Introduction:

            In this example you will model fluid flow in the entrance region

            between two infinite plates with constant wall and fluid temperatures.

Problem Description:

·         Air at 100 degrees Celsius travels between two infinite plates.  For the sake of modeling, these plates will be assumed to be 1.5 m long and 5 cm apart.

·         All units are S.I.

·         Boundary Conditions:

            1) Air enters between the plates at a uniform velocity of 0.1 m/s and 20 degrees

            Celsius.

            2.) The wall temperature is 100 degrees Celsius

·         Material Properties: AIR-SI

·         Dimensions

            Length = 1.5 m

            Width = 0.05 m

·         Objective: Find the nodal velocity distribution within the air gap between the two plates. Compare that to the temperature distribution between the two plates.

·         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 iterations for the solution.

8. Solve.

Postprocessing:

9. Plot the contour plot of the velocity distribution.

10. Plot the contour plot of the temperature distribution.

11. Plot the vector plot of the velocity distribution.

Exit:

12. Exit the ANSYS program, saving all data.

Starting ANSYS:

·         Click on ANSYS 6.1 in the programs menu.

·         Select Interactive.

·         The following menu comes up. Enter the working directory. All your files will be stored in this directory. Also under Use Default Memory Model make sure the values 64 for Total Workspace, and 32 for Database are entered.  To change these values unclick Use Default Memory Model.

·         Click RUN

Modeling the Structure:

·         Go to the ANSYS Main Menu (on the left hand side of the screen) and click Preprocessor>Modeling>Create>Areas>Rectangle>By 2 Corners.

·         The following window comes up:

·         Click OK once the proper values have been entered.

·         The model should look like this now: (note, you have a black background)

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 a Flotran element. The component will now be modeled using the principles of fluid dynamics. This finishes the selection of element type.

Fluid Properties (air):

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

·         On the box, shown below, set all the input fields to Constant. Then click on OK.

• Another box will appear. Enter the values for Density, Viscocity, Conductivity, and Specific Heat for air at the mean temperature (Tw+Tinfin)/2 = 35C.

These values correspond to the following constant properties:

NOTE: If you want to use fluid's other than air use the following procedure for setting fluid properties:

Fluid Properties (any fluid with constant properties):

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

·         In the box that appears, set all the input fields to Constant. Then click on OK.

·         Another box will appear. Enter the values for Density, Viscocity, Conductivity, and Specific Heat for the fluid you are working with.

Here are the properties of nitrogen gas (N2) as an example:

·         Click Ok. Now your fluid properties are set. Continue solving the problem as usual.

Meshing:

·         This section is responsible for telling ANSYS how to divide the block such that it has enough nodes, or points, to produce accurate results.

·         Go to Preprocessor>Meshing>Size Controls>Manual Size>Lines>Picked Lines. Select the top and bottom lines of the rectangle and click OK.  In the menu that comes up type 100 in the field for 'No. of element divisions'. Then click OK.

·        Repeat the same procedure for the left and right lines, except enter 50 into the 'No element divisions' field.

·         Now go to Preprocessor>Meshing>Mesh Attributes>Default Attributes. The window is shown below:

·         Make sure that the window matches the one above, click OK, and proceed to Preprocessor>Meshing>Mesh>Areas>Free

·         A popup window will appear on the left hand side of the screen.  This window allows you to select the area to be meshed.  Click within the rectangle you created before and click OK.

·         Your mesh will now look like this (it's hard to see the individual elements, but if you zoom in they are easy to see):

Boundary Conditions and Constraints:

• Go to  Preprocessor>Loads>Define Loads>Apply>Fluid CFD>Velocity>On lines. Pick the left edge block and Click OK. The following window comes up.

• Enter 0.1 in the VX value field and click OK. The 0.1 corresponds to the velocity of 0.1 meters per second of air flowing from the left side.

• Repeat the above and set the Velocity to ZERO for the air along all of the top and bottom edges.  This is due to the no slip condition.  (VX=VY=0 for all sides)

• Go to Main Menu>Preprocessor>Loads>Define Loads>Apply>Fluid  CFD>Pressure DOF>On Lines.  Pick the right side of the block and click OK.  This signifies the open end of the pipe.

• Apply the temperature boundary conditions. Go to Main Menu>Preprocessor>Loads>Define Loads>Apply>Thermal>Temperature>On Lines. Select the left side and enter 20.

• Repeat the above and set the temperature to 100 along the top and bottom edges. This is due to the constant wall temperature.

• NOTE: If you wanted to apply constant heat flux instead of constant wall temperature, you would goto Main Menu>Preprocessor>Loads>Define Loads>Apply>Thermal>Heat Flux>On Lines instead of  Apply>Thermal>Temperature in the steps above.

• Once all the Boundary Conditions have been applied, the boundary conditions on the plates should look like this:

·         Now the Modeling of the problem is done.

SOLUTION

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

·         The following window appears.  Change Adiabatic to Thermal in the drop down menu.  No other changes are needed.  Click OK.

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

·         The following window appears.  Change the first input field value to 300, 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 DOF Solution and Velocity VSUM and Click OK.

·                     This is what the solution should look like:

• Plotting the temperature distribution…

• Then go to General Postproc>Plot Results>Contour Plot>Nodal Solution. The following window appears:

·                     Select DOF Solution and Temperature TEMP and Click OK.

·                     This is what the solution should look like:

• a closeup of the entrance region:

·         Now go to General Postproc>Plot Results>Vector Plot>Predefined. The following window will appear:

·         Enter the values as shown and click OK. The plot of velocities will appear. Zoom in to examine different velocity profiles.

• Here is the Entrance region:

• Here is the fully developed exit region:

Local Nusselt Number Extraction:

There is no direct way to extract nusselt numbers from ansys, however it is still possible to calculate these number's using the results of the simulation. Remember from Newton's Law of Cooling that:

and from heat transfer:

Using these two relations we can get Nu using heat flux (q") values from ANSYS. The details of this procedure are beyond the scope of this tutorial. However, it requires defining a path along the wall and extracting n heat flux values along it. At each n points, you must take the average temperature (Tm) between the two plates. The other values are known from the problem statement: Hydraulic diameter (Dh) is twice the distance between the two plates. Thermal conductivity (K) is a property of air and Tw is the constant wall temperature.

·        The results of this procedure are available as an excel spreadsheet for you to download. The results of a constant wall temp and constant heat flux are graphed, and reproduced here. Notice how the Nusselt number approaches a constant value in the fully developed flow region.

Constant Wall Heat Flux:

If the same problem is repeated, but this time with constant heat flux boundary conditions of 200 W/m², the following temperature distribution results:

Temperature Distribution:

High Prandtl Number (Pr=50):

• If the constant wall temperature scenario is repeated, except this time with ethlene glycol, a liquid with a relatively high Pr number at the mean temperature, you get the following results

• Note: For high Pr velocity develops much faster than temperature.  This means that your velocity becomes fully developed over a short distance, while your fluid still has the inlet temperature. Notice this effect in the graph

Thermophysical properties:

Density (ρ)	1.08E3 Kg/m^3
Dynamic Viscocity (μ)	5.7E-3 Kg/m*s
Conductivity (K)	0.26 W/m*K
Specific Heat (Cp)	2.56E3 J/Kg*K
Prandtl Number (Pr)	56.3

Temperature distribution:

Velocity Distribution:

entrance region velocity:

fully developed region:

Temperature Entrance Region VS Velocity Entrance Region:

Low Prandtl Number (Pr<<1):

• If the constant wall temperature scenario is repeated, except this time with mercury, a liquid metal with a very low Pr number, you get the following results:

• Note: For the case of low Pr, heat reaches the centerline very soon while the velocity is still uniform.

Thermophysical properties:

Temperature Distribution:

Velocity Distribution:

Entrance region velocity distribution:

Exit region velocity distribution:

Temperature Entrance Region VS Velocity Entrance Region:

Saving Projects

·          Simply go to Utility Menu>File>Save As… and save the project using the desired filename. To open the file later, run Interactive (the first thing explained in this tutorial) as usual, and when that is done, go to Utility Menu>File>Resume From… and choose the saved job from the directory it is saved in.