Introduction: In this example you will examine thermal and hydrodynamic boundary layer's in a heated flow over a flat, heated plate . We will deal with the cases where the plate has a constant temperature, a constant heat flux, and these two cases with an initial unheated region.

Physical Problem: Compute and plot the velocity and temperature distribution of a flow of air over a flat plate. Compare ANSYS resulst with theory.

Problem Description:

·     The plate is 1 meter in length and infinitely thin.. 

• Objective:

  • To plot the velocity profile on the plate.

  • To plot the temperature profile on the plate.

  • To repeat the problem with constant heat flux on the wall, and with unheated starting lengths.

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

• Dimensions:

  • The plate is 1 m long.

  • Theflow area is  1 m by .25 m.  This arbitrary size serves to set up the boundary conditions of air traveling over the plate.

  • The velocity of the air at infinite distance from the plate is 0.5 m/s.

  • Atmospheric pressure is assumed on all faces except the face where velocity is input into the system.

• Figure:

Basic Outline of the Problem:

Preprocessing:

1. Start ANSYS.

2. Create areas.

3. Define the material properties.

4. Define fluid element type. (2D Flotran 141 element, which is a 2-D element for fluid analysis.)

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

Solution:

6. Specify boundary conditions.

7. Specify number of solution iterations.

8. Solve.

Postprocessing:

9. Plot the contour plot of the velocity distribution.

10. Plot the velocity plot of the velocity distribution.

Exit:

11. Exit the ANSYS program, saving all data.

STARTING ANSYS

·         Click on ANSYS 8.1 in the programs menu.

MODELING THE STRUCTURE:

·         Go to the ANSYS Main Menu

·         Click Preprocessor>-Modeling->Create>Areas>Rectangle->By 2 Corners. The width is 1 and the height is .25. Starting position is at (0,0).

·         The modeling of the problem is done.

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 Flotran CFD and select 2D Flotran 141. Click OK. Close the Element types window.

·         So now we have selected Element type 1 to be solved using Flotran, the computational fluid dynamics portion of ANSYS. This finishes the selection of element type.

MESHING

DIVIDING THE CHANNEL INTO ELEMENTS:

• Go to Preprocessor>Meshing>Size Cntrls>ManualSize>Lines>Picked Lines. Select the top and bottom lines.

• In the window that comes up type 50 in the field for 'No. of element divisions'.

• Now Click OK. 

• Go to Preprocessor>Meshing>Size Cntrls>ManualSize>Lines>Picked Lines. Select the left and right lines.

• In the window that comes up type 100 in the field for 'No. of element divisions' and type 10 in the field for 'Spacing ratio'

• Now click OK

• Go to Preprocessor>Meshing>Size Cntrls>ManualSize>Lines>Flip Bias. Select the left line of the rectangle and click OK.

• Now go to Preprocessor>Meshing>Mesh>Areas>Free. Click the area and the OK.

• Since the only area we really care about is along the bottom wall, you will notice there is the highest concentration of elements there. This saves computation time because we don't have to compute accurate data for elements far away from the wall. You mesh should look like this:

Fluid Properties (air):

·         Go to Preprocessor>Flotran Set Up>Fluid Properties.

·         On the box, shown below, set all the input fields to Constant. Then click on OK.

• Another box will appear. Enter the values for Density, Viscocity, Conductivity, and Specific Heat for air at the mean temperature (Tw+Tinfin)/2 = 35C.

These values correspond to the following constant properties:

NOTE: If you want to use fluid's other than air use the same method and input the appropriate values:

BOUNDARY CONDITIONS AND CONSTRAINTS

• Go to  Preprocessor>Loads>Define Loads>Apply>Fluid CFD>Velocity>On lines. Pick the left and top edges of the rectangle and Click OK. The following window comes up.

• Enter 0.5 in the VX field and 0 in the VY and VZ fields. Make sure 'Apply to endpoints' is set to Yes. Then click OK. This number corresponds to the velocity of 0.5 meter per second of air flowing from the left side and the assumed velocity of 0.5 m/s far from the plate.

• Repeat the step above, this time setting the top of the rectangle velocity to ZERO. This time select 'Apply to endpoints'

• Repeat the above and set the Velocity to ZERO for the bottom of the rectangle.  (VX=VY=0). This is due to the no-slip condition along the wall. This time make sure 'Apply to endpoints' is set to Yes.

• Go to  Preprocessor>Loads>Define Loads>Apply>Thermal>Temperature>On lines. Pick the left edge of the rectangle and Click OK. The following window comes up. Enter 20 to apply a twenty degree celcius temperature to the incoming air. Set 'Apply TEMP to endpoints' to No.

• Repeat the above and set the Temperature to 50 along the bottom edge of the rectangle. Set 'Apply TEMP to endpoints' to Yes.

• Now Atmospheric Pressure must be set for the right side of the rectangle.

• To do this, select Preprocessor>Loads>Define Loads>Apply>Fluid CFD>Pressure DOF>On lines.  Click the right line and then OK.  The following window will now appear.

• Enter 0 for the constant pressure value for these faces and click OK.  This sets the pressure to Atmospheric.

• Now the Modeling of the problem is done. The loads on the model will look like this (To get a screen like this, goto Plot->Lines on the main menu):

SOLUTION

• Go to ANSYS Main Menu>Solution>Flotran Set Up>Execution Ctrl.

·         The following window appears.  Change the first input field value to 400, as shown.  No other changes are needed.  Click OK.  (The reason behind setting the iterations so high is that when you run the Flotran Analysis, it stops only when the solution converges, or the solution reaches the number of iterations.  In this case the solution should converge at around 500 iterations. (this value was taken experimentally)  By setting the value at 250 we arrange the problem such that the solution is found before we terminate the iterations.)

• Go to ANSYS Main Menu>Solution>Flotran Set Up>Solution Options

• Change the TEMP field to Thermal and then click OK

• Go to Solution>Run FLOTRAN.

• Wait for ANSYS to solve the problem. It takes around a minute to solve on a fast computer. It will say 'Solution is Done!' when it completes.

• Click on OK and close the 'Information' window.

POST-PROCESSING

• Plotting the velocity distribution…

• Go to General Postproc>Read Results>Last Set.

• Then go to General Postproc>Plot Results>Contour Plot>Nodal Solution. The following window appears:

• Select VSUM and click OK. The velocity distribution will look like this:

• Now go to General Postproc>Plot Results>Vector Plot>Predefined and select Velocity. Enter a scale factor (VRATIO) of 0.4. The vector plot looks like this:

• and a zoomed in portion (notice boundary layer formation):

• Then go to General Postproc>Plot Results>Contour Plot>Nodal Solution and select Temperature:

• A Plot of the Heat flux along the plate looks like this (NOTE: in order to get this plot, you must define a path along the bottom edge of the rectangle and map Heat Flux onto it). We will use this data to get local Nusselt Numbers:

• Comparing the boundary layer thickness to theoretical equations, the correlation is apparent: (download this excel worksheet)

Constant Heat Flux:

• The results for a constant heat flux of 300 W/m² are shown below. The procedure for this problem is exactly the same as the constant wall temperature, except when defining loads, the wall temperatures are replaced with constant heat flux:

• Temperature Distribution:

Unheated Starting Length Constant Wall Temperature:

• The modeling for an unheated starting length is slightly different from the above example. Assume an unheated starting length of 0.25 m, a heated length of 0.5 m, and again an unheated region of 0.25 m and a constant wall temperature of 50 C. All other parameters are the same.

• Instead of creating 1 rectangle for the model, we will create 3 connected rectangles like this (the first rectangle represents the initial unheated region of .25 m. The second rectangle is the .5 m heated region. The third rectangle is the 2nd .25 m unheated region):

• After creating these three areas, you must glue the connecting lines together. Go to Preprocessor>-Modeling->Operate>Booleans>Glue>Areas  and select the three areas. Click OK.

• Meshing this model is slightly different to get the same results. For the top and bottom lines you must select an 'Element edge length' of 0.2. The three vertical lines get the same 50 element divisions with a ration of 10. Make sure to use flip bias on any meshed lines with a ratio that are backwards. Your meshed lines will now look like this:

• Goto Preprocessor>Meshing>Mesh>Areas>Free and the meshed area will look like this:

• The loading of the problem is exactly the same as before. The Loads will look like this:

• Solving the problem gives the following temperature distribution:

Unheated Starting Length Constant Wall Heat Flux:

• Assume the same configuration as the previous problem, except this time the wall condition is a constant heat flux of 300 W/m2. All other parameters are the same.

• The modeling procedure is the same as the unheated starting length constant wall temperature problem above, except the contant temperature loading is replaced with constant heat flux loading.

• Temperature Distribution: