www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS
Applicable ANSYS Products:  ANSYS Multiphysics, ANSYS FLOTRAN, ANSYS ED 
Level of Difficulty:  advanced 
Interactive Time Required:  11/2 to 2 hours 
Discipline:  Computational Fluid Dynamics (CFD) 
Analysis Type:  steadystate 
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. 
This problem models air flow in a twodimensional 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.
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 }lb_{f}s^{2}/in^{4} 
Air viscosity  2.642x10^{9 }lb_{f}s/in^{2} 
Inlet velocity  1 in/sec* 
Outlet pressure  0 psi 
*Initial value of 1 will be changed to 50 upon restart. 
You will perform twodimensional 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 noslip (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 twodimensional 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 20003000. 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.
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 stepbystep 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.
3. Create rectangle for the inlet region.
4. Create the outlet rectangle.
5. Create the transition region between the rectangles.
7. Create the finite element mesh.
8. Create command on the Toolbar.
10. Establish fluid properties.
12. Change reference conditions.
14. Read in the results for postprocessing.
16. Plot total pressure contours.
17. Animate velocity of trace particles.
18. Make a path plot of the velocity through the outlet.
19. Increase the inlet velocity.
21. Plot total pressure contours.
22. Animate velocity of trace particles.
23. Make a path plot of the velocity through the outlet.
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.
28. Change the jobname and execute solution.
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.
34. Specify FLOTRAN solution options and execution controls.
36. Plot total pressure contours.
37. Animate velocity of trace particles.
You will now set preferences in order to filter quantities that pertain to this discipline only.




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.

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) direction  10 divisions  bias towards walls 
Inlet region, flow direction (X)  15 divisions  bias towards inlet and transition 
Transition region  12 divisions  uniform spacing 
Outlet region (initial)  15 divisions  larger elements near outlet 
Before attempting this step, plot the lines for clarity.


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.

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.

Fluid properties will be established for air in the “inches” set of units, where the unit of mass is (lb_{f}sec^{2})/in.

Choose the execution control from the FLOTRAN Set Up Menu.

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 293^{o}K to 530^{o}R by setting them to 70^{o}R and adding an offset temperature of 460^{o}R.


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

The resulting vector plot shows the recirculation region that occurs in the upper region of the duct. 
The resulting contour plot shows the total static and dynamic pressures that occur in the duct. 

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. 
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.

You will now restart the analysis from the initial result.

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


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.
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.



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.

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.



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

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

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.
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 = 1.21e7
V = Velocity = 50
D_{h} = hydraulic diameter = 2*inlet height = 2
µ = Viscosity= 2.642e9
Therefore, Re = 4600, which is turbulent.
So the next step is to restart the analysis using the turbulent model.

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.


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


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.

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.