This tutorial was completed using ANSYS 7.0 The purpose of this tutorial is to outline a simple coupled thermal/structural analysis. A steel link, with no internal stresses, is pinned between two solid structures at a reference temperature of 0 C (273 K). One of the solid structures is heated to a temperature of 75 C (348 K). As heat is transferred from the solid structure into the link, the link will attemp to expand. However, since it is pinned this cannot occur and as such, stress is created in the link. A steady-state solution of the resulting stress will be found to simplify the analysis.
Loads will not be applied to the link, only a temperature change of 75 degrees Celsius. The link is steel with a modulus of elasticity of 200 GPa, a thermal conductivity of 60.5 W/m*K and a thermal expansion coefficient of 12e-6 /K.
According to Chapter 2 of the ANSYS Coupled-Field Guide, "A sequentially coupled physics analysis is the combination of analyses from different engineering disciplines which interact to solve a global engineering problem. For convenience, ...the solutions and procedures associated with a particular engineering discipline [will be referred to as] a physics analysis. When the input of one physics analysis depends on the results from another analysis, the analyses are coupled."
Thus, each different physics environment must be constructed seperately so they can be used to determine the coupled physics solution. However, it is important to note that a single set of nodes will exist for the entire model. By creating the geometry in the first physical environment, and using it with any following coupled environments, the geometry is kept constant. For our case, we will create the geometry in the Thermal Environment, where the thermal effects will be applied.
Although the geometry must remain constant, the element types can change. For instance, thermal elements are required for a thermal analysis while structural elements are required to deterime the stress in the link. It is important to note, however that only certain combinations of elements can be used for a coupled physics analysis. For a listing, see Chapter 2 of the ANSYS Coupled-Field Guide located in the help file.
The process requires the user to create all the necessary environments, which are basically the preprocessing portions for each environment, and write them to memory. Then in the solution phase they can be combined to solve the coupled analysis.
Thermal Environment - Create Geometry and Define Thermal Properties
We are going to define 2 keypoints for this link as given in the following table:
| Keypoint | Coordinates (x,y,z) |
| 1 | (0,0) |
| 2 | (1,0) |
Create a line joining Keypoints 1 and 2, representing a link 1 meter long.
For this problem we will use the LINK33 (Thermal Mass Link 3D conduction) element. This element is a uniaxial element with the ability to conduct heat between its nodes.
In the 'Real Constants for LINK33' window, enter the following geometric properties:
This defines a beam with a cross-sectional area of 2 cm X 2 cm.
In the window that appears, enter the following geometric properties for steel:
For this example we will use an element edge length of 0.1 meters.
In the window that appears, enter the TITLE Thermal and click OK.
Doing this clears all the information prescribed for the geometry, such as the element type, material properties, etc. It does not clear the geometry however, so it can be used in the next stage, which is defining the structural environment.
Structural Environment - Define Physical Properties
Since the geometry of the problem has already been defined in the previous steps, all that is required is to detail the structural variables.
Choose Thermal to Struc from the scoll down list.
This will switch to the complimentary structural element automatically. In this case it is LINK 8. For more information on this element, see the help file. A warning saying you should modify the new element as necessary will pop up. In this case, only the material properties need to be modified as the geometry is staying the same.
In the window that appears, enter the following geometric properties for steel:
Preprocessor > Material Props > Material Models > Structural > Thermal Expansion Coef > Isotropic
In the window that appears, enter the TITLE Struct
Choose thermal and click OK.
If the Physics option is not available under Solution, click Unabridged Menu at the bottom of the Solution menu. This should make it visible.
Set the temperature of Keypoint 1, the left-most point, to 348 Kelvin.
It is very important to click Finish as it closes that environment and allows a new one to be opened without contamination. If this is not done, you will get error messages.
The thermal solution has now been obtained. If you plot the steady-state temperature on the link, you will see it is a uniform 348 K, as expected. This information is saved in a file labelled Jobname.rth, were .rth is the thermal results file. Since the jobname wasn't changed at the beginning of the analysis, this data can be found as file.rth. We will use these results in determing the structural effects.
Choose struct and click OK.
Fix Keypoint 1 for all DOF's and Keypoint 2 in the UX direction.
As shown below, enter the file name File.rth. This couples the results from the solution of the thermal environment to the information prescribed in the structural environment and uses it during the analysis.
For this example set the reference temperature to 273 degrees Kelvin.
As shown, the stress in the link should be a uniform 180 MPa in compression.
General Postproc > Element Table > Define Table > Add
Fill in the window as shown below. [CompStr > By Sequence Num > LS > LS,1
ETABLE,CompStress,LS,1
The following list should appear. Note the stress in each element: -0.180e9 Pa, or 180 MPa in compression as expected.
