Coupled Structural/Thermal Analysis using Ansys

Introduction

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.

---

Preprocessing: Defining the Problem

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

1. Give example a TitleUtility Menu > File > Change Title ...
   /title, Thermal Stress Example
2. Open preprocessor menuANSYS Main Menu > Preprocessor
   /PREP7
3. Define KeypointsPreprocessor > Modeling > Create > Keypoints > In Active CS...
   K,#,x,y,zWe 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)

4. Create LinesPreprocessor > Modeling > Create > Lines > Lines > In Active Coord
   L,1,2Create a line joining Keypoints 1 and 2, representing a link 1 meter long.
5. Define the Type of Element
Preprocessor > Element Type > Add/Edit/Delete...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.

6. Define Real Constants
Preprocessor > Real Constants... > Add...In the 'Real Constants for LINK33' window, enter the following geometric properties:

1. Cross-sectional area AREA: 4e-4
This defines a beam with a cross-sectional area of 2 cm X 2 cm.

7. Define Element Material PropertiesPreprocessor > Material Props > Material Models > Thermal > Conductivity > IsotropicIn the window that appears, enter the following geometric properties for steel:
   
   1. KXX: 60.5
8. Define Mesh SizePreprocessor > Meshing > Size Cntrls > ManualSize > Lines > All Lines...For this example we will use an element edge length of 0.1 meters.
9. Mesh the framePreprocessor > Meshing > Mesh > Lines > click 'Pick All'
10. Write EnvironmentThe thermal environment (the geometry and thermal properties) is now fully described and can be written to memory to be used at a later time.
    Preprocessor > Physics > Environment > WriteIn the window that appears, enter the TITLE Thermal and click OK.
    
11. Clear EnvironmentPreprocessor > Physics > Environment > Clear > OKDoing 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.

1. Switch Element Type
Preprocessor > Element Type > Switch Elem TypeChoose 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.

2. Define Element Material PropertiesPreprocessor > Material Props > Material Models > Structural > Linear > Elastic > IsotropicIn the window that appears, enter the following geometric properties for steel:
   
   1. Young's Modulus EX: 200e9
   2. Poisson's Ratio PRXY: 0.3
   Preprocessor > Material Props > Material Models > Structural > Thermal Expansion Coef > Isotropic
   
   1. ALPX: 12e-6
3. Write EnvironmentThe structural environment is now fully described.
   Preprocessor > Physics > Environment > WriteIn the window that appears, enter the TITLE Struct

---

Solution Phase: Assigning Loads and Solving

1. Define Analysis Type
Solution > Analysis Type > New Analysis > Static
ANTYPE,0

2. Read in the Thermal Environment
Solution > Physics > Environment > ReadChoose 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.


3. Apply Constraints
Solution > Define Loads > Apply > Thermal > Temperature > On KeypointsSet the temperature of Keypoint 1, the left-most point, to 348 Kelvin.

4. Solve the System
Solution > Solve > Current LS
SOLVE

5. Close the Solution Menu
Main Menu > FinishIt 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 labelledJobname.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.


6. Read in the Structural Environment
Solution > Physics > Environment > ReadChoose struct and click OK.

7. Apply Constraints
Solution > Define Loads > Apply > Structural > Displacement > On KeypointsFix Keypoint 1 for all DOF's and Keypoint 2 in the UX direction.

8. Include Thermal EffectsSolution > Define Loads > Apply > Structural > Temperature > From Therm AnalyAs 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.
   
9. Define Reference TemperaturePreprocessor > Loads > Define Loads > Settings > Reference TempFor this example set the reference temperature to 273 degrees Kelvin.
   
10. Solve the System
Solution > Solve > Current LS
SOLVE

---

Postprocessing: Viewing the Results

1. Hand CalculationsHand calculations were performed to verify the solution found using ANSYS:
   As shown, the stress in the link should be a uniform 180 MPa in compression.
2. Get Stress DataSince the element is only a line, the stress can't be listed in the normal way. Instead, an element table must be created first.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
   
3. List the Stress DataGeneral Postproc > Element Table > List Elem Table > COMPSTR > OK
   PRETAB,CompStr
   The following list should appear. Note the stress in each element: -0.180e9 Pa, or 180 MPa in compression as expected.