5.1. Laminar and Turbulent Flow Analyses in a 2-D Duct

www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS



5.1.1. Problem Specification

Applicable ANSYS Products:ANSYS Multiphysics, ANSYS FLOTRAN, ANSYS ED
Level of Difficulty:advanced
Interactive Time Required:1-1/2 to 2 hours
Discipline:Computational Fluid Dynamics (CFD)
Analysis Type:steady-state
Element Types Used:FLUID141
ANSYS Features Demonstrated:solid modeling, mapped meshing, defining an abbreviation on the Toolbar, restart of FLOTRAN solution, multiple solutions, vector displays, line graphs, path operations, trace particle animation
Applicable Help Available:Overview of FLOTRAN CFD Analyses in the Fluids Analysis Guide, FLUID141 in the Elements Reference.

5.1.2. Problem Description

This problem models air flow in a two-dimensional duct. First, you define an arbitrary inlet velocity to simulate laminar flow with a Reynolds number of 90. After you obtain the solution and examine the results, you will increase the inlet velocity to investigate its effects on the flow profile and obtain a new solution. Then, in the third part, you will increase the duct length to allow the flow to achieve a fully developed profile in the solution. Finally, after calculating that the Reynold's number is greater than 4000, you will restart the solution using the turbulent model.

5.1.2.1. Given

Dimensions & Properties

 

Inlet length

4 in

Inlet height

1 in

Transition length

2 in

Outlet height

2.5 in

Initial outlet length

4 in

Added outlet length

30 in

Air density

1.21x10-7 lbf-s2/in4

Air viscosity

2.642x10-9 lbf-s/in2

Inlet velocity

1 in/sec*

Outlet pressure

0 psi

*Initial value of 1 will be changed to 50 upon restart.

 

5.1.2.2. Approach and Assumptions

You will perform two-dimensional analyses using the FLOTRAN element FLUID141. This problem is divided into four parts:

A laminar analysis of the flow of air with a Reynolds number of 90

An investigation of how a higher inlet velocity affects the flow profile using the laminar model

A laminar analysis of air with a longer duct length to observe a more fully developed flow profile

A turbulent analysis of the flow of air with a Reynolds number of ~4600

For all solutions, you will apply a uniform velocity profile at the inlet. This includes specification of a zero velocity condition at the inlet in the direction normal to the inlet flow. You will apply no-slip (zero velocity) conditions all along the walls (including where the walls intersect the inlets and outlets). The fluid is considered incompressible and you can assume that the properties will be constant. In such cases, only the relative value of pressure is important, and a zero relative pressure is applied at the outlet.

For the initial analysis, the flow is in the laminar regime (Reynold's number < 3000). To compute the Reynolds number of the flow for internal duct flows, the equation is as follows:

(Note that in a two-dimensional geometry, the hydraulic diameter is twice the inlet height.)

You will increase the inlet velocity to 50 in/s for the second analysis (which will increase the Reynolds number accordingly) and you will rerun the solution.

The flow profile for the second analysis shows that the flow is not fully developed, therefore the logical next step would be to increase the duct length in order to allow for a more complete profile. You will increase the length of the duct by 30 inches and rerun the solution.

For internal flows, the transition to turbulence occurs within the Reynolds number range of 2000-3000. Therefore for the last solution of air in the duct (Reynolds number ~4,500), the flow will be turbulent. For the last analysis, you will initiate the solution using the turbulent model. You will restart the analysis here (instead of rerunning it) because the problem domain has not changed.

5.1.2.3. Summary of Steps

Use the information in the problem description and the steps below as a guideline in solving the problem on your own. Or, use the detailed interactive step-by-step solution by choosing the link for step 1.

Before you begin, delete any results files (.rfl) from previous CFD analyses that still reside in your working directory. If you begin an ANSYS session to start a new CFD analysis, and use the same jobname from a file stored from a previous CFD analysis, the program will not start from scratch, but will restart and append to files with the same name (Jobname.rfl and Jobname.pfl). To avoid this situation, delete these results files when starting a new CFD analysis. Another way of avoiding this situation is to change the jobname to one that was not used in a previous CFD analysis. You can change the jobname in the product launcher before starting ANSYS, or during an ANSYS session by choosing Utility Menu> File> Change Jobname.

Preprocessing (Laminar Analysis)

1. Set preferences.

2. Define element type.

3. Create rectangle for the inlet region.

4. Create the outlet rectangle.

5. Create the transition region between the rectangles.

6. Establish mesh patterns.

7. Create the finite element mesh.

8. Create command on the Toolbar.

9. Apply boundary conditions.


Back To Top

Solution (Laminar Analysis)

10. Establish fluid properties.

11. Set execution controls.

12. Change reference conditions.

13. Execute FLOTRAN solution.


Back To Top

Postprocessing (Laminar Analysis)

14. Read in the results for postprocessing.

15. Plot velocity vectors.

16. Plot total pressure contours.

17. Animate velocity of trace particles.

18. Make a path plot of the velocity through the outlet.


Back To Top

Solution (Laminar Analysis with Change in Inlet Velocity)

19. Increase the inlet velocity.

20. Run the analysis.


Back To Top

Postprocessing (Laminar Analysis Using New Inlet Velocity)

21. Plot total pressure contours.

22. Animate velocity of trace particles.

23. Make a path plot of the velocity through the outlet.


Back To Top

Preprocessing (Laminar Analysis with Increase in Duct Length)

24. Delete pressure boundary condition.

25. Construct additional outlet region.

26. Establish mesh divisions for the new rectangle and mesh.

27. Apply boundary conditions on new region.


Back To Top

Solution (Laminar Analysis Using New Duct Length)

28. Change the jobname and execute solution.


Back To Top

Postprocessing (Laminar Analysis Using New Duct Length)

29. Read in the new results and plot velocity vectors.

30. Plot total pressure contours.

31. Animate velocity of trace particles.

32. Make a path plot of the velocity through the outlet.

33. Calculate Reynolds number.


Back To Top

Solution (Turbulent Analysis)

34. Specify FLOTRAN solution options and execution controls.

35. Restart the analysis.


Back To Top

Postprocessing (Turbulent Analysis)

36. Plot total pressure contours.

37. Animate velocity of trace particles.

38. Make a path plot of the velocity through the outlet.

39. Exit the ANSYS program.

5.1.3. Preprocessing (Laminar Analysis)

5.1.3.1. Step1: Set preferences.

You will now set preferences in order to filter quantities that pertain to this discipline only.

  1. Main Menu > Preferences

  2. Turn on FLOTRAN CFD filtering.

  3. OK.

5.1.3.2. Step 2: Define element type.

  1. Main Menu > Preprocessor > Element Type > Add/Edit/Delete

  2. Add an element type.

  3. Choose FLOTRAN CFD.

  4. Choose 2D FLOTRAN element (FLUID141).

  5. OK.

  6. Close.

5.1.3.3. Step 3: Create rectangle for the inlet region.

  1. Main Menu> Preprocessor> Modeling> Create> Areas> Rectangle> By Dimensions

  2. Enter the following:

    X1 = 0

    X2 = 4

  3. Enter the following:

    Y1 = 0

    Y2 = 1

  4. Apply to create the first rectangle and preserve the dialog box for the second rectangle.

5.1.3.4. Step 4: Create the outlet rectangle.

  1. Enter the following:

    X1 = 6

    X2 = 10

  2. Enter the following:

    Y1 = 0

    Y2 = 2.5

  3. OK.

  4. Toolbar: SAVE_DB.

5.1.3.5. Step 5: Create the transition region between the rectangles.

The transition region, where the flow expands, is bordered on the top by a smooth line tangent to the upper line of both rectangles. This line is created with the "Tangent to 2 lines" option. Note that the prompt in the Input Window will indicate what is to be picked (lines, ends of lines).

The area is then created as an arbitrary area through the four keypoints. Note that the area will be bounded by existing lines through those keypoints.

  1. Main Menu> Preprocessor> Modeling> Create> Lines> Lines> Tan to 2 Lines

  2. Pick first line (upper line of left rectangle).

  3. OK (in picking menu).

  4. Pick the tangency end of the first line (upper right corner).

  5. OK (in picking menu).

  6. Pick the second line (upper line of the larger rectangle.

  7. OK (in picking menu).

  8. Pick the tangency end of the second line.

  9. OK to create the line

    The result is a smooth line between the two areas.

    Now create the third area as an arbitrary area through keypoints.

  10. Main Menu> Preprocessor> Modeling> Create> Areas> Arbitrary> Through KPs

  11. Pick 4 corners in counterclockwise order.

  12. OK in the picking menu.

  13. Toolbar: SAVE_DB

 

5.1.3.6. Step 6: Establish mesh patterns.

To create a mapped mesh, set the specific size controls along the lines (LESIZE command). The establishment of a good finite element mesh is quite important in CFD analyses.

The general finite element philosophy of putting more elements in regions with higher solution gradients applies here. The mesh density should be sufficient to enable the program to capture the nature of the phenomena. For example, a small recirculation region is likely to develop in the expansion region. The greater the number of applied elements implies a higher level of flow details that will be captured.

Apply 10 elements in the transverse direction (Y) and bias them slightly towards the top and bottom boundaries. This will help capture boundary layer effects. For high Reynolds number problems, finer meshes should be used. Along the inlet flow direction (X) in the inlet, use the number of divisions tabulated below.

Mesh Division Strategy
Transverse (Y) direction10 divisions - bias towards walls
Inlet region, flow direction (X)15 divisions - bias towards inlet and transition
Transition region12 divisions - uniform spacing
Outlet region (initial)15 divisions - larger elements near outlet

Before attempting this step, plot the lines for clarity.

  1. Utility Menu> Plot> Lines

  2. Main Menu> Preprocessor> Meshing> Mesh Tool

  3. Choose Lines Set.

  4. Pick lines in flow direction along the inlet.

  5. Apply (in the picking menu).

  6. Enter 15 as the No. of element divisions.

  7. Enter -2 as the Spacing ratio (this produces smaller elements near both ends of the line).

  8. Apply.

    The mesh ratio chosen results in smaller elements near the inlet, where the flow is developing, and near the expansion, in which more elements will be placed because of the high solution gradients in that region. There should be a relatively smooth transition in element size from region to region throughout the entire problem domain.

    You will repeat this process of picking the lines and entering the number of divisions and the ratios, using the mesh division strategy above. Note that the mesh division ratio is applied to the direction of the lines, the larger elements being at the end of the line. This is the reason for the use of a number less than 1 for the upper line of the outlet region and a number greater than 1 for the lower line. (The line directions follow a counterclockwise direction, according to how they were generated.)

    Transition region:

  9. Pick the top and bottom lines in the center area.

  10. Apply (in the picking menu).

  11. Enter 12 as the No. of element divisions.

  12. Enter 1 as the Spacing ratio (uniform spacing).

  13. Apply.

    Outlet region:

  14. Pick the top and bottom lines in the outlet region.

  15. Apply (in the picking menu).

  16. Enter 15 as the No. of element divisions.

  17. Enter 3.0 as the Spacing ratio (bias towards outlet).

  18. OK.

    Notice that the upper line is not biased towards the transition. The line bias needs to be "flipped."

  19. Choose Flip in the Mesh Tool. (toggle to Mesh Tool as necessary.)

  20. Pick the upper line only.

  21. OK (in the picking menu).

    Transverse direction:

  22. Choose Lines Set.

  23. Pick the 4 transverse direction lines.

  24. OK to close picking menu.

  25. Enter 10 as the No. of element divisions.

  26. Enter -2 as the Spacing ratio (bias towards top and bottom walls).

  27. OK.

  28. Toolbar: SAVE_DB.

5.1.3.7. Step 7: Create the finite element mesh.

  1. Choose Mapped mesher.

  2. Choose Mesh.

  3. Pick All.

  4. Close the Mesh Tool. (Toggle to the Mesh Tool as necessary.)

5.1.3.8. Step 8: Create command on the ANSYS Toolbar.

The ANSYS Toolbar contains a set of buttons that execute commonly used ANSYS functions. It is convenient to establish a command on the ANSYS Toolbar that turns off the display of the triad at the origin. You will accomplish this by accessing the menu controls on the Utility Menu and then choosing to edit the Toolbar.

Enter the command name and command itself as an abbreviation.

  1. Utility Menu> MenuCtrls> Edit Toolbar

  2. Type TRI,/triad,off after *ABBR.

  3. Accept.

  4. Close.

  5. Turn off triad display using the new button TRI.

    This will unclutter subsequent result displays.

  6. Utility Menu> Plot> Lines

5.1.3.9. Step 9: Apply boundary conditions.

A velocity of 1 inch/second is applied in the X direction (VX) at the inlet, and a zero velocity is applied in the transverse direction at the inlet (VY in the Y direction). Zero velocities in both directions are applied all along the walls, and a zero pressure is applied at the outlet. These boundary conditions are being applied to the lines now so that they do not have to be applied again if remeshing is required.

Apply the inlet boundary condition.

  1. Main Menu> Preprocessor> Loads > Define Loads> Apply> Fluid/CFD> Velocity> On Lines

  2. Pick the inlet line (the vertical line at the far left).

  3. OK in the picking menu.

  4. Enter 1.0 for VX.

  5. Enter 0.0 for VY.

  6. OK.

    Apply the wall boundary conditions. Choose the lines which make up the walls and then apply zero velocities in the X and Y directions.

  7. Main Menu> Preprocessor> Loads> Define Loads> Apply> Fluid/CFD> Velocity> On Lines

  8. Pick the six lines on the top and bottom.

  9. OK in picking menu.

  10. Enter 0.0 for VX and VY.

  11. OK to apply the condition.

    You will subsequently see that the wall condition of zero velocity will automatically prevail at the corners where the inlets intersect the walls.

    Apply the outlet condition.

  12. Main Menu> Preprocessor> Loads> Define Loads> Apply> Fluid/CFD> Pressure DOF> On Lines

  13. Pick the outlet line (vertical line on the far right).

  14. OK (in picking menu).

  15. Enter 0 for the Pressure value.

  16. Set endpoints to Yes.

  17. OK.

  18. Toolbar: SAVE_DB.

    At this point, the finite element model is complete and the FLOTRAN menus are accessed to specify the fluid properties along with any other FLOTRAN controls that may be required.

5.1.4. Solution (Laminar Analysis)

5.1.4.1. Step 10: Establish fluid properties.

Fluid properties will be established for air in the “inches” set of units, where the unit of mass is (lbf-sec2)/in.

  1. Main Menu> Solution> FLOTRAN Set Up> Fluid Properties

  2. Choose AIR-IN for both density and viscosity.

  3. OK.

  4. OK.

5.1.4.2. Step 11: Set execution controls.

Choose the execution control from the FLOTRAN Set Up Menu.

  1. Main Menu> Solution> FLOTRAN Set Up> Execution Ctrl

  2. Enter 40 Global iterations (Note: 40 global iterations is arbitrary with no guarantee of convergence.)

  3. OK to apply and close.

5.1.4.3. Step 12: Change reference conditions.

The reference pressure is changed from the default value of 101 KPa to 14.7 psi to maintain a consistent set of units. Likewise, the nominal stagnation and reference temperatures are changed from 293oK to 530oR by setting them to 70oR and adding an offset temperature of 460oR.

  1. Main Menu> Solution> FLOTRAN Set Up> Flow Environment> Ref Conditions

  2. Change the reference pressure to 14.7 psi (equivalent to 1 atmosphere).

  3. Change the nominal, stagnation, and reference temperatures (in oR) to 70.

  4. Change the temperature offset (in oR) from absolute 0 to 460.

  5. OK.

  6. Toolbar: SAVE_DB.

5.1.4.4. Step 13: Execute FLOTRAN solution.

  1. Main Menu> Solution> Run FLOTRAN

    While running the FLOTRAN solution, ANSYS will plot the "Normalized Rate of Change" as a function of the "Cumulative Iteration Number." This is the Graphical Solution Tracker which allows visual monitoring of the solution for convergence.

  2. Close the information window when the solution is done.

5.1.5. Postprocessing (Laminar Analysis)

5.1.5.1. Step 14: Read in the results for postprocessing.

Enter the general postprocessor and read in the latest set of solution results, and then create a vector plot.

  1. Main Menu> General Postproc> Read Results> Last set

 

5.1.5.2. Step 15: Plot velocity vectors.

  1. Main Menu> General Postproc> Plot Results> Vector Plot> Predefined

  2. Choose DOF solution.

  3. Choose Velocity V.

  4. OK.

The resulting vector plot shows the recirculation region that occurs in the upper region of the duct.

5.1.5.3. Step 16: Plot total pressure contours.

  1. Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu

  2. Choose Other FLOTRAN Quantities.

  3. Choose Total Stagnation Pressure.

  4. OK.

The resulting contour plot shows the total static and dynamic pressures that occur in the duct.

5.1.5.4. Step 17: Animate velocity of trace particles.

  1. Main Menu> General Postproc> Plot Results>Defi Trace Pt

  2. Pick two or three points around the inlet region and one or two points in the recirculation region (along the upper wall of the transition region).

  3. OK (in picking menu).

  4. Utility Menu> PlotCtrls> Animate> Particle Flow

  5. Choose DOF Solution.

  6. Choose Velocity VX.

  7. OK.

    Ignore any warning messages about maximum number of loops (Choose Close). ANSYS creates a particle flow path based upon approximations that do not form closed loops.

    The resulting trace plot shows the path of flow particles through the duct.

  8. Make choices in the Animation Controller (not shown), if necessary, then choose Close.

5.1.5.5. Step 18: Make a path plot of velocity through the outlet.

  1. Main Menu> General Postproc> Path Operations> Define Path> By Nodes

  2. Pick the lowest and then the highest point of the outlet.

  3. OK (in picking menu).

  4. Enter OUTLET for the Path Name.

  5. OK.

  6. File> Close (Windows)

    or

    Close (X11/Motif)

    Now specify the velocity in the X direction (VX) to map onto the path.

  7. Main Menu> General Postproc> Path Operations> Map onto Path

  8. Enter VELOCITY as label.

  9. Choose DOF Solution.

  10. Choose Velocity VX.

  11. OK.

  12. Main Menu> General Postproc> Path Operations> Plot Path Item> On Graph

  13. Choose the label VELOCITY that you previously defined.

  14. OK to create path plot.

  15. Close any warning messages.

The resulting path plot shows the flow has an almost fully developed laminar profile. The curve looks relatively uniform and has a parabolic shape.

Now for the next study, investigate the effects of increasing the inlet velocity to 50 inches/second.

5.1.6. Solution (Laminar Analysis with Change in Inlet Velocity)

5.1.6.1. Step 19: Increase the inlet velocity.

The inlet velocity affects the flow profile. Increasing the inlet velocity by a factor of 50 will increase the Reynolds number accordingly. Return to the apply loads function and change the inlet velocity, then execute the solution from a different jobname.

  1. Utility Menu> Plot> Lines

  2. Main Menu> Solution> Define Loads> Apply> Fluid/CFD> Velocity> On Lines

  3. Pick the inlet line (the vertical line at the far left).

  4. OK (in picking menu)

  5. Enter 50 for VX.

  6. Enter 0 for VY.

  7. OK.

5.1.6.2. Step 20: Run the analysis.

You will now restart the analysis from the initial result.

  1. Main Menu> Solution> Run FLOTRAN

    An error message appears stating that the coefficient matrix has a negative diagonal. ANSYS produced this message because it uses the Streamline Upwind/Petrov-Galerkin (SUPG) advection scheme by default. Although it is more accurate than other advection schemes, the SUPG scheme can lead to spurious oscillations in the solution, and may cause nonphysical solutions or convergence difficulties. To remedy this situation without changing to another advection scheme, you will first add some modified inertial relaxation, and then will execute the solution again.

  2. OK to remove the error message.

  3. Close.

  4. Main Menu> Solution> FLOTRAN Setup> Relax/Stab/Cap> MIR Stabilizatio

  5. Enter 0.1 for the Momentum Equation.

  6. OK.

  7. Main Menu> Solution> Run FLOTRAN Once again, the Graphical Solution Tracker is displayed.

  8. Close.

    You will now repeat the preceding postprocessing steps exactly to show the effects of the higher inlet velocity. These steps are as follows:

  9. Main Menu> General Postproc> Read Results> Last Set

  10. Main Menu> General Postproc> Plot Results> Vector Plot> Predefined

  11. Choose DOF Solution.

  12. Choose Velocity V.

  13. OK.

5.1.7. Postprocessing (Laminar Analysis Using New Inlet Velocity)

5.1.7.1. Step 21: Plot total pressure contours.

  1. Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu

  2. Choose Other FLOTRAN Quantities.

  3. Choose Total stagnation pressure.

  4. OK.

The resulting contour plot shows the total static and dynamic pressures that occur in the duct.

5.1.7.2. Step 22: Animate velocity of trace particles.

  1. Main Menu> General Postproc> Plot Results> Defi Trace Pt

  2. Pick two or three points around the inlet region and one or two points in the recirculation region (along the upper wall of the transition region).

  3. OK (in picking menu).

  4. Utility Menu> PlotCtrls> Animate> Particle Flow

  5. Choose DOF Solution.

  6. Choose Velocity VX.

  7. OK.

    Ignore the warning messages about maximum number of loops (Choose Close). ANSYS creates a particle flow path based upon approximations that do not form closed loops.

    The resulting trace plot shows the path of flow particles through the duct.

  8. Make choices in the Animation Controller (not shown), if necessary, then choose Close.

5.1.7.3. Step 23: Make a path plot of velocity through the outlet.

  1. Main Menu> General Postproc> Path Operations> Define Path> By Nodes

  2. Pick the lowest and then the highest point of the outlet.

  3. OK (in picking menu).

  4. Enter OUTLET for the Path Name.

  5. OK.

  6. File> Close (Windows) or Close (X11/Motif).

    Now specify the velocity in the X direction (VX) to map onto the path.

  7. Main Menu> General Postproc> Path Operations> Map onto Path

  8. Enter VELOCITY as label.

  9. Choose DOF Solution.

  10. Choose Velocity VX.

  11. OK.

  12. Main Menu> General Postproc> Path Operations> Plot Path Item> On Graph

  13. Choose the label VELOCITY that you previously defined.

  14. OK to create path plot.

  15. Close any warning messages.

The resulting path plot shows the curve has a bias towards one edge of the outlet. This indicates that the flow has not yet fully developed. (Note that if your plot appears as a mirror image of this one, it is because you reversed the order of picking, that is, you picked from highest to lowest instead of from lowest to highest points at the outlet.)

Now in the next study, if the length of the duct's outlet region is increased, the flow may reach a fully developed profile. Increase the duct length by 30 inches.

5.1.8. Preprocessing (Laminar Analysis with Increase in Duct Length)

5.1.8.1. Step 24: Delete pressure boundary condition.

The results for the lower viscosity case indicate that the recirculation region has extended well beyond the outlet. To allow the flow to fully develop by the time it reaches the exit, it must be given more room to do so.

  1. Main Menu> Preprocessor> Loads> Define Loads> Delete> Fluid/CFD> Pressure DOF> On Lines

  2. Pick All (in picking menu) to delete all pressure boundary conditions.

 

5.1.8.2. Step 25: Construct additional outlet region.

  1. Main Menu> Preprocessor> Modeling> Create> Areas> Rectangle> By Dimensions

  2. Enter the following:

    X1 =10

    X2 = 40

  3. Enter the following:

    Y1 = 0

    Y2 = 2.5

  4. OK.

    The new rectangle has unique keypoints and lines. These must be merged with their counterparts on the existing areas.

  5. Main Menu> Preprocessor> Numbering Ctrls> Merge Items

  6. Choose All for the Type of items to be merged.

  7. OK.

    A warning message appears stating that an unmeshed line is to merged into a previously meshed line. This is as it should be. Close the message box.

  8. Close.

  9. Utility Menu> Plot> Lines

5.1.8.3. Step 26: Establish mesh divisions for the new rectangle and mesh.

  1. Main Menu> Preprocessor> Meshing> MeshTool

  2. Choose Lines Set.

  3. Pick line at new outlet.

  4. OK (in picking menu).

  5. Enter 10 for No. of element divisions (as before).

  6. Enter -2 for Spacing ratio.

  7. Apply.

    Repeat the procedure for the upper and lower lines of the rectangle.

  8. Pick lines at the top and bottom of new outlet.

  9. OK (in picking menu).

  10. Enter 20 for No. of element divisions.

  11. Enter 3 for Spacing ratio.

  12. OK.

    Flip the line bias on the upper line.

  13. Choose Lines Flip.

  14. Pick the upper line.

  15. OK (in picking menu).

  16. Toolbar: SAVE_DB.

  17. Choose Mesh.

  18. Pick the outlet area.

  19. OK (in picking menu) to begin mesh.

  20. Close the Mesh Tool.

5.1.8.4. Step 27: Apply boundary conditions on new region.

You must apply boundary conditions to the new region. You will apply zero velocities in both directions along the walls, and a zero pressure at the outlet.

  1. Utility Menu> Plot> Lines

  2. Main Menu> Preprocessor> Loads> Define Loads> Apply> Fluid/CFD> Velocity> On Lines

  3. Pick the new upper and lower walls that don't have boundary conditions.

  4. OK (in picking menu).

  5. Enter 0 for VX and VY.

  6. OK.

    Now apply the pressure boundary condition at the outlet.

  7. Main Menu> Preprocessor> Loads> Define Loads> Apply> Fluid/CFD> Pressure DOF> On Lines

  8. Pick the new outlet.

  9. OK (in picking menu).

  10. Enter 0 for the Pressure value.

  11. Set endpoints to Yes.

  12. OK to apply the boundary condition.

  13. Utility Menu> Plot> Lines

5.1.9. Solution (Laminar Analysis Using New Duct Length)

5.1.9.1. Step 28: Change the jobname and execute solution.

Because the addition of an outlet has changed the problem domain, a new analysis is required. You can start a new analysis by changing the jobname from the Utility Menu.

Note that a warning message will appear stating that you must exit the Solution processor in order to change the name.

  1. Utility Menu> File> Change Jobname

  2. Close to exit Solution.

  3. Enter "newLength" for the new jobname.

  4. OK.

    Another way to start a new analysis is by deleting the results file, named file.rfl (by default). You can delete a file in one of two ways:

    Utility Menu> File> File Operations> Delete

    Pick the file name, then choose OK

    OR

    Execute a /SYS command and remove the file with the appropriate operating system command.

    ANSYS will automatically rename an incorrect results file.

    Now execute the new solution.

  5. Main Menu> Solution> Run FLOTRAN

  6. Close the information window when solution is done.

5.1.10. Postprocessing (Laminar Analysis Using New Duct Length)

5.1.10.1. Step 29: Read in the new results and plot velocity vectors.

  1. Main Menu> General Postproc> Read Results> Last Set

  2. Main Menu> General Postproc> Plot Results> Vector Plot> Predefined

  3. Choose DOF Solution.

  4. Choose Velocity V.

  5. OK.

5.1.10.2. Step 30: Plot total pressure contours.

  1. Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu

  2. Choose Other FLOTRAN Quantities.

  3. Choose Total Stagnation Pressure.

  4. OK.

The resulting contour plot shows the total static and dynamic pressures that occur in the duct.

5.1.10.3. Step 31: Animate velocity of trace particles.

  1. Main Menu> General Postproc> Plot Results>Defi Trace Pt

  2. Pick two or three points around the inlet region and one or two points in the recirculation region (along the upper wall of the transition region).

  3. OK (in picking menu).

  4. Utility Menu> PlotCtrls> Animate> Particle Flow

  5. Choose DOF Solution.

  6. Choose Velocity VX.

  7. OK.

    Ignore the warning messages about maximum number of loops (choose Close). ANSYS creates a particle flow path based upon approximations that do not form closed loops.

    The resulting trace plot shows the path of flow particles through the duct.

  8. Make choices in the Animation Controller (not shown), if necessary, then choose Close.

5.1.10.4. Step 32: Make a path plot of the velocity through the outlet.

The outlet velocity profile can be examined with a path plot. First, establish a path for the path plot.

  1. Main Menu> General Postproc> Path Operations> Define Path> By Nodes

  2. Pick the lowest point, and then the highest point of the outlet.

  3. OK (in the picking menu).

  4. Enter "outlet" for the path name.

  5. OK.

  6. File> Close (Windows)

    or

    Close (X11/Motif)

    Now specify the velocity in the X direction (VX) to map onto the path.

  7. Main Menu> General Postproc> Path Operations> Map onto Path

  8. Enter "velocity" as the User label.

  9. Choose DOF solution.

  10. Choose Velocity VX.

  11. OK.

  12. Main Menu> General Postproc> Path Operations> Plot Path Item> On Graph

  13. Choose the label VELOCITY that you previously defined.

  14. OK to create path plot.

  15. Close any warning messages.

The resulting path plot shows that the flow is almost fully developed. Since the velocity has been increased so much, the flow may be in the turbulent regime. The next step is to check the Reynold's number and activate turbulence if necessary. A consequence of the increased diffusion associated with turbulence is a decrease in the size of the recirculation region.

5.1.10.5. Step 33: Calculate Reynolds number.

Calculate Reynolds number in order to determine if the analysis is indeed in the turbulent region (Re > 3000).

Recall that the Reynolds number is determined by the following formula:

Our flow material is AIR, which has the following properties:

p = density = 1.21e-7

V = Velocity = 50

Dh = hydraulic diameter = 2*inlet height = 2

µ = Viscosity= 2.642e-9

Therefore, Re = 4600, which is turbulent.

So the next step is to restart the analysis using the turbulent model.

5.1.11. Solution (Turbulent Analysis)

5.1.11.1. Step 34: Specify FLOTRAN solution options and execution controls.

  1. Main Menu> Solution> FLOTRAN Set Up> Solution Options

  2. Choose Turbulent option.

  3. OK.

    With the increased turbulence resulting from the low viscosity, the nonlinear effects in the problem are more pronounced and more global iterations will be required to achieve a good solution. You will increase this number in the Execution Control dialog box.

  4. Main Menu> Solution> FLOTRAN Set Up> Execution Ctrl

  5. Enter 80 Global iterations.

  6. OK.

5.1.11.2. Step 35: Restart the analysis.

Note that this is a restart of the analysis. Restarting an ANSYS FLOTRAN solution requires that the problem domain (specifically, the nodal geometry) is not changed. Since the only changes that were specified were a change the model (from laminar to turbulent) and a change in the number of equilibrium iterations, restarting the analysis is acceptable. Therefore, the solution will pick up where it left off, and 80 global iterations will be executed.

  1. Main Menu> Solution> Run FLOTRAN

    Once again, the Graphical Solution Tracker is displayed.

  2. Close.

    You will now repeat the preceding postprocessing steps exactly to show the effects of the higher inlet velocity. These steps are as follows:

  3. Main Menu> General Postproc> Read Results> Last Set

  4. Main Menu> General Postproc> Plot Results> Vector Plot> Predefined

  5. Choose DOF Solution.

  6. Choose Velocity V.

  7. OK.

5.1.12. Postprocessing (Turbulent Analysis)

5.1.12.1. Step 36: Plot total pressure contours.

  1. Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu

  2. Choose Other quantities.

  3. Choose Total Pressure PTOT.

  4. OK.

The resulting contour plot shows the total static and dynamic pressures that occur in the duct.

5.1.12.2. Step 37: Animate velocity of trace particles.

  1. Main Menu> General Postproc> Plot Results> Defi Trace Pt

  2. Pick two or three points around the inlet region and one or two points in the recirculation region (along the upper wall of the transition region).

  3. OK (in picking menu).

  4. Utility Menu> PlotCtrls> Animate> Particle Flow

  5. Choose DOF Solution.

  6. Choose Velocity VX.

  7. OK.

    Ignore any warning messages about maximum number of loops (choose Close). ANSYS creates a particle flow path based upon approximations that do not form closed loops.

    The resulting trace plot shows the path of flow particles through the duct.

  8. Make choices in the Animation Controller (not shown), if necessary, then choose Close.

5.1.12.3. Step 38: Make a path plot of velocity through the outlet.

  1. Main Menu> General Postproc> Path Operations> Define Path> By Nodes

  2. Pick the lowest and then the highest point of the outlet.

  3. OK (in the picking menu).

  4. Enter OUTLET as the Path Name.

  5. OK.

  6. File> Close (Windows).

    or

    Close (X11/Motif)

    Now specify the velocity in the X direction (VX) to map onto the path.

  7. Main Menu> General Postproc> Path Operations> Map onto Path

  8. Enter VELOCITY as label.

  9. Choose DOF Solution.

  10. Choose Velocity VX.

  11. OK.

  12. Main Menu> General Postproc> Path Operations> Plot Path Item> On Graph

  13. Choose the label VELOCITY that you previously defined.

  14. OK to create path plot.

  15. Close any warning messages.

Note that with the turbulent model is turned on for the analysis, the flow looks fully developed and the path plot appears to be flatter on the top (instead of parabolic, as in the laminar analyses). Thus the flow is turbulent and the observed results are as expected.

5.1.12.4. Step 39: Exit the ANSYS program.

  1. Toolbar: QUIT.

  2. Choose Quit - No Save!

  3. OK.

Congratulations! You have completed this tutorial.

Even though you have exited the ANSYS program, you can still view animations using the ANSYS ANIMATE program. The ANIMATE program runs only on the PC and is extremely useful for:

  • Viewing ANSYS animations on a PC regardless of whether the files were created on a PC (AVI files) or on a UNIX workstation (ANIM files).

  • Converting ANIM files to AVI files.

  • Sending animations over the web.