The heat sink is a cooling component adhered to an electronic device. For the sake of simplicity we assume that the device can be modeled as a rectangular block. This block, made of steel, contains a cylindrical copper rod of thermal conductivity 386 W/m-K that generates a total Q = 27.2 W. Also, the block loses heat through the bottom, totaling 20% of the heat generated (20% of the total Q).

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

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

Units: Use S.I. units ONLY

Geometry: See figure.

Boundary conditions: There is convection along all boundaries of the fin assembly except the bottom, which is attached to the electronic component. The Film Coefficient is 20 W/m²K and the Bulk (ambient) temperature is 20^oC. The block is insulated on the sides but loses some heat through its bottom.

Objective:

	To determine the nodal temperature distribution
	To determine the heat flux throughout the component
	To determine the maximum value of temperature in the component.

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

Figure:

Go to the ANSYS Utility Menu.

	Click Workplane>WP Settings.
	The following window comes up

Check the Cartesian and Grid Only buttons.

Enter the values shown in the figure. Hit OK.

In this tutorial we will explore the use of creating areas by corners as well as copying those areas to accomplish modeling more efficiently.

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

The following window comes up:

Enter the values above to create the base plate of the fin assembly (Aluminum base plate) and hit OK.

Next, we want to create the fins that will constitute the assembly. Use Create Area by 2 Corner again to create the first fin.

The next step is to populate the assembly with these fins. This can be accomplished by using the copy function

Choose Preprocessor>Modeling>Copy>Areas Choose the fin area and hit OK in the dialog window. Fill in the following values for the offset:

Repeat the process and choose the newest area. This way you can continue using an offset of 7mm (add the fin thickness for 0.007+0.002 = .009). When finished with all fins, continue.

The model should look like the following:

Choose Preprocessor>Modeling>Operate>Booleans>Add>Areas.  Choose PickAll. It will be on the bottom of the dialog window, and might be cut off if the window is too close to the bottom of the screen. Either move the window or just manually select all the lines. Hit OK

This is what your assembly should look like now. Note that the lines are gone separating the areas and that it is all one piece now.

To model the block, the electronic component, use create area>rectangle by 2 corners again. Remember its dimensions are 56mm x 45mm. This is similar to the first steps you made in making the fin assembly. If you want to build downward, use negative values. (refer to the solid circular area below for an example of negative values)

Also, create the heat source area using

This is what everything looks like now.

The next step is to glue the base block to the fin assembly and to use the overlap function to make the heat generating element separate from the block. When you first create areas within areas, the original larger area still spans the entire space. Overlap breaks the pieces into separate sections.

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.

Now, choose Preprocessor>Modeling>Operate>Booleans>Glue>Areas and select the fin assembly and the base. Hit OK

Now, choose Preprocessor>Modeling>Operate>Booleans>Overlap>Areas and select the block and the copper rod. Hit OK

The modeling is now finished.

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

Go to the ANSYS Main Menu

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

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

Fill in 20 for Thermal conductivity. Click OK.

Now the material 1 has the property defined in the above window. This represents the material property 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 first selecting Material>New Model in the “Define Material Model Behavior” window.

SELECTING ELEMENT TYPE:

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

Type 1 in the Element type reference number.

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

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.

DIVIDING THE TOWER INTO ELEMENTS:

Go to Preprocessor>Meshing>Size Controls>Manual Size>Lines>All Lines. In the menu that comes up type 0.0015 in the field for 'Element edge length'.

Click on OK. Now when you mesh the figure ANSYS will automatically create meshes that have an edge length of 0.0015m along the lines you selected.

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

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

When you mesh the area, the other areas may disappear. They are still there, ANSYS is just not displaying them, as usual. Just go to Utility>Plot>Areas to see the areas again.. And even though the mesh on the area you just meshed doesn’t show.. it is also still there.

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. If you mesh the wrong area, use Preprocessor>Meshing>Clear to select the erroneous mesh, delete it, and then repeat the previous steps. The meshed area should look like this:

Go to Preprocessor>Loads>Define Loads>Apply>Thermal>Heat Generate>On Areas

Select the quadrants of the copper rod. Click OK. The following window comes up.

Since the volume of the rod is 9.19e-6 and the total Q = 27.2 W, heat generation is 2.96MW/m³.

Enter the value for the HGEN value and click OK.

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 connected to the block. Remember to pick the small lines on the size of the assembly that were part of the mock base of the assembly. Click OK. The following window comes up.

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

Choose Preprocessor>Loads>Define Loads>

Pick the bottom of the rectangular block. Click OK. The following window comes up.

Now add heat loss through the bottom of the model, which has a surface area of .007224m²

Given that the heat lost from the base is 5.44 W, the heat flux will be -753.045 W/m²

Enter the value for heat lost through the bottom of the component.

Now the Modeling of the problem is done.

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

Select Steady State and click on OK.

Go to Solution>Solve>Current LS.

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

Wait for ANSYS to solve the problem.

Click on OK and close the 'Information' window.

Listing the results.

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

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

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

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

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

Repeat the step, this time selecting Flux & gradient and TFSum to be plotted and click OK.  The output will be like this: