Carnegie Mellon

Mechanical Engineering

Self-paced learning on the Web
FEM/ANSYS

F5 Mountain Range

Fluid #5: Predicting the Weather Using 3D Flow

Introduction: In this example you will model a mountain range with a given wind velocity over it.

Physical Problem: Compute and plot the velocity and pressure distribution of the air over the mountain.

Problem Description:

·         Air at a given velocity travels over the Rocky Mountains into Denver Colorado.  As a result, this 3D flow then alters the pressure around the city in some distribution.  This pressure distribution in turn determines the weather patterns around the city.  The objective of this problem is to show that distribution.

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

(Aerial View of the Rocky Mountains near Denver Colorado)

Important Dimensions: (Everything is decreased by a factor of 1000 to scale the problem down)

The cube of air over the mountains measures 10mX10mX10m.

The mountains are positioned at these points, with radii as listed:  (assuming what was the XY Plane is now the XZ

plane as it has been rotated)

**Note: The peak height of the rocky mountains is 4,346 m.

(2.5,2.5)

depth:   -4.346

(5.0,3.0)

depth:   -3.7

The wind traveling over the mountains is going 0.013 m/s. (approx 30mph in real life)

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 mountain range, then model the wind around it, then subtract the volume of the mountains from the block of air.  At this point we will then apply fluid flow to the air over the mountains and see how its flow is impeded due to the shape of the “Rocky Mountains.”

·         Now, we will create the model.

·         Click Preprocessor>-Modeling-> and create the volume to define the air around the mountains.

·         NOTE: It makes the creation of the mountain range 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 volumes as you form them.

·         Once the outer volume is finished, rotate the working plane 90° along the X axis such that it’s situated at the base of the cube.

·         Once the plane is in place, create the 2 Conic Volumes ”By Picking”.

·         Enter the values given in the problem description for each Cone position and dimensions.

·         Once the cones have been created, go to Preprocessor>Modeling>Operate>Boolean>Add and add the volumes such that both cones become one volume.

·         This volume is then to be subtracted from the bigger cube such that the space where the mountains would be is now an empty volume.  This is because the large cube is defined as a section of air around the mountain range.  This air never penetrates the mountain, so the volume of air is represented as a large cube with the mountain section removed.

·         At this point, the finished model should look like this: (If you plot lines, not volumes)

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>All lines.

·         In the window that comes up type 15 in the field for 'No. of element divisions'.

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

NOTE: The mountains are meshed safely inside the block.  Do not be alarmed that you can not see them.

BOUNDARY CONDITIONS AND CONSTRAINTS

1.       Go to Preprocessor>Loads>Define Loads>Apply>Fluid CFD>Velocity>On Areas. Pick the area of the square that forms the XY plane intersecting with the origin and Click OK. The following window comes up.

·         Enter 0.013 in the VZ value field and click OK. The 0.013 corresponds to the velocity of 13 meters per second of air flowing over the mountains scaled down by 1000.

·         Then, set the Velocity to ZERO along all of the areas defining the mountains and the ground.  This is because of the “No Slip Condition” acting on those surfaces.  (VX=VY=0 for all sides)

·         Go to Main Menu>Preprocessor>Loads>Define Loads>Apply>Fluid CFD>Pressure DOF>On Areas.  Pick the areas without previously defined boundary conditions (ie: the Top, Sides, and face opposite the face with the velocity applied) and click OK.

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

·         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 10, 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 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 mountains within the block of air we must move the working plane so that it’s positioned along the Z axis and tell ANSYS to show a cut away view using the workplane as it’s cutting plane.  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 intersects a section of one of the mountains.  When you are finished moving the plane it should look like this: (in TOP view after plotting Lines)

(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.

In this particular problem, however, note the velocity distribution as it effects pressure.  Due to the air flow, a low pressure zone is created on the opposite side of the mountain range.  If this situation actually occurred, this low pressure zone in turn would then influence the weather and cause some sort effect on the atmosphere around the city of Denver.   Therefore, it is important to realize that ANSYS’ capabilities are not limited to small scale items, and the world around us demonstrates many of the same phenomena that we study on a day to day basis as engineers.