer analysis presumably has an accurate history of the temperatures versus time, it may be unusual to read these temperatures and use a load curve multiplier other than 1. In some cases though, such as when the model begins at a temperature other than Tref, the impact that occurs due to the application of the temperatures at time 0 can be reduced by ramping up the load curve multiplier over a portion of the event. This will help the solution to converge.

Where steady-state thermal results are used as the source of temperatures for a nonlinear structural analysis, use the load curve to gradually increase the temperature from Tref to the input temperature values.

Parent topic: Loads and Constraints