Introduction: In this example you will examinehydrodynamic boundary layer's in a flow over a flat plate .

Physical Problem: Compute and plot the velocity distribution of a flow of air over a flat plate.

Problem Description:

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

• Objective:

  • To plot the velocity profile on the plate.

• 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 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 (horizontal lines of the rectangle).

• 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 two vertical lines of the rectangle.

• 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 the first 2 input fields to Air-Si. Then click on OK.

•  Click OK in the next screen that appears.

BOUNDARY CONDITIONS AND CONSTRAINTS

• The boundary conditions in this problem are an imposed velocity over the plate, and the no-slip condition on the plate itself.

• To apply the imposed velocity, go to  Preprocessor>Loads>Define Loads>Apply>Fluid CFD>Velocity>On lines. Pick the left edge and the top edge 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 assumption that the velocity is equal to 0.5 far from the plate..

• To set the no-slip condition on the plate, repeat the above procedure but this time set the Velocity to ZERO for the bottom line of the rectangle.  (VX=VY=0). This time make sure 'Apply to endpoints' is set 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 Boundary Conditions are now set and should look like the picture below:

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 Global Iterations.  In this case the solution should converge at around 350 iterations. (this value was taken experimentally)  By setting the value at 400 we arrange the problem such that the solution is found before we reach the max number of Global Iterations)

• 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 that may appear.

POST-PROCESSING

• The first post-processing step we will show is how to plot 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):

• To get a plot of Velocity vs Y at a point x, you must define a path to plot along. The easiest way to do this is to use the vector plot from above, and zoom in on the section you want. In this example we will look at the boundary layer X velocity at x=.5m (half way along the plate).

• Select General Postproc>Path Operations>Define Path>By Nodes and pick 1 node at the bottom and 1 node near the top of the boundary layer (x=0.5) (nodes 27 and 2708 should work well). Then click OK:

• In the window that appears enter 'Center' as the name and then click OK.

• Now select General Postproc>Path Operations>Map onto Path and select X-component of velocity. In the User label for item box type in 'velocity':

• Now select General Postproc>Path Operations>Plot Path Item>On Graph , select VELOCITY, and click OK. You should get a plot that looks like this:

• Here is the same data in a standard format plotted using excel: