Fluent-Intro 17.0 WS06 Turbulent Flow Past A Backward Facing Step [PDF]

Zitiervorschau

Turbulent Flow Past a Backward Facing Step 1. Introduction The purpose of this workshop is to simulate flow over a backward facing step. The simulation is performed to determine, how the results from different turbulence models compare with one another, and with experimental results. You will also check if the models can predict the reattachment point downstream of the step. The workshop covers many aspects of turbulent flow modeling in Fluent, including specifying models and near wall treatments, checking y+, selecting boundary conditions, comparison with experimental results, and comparison of results obtained with different turbulence models. It will show how to do the following: • Set up and solve turbulent flows in Fluent using different models and near wall treatments. • Postprocess y+ in Fluent. • Understand the importance of realistic boundary conditions. • Compare results with data using CFD-Post and easily perform results comparisons using Workbench.

2. Prerequisites This tutorial assumes that you are already familiar with the ANSYS Workbench interface and its project workflow. This tutorial also assumes that you have completed the first workshop and that you are familiar with the ANSYS Fluent tree and ribbon structure. Some steps in the setup and solution procedure will not be shown explicitly.

3. Problem Description Flow over a backward facing step is a standard test case for turbulence models. You will see how to set up and solve turbulent flow problems in Fluent and learn to use CFD-Post and Workbench to compare the results from different turbulence models with each other and with experimental data. You will also examine how the results are affected by boundary conditions.

4. Setup and Solution 4.1. Loading a Mesh and Starting Fluent 1.

Copy the files (driver.msh.gz, rke-prof.prof, sst-prof.prof, and x-wall-shear-ds.csv) to your working folder.

2.

Start ANSYS Workbench.

3.

Drag a Fluent Component System to the Project Schematic. Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

1

Turbulent Flow Past a Backward Facing Step 4.

Right-click on Setup, cell 2, and select Import Fluent Case → Browse.

5.

In the window that opens, from the drop-down list next to File name, select FLUENT Mesh File.

6.

Select the file driver.msh.gz and click Open.

7.

Save the project as 06_Backward_Facing_Step. File → Save

8.

Double-click Setup, cell 2 of the Fluent system to open Fluent Launcher.

9.

Click OK in the Fluent Launcher dialog box to open ANSYS Fluent.

Note IF HPC licenses are available, you can select Parallel under Processing Options and enter the number of processes.

4.2. Setting Up Domain In this step, you will perform mesh-related activities using the Setting Up Domain ribbon tab (Mesh group). 1.

Check the mesh. Setting Up Domain → Mesh → Check

Note ANSYS Fluent will perform various checks on the mesh and will report the progress in the console. Make sure that the reported minimum volume is a positive number.

2.

2

Zoom in on the mesh near the bottom wall downstream of the step.

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setup and Solution

Flow separates at the step and reattaches some distance downstream.

Note It is intended for the simulation to resolve the viscous sublayer with the mesh (no wall functions), which requires a very fine near wall mesh to get y+ ≈ 1. Later in the workshop, you will evaluate whether this has been achieved.

4.3. Setting Up Physics 1.

In the Solver group of the Setting Up Physics ribbon tab, retain the default selection of Steady for Time. Setting Up Physics → Solver

2.

Set up your models for the CFD simulation using the Models group of the Setting Up Physics ribbon tab. •

Enable the - epsilon model. Setting Up Physics → Models → Viscous... i.

In the Viscous Model dialog box, select k-epsilon from the Model list.

ii.

Select Realizable from the k-epsilon Model group.

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

3

Turbulent Flow Past a Backward Facing Step iii.

Select Enhanced Wall Treatment from the Near-Wall Treatment group.

Note When using any k-epsilon model, the Enhanced Wall Treatment is the only viscous sublayer resolving near wall treatment.

iv.

Retain the other default settings and click OK to accept the model and close the Viscous Model dialog box.

Note Later on you will calculate the flow with the SST k-omega model and compare results.

3.

Set the air material properties.

Setting Up Physics → Materials → Create/Edit... a.

In the Create/Edit Materials dialog box, the default fluid material is air.

b.

Enter 1.18 for Density.

c.

Enter 1.85e-05 for Viscosity.

d.

Click Change/Create in the Create/Edit Materials dialog box and close it.

Note These values will allow you to match the Reynolds number reported in the experiment.

4.

4

Set up the boundary conditions for the CFD analysis using the Zones group of the Setting Up Physics ribbon tab.

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setup and Solution Setting Up Physics → Zones → Boundaries → All This opens the Boundary Conditions task page. a.

b.

In the Boundary Conditions task page, in the Zone list, select inlet_v and click Edit... to open the Velocity Inlet dialog box.

i.

In the Velocity Inlet dialog box, enter 41.7 for Velocity Magnitude (m/s).

ii.

Select Intensity and Hydraulic Diameter from the Specification Method drop-down list.

iii.

Enter 0.2032 for Hydraulic Diameter (m).

iv.

Click OK and close the Velocity Inlet dialog box.

Retain the default conditions for the outlet.

4.4. Solving 1.

Set up solution methods. Solving → Solution → Methods...

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

5

Turbulent Flow Past a Backward Facing Step

a.

In the Solution Methods task page, select Coupled for Scheme in the Pressure-Velocity Coupling group box.

b.

Select PRESTO! from the Pressure drop-down list.

Note PRESTO! is often a better choice for structured hexahedral or quadrilateral meshes such as the one used in this problem.

c.

Enable Pseudo Transient.

Note In many cases, the solution will converge in fewer iterations using Coupled plus the Pseudo Transient method.

6

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setup and Solution 2.

Create a surface report definition to track wall shear stress. Solving → Reports → Definitions → New → Surface Report → Area-Weighted Average...

a.

In the Surface Report Definition dialog box, enter wall-shear-mon for the Name.

b.

Under the Create group, enable Report File and Report Plot.

c.

Select Wall Fluxes... and Wall Shear Stress from the Field Variable drop-down lists.

d.

Select bottom_wall from the list of Surfaces.

e.

Click OK to save and close the Surface Report Definition dialog box.

Note The Wall Shear Stress on the wall downstream of the step is the quantity of interest in this simulation, so it is natural to track it with a surface report definition.

3.

Similarly, create a surface report definition to track the turbulent viscosity ratio at the outlet. Solving → Reports → Definitions → New → Surface Report → Area-Weighted Average... Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

7

Turbulent Flow Past a Backward Facing Step a.

In the Surface Report Definition dialog box, enter turb-out-mon for the Name.

b.

Under the Create group, enable Report File and Report Plot.

c.

Select Turbulence... and Turbulent Viscosity Ratio from the Field Variable drop-down lists.

d.

Select outlet_p from the list of Surfaces.

e.

Click OK to save and close the Surface Report Definition dialog box.

Note The solution for turbulence model variables can change very slowly in regions far downstream from inlets. Because of this, they are often good to use for monitoring the solution. Turbulent viscosity ratio is selected here, because it includes contributions from both the turbulent kinetic energy and the turbulent dissipation rate, meaning both fields have to converge before the monitor stops changing.

4.

Initialize the solution. Solving → Initialization Retain the selection of Hybrid for Method and click Initialize.

5.

Run the solution for 100 iterations. Solving → Run Calculation → Calculate

You can see that the residuals converge in a small number of iterations, but the monitor plots do not definitively indicate that the solution has stopped changing.

8

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setup and Solution 6.

Before performing more iterations, you will clear the monitors.

Note This step is not necessary but it helps to make the y-axis range in the monitor plots tighter, thus making it easier to see changes in the monitored variable. a.

Close the wall-shear-mon-rplot and turb-out-mon-rplot windows in the graphics display window.

b.

Remove the old plots and add new ones. Solving → Reports → Plot...

i.

In the Report Plot Definitions dialog box that opens, select and delete wall-shear-mon-rplot and turb-out-mon-rplot from the list of Report Plots.

ii.

Click New.... A.

In the New Report Plot dialog box that opens, select wall-shear-mon from the list of Available Report Definitions list and click Add>>.

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

9

Turbulent Flow Past a Backward Facing Step

iii.

10

B.

Enter wall-shear-mon-rplot for Name and Plot Title.

C.

Click OK to close the New Report Plot dialog box.

In the Report Plot Definitions dialog box, click New.... A.

Following the steps done previously, select and add turb-out-mon.

B.

Enter turb-out-mon-rplot for Name and Plot Title and click OK.

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setup and Solution

iv.

7.

Close the Report Plot Definitions dialog box.

Change the continuity residual convergence criterion. Solving → Reports → Residuals

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

11

Turbulent Flow Past a Backward Facing Step

a.

In the Residual Monitors dialog box, enter 1e-06 under Absolute Criteria for continuity.

Note There is no significance to 1e-6. It is just desired to select a low value so the iterations do not stop prematurely. Additional iterations will be performed and convergence will be judged by whether the surface monitor plots are still changing.

b. 8.

Click OK to close the Residual Monitors dialog box.

Run the solution for 100 more iterations. Solving → Run Calculation → Calculate

Note In the dialog box that appears, retain the selection of Use settings changes for current calculation only. and click OK.

12

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setup and Solution

You can see that neither surface monitor plot is changing and the residuals have all reached very low levels. Together, these conditions indicate the solution is converged. 9.

Save the project. File → Save Project

4.5. Displaying Results in ANSYS Fluent 1.

Plot the y+ values along the bottom wall. Postprocessing → Plots → XY Plot...

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

13

Turbulent Flow Past a Backward Facing Step a.

In the Solution XY Plot dialog box, select Turbulence... and Wall Yplus from the Y Axis Function drop-down lists.

b.

Retain the selection of Direction Vector from the X Axis Function drop-down list.

c.

From the list of Surfaces, select bottom_wall.

d.

Clear the selection of Node Values from the list of Options.

Note For 2D problems such as this, XY plots are an ideal way to check the y+ distribution. Node values have been unselected because, although y+ is calculated at wall faces, its value is stored for postprocessing in the wall adjacent cells.

e.

Click Plot.

Note These values are a little bit higher than ideal. You will see later how it affects comparison with experiment. If this were an actual study as opposed to a workshop exercise, a mesh sensitivity study should be done.

2.

Display velocity vectors. Postprocessing → Graphics → Vectors... → Edit...

14

a.

In the Vectors dialog box, enter 5 for Scale and 2 for Skip.

b.

Retain the default settings for others and click Display.

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setup and Solution Zoom in at the step and check the vectors.

Note The vectors show the recirculation zone behind the step and the subsequent reattachment of the flow. Adjust the Scale and Skip settings for optimal viewing of the vectors.

c. 3.

Close the Vectors dialog box.

Exit Fluent. File → Close Fluent

4.

In Workbench, save the project. File → Save

4.6. Changing the Turbulence Model 1.

In the Project Schematic, rename the Fluent system to RKE.

2.

Right-click on the Fluent cell of the RKE system and select Duplicate from the context menu.

3.

Rename the new system to SST.

4.

Double-click on Setup, cell 2, of the SST system.

5.

Click OK in the Fluent Launcher dialog box to open ANSYS Fluent.

6.

Enable the - omega model. Setting Up Physics → Models → Viscous... Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

15

Turbulent Flow Past a Backward Facing Step a.

In the Viscous Model dialog box, select k-omega from the Model list.

b.

Select SST from the k-omega Model group.

c.

Retain the other default settings and click OK to accept the model and close the Viscous Model dialog box.

Note In Fluent, the turbulence models that use omega do not require the selection of a near wall treatment. This is because the near wall treatment that is used is a y+ insensitive method. This means it automatically behaves either as a viscous sublayer resolving treatment or as a wall function, depending on how fine or coarse the near wall mesh is.

7.

Initialize the solution as before and run for 100 iterations. Solving

8.

As done previously, delete and then add the report plots (Step 4.4.6 (p. 9)), change the convergence criteria of continuity to 1e-06 (Step 4.4.7 (p. 11)), and then calculate an additional 100 iterations.

As you can see, the convergence is good. 9.

Check the y+ values. Postprocessing → Plots → XY Plot...

16

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setup and Solution

Y+ is qualitatively similar. 10. Save the project. File → Save Project 11. Exit Fluent. File → Close Fluent

4.7. Displaying Results in CFD-Post 1.

Drag a Results system from under Component Systems and drop on Solution, cell 3, of the RKE system.

2.

Click on Solution, cell 3, of the SST system and drag to Results, cell 2, of the Results system.

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

17

Turbulent Flow Past a Backward Facing Step

3.

Double-click Results, cell 2, to launch CFD-Post.

4.

Change the graphics window layout so that the two wireframes are displayed one below the other

5.

Lock the views and visibility so that they are synchronized

6.

Click the vector button

.

in the toolbar.

a.

Retain the default name in the Insert Vector dialog box and click OK.

b.

In Details of Vector 1, select symmetry 1 from the Locations drop-down list.

Note For 2D models, CFD-Post extrudes the geometry a small distance in the 3rd direction. The resulting symmetry planes are used for results display.

18

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

.

Setup and Solution c.

Enter 2 for Factor.

Note Changing the reduction factor to 2 means that only every other vector will be displayed, which makes the vectors easier to see.

d.

In the Symbol tab, enter 0.5 for Symbol Size.

e.

Click Apply and zoom in to the region near the step.

As you can see, both velocity fields are very similar. 7.

You will use variables and expressions to compare the results. a.

Above the tree, click the Expressions tab. i.

Right-click in the Expressions area and select New from the context menu.

ii.

In the New Expression dialog box, enter step height for Name and click OK.

iii.

In Details of step height, enter the following for expression:

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

19

Turbulent Flow Past a Backward Facing Step ave(Y)@inlet_bottom - ave(Y)@bottom_wall

Note You can right-click in the details field for context menus to add functions and locations without having to type them manually.

iv.

Click Apply.

Note The value displayed is 0.0127 [m]. It is also possible to type 0.0127 [m] in the Definition field. Defining the expression as shown here will allow it to update automatically if the step height were to be changed, for instance in a parametric study.

20

b.

Create another expression for the dimensionless X-coordinate, named xh expression, and define it as X / step height .

c.

Create a variable to use the previous expression to plot the wall shear stress. i.

Click the Variables tab.

ii.

Right-click and select New from the context menu. Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setup and Solution

d.

iii.

In the New Variable dialog box, enter Xh for Name and click OK.

iv.

In Details of Xh (scalar), retain the selection of Expression from the Method drop-down list.

v.

Select xh expression from the Expression drop-down list and click Apply.

Define a polyline to plot the wall shear stress.

i.

From the Location drop-down list in the toolbar, click Polyline.

ii.

Retain the default name in the Insert Polyline dialog box and click OK.

iii.

In Details of Polyline 1, select Boundary Intersection from the Method drop-down list.

iv.

Select symmetry 1 from the Boundary List drop-down list.

v.

Retain the selection of bottom_wall from the Intersect With drop-down list and click Apply.

Note There is more than one way to define this polyline, but the Boundary Intersection method is the most convenient in this case and its use ensures the polyline definition would remain consistent if changes were made upstream in the project workflow.

e.

Create a chart. Insert → Chart i.

Retain the default name in the Insert Chart dialog box and click OK.

ii.

In Details of Chart 1, click the Data Series tab.

iii.

Select Polyline 1 from the Location drop-down list.

iv.

In the X Axis tab, select Xh from the Variable drop-down list.

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

21

Turbulent Flow Past a Backward Facing Step

v.

In the Y Axis tab, select Wall Shear X from the Variable drop-down list.

Note Wall Shear X is used instead of Wall Shear because the location where it changes sign identifies the flow reattachment point.

vi.

Click Apply.

Note The reattachment point is identified where the shear stress changes sign (around 6 Xh). Also, the positive values very close to the step indicate the presence of a small secondary recirculation zone. This can also be seen by zooming in on the vector plot and increasing the symbol size. The size and strength of the recirculation zone predicted by either model is remarkably similar. However, because of the proximity of the inlet to the step, the use of uniform inlet profiles is questionable.

22

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setup and Solution

f.

Add external data to chart. i.

In Details of Chart 1, click the Data Series tab.

ii.

Right-click and select New from the context menu.

iii.

Select Series 2 in the list.

iv.

Select File in the Data Source group box.

v.

Click the Browse button next to it and go to your working folder.

vi.

In the Import CFX Data File dialog box, at the bottom, select All Files from the Files of type drop-down list.

vii. Select x-wall-shear-ds.csv from your working folder and click Open. viii. Click the Line Display tab. A.

Select None from the Line Style drop-down list.

B.

Select X Cross from Symbols drop-down list.

C.

Select black from the Symbol Color drop-down list.

D.

Click Apply. Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

23

Turbulent Flow Past a Backward Facing Step

Note The external data is from the experiment of Driver and Seegmiller. Agreement between the CFD results and the data is not very good, however the uniform inlet boundary conditions do not correspond to those seen experimentally in the same location.

4.8. Changing the Inlet Boundary Condition In the following steps, more accurate, non-uniform velocity and turbulence profiles will be applied at the inlet in order to mimic the experimental conditions. 1.

In Workbench, right-click on the RKE system and select Duplicate from the context menu.

2.

Rename the new system as RKE Profile.

3.

Double-click on Setup, cell D2, of the RKE Profile system.

4.

Click OK in the Fluent Launcher dialog box to open ANSYS Fluent.

5.

Read the profile file. Setting Up Physics → Zones → Profiles...

24

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setup and Solution

6.

a.

In the Profiles dialog box, click Read....

b.

From your working folder, select rke-prof.prof and click OK.

c.

Close the Profiles dialog box.

Set the profile to the inlet boundary condition. Setting Up Physics → Zones → Boundaries → Inlets

a.

In the Boundary Conditions task page, double-click on inlet_v.

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

25

Turbulent Flow Past a Backward Facing Step b.

In the Velocity Inlet dialog box, select Components from the Velocity Specification Method dropdown list.

c.

Select x-coordinate-3 x-velocity from the X-Velocity (m/s) drop-down list.

d.

Select x-coordinate-3 y-velocity from the Y-Velocity (m/s) drop-down list.

e.

Select K and Epsilon from the Specification Method drop-down list in the Turbulence group box.

f.

Select x-coordinate-3 turb-kinetic-energy from the Turbulent Kinetic Energy (m2/s2) drop-down list.

g.

Select x-coordinate-3 turb-diss-rate from the Turbulent Dissipation Rate (m2/s3) drop-down list.

h.

Click OK to close the Velocity Inlet dialog box.

Note The non-uniform profiles were produced by running an auxiliary calculation of the wind tunnel section upstream of the inlet to generate a profile with the same boundary layer thickness as the experiment.

7.

Initialize the solution and run for 100 iterations. Solving

8.

26

Following the same steps as before, delete and then add the report plots (Step 4.4.6 (p. 9)), change the convergence criteria of continuity to 1e-06 (Step 4.4.7 (p. 11)), and then calculate an additional 100 iterations.

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setup and Solution As you can see, the convergence behavior is good with the new boundary conditions.

Note By creating a duplicate of the original Fluent object, it was not necessary to redefine any of the solution monitors, material properties or solver settings. Only the boundary conditions needed to be changed.

9.

Check the inlet velocity profile. Postprocessing → Plots... → XY Plot... a.

In the Solution XY Plot dialog box, enter 0 for X and 1 for Y under Plot Direction.

b.

Select Velocity... and X Velocity from the Y Axis Function drop-down list.

c.

Select inlet_v from the list of Surfaces.

d.

Click Axes.

e.

i.

In the Axes - Solution XY Plot dialog box, select X from the Axis group.

ii.

Under Options enable Major Rules and Minor Rules.

iii.

Click Apply.

iv.

Similarly, select Y from the Axis group and enable Major Rules and Minor Rules.

v.

Click Apply and close the Axes - Solution XY Plot dialog box.

In the Solution XY Plot dialog box, click Plot.

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

27

Turbulent Flow Past a Backward Facing Step

The profile is from a developing boundary layer with freestream velocity = 44.2 m/s and a boundary layer thickness just below 2 cm, as measured in the experiment. 10. Save the project and close Fluent. File → Save Project... 11. Similar to the steps followed previously, duplicate the SST system in Workbench and rename it as SST Profile. 12. Open Fluent from the SST system and read the profile file sst-prof.prof. Setting Up Physics → Zones → Profiles... 13. Set the profile to the inlet boundary condition (inlet_v) as shown in the table below. Setting Up Physics → Zones → Boundaries → Inlets Component

28

Value

Velocity Specification Method

Components

X-Velocity

x-coordinate-3 x-velocity

Y-Velocity

x-coordinate-3 y-velocity

Turbulence Specification Method

K and Omega

Turbulent Kinetic Energy

x-coordinate-3 turb-kinetic-energy

Specific Dissipation Rate

x-coordinate-3 specific-diss-rate

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setup and Solution 14. Initialize the solution and run for 100 iterations. Then, delete the report plots and add them back (Step 4.4.6 (p. 9) ), and continue iterating for 100 iterations after changing the convergence criteria of continuity to 1e-06 (Step 4.4.7 (p. 11)).

Note Select Yes if prompted whether to add a new file. (This happens in SST case. It is because, Workbench is writing the report plot files to the directory where the .prof files are located, and not to the directory in the Workbench project.)

15. Save the project and close Fluent. File → Save Project... 16. In the Workbench Project Schematic, duplicate the Results system and rename the new one as Results with Profiles. 17. Right-click on the connection of Results with Profiles with the SST system and select Delete from the context menu.

18. Similarly, delete the connection of Results with Profiles with the RKE system. 19. Click on Solution, cell 3, of the RKE Profile system and drag to Results, cell 2, of the Results with Profiles system. 20. Add a similar connection from the SST Profile system to Results with Profiles.

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

29

Turbulent Flow Past a Backward Facing Step

21. Double-click on Results, cell 2, of the Results with Profiles system to open CFD-Post. 22. Double-click on Chart 1 in the tree and check the updated plot of comparison.

30

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Further Improvements As the original Results cell was duplicated, none of the setup steps, such as defining variables and expressions and loading the experimental data, needed to be repeated.

Note Use of realistic, non-uniform velocity and turbulence profiles at the inlet greatly improves the agreement between the results and the experiment. These results do not represent a formal validation study. In particular, the issue of mesh independence has not been addressed here. The intent of this workshop is to show how to run turbulent flow calculations, the importance of boundary conditions and how Workbench can be used to compare results from different turbulence models.

5. Summary This workshop has shown the steps for setting up and solving a turbulent flow: • Selecting the model and if necessary the near wall treatment. • Checking wall y+. • Running a simulation and using both residuals and solution monitors to determine convergence. • Post-processing the results, both in Fluent and CFD-Post. When solving a particular type of flow for the first time, it can be useful to compare results from different turbulence models and compare with data if available.

6. Further Improvements There are many ways the simulation in this tutorial could be extended: Mesh independence • Check that results do not depend on the mesh. • Use Adapt → Region to adapt all the cells in the mesh and re-run the calculation. Turbulence profile effects To see whether the use of detailed turbulence profiles matters, run the profile cases using the x-velocity profile. The intensity and hydraulic diameter for turbulence should be as in the original setting.

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

31

32

Release 17.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.