Carnegie Mellon

Mechanical Engineering

Self-paced learning on the Web
FEM/ANSYS

## T2 Composite Wall

Thermal #2: Heat flux analysis of a composite modular wall

Introduction: In this example you will determine the heat flux through the composite modular wall shown in the figure.

Physical Problem: A composite wall is widely used in cold places to insulate buildings from the cold outside surroundings. It typically consists of insulating material packed inside a wall. The insulating material is usually in two layers and is staggered. In this problem we will model a section of such a wall and determine the heat flux through the wall. This gives an estimate of the amount of heat that needs to be supplied to maintain the room temperature.

Problem Description:

The outer material of the composite wall is steel with thermal conductivity of 20 W/m K

The insulating material has a thermal conductivity of 0.1 W/m K.

Units: Use S.I. units ONLY

Geometry: See figure.

Boundary Conditions: The bulk temperature on the left of the wall is 220K, and the Film Coefficient is 200 W/m2K. On the right side the bulk temperature is 300K, and the Film Coefficient is 20 W/m2K.

Objective:
 To determine the heat flux through the given length of the wall. To plot the temperature distribution. To generate the vector plot of the heat flux.

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

Figure:

 IMPORTANT: Convert all dimensions and forces into SI units.

STARTING ANSYS

 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.

MODELING THE STRUCTURE

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 5.25 cm X 6.75 cm, i.e. 42 units by 54 units on the grid. Similarly make the other rectangles. Click on Preprocessor>Modeling>Operate>Booleans>Overlap>Areas.  For each separate insulation area, first select the steel area, then select the particular insulation area. If you cannot see the complete workplane then go to Utility Menu>PlotCntrls>Pan Zoom Rotate and zoom out to see the entire The model should look like the one below:

MATERIAL PROPERTIES

 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 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 properties defined in the above table. This represents the material properties for steel. Click Material>New Model in the Define Material Behavior Window to define properties for material 2. Repeat the above steps to create material properties for the insulation (k=0.1 W/m K).

ELEMENT PROPERTIES

 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.

MESHING:

 DIVIDING THE WALL INTO ELEMENTS: Go to Preprocessor>Meshing>Size Controls>Manual Size>Lines>All Lines. In the menu that comes up type 0.0025 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 an edge length of 0.0025m 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".  This function tells Ansys which material is being used while you perform meshing functions. The window is shown below:

 Now go to Preprocessor>Meshing>Mesh>Areas>Free. Pick the steel area and click OK. Repeat the same process for the insulation areas. Make sure you use the correct material number (number 2) for the insulation areas. Also since the steel and the insulation 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 will look like this:

BOUNDARY CONDITIONS AND CONSTRAINTS

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

 Enter 200 for "Film Coefficient" and 220 for "Bulk Temperature" and click OK. Repeat the above for the right side of the wall. (VALI=20, VAL2I=300) Now the Modeling of the problem is done.

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

 Listing the results. Go to ANSYS Main Menu and click on 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:

 The maximum value of temperature is given at the end of the above table

MODIFICATION

 You can also plot the temperature distribution for this steady state case. 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:

 For the vector plot go to Main Menu>General Postprocessing>Plot Results>Vector Plot>Predefined. The following window comes up:

 Select Flux & Gradient and Thermal flux ad click OK. The plot looks like the following picture. Notice that the maximum heat flux occurs along the steel material that is horizontal and closer to the right wall.