ntroduction: In this example laminar fluid flow over an infinite cylinder.

Physical Problem: Compute and plot the velocity distribution of a flow of air over an infinite cylinder.

Problem Description:

• Objective:

  • To plot the velocity profile

• Dimensions:

  • The cylinder is .25 m in diameter

  • Because of symmetry, the problem is simplified so that only half of the cylinder is computed. The results are assumed to be the same on the other side of the x axis (axis of symmetry)

  • The flow area is  2 m by 0.5 m.  This arbitrary size serves to set up the boundary conditions of flow over a cylinder.

  • The velocity of the air at infinite distance from the plate is 5 mm/s (.005m/s).

• 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

• Click Preprocessor>Modeling>Create>Areas>Rectangle>By 2 Corners. The width is 2 and the height is .5. Starting position is at (0,0).

• To create the cylinder click Preprocessor>Modeling>Create>Areas>Circle>Solid Circle. The radius is .125 and the center is at (.5,0)

• To subtract the circular area from the rectangle click Preprocessor>Modeling>Operate>Booleans>Subtract>Areas. Select the rectangle and click OK. Next select the circle and click Ok. You will be left with this area:

• 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

DIVIDING THE CHANNEL INTO ELEMENTS:

• Go to Preprocessor>Meshing>Size Cntrls>ManualSize>Lines>Picked Lines. Click 'Pick all' or manually pick all the lines

• In the window that comes up type .02 in the 'Element edge length' box:

• Now Click OK. 

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

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 and top edge of the rectangle and Click OK:

• Enter 0.005 in the VX field and 0 in the VY. Leave VZ blank. Then click OK. This number corresponds to the velocity of 0.005 meter per second of air flowing from the left side:

• To account for symmetry, the normal component to the axis of symmetry is set to zero. To set this go to Preprocessor>Loads>Define Loads>Apply>Fluid CFD>Velocity>On lines. and select the bottom line of the rectangle. Enter 0 in the VY field. Leave VX and VZ blank.

• Repeat the above and set the Velocity to ZERO for the 2 lines that make up the half-circle.  (VX=VY=0, VZ can be left blank). This is due to the no-slip condition along the cylinder. Your screen should look like this so far:

• The last step is to apply atmospheric pressure to the outlet of the fluid region. 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):