Turbulent flow around a bluff rectangular plate CFD Lab in SG2218 – 2016 Stefan Wallin Department of Mechanics, KTH
Aim We have learned in the lectures that standard eddy‐viscosity RANS models (EVM) have some limitations and that different improvement and corrections are available. In this lab we will look at the interaction between stagnation and separated flow by CFD computations of the turbulent flow around the bluff plate shown below. One of the problems with std EVM is excessive production of turbulence in stagnation regions seen in the example computation below. High turbulence levels are convected into the separated region resulting in a severe underprediction of the separation length. Your task is to confirm this deficit of std EVMs and to demonstrate the improvements available.
Figure 1. Experimental setup (top) and computational results (streamlines and turbulence kinetic energy) using one std EVM (bottom) (ref: N. Djilali and I. S. Gartshore (1991), “Turbulent Flow Around a Bluff Rectangular Plate, Part I: Experimental Investigation,” JFE, Vol. 113, pp. 51–59.)
Case definition The case is geometrically very simple and defined in Figure 1. The experiment is made in a low‐speed wind tunnel and incompressible flow can be assumed (Mach number less than 0.2). The Reynolds number based on the plate thickness ≡
and incoming velocity
is
50 000
where
is the kinematic viscosity. The incoming isotropic turbulence level can be prescribed
as
1% and the turbulence length scale Λ
. These are defined as
/
≡ ≡
where
,
≡
, Λ ≡ /2 and are the rms of the stream‐wise
fluctuations, turbulence kinetic energy and dissipation rate respectively. Isotropic turbulence 2 /3. Figure 2 shows the experimental skin friction and
implies that
pressure coefficients defined as ≡
where
≡
,
1 2
is the wall skin friction and
≡
and
1 2 are the free‐stream density and
pressure respectively. The experimental data are available in text files. The experimentally observed reattachment point is
/
4.7.
Figure 2. Experimental skin friction and pressure coefficients.
Computational setup The computational mesh is provided and consists of about 26 000 nodes and elements (shown in Figure 3). Symmetry is utilised so only the half geometry is meshed. The thickness of the near‐wall cells are about 80μm resulting in
≲ 1. The plate thickness
0.1m, the
height of the domain is 1m, the upstream and downstream extents are 1m and 2m respectively. The following boundary conditions apply:
inlet: Velocity inlet. Set inlet velocity and turbulence levels.
outlet: Pressure outlet. Set pressure.
upper: Symmetry. Prescribing symmetry will approximately act as a wind‐tunnel wall.
sym: Symmetry. This is the boundary upstream of the plate where symmetry applies.
frontwall: Wall. This is the upstream vertical part of the plate.
upperwall: Wall. This is the upper wall of the plate.
Use air at std. atmosphere conditions ( 288.16K,
1.225kg/m ,
≡
1.7894 ⋅ 10 kg/ms,
101325Pa). Set the incoming velocity and turbulence quantities to match
the experimental case definition.
Figure 3. Computational domain and mesh. Right figure is a zoom in on the corner.
Expected results You must complete all assignments specified below and present the results in the lab report. 1. Matching the experimental setup. a. What is the inlet velocity ( ) and turbulence quantities ( and ) used for matching the experimental case definition. b. What is the corresponding Mach number. 2. Turbulence model results. a. For each turbulence model result, plot the velocity magnitude, stream lines, turbulence kinetic energy ( ) and production of turbulence kinetic energy ( similar to the plots in Figure 1. Use the same colour scale for all plots for easy comparison. b. Make one diagram with
with experimental data as symbols (as in Figure 2)
and each model as a line with different line styles or colours. Export the pressure ( ) from the computations to e.g. matlab, compute
according to
the definition and plot. Note that the absolute pressure is irrelevant for the incompressible assumption and that c. Make one diagram with
0 is default in Fluent.
with experimental data as symbols (as in Figure 2)
and each model as a line with different line styles or colours. Export the skin friction (
) from the computations to e.g. matlab, compute
according to
the definition and plot. Use the same line styles and colours as for
.
d. Make one diagram with turbulence kinetic energy ( ) along the symmetry line upstream of the plate. Use the same line styles and colours as for
.
3. Discussion and analysis Compare the different results and try to explain the different sizes of the separation bubble by the turbulence levels in the stagnation region. Why do the different models show such large differences in the stagnation region?
)
Fluent setup and running The zip file FluentLabSG2218.zip contain:
ANSYS Workbench setup (FluentLabSG2218.wbpj, FluentLabSG2218_files)
Fluent mesh file (BluntPlate.msh)
Publication of the experiment Djilali_Gartshore_JFE_1991‐Expr.pdf)
Experimental data (Cp.tab, Cf.tab)
This file (CFD‐lab.pdf)
You can open and use the ANSYS workbench setup including the geometry and mesh. Most settings are here predefined. Alternatively, you can open the Fluent mesh directly in Fluent and do all settings yourself. Or you can import the Fluent mesh to your favourite CFD solver (e.g. OpenFOAM) and do the computations there. You don’t need to use Fluent and you can replace some of the turbulence models if they are missing in your CFD solver. Start ANSYS Workbench Available under All Programs ‐> ANSYS ‐> Workbench Open: FluentLabSG2218.wbpj Here you will see the setup of the test case. The Geometry and Mesh are already available. And also the basic Setup of the case in Fluent. You are free to modify everything.
Start Fluent Double‐click on Solution to open Fluent. (press Yes to any warning of changed upstream data). You should see the following mesh when Fluent have started.
You now have the following menu on the left side
Most things are already setup, mostly with default values. In the following, the necessary steps are explained Turbulence model Under Tree ‐> Setup ‐> Models ‐> Viscous, press Edit. Here you will choose the turbulence model. The standard k‐eps model is already chosen. Use enhanced wall treatment, which will be able to handle any near‐wall resolution. The mesh is too fine to use wall function BCs. The different turbulence models you should test are: 1. Std k‐eps: k‐epsilon + Standard + Enhanced Wall Treatment. 2. Realizable k‐eps: k‐epsilon + Realizable + Enhanced Wall Treatment. 3. Std k‐omega: k‐omega + Standard (uncheck all options). 4. SST k‐omega: k‐omega + SST + Production Limiter. 5. RST k‐omega: Reynolds Stress + Stress BSL. For each turbulence model you can either do a new initialization of the solution or continue to run from the previous solution. You are also very welcome to try other models and model options. The complete documentation is available under the small ? at the top right corner. The turbulence models are documented at: Users Guide ‐> Fluent ‐> Theory Guide ‐> Turbulence. Boundary conditions Under Tree ‐> Setup ‐> Boundary Conditions: All boundary condition types are already set according to the setup earlier in this document. The values on the inlet boundary must be set. Mark inlet and press Edit.
Here you should give Velocity Magnitude, Turbulent Intensity and Turbulent Length Scale in order to match the Reynolds number and the setup. Reference Values Under Tree ‐> Setup ‐> Reference Values you will see
Here you need to set the reference values for the normalized. The Area and Length should be
and
coefficients to be correctly
0.1m. The other data should be the same as
the inlet boundary condition. You can easily do that by choosing Compute from ‐> inlet. Solution Monitor Under Tree ‐> Solution ‐> Monitors, choose Residuals and press Edit.
We will avoid using any convergence criteria, so uncheck Check Convergence for all equation. You might need to scroll down to see and uncheck everything. Instead we will use a certain number of iterations. Under Tree ‐> Solution ‐> Monitors, you can also define to monitor the convergence of other properties. It is recommended to monitor a typical global force and the
coefficient is
chosen to be plotted during the iteration to steady state. Solution Initialization Under Tree ‐> Solution ‐> Solution Initialization, choose Hybrid Initialization and press Initialize. This will compute the case with a coarse grid and simplified physics and numeric. Takes a few seconds. After initialization you can plot the velocity field if you are interested (see below for plotting). Run Calculation Under Tree ‐> Solution ‐> Run Calculation, set Number of Iterations to 500 and press Calculate. During iteration you can monitor the cd‐1 and the residuals. 500 iterations might not be enough. You can press Calculate one more time if you want to do another 500 iterations. You can compare the solution after 500 and 1000 iterations to see if there are any differences. If not, 500 iterations are sufficient. You should also look at the residuals, which should monotonically decrease at least during the last 3‐400 iterations and the largest residual should be smaller than 10 . Colour Plotting Under Tree ‐> Results ‐> Graphics, choose Contours and press Set Up. E.g. plot the positive x‐velocity using the following setting.
The image can be saved by using the camera symbol in the plotting window. X‐Y Plots Under Tree ‐> Results ‐> Plots, choose XY Plot and press Set Up. E.g. plot the upperwall skin friction using the following setting:
The thickness of the first near‐wall cell in terms of
can be plotted by Turbulence ‐> Wall
Yplus. along the wall is plotted by Pressure ‐> Pressure Coefficient. Turbulence quantities along the symmetry line upstream of the plate can be plotted by choosing the sym surface and plot Turbulence ‐> Turbulent Kinetic Energy (k) or Production of k. There is an option Write to File that should be used for exporting the data to a text file. Edit the text file to keep only the data table to import into matlab, python or excel for normalization and plotting. The data is not necessary written in any particular order and you might need to sort the data for increasing plotting.
in order to be able to use line styles in the
