The slab is made of material with density 5000 kg/m3. Its specific heat is 200 J/Kg K, and thermal conductivity is 5 W/m K.

The bulk temperature on the right of the slab is 293K, and the Film Coefficient is 100 W/m2K.

On the left side the temperature on the boundary is 773K.

Units: Use S.I. units ONLY

Geometry: The hole in the center has a radius of 1cm. The hole is located at the center of the slab. See figure for the rest of the dimensions.

Boundary conditions: There is convection along the side walls. The top and the bottom walls are insulated. The initial temperature of the slab is 293K throughout.

Objective:

	To plot the temperature field in the slab 50 seconds after the boundary conditions have been suddenly applied to the slab.
	To animate the temperature field to see how it develops as time elapses.

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

Figure:

IMPORTANT: Convert all dimensions and forces into SI units.

Click on ANSYS 6.1 in 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.

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 above.

Go to the ANSYS Main Menu and click Preprocessor>Modeling>Create>Area>Rectangle>By 2 Corners

The following window comes up:

Now we will pick the end points of the rectangles.

First make the outer rectangle of dimensions 15 cm X 5 cm (30 X 10 units on the grid).

Now got to Preprocessor>Modeling>Create>Area>Circle>Solid Circle. Create a circle of radius 1cm and with center at the center of the rectangle.

Now go to Preprocessor>Modeling>Operate>Booleans>Subtract>Areas, and subtract the circle from the rectangle by choosing the rectangle first, then the circle.

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.

The model should look like the one below:

We need to define material properties separately for steel, and the insulation material.   

Go to the ANSYS Main Menu and click Preprocessor>Material Props>Material Models.  In the window that comes up choose Density. Put in 5000 for density.  From the same window choose Thermal>Specific Heat and enter 200.  From the same window choose Thermal>Conductivity>Isotropic and enter 5 for the thermal conductivity.  The following windows will appear as follows:

Fill in the appropriate values as shown in the figure above. Click OK.

Now the material 1 has the properties defined in the above table. This represents the material of the slab.

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 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 WALL INTO ELEMENTS:

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'.

Click on OK. Now when you mesh the figure ANSYS will automatically create a mesh, whose elements have a edge length of 0.005m along the lines you selected.

Now go to Preprocessor>Meshing>Mesh>Areas>Free. Pick the slab area and click OK. The meshed slab look like the following:

Go to  Preprocessor>Loads>Define Load>Apply>Thermal>Convection>On Lines. Pick the right line along the outer boundary. Click OK. The following window comes up.

Enter 100 for "Film Coefficient" and 293 for "Bulk Temperature" and click OK.

Go to Preprocessor>Loads>Define Load>Apply>Thermal>Temperature>On Lines. Pick the left line along the outer boundary. The following window comes up.

Enter the value of the boundary temperature on the left edge of 773 K.

Now the Modeling of the problem is done.

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

Select Transient"and click on OK, then select Full in the window that comes up.

Go to Main Menu>Solution>Load Step Opts>Time/Frequency>Time-Time Step.

The following window comes up:

Fill in the values as shown and click OK.

Now click Solution>Load Step Options>Output Controls>Solution Printout.

The following window comes up. Enter the values as shown and click OK.

Now click Solution>Load Step Options>Output Controls>DB/Results File.

The following window comes up. Enter the values as shown and click OK.

Now go to Solution>Define Loads>Settings>Reference Temp.

The following window comes up. Fill in the values shown and click OK.

Go to Solution>Define Loads>Apply>Thermal>Temperature>Uniform Temperature.

The following window comes up. Enter the values as shown and click OK.

Now go to Solution>Solve>Current LS.

Wait for the solution to get done.

Close the "Stat Command" window.

Now the solution is done.

Plotting the temperature field after 50 secs.

Go to ANSYS Main Menu and click on General Postprocessing>Read Results>By Load Step. The following window will come up.

Enter values as shown and click OK.

Now go to General Postprocessing>Plot Results>Contour Plot>Nodal Solution.

The following window comes up. Enter the values as shown and click OK.

The temperature distribution looks something like the plot below.

Animating the development of the temperature field

Go to Utility Menu>Plot Controls>Animate>Over Time. The following window comes up. Enter the values as shown and click OK:

Click below to take a look at the animation.

Temperature field animation