Carnegie Mellon

Mechanical Engineering

Self-paced learning on the Web
FEM/ANSYS

 

T1 2D Heatsink
Home Course Info Problems Test Problems Students Reference

Thermal #1: Temperature distribution in a fin cooled electronic component

 

Introduction: In this example you will learn to model a cooling fin for electronics. This involves heat generation, conduction and convection.

Physical Problem: All electronic components generate heat during the course of their operation. To ensure optimal working of the component, the generated heat needs to be removed and thus the electronic component be cooled. This is done by attaching fins to the device which aid in rapid heat removal to the surroundings.

Problem Description:

 

bullet

For the sake of simplicity we assume that the electronic circuit is made of copper with thermal conductivity of 386 W/m K. Also it generates heat at the rate of 10e6 W.

bullet

The enclosing container is made of steel with thermal conductivity of 20 W/m K.

bullet

The fins are made of aluminum with thermal conductivity of 180 W/m K.

bullet

Units: Use S.I. units ONLY

bullet

Geometry: See figure.

bullet

Boundary conditions: There is convection along all the boundaries except the bottom, which is insulated. The Film Coefficient is 50 W/m2K and the Bulk Temperature is 20oC.

bullet

Objective:
bullet

To determine the nodal temperature distribution.

bullet

To determine the maximum value of temperature in the component.

bullet

You are required to hand in print outs for the above.

bullet

Figure:

 

 

IMPORTANT: Convert all dimensions and forces into SI units.

 

STARTING ANSYS

 

Click on ANSYS 6.1in the programs menu.

Select Interactive.

The following menu that comes up. Enter the working directory. All your files will be stored in this directory. Also enter 64 for Total Workspace and 32 for Database.

Click on Run.

 

          

 

MODELING THE STRUCTURE

 

bullet

Go to the ANSYS Utility Menu.
bullet

Click Workplane>WP Settings.

bullet

The following window comes up

 

 

bullet

Check the Cartesian and Grid Only buttons.

bullet

Enter the values shown in the figure below.

 

bullet

Go to the ANSYS Main Menu Preprocessor>Modeling>Create>Areas>Rectangle>2 Corners.

bullet

The following window comes up:

 

 

 

 

bullet

Now we will pick the end points of the rectangles.

bullet

First make the steel rectangle of dimensions 5cm X 3 cm, i.e. 5 units by 3 units on the grid.

bullet

Next make the copper square of dimensions 1cm X 1cm.

bullet

Next make the aluminum part by making a rectangle of dimensions 5cm X 2cm and then creating two smaller rectangles, which can then be subtracted from the main part to make the fins.

bullet

From Preprocessor, choose Modeling>Operate>Boolean>Overlap>Areas.  Choose the Steel area and then the Copper area, then click OK.

bullet

From Preprocessor, choose Modeling>Operate>Boolean>Glue>Areas.  Choose the Steel area and then the Aluminum area, and then click OK.  The reason why we don’t glue the copper and the steel is that they overlap. Picture a copper plate resting on the steel area.  The steel and aluminum are connected more intimately, and must be glued together.

bullet

If you cannot see the complete workplane then go to Utility Menu>Plot Controls>Pan Zoom Rotate and zoom out to see the entire workplane.

bullet

The model should look like the one below.

 

 

MATERIAL PROPERTIES

 

bullet

We need to define material properties separately for steel, aluminum, and copper.   

bullet

Go to the ANSYS Main Menu

bullet

Click Preprocessor>Material Props>Material Models.  In the window that comes up choose Thermal>Conductivity>Isotropic

 

 

bullet

Enter 1 for the Material Property Number and click OK. The following window comes up.

 

 

bullet

Fill in 20 for Thermal conductivity. Click OK.

bullet

Now the material 1 has the properties defined in the above table. This represents the material properties for steel. Repeat the above steps to create material properties for aluminum (k=180, Material number 2), and copper (k=386, Material number 3).  Do this by selecting Material>New Model in the “Define Material Model Behavior” window.

 

ELEMENT PROPERTIES

 

bullet

SELECTING ELEMENT TYPE:

bullet

Click Preprocessor>Element Type>Add/Edit/Delete... In the 'Element Types' window that opens click on Add... The following window opens.

 

 

bullet

Type 1 in the Element type reference number.

bullet

Click on Thermal Mass Solid and select Quad 8node 77. Click OK. Close the 'Element types' window.

bullet

So now we have selected Element type 1 to be a thermal solid 8node element. The component will now be modeled with thermal solid 8node elements. This finishes the selection of element type.

 

MESHING

 

bullet

DIVIDING THE TOWER INTO ELEMENTS:

bullet

Go to Preprocessor>Meshing>Size Controls>Manual Size>Lines>All Lines. In the menu that comes up type 0.005 in the field for 'Element edge length'.

 

 

bullet

Click on OK. Now when you mesh the figure ANSYS will automatically create meshes that have an edge length of 0.005m along the lines you selected.

bullet

First we will mesh the steel area. Go to Preprocessor>Meshing>Mesh Attributes>Default Attributes. Make sure the window indicates "Material Ref.#1". The window is shown below.

 

 

bullet

Now go to Preprocessor>Meshing>Mesh>Areas>Free. Pick the steel area and click OK.

bullet

Repeat the same process for the aluminum and copper areas. Make sure you use the correct material number (2 and 3 respectively) for both the areas. Also since the steel and the copper areas overlap make sure you pick the right area. If you choose the wrong area, use Preprocessor>Meshing>Clear to undo the previous mesh and then repeat the previous steps. The meshed area should look like this:

 

 

BOUNDARY CONDITIONS AND CONSTRAINTS

 

bullet

Go to Preprocessor>Loads>Define Loads>Apply>Thermal>Heat Generate>On Keypoints.

bullet

Select the corners of the copper square. Click OK. The following window comes up.

 

 

bullet

Enter 10e6 for the HGEN value and click OK.

bullet

Go to Preprocessor>Loads>Define Loads>Apply>Thermal>Convection>On Lines. Pick all the lines on the outside of the object except the bottom one where the object is considered insulated. Click OK. The following window comes up.

 

 

bullet

Enter 50 for "Film Coefficient" and 20 for "Bulk Temperature" and click OK.

bullet

Now the Modeling of the problem is done.

 

SOLUTION

 

bullet

Go to ANSYS Main Menu>Solution>Analysis Type>New Analysis.

bullet

Select Steady State and click on OK.

bullet

Go to Solution>Solve>Current LS.

bullet

An error window may appear. Click OK on that window and ignore it.

bullet

Wait for ANSYS to solve the problem.

bullet

Click on OK and close the 'Information' window.

 

POST-PROCESSING

 

bullet

Listing the results.

bullet

Go to ANSYS Main Menu General Postprocessing>List Results>Nodal Solution. The following window will come up.

 

 

bullet

Select DOF solution and Temperature. Click on OK. The nodal displacements will be listed as follows.

 

 

bullet

You will find the maximum value of temperature at the end of the above table.

 

MODIFICATION

 

bullet

You can also plot the displacements and stress.

bullet

Go to General Postprocessing>Plot Results>Contour Plot>Nodal Solution. The following window will come up:

 

 

bullet

Select DOF solution and Temperature to be plotted and click OK.  The output will be like this:

 

 

 

Home Course Info Problems Test Problems Students Reference
Send mail to the Teaching Staff with questions or comments about this web site.