Carnegie Mellon

Mechanical Engineering

Self-paced learning on the Web
FEM/ANSYS

## F4 Car

Fluid #4: 3D Flow Over a Car USING FLOTRAN

Introduction: In this example you will model a car inside a wind tunnel.

Physical Problem: Compute and plot the velocity distribution in the wind tunnel shown in the figure.

Problem Description:

·         The shape of the car within the wind tunnel is shown in the figure.

Objective:
 To plot the velocity profile within the wind tunnel.

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

Figure:

Important Dimensions:

Keypoints to form the Car: (all dimensions are in meters)

 Pt X Y Z 1 1.4 0.4 4.5 2 1.4 0 4.5 3 2.1 0.4 4.5 4 2.1 0 4.5 5 1.2 0 3.5 6 1.2 0.8 3.5 7 2.3 0 3.5 8 2.3 0.8 3.5 9 1.2 0 2.5 10 1.2 0.8 2.5 11 2.3 0 2.5 12 2.3 0.8 2.5 13 1.3 0 1.75 14 1.3 0.4 1.75 15 2.2 0 1.75 16 2.2 0.4 1.75

Dimensions of the Block defining the Wind Tunnel:

The X and Y position of the corner of the block is (0,-1.8)

Width = 3.6 m

Height = 4 m

Depth = 10.25 m

The wind traveling over the car is going 24.6m/s. (or 55mph)

STARTING ANSYS

·         Click on ANSYS 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.

In this problem we will model the car, then model the wind tunnel around it, then subtract the volume of the car from the wind tunnel.  At this point we will then apply fluid flow to the wind tunnel and see how its flow is impeded due to the car.

·         Now, we will create the model.

·         Click Preprocessor>-Modeling-> and create the keypoints to define the car.

·         NOTE: It makes the creation of the car MUCH easier to go to the ANSYS Main Menu (the top bar) and select PlotCntrls>Pan Zoom Rotate and select the Isometric view (ISO).  This simply allows you a better view of the 3 dimensional keypoints forming the car.

·         Once the keypoints are finished, the model should look like the figure below.

·         Now that the keypoints have been created, connect them with lines to form the body of the car.

·         If any lines are created incorrectly, proceed to Preprocessor>Modeling>Delete>Lines Only to delete the incorrect line without deleting the keypoints forming it.

·         The car should now look like this:

·         Once the lines have been created, create Arbitrary Areas defined by Lines to form the outer shell of the car.

·         NOTE:  DO NOT FORM THE 2 VERTICAL AREAS WITHIN THE CAR.  This will only make creating the volume of the car much more difficult.

·         Once the areas defining the shape of the car are all created, define a volume by areas.  Since only the areas on the outside of the car have been created you may choose “PICK ALL” to select all the areas that make up the car and form them into a single volume.

·         If an error appears it is most likely because either an area was not selected (if you chose to do the selection by hand) OR an area was created within the volume unintentionally.  If this is the case, you need to go to Preprocessor>Modeling>Delete>Areas Only and delete the incorrect area.

·         Once the car volume is finished, create the Block surrounding it that will form the wind tunnel.

·         Now go to Preprocessor>Modeling>Operate>Booleans>Subtract>Volumes and select the wind tunnel block, then the car and click OK.  This now deletes the car volume and leaves a hollow space within the wind tunnel in the shape of the car.  The reason for this step is that the wind tunnel block will be defined as nothing but Air, so the volume that was removed (in the shape of the car) acts as an impedance for air (as it would in real life) and causes the deflection we desire to plot.

·         If you have done everything correctly the model should look like this: (in an isometric view)

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 3D Flotran 142. Click OK. Close the 'Element types' window.

·         So now we have selected Element type 1 to be a Flotran element. The component will now be modeled using the principles of fluid dynamics. This finishes the selection of element type.

DEFINE THE FLUID PROPERTIES:

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

·         On the box, shown below, make sure the first two input fields read AIR-SI, and then click on OK.  Another box will appear.  Click OK to accept the default values.

·         Now we’re ready to define the Material Properties

MATERIAL PROPERTIES

·         Go to the ANSYS Main Menu

·         Click Preprocessor>Material Props>Material Models. The following window will appear

·         As displayed, choose CFD>Density. The following window appears.

·         Fill in 1.23 to set the density of Air. Click OK.

·         Now choose CFD>Viscosity. The following window appears:

·         Fill in 1.79e-5 to set the viscosity of Air. Click OK

·         Now the Material 1 has the properties defined in the above table so the Material Models window may be closed.

MESHING:

DIVIDING THE CHANNEL INTO ELEMENTS:

·         Go to Preprocessor>Meshing>Size Cntrls>ManualSize>Lines>Picked lines. Now select all the lines that form the car and Click OK.  (NOTE: It will make selection much easier if you go to the ANSYS Main Menu (Top Bar) and select Plot>Lines.  This will allow you to view the lines that form the volume.) In the window that comes up type 0.05 in the field for 'Element edge length'.

·         Click on OK. Now return to Preprocessor>Meshing>Size Cntrls>ManualSize>Lines>Picked lines and select the edges of the block forming the wind tunnel around the car.

·         Set the ‘element edge length’ to 0.5.

·         Now when you mesh the figure ANSYS will automatically create a mesh, whose elements have a edge length of 0.05 m at the car, and slowly lengthen until they are approximately 0.5 m at the edge of the wind tunnel.  This is because the mesh should be finer at the car because that’s where we want a more precise analysis.

·         Now go to Preprocessor>Meshing>Mesh>Areas>Free. Click Pick All. The mesh will look like the following.

NOTE: The car is meshed safely inside the block.  Do not be alarmed that you can not see it.

BOUNDARY CONDITIONS AND CONSTRAINTS

·         Go to Preprocessor>Loads>Define Loads>Apply>Fluid CFD>Velocity>On Areas. Pick the area of the wind tunnel block facing the front of the car and Click OK. The following window comes up.

·         Enter -24.6 in the VZ value field and click OK. The -24.6 corresponds to the velocity of 24.6 meters per second of air flowing over the car.

·         Then, set the Velocity to ZERO along all of the axial sides of the block enclosing the car.  This is because of the “No Slip Condition” acting on the walls of the wind tunnel.  (VX=VY=0 for all sides)

·         Go to Main Menu>Preprocessor>Loads>Define Loads>Apply>Fluid CFD>Pressure DOF>On Areas.  Pick the area behind the car and click OK.

·         Enter 0 as the pressure value.  (This sets the pressure as atmospheric allowing the air to pass over the car)

·         Once all the Boundary Conditions have been applied, we can move on to solving the problem.

SOLUTION

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

·         The following window appears.  Change the first input field value to 25, as shown.  No other changes are needed.  Click OK.

·         Go to Solution>Run FLOTRAN.

·         Wait for ANSYS to solve the problem.

·         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 DOF Solution and Velocity VSUM and Click OK.

·                     This is what the solution should look like:

Despite what you may think this is the correct solution.  Now, in order to view the effects of the air flow on the car within the wind tunnel we must move the working plane so that it’s positioned along the longest axis of the car and tell ANSYS to show a cut away view.  This is how you accomplish that:

 First, go to the ANSYS Main Menu>WorkPlane and select Display Working Plane.  Now that the working plane is selected, go to ANSYS Main Menu>WorkPlane >Offset WP by Increments and adjust the working plane such that it sits along the long axis of the car.  When you are finished moving the plane it should look like this:

(NOTE: you can make sure it is properly positioned by selecting ANSYS Main Menu>PlotCntrls>Pan Zoom Rotate and changing the views to verify).

·         Once the plane is in line, select ANSYS Main Menu>PlotCntrls>Style…>Hidden Line Options..  a pop up window will now appear:

 In this window change “Type of Plot” to Q-Slice Z-buffer, and “Cutting Plane is” to Working Plane and click OK.  ANSYS will now display the results of the analysis with the working plane as the cutting plane. The final solution now looks like this:

·         Next, go to Main Menu>General Postproc>Plot Results>Vector Plot>Predefined. The following window will appear:

·         Select OK to accept the defaults.  This will display the vector plot of the velocity gradient.

Now that the solution is finished, the Workplane can be moved and different cut-away images of the velocity gradient can be plotted using the same method of moving the Workplane and setting the Hidden Line Options such that the cutting plane is the Workplane.

 Send mail to the Teaching Staff with questions or comments about this web site.