Workshop 6: Thermal Analysis of a Plate with a Hole University of Puerto Rico at Mayagüez Department of Mechanical Engineering Modified by (2008): Dr. Vijay K. Goyal Associate Professor, Department of Mechanical Engineering University of Puerto Rico at Mayagüez Thanks to UPRM students enrolled in INME 4058 sections

Introduction: In this workshop we will use ANSYS to do a thermal analysis on a plate with a hole. The plate will consist of two materials, each with different conductivities and sizes. The list on the following page gives a list of material properties and design parameters that we’ll be using. Thermal Analysis with ANSYS

Material #1: Conductivity: 20 Size: 0.05 × 0.05 × Material #2: Conductivity: 50 Size: 0.10 × 0.05 × Hole: Center: At center of Material #1 Radius: 0.01 Other Parameters: Analysis Type: Thermal, h-method Element Type: thermal solid Film Coefficient: 150 Bulk Temperature: 25 Heat Flux: 150 Temperature at leftmost edge: 200 Temperature at rightmost edge: 50 Properties and Parameters Thermal Analysis with ANSYS

Starting ANSYS From your desktop: Click on: START > All Programs > ANSYS 10.0 > ANSYS Product Launcher. Here we will set our Working Directory and the Graphics Manager

This is the 10.0 ANSYS Product Launcher main window. Select the Working Directory and type the name of work shop on Job Name. Working Directory Setup

Click the button: Customization/Preferences. On the item of Use custom memory settings type 128 on Total Workspace (MB): and type 64 on Database (MB): Then click the Run bottom. Graphics Setup * This setup applies to computers running under 512 MB of RAM

This is ANSYS’s Graphical User Interface window. ANSYS GUI Overview

Once the program starts, save your work with a name. Go to the Utility Menu, choose File > Save. Make sure you save it with a name you can recognize later (such as workshop6 or WS_6). Also, remember to save your file every so often (each time you get the right result), to make sure your work is saved and you won't have to start all over again if for any reason you have to quit working, since ANSYS does not have “undo”. Getting Started

We’ll set preferences in order to filter quantities that relate to this discipline only. Click Preferences from ANSYS Main Menu. Select (check): “Thermal ” & h-Method ” Step 1: Set Preferences

Preprocessing: Now we choose the element type. Go to Preprocessor > Add/Edit/Delete Click Add button, and choose the element type. For this case, we choose: Thermal Mass > Solid > Quad4node Step 2: Element Type

Preprocessing: The next step in preprocessing is choosing the element materials properties. Go to Preprocessor > Material Props > Material Models. Select Thermal > Conductivity > Isotropic. Enter the thermal conductivity for the first material. (=20) Step 3: Define Materials

Preprocessing: To choose a second material model, go to the window for Material Model. Choose the New Model option from the Material Menu. Repeat the same process, and enter the thermal conductivity for the second model. (=50) Step 3: Define Materials

Preprocessing: Now we create the model. Go to: Preprocessor > Modeling > Create > Areas > Rectangle > By Dimensions. Enter the dimensions of the first rectangle: (X1,X2; 0, 0.05) (Y1,Y2; 0,0.05); Click By Dimensions again and enter the coordinates of the second rectangle: (X1,X2; 0.05, 0.1) (Y1,Y2; 0,0.05) Click OK Step 4: Build Geometry

Preprocessing: Now we create the hole. Go to Preprocessor > Modeling > Create > Area > Circle > Solid Circle. Enter the center coordinates and the radius: (WP X=0.025, WP Y=0.025, Radius: 0.01) Step 4: Build Geometry

Preprocessing: To actually create the hole, that is, we’ll remove or subtract the hole area from whole area. Go to Preprocessing > Modeling > Booleans > Subtract> Areas Step 4: Build Geometry

Preprocessing: We select the base area (the square we want to keep), click OK (if a menu allowing you to choose which area pops up, make sure you choose the correct area and click OK). Then, we choose the area we want to subtract (the circle), and click OK. Step 4: Build Geometry

Preprocessing: Now we join the areas. Go to Preprocessor > Modeling > Operate > Booleans > Glue > Areas. We select the two areas we want to join, and click OK. *They will continue to be two separate areas, with different properties. Step 4: Build Geometry

Preprocessing: Now we create the mesh. Go to Preprocessor > Meshing > Mesh Tool In the Element Attribute option menu, select Area, then choose the area. An area attribute menu will pop up, make sure to choose the correct material properties. Repeat for the second area. Step 5: Create Mesh

Preprocessing : In the Mesh Tool Window, choose the size of the mesh areas. We chose Smart Size 4. You can choose whichever size you want, or you can enter your own mesh parameters in the next menu of the window. To create the Mesh, click the Mesh button, choose the areas you want to mesh (Pick All), and then click OK. Step 5: Create Mesh

Processing: Now we can begin the Processing. The first thing we’ll do is apply a temperature gradient to the bar. Choose: Preprocessor > Define Loads > Apply > Thermal > Temperature > On Nodes Choose the leftmost nodes, click OK. Enter the temperature for that side and click enter. Repeat for the other side. Step 6: Apply Loads (Temp. Gradient)

Processing: We continue with convection. Go to Preprocessor > Define Loads > Apply >Thermal > Convection > On Nodes. Choose the top nodes, and click OK. Enter the film coefficient and the bulk temperature: Film Coefficient: 150 Bulk Temperature: 25 Step 6: Apply Loads (Temp. Gradient)

Processing: We now apply the heat flux. Go to Preprocessor > Define Loads > Apply >Thermal > Heat Flux > On Nodes Choose the nodes at the circle, click OK. Enter: Load HFLUX value: 150 Step 6: Apply Loads (Temp. Gradient)

Processing: We are now ready to Solve! Go to: Solution > Solve > Current LS. Click OK. Step 7: Obtain Solution

Processing: A window that says "Solution is done!" will pop up. Click Close. Step 7: Obtain Solution

Post-Processing: Now, we can view the results of the analysis. We go to: General Postproc > Plot Results > Contour Plot > Nodal Solu. From here we can choose almost any plot we want. The plot we chose was the Temperature plot, given on the following pages. It includes a brief description and the instructions to obtain it. Step 8: Review Results

Post-Processing: Temperature Plot: In the Contour Nodal Solution Window, choose: Nodal Solution > DOF Solution and Temperature Click OK, and the plot to the right should appear. Step 8: Review Results

For different results, you can change the parameters and values, such as conductivities, temperatures, film coefficients and bulk temperature - or you could change the mesh size. Try it out and see what you get! Step 8: Review Results