Introduction:

            Predicting the thermal behavior of a nano device requires accurate knowledge of the thermal properties such as thermal conductivity and heat capacity. Thermal properties of nano structures, on the other hand, change with size, fabrication method, impurity, etc and are usually smaller than the bulk values. Different techniques are used to measure the thermal properties of the think films. The steady state technique of a uniformly heated suspended bridge is used to measure the lateral thermal conductivity of the thin films. In this method, heat loss from the bridge surface should be found as part of the measurement. A 2-D heat conduction model may be used to predict the heat loss from the lower surface of the bridge to the substrate through the air gap. The rate of heat transfer changes with relative width of the bridge and the air gap.

 

Problem Description:

·         We are modeling 2D heat transfer from a long Aluminum bridge to a silicon substrate a distance of 5E-6 m apart. We will vary the length of the bridge and iterate the solution to determine the shape factor of the model.

·         All units are S.I.

·         Boundary Conditions:

1)     Temperature

·         Dimensions

            Bridge Width = 20 x 10^-6 m

            Bridge Length = 250 x 10^-6 m

            Gap Distance = 50 x 10^-6 m

·         Objective: Find the nodal distribution of the temperature between the aluminum bridge and the silicon substrate.

·         Figure:

Figure: The Fabricated suspended microbridge structure.

Figure: A front view of the suspended structure showing the separate distance d.

Figure: A schematic of the model that we will use in ANSYS, modeling the air in between the two plates as a solid with conductivity equal to air…

Basic Outline of the Problem:

Preprocessing:

1. Start ANSYS.

2. Create areas using keypoints and lines.

3. Define the material properties.

4. Define element type. (Quad 8node 77 element, which is a 2-D element for heat transfer analysis.)

5. Specify meshing controls / Mesh the areas to create nodes and elements.

Solution:

6. Specify boundary conditions.

7. Solve.

Postprocessing:

8. List the temperature results.

9. Plot the temperature distribution.

Exit:

10. Exit the ANSYS program, saving all data.

Starting ANSYS:

·         Click on ANSYS 6.1 in the programs menu.

·         Select Interactive.

·         The following menu comes up. Enter the working directory. All your files will be stored in this directory. Also under Use Default Memory Model make sure the values 64 for Total Workspace, and 32 for Database are entered.  To change these values unclick Use Default Memory Model.

·         Click RUN

Modeling the Structure:

·         Go to the ANSYS Utility Menu (the top bar). Click Workplane>WP Settings…

·         The following widow comes up: (notice the numbers are different)

·         Check the Cartesian and Grid Only buttons

·         Enter the values shown in the figure above. Click OK

·         Go to the ANSYS Utility Menu (the top bar). Click Workplane>Display Working Plane.

·         Use Utility Menu>PlotCtrls>Pan Zoom Rotate to display the grid as shown in the next step below. Note that you have to zoom in a lot to see anything at all!

·         Next, go to the ANSYS Main Menu (on the left hand side of the screen) and click Preprocessor>Modeling>Create>Keypoints>In Active CS.

·         The following window comes up:

·         Enter these points such that they make the shape as shown on the working plane after the next step. If you accidentally make two points with the same keypoint number, replot the keypoints, and you will see that ANSYS actually deleted your first point and that all points correspond to only one number each.

·         Now you have created the points to make the block. 

·         Now click Preprocessor>Modeling>Create>Lines>Lines>Straight Line.

·         A Window will now appear.  Connect the lines as shown in the figure, then Press OK to finish. It may be helpful to first make the long lines, then to use Pan-Zoom Rotatee to zoom in on the other keypoints. Then it becomes trivial to make those lines correctly. Zoom out afterward.

·         The model should look like this now: (note, you have a black background)

·         Now select Preprocessor>Modeling>Create>Areas>Arbitrary>By Lines.  A window will now appear on the left of the screen.

·         Create an area using all of the lines (remember, we have separate segments along the top because the middle segment is aluminum and the rest is just insulated area)

·         The final model should look like this:

Material Properties:

·         Now that we have built the model, material properties need to be defined such that ANSYS understands how heat travels through the air separating the two planes.

·         Go to the ANSYS Main Menu

·         Click Preprocessor>Material Props>Material Models.

·         The pop-up window will now look like this:

·         Choose Thermal>Conductivity>Isotropic.

·         The following window comes up:

·         Fill in 0.06 for Thermal conductivity. Click OK.  This is the average thermal conductivity air given our temperature range as explained in the graph below, referred from this website: users.wpi.edu/~ierardi/PDF/air_k_plot.pdf

·         Please note that if you were to solve this problem analytically, as you will in lab, you would not need the conductivity of air, because after a certain amount of time, the distribution will become constant, and it won’t matter how fast heat conducts through the medium. The same answer would arise if we used helium, etc.

·         Now exit the “Define Material Model Behavior” Window.

Element Properties:

·         Now that we’ve defined what material ANSYS will be analyzing, we have to define how ANSYS should analyze our block. 

·         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.

·         Now we have selected Element Type 1 to be a Thermal Solid 8node Element.

·         This finishes the section defining how the part is to be analyzed.

Meshing:

·         This section is responsible for telling ANSYS how to divide the block such that it has enough nodes, or points, to produce accurate results.

·         Go to Preprocessor>Meshing>Size Controls>Manual Size>Lines>All Lines. In the menu that comes up type 10e-7 in the field for ”Element edge length”.

·         Click on OK. Now when you mesh the figure ANSYS will automatically create square meshes that have an edge length of 10e-7m along the lines you selected.

·         Now go to Preprocessor>Meshing>Mesh Attributes>Default Attributes. The window is shown below:

·         This window appears such that the program knows you are sure that you have selected the right material to mesh (selected by the Element Type Number), and the right Material Number (1, as defined in the Material Properties section). Make sure that the window has the same selection, and then click OK and proceed to Preprocessor>Meshing>Mesh>Areas>Free

·         The block should now look like this when you are done meshing:

Boundary Conditions and Constraints:

·         Now that we have modeled the block and defined how ANSYS is to analyze the block we will apply the appropriate Boundary Conditions.  ANSYS refers to all Thermal Boundary Conditions under the Loads category, so remember that when looking for commands within the main menu…

·         Go to Preprocessor>Loads>Define Loads>Apply>Thermal (from here one can apply any of the loads, or Boundary Conditions, offered by ANSYS.)

Apply Constant Temperature

·         Select Temperature>On Lines.

·         A popup window will appear on the left hand side of the screen.  This window allows you to select the line you wish the load to be applied.

·         Click the first short line segment at the top left side of the block and then OK.

·         Enter 50 C in the popup window as the set temperature for the underside of the aluminum bridge:

·         Click OK and repeat the process to apply a uniform temperature of 20 C to the bottom of the component

The model will appear as follows:

Solution:

·         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.

Post-Processing:

·         This section is designed so that one can list the results of their analysis as a nodal solution

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

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

·         Within this window one can numerically find the maximum and minimum value of the temperature within the block.

Modification / Plotting the Results:

The last section displayed the numerical results, but most analyses will require a plot of the temperatures on the block in addition to the numerical results.  This is how you go about doing that…

First 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:

·         This is the Final Solution

·         Also, plot the flux

·         Postprocessing>Plot Results>Contour Plot>Nodal Solution

·         Choose Flux & Gradient and TFSum

·         Here is the plot. Record the max Flux for your records, in solving for the shape factor.

Iteration:

·         The next step is to take the information we have gathered on this first run, document it and then return to the boundary conditions step. Since you already know how to modify loads and such, I won’t explain those steps. However, for this tutorial, the model has been set up so that you don’t need to change any existing loads. The next step is to apply constant temperature to the next line segment that extends from the current Al bridge. The purpose of this step is that as you apply temperature to that line, you effectively increase the length of the Al bridge by the length of the segment. Here is a glimpse of that step.

·          

·         Once you have added the constant temperature of 50C to that new segment, continue from the Solution step of the tutorial, and find the steady state solution. The new plot looks exactly similar to the original. Continue iterating until you have added a temperature constraint to all the small segments. This will total up to 60 microns (and when taking into consideration the symmetry, means a bridge width that ranges from 20 microns to 120 microns).

Saving Projects

·         Simply go to Utility Menu>File>Save As… and save the project using the desired filename. To open the file later, run Interactive (the first thing explained in this tutorial) as usual, and when that is done, go to Utility Menu>File>Resume From… and choose the saved job from the directory it is saved in.