Introduction: In this example laminar fluid flows over an angled flate plate

Physical Problem: Compute and plot the velocity distribution of a flow

Problem Description:

• Objective:

  • To plot the velocity profile

• Dimensions:

  • The duct has an entrance region of 1m by .5m and an exit region of 1m by 1m. These two regions are seperated by a horizontal distance of 1m.

  • The velocity of the air at infinite distance from the plate is 3 mm/s (.003m/s). This velocity best demonstrates the recirculation zone while keeping the flow inside the duct laminar.

• 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 5.6 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 Main Menu

• To create the entrance region click Preprocessor>Modeling>Create>Areas>Rectangle>By 2 Corners. The width is 1 and the height is .5. Starting position is at (0,0).

• To create the exit region click Preprocessor>Modeling>Create>Areas>Rectangle>By 2 Corners. The width is 1 and the height is 1. Starting position is at (2,0).

• To create the connecting region, click Preprocessor>Modeling>Create>Areas>Arbitrary>Through KPs. Select the four keypoints that make up the region and click OK. The area will be created automatically:

• Modeling is now 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

• To clarify meshing you should plot by lines. To do this click Plot>Lines on the file menu.

• Go to Preprocessor>Meshing>Size Cntrls>ManualSize>Lines>Picked Lines. Select the four vertical lines and click OK

• In the window that comes up type 20 in the 'Element edge length' box and -2 in the Spacing Ratio box. This puts more elements near the walls than in the middle:

• Now Click OK. 

• Now go to Preprocessor>Meshing>Size Cntrls>ManualSize>Lines>Picked Lines and select the top and bottom lines of the entrance and exit region:

• Enter 15 for the number of element divisions, and enter 1 for the Spacing Ratio.

• Now go to Preprocessor>Meshing>Size Cntrls>ManualSize>Lines>Picked Lines and select the top and bottom of the transition region. Enter 20 for the number of element divisions, and 1 for the Spacing Ratio. Click OK.

• Now go to Preprocessor>Meshing>Mesh>Areas>Free. Click the three area's or click 'Pick All' and then OK.

• Meshing is done. Your mesh should look like this:

Fluid Properties (air):

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

• On the box, shown below, set the first two input fields to Air-SI. Then click on OK.

BOUNDARY CONDITIONS AND CONSTRAINTS

• To make loading easier, go to Plot>Lines on the main file menu.

• Go to  Preprocessor>Loads>Define Loads>Apply>Fluid CFD>Velocity>On lines. Pick the left line of the entrance region and Click OK:

• Enter 0.003 in the VX field and 0 in the VY. Leave VZ blank. Then click OK. This number corresponds to the velocity of 0.003 meter per second of air flowing from the left side:

• The walls of the duct are stationary and therefore must have the no-slip condition applied to them. To set this go to Preprocessor>Loads>Define Loads>Apply>Fluid CFD>Velocity>On lines. and select the lines that make up the walls of the duct. There are 6 of them:

• Click OK. In the window that appears set VX = 0 and VY = 0. Leave VZ blank.

• The last step is to apply atmospheric pressure to the outlet of the duct. Go to Preprocessor>Loads>Define Loads>Apply>Fluid CFD>Pressure DOF>On Lines and select the right most vertical line and click OK. In the window that appears, enter 0 for the constant pressure value and click OK:

• Now the Modeling of the problem is done. The loads on the model will look like this:

SOLUTION

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

·         The following window appears.  Change the first input field value to 1000, as shown.  No other changes are needed.  Click OK.

• Go to Solution>Run FLOTRAN.

• Wait for ANSYS to solve the problem.

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. The vector plot looks like this:

• To view the recirculation zone in more detail it helps to animate the results. To do this go to General Postproc>Plot Results>Def Trace Pt. Select a few nodes in the entrance region (1) and select a few nodes in the recirculation region (2). Then click OK:

• Now go to PlotCtrls>Animate>Particle Flow... Select VX. The other default options are fine. Click OK

• ANSYS will then animate the flow. It will look similar to this (notice the recirculation region):