Flat plate analysis in cfx
 

Hi,
I have done a subsonic flow over a flat plate in ANSYS CFX. Please have a look on the analysis and give any suggestions possible. I have created a tutorial type analysis for anyone to easily replicate. Please do give your input.
My plans in future are to actually test the boundary layer (viscous) using Immersed Boundary Method. Also, suggest any recommendations for that.
Thank you.


Problem statement
Consider flow over a flat plate of length 5 m. Free stream velocity is Uinf = 17.8 m/s. y+ value for flat plate is 50. Turbulent model used is SST and k ε.
The values of these parameters are taken from [1].

Two analyses are performed mentioned below:
1. Transient problem
2. Immersed body problem


The flow model selected is either k epsilon or SST, both are used here.


Transient problem
I used Design modeler for modeling of flat plate. CFX meshing is used for meshing. ANSYS V. 14 was used for the analysis. The problem is dealt as 2D case, however, in CFX 2D cases are dealt by creating 3D domain with thickness of one element size. Symmetry conditions are applied on opposite faces.
Estimate y+
y+ is the non-dimensional distance from the wall. It is used to measure the distance of the first node away from the wall. Thus, meshing can be defined by considering y+.
Estimate y+ using the formula:

Δy is the actual distance between the wall and first node [this indicates the mesh needed].
L is a flow length scale
y+ is the desired y+ value
ReL is the Reynolds Number based on the length scale L
In our problem y+ is taken 50. Thus we find Δy.
y+ = 50, L = 5m, kinematic viscosity of air = 1.51×〖10〗^(-5) m^2/s (white)
〖Re〗_L=UL/ν=((17.8 m/s)×5m)/(1.51×〖10〗^(-5) m^2/s)≈6×〖10〗^6
Reynolds number such high indicates that the flow is turbulent.
Thus, Δy = 0.00109 m
This is the distance of 1st node from the plate.
Also for turbulent flow, the boundary layer thickness δ is,
δ_T=(0.382×L)/(〖Re〗_L^0.2 ) = 0.084 m
Since the boundary layer is of thickness 0.084 m we let the domain of width 10 times of boundary layer thickness i.e. width of domain = 0.42 m


Geometry
Geometry is created in Design Modeler. Create > Primitives > Box, is used to create a box of dimensions 5 m × 0.42 m × 0.00109 m.
http://s19.postimage.org/ke3ru73s3/untitled1.png


Meshing
Meshing of the flat plate is done by “Edge sizing”.
http://s19.postimage.org/naqsuh9lv/untitled2.png


Setup
Double click on the “Default Domain. Setup the following.

http://s19.postimage.org/95kzso0kj/untitled3.png


Boundary conditions
Inlet

http://s19.postimage.org/k6g4xostf/untitled4.png
Uinf = 17.8 m/s inserted as an expression.
Outlet
http://s19.postimage.org/la4une2ub/untitled5.png

Symmetry
The front and back faces are given symmetry boundary conditions.


Top
The top of the fluid domain can be given any one of the following boundary conditions.
1. Inlet Boundary condition with Uinf = 17.8
2. Symmetry boundary condition
3. Free shear wall boundary conditions.
I used option 3 for top BC.

http://s19.postimage.org/h3k08238j/untitled7.png
http://s19.postimage.org/5fpydie3n/untitled8.png


Setup Solver Controls
In the model tree, Simulation > Flow Analysis 1 > Solver > Solver control (double click)
Advection Scheme > High Resolution
Minimum Iterations > 1
Maximum Iterations > 1000
Convergence criteria:
Residual type> RMS
Residual target > 1e-7 > OK

[please suggest how do I optimize these parameters]

Expressions
Expressions are inserted here to be used either in chart or reference for later changes.
Uinf is the inflow velocity, here Uinf = 17.8
cF is the friction coefficient


Results
Contour plot
We need to plot velocity contour around the plate.
Insert (menu bar) > Contour > enter Velocity > OK
Domain > All domains
Location > symmetry1
Variable > Velocity
# of contours = 100 > Apply
The contour plot created is as follows:
http://s19.postimage.org/za6wfj4kj/untitled10.png


Velocity vs. Perpendicular distance from the wall
Creating a line perpendicular to the plat
Insert (menu bar) > Location > Line > keep name Line 1 > Ok
Let the 2 ends of the Line 1 be at (5, 0, 0) & (5, 0.15, 0) > Enter these co-ordinates
Line type > Sample > 100 > Apply
Creating a chart
Insert > Chart > Chart 1 > OK
(Tab) General > Type -XY
(Tab) Data series > Click on New > Location Line 1
(Tab) X-Axis > variable –Velocity (from drop down menu)
Y-Axis > variable –Y (displacement)

CF skin friction coefficient vs. X
Create line (polyline 2) along the length of the plate. Experimental results are taken from a CP.csv file Experimental values are the incompressible flow over a smooth flat plate originally reported by Wieghardt [2] and later included in the 1968 AFOSR-IFP Stanford Conference on turbulent flows [3]. Insert a new variable by the name CF.

Results
The boundary layer thickness closely matches with the value of boundary layer calculated empirically.
Numerical vs. Experimental (SST turbulence model)

http://s19.postimage.org/fgusmtr6r/untitled11.png

Numerical vs. Experimental (k ε turbulence model)

http://s19.postimage.org/582bh034z/untitled12.png

My email address is
hamed_majeed@hotmail.com

Comments
We observe that k-epsilon performs better than SST model. This is because the mesh used was with y+ 50 which is good for k epsilon model.
References
[1]. http://www.grc.nasa.gov/WWW/wind/val...rb/fpturb.html
[2]. Wieghardt, K., and Tillman, W., "On the Turbulent Friction Layer for Rising Pressure," NACA TM-1314, 1951.
[3]. Coles, D.E., and Hirst, E.A., Computation of Turbulent Boundary Layers-1968 AFOSR-IFP-Stanford Conference, Vol. II, Stanford University, CA, 1969.

This is not a valid reason at all.


But It is overall good work and thanks for sharing whole procedure with forum.

Well I gained concepts about y+ in the following research paper.
y+ strategy for dealing with wall bounded turbulent flow by Salim .M. Salim, and S.C. Cheah. It is an excellent paper regarding y+ understanding. Here is the link.
http://www.iaeng.org/publication/IME...p2165-2170.pdf

Thank you.
Regards
Hamed

You really should do a mesh and convergence sensitivity study before you make conclusions about one turbulence model being more accurate than another. For a model like this I would expect both models to be more accurate than the results you show.

Hi,
The research paper after doing a series of cfd experiments on grids with varying y+. I mentioned earlier gave the following conclusion.

1. For y+ <= 1 use the SST k omega turbulence model.
2. For y+ <=50 use the k epsilon turbulence model.

Since, the grid I created was considered for y+ = 50, so the k epsilon model should hold valid. If SST is to be used I might need to refine the grid further.
And yes you people are right, I need to check for mesh independency for final conclusion.
Thank you.

Regards
Hamed

Verification of the results
 

Verification of the results

For tolerance of 1e-5 and no. of divisions along x axis 5 times of previous case (to check mesh independency). Monitor object is the velocity at exit of the plate, shown below.

http://s19.postimage.org/467cdcfs3/Untitled13.png
http://s19.postimage.org/az7p9m6lf/Untitled14.png
Results for 5 x refined grid in x direction

http://s19.postimage.org/lbyl9fpib/Untitled15.png
http://s19.postimage.org/r1ettqvoj/Untitled16.png

mesh refining needed for mesh independency
 

Hi

Can anybody tell me what should be the mesh refining criterion for testing mesh independency. A valid reference would be beneficial.
I have heard that we may increase the number of elements to 2 times for three runs!
Also, guys help me out with the following mesh creation, just reply on the respective page.
http://www.cfd-online.com/Forums/ans...sed-solid.html
Thank you.

Regards
Hamed

First of all, I would like to say nice work done and thanks for sharing again. You can increase mesh in x and y by the factor of 1.44 so that you get the 2*mesh size for next level of refinement. For example you have mesh size 100 * 30 = 3000 and now you have (100*1.44)*(30*1.44)= (100*30)*2 = 6000. Try to keep the first cell distance same from the wall.

This FAQ has a link to soem very useful information about mesh sensitivity studies: http://www.cfd-online.com/Wiki/Ansys...publishable.3F

The textbook "Computational Fluid Dynamics" by Roache is the key textbook in the field of CFD accuracy. If you really want to know the details of CFD accuracy have a read of it.

Thank you.
Please could you help me out with the following mesh requirement for flat plate.
http://www.cfd-online.com/Forums/ans...sed-solid.html
I am using the cfx mesh.

Regards
Hamed

For hexahedral meshing, I would not recommend the Ansys mesher.
There are workarounds to get what you want, but compared to tools like ICEM, the amount of work is much higher.

Once you want to mesh slightly complex geometry with hexahedrons, you can forget about the Ansys mesher.
So try a "real" meshing program like ICEM, it is worth the time you spend learning it.

Can you please tell me if u use an expression for plotting the Cf? i should do the same for a backwarding step and compare the results with DNS ones and i have not yet figured out how to do it!

Do you mean skin friction coefficient? http://www.cfd-online.com/Wiki/Skin_...on_coefficient

Easy. Put this in CFD-Post as variables:
Uinf = {whatever your free stream or reference velocity is}
C = Wall Shear Stress / (0.5*density*Uinf^2)

Done. Note the variable will only exist on wall boundaries.

Thanks for the quick reply!
the problem is the inlet velocity is derived from a *.csv data from the DNS as well which i used as the Inlet Velocity, i should plot the Cf in the bottom wall, but i cannot find the right expression for it!
And could you please tell me how can i calculate the turbulent kinetik energy?