CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Flat plate analysis in cfx

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree3Likes
  • 1 Post By Far
  • 1 Post By ghorrocks
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   July 10, 2012, 00:55
Default Flat plate analysis in cfx
  #1
Member
 
Hamed Abdul Majeed
Join Date: May 2012
Posts: 72
Rep Power: 5
hamed.majeed is on a distinguished road
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.



Meshing
Meshing of the flat plate is done by “Edge sizing”.



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




Boundary conditions
Inlet


Uinf = 17.8 m/s inserted as an expression.
Outlet


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.





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:



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)



Numerical vs. Experimental (k ε turbulence model)

hamed.majeed is offline   Reply With Quote

Old   July 10, 2012, 00:57
Default
  #2
Member
 
Hamed Abdul Majeed
Join Date: May 2012
Posts: 72
Rep Power: 5
hamed.majeed is on a distinguished road
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.
hamed.majeed is offline   Reply With Quote

Old   July 10, 2012, 01:08
Default
  #3
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by hamed.majeed View Post
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.
This is not a valid reason at all.


But It is overall good work and thanks for sharing whole procedure with forum.
Far is offline   Reply With Quote

Old   July 10, 2012, 12:33
Default
  #4
Member
 
Hamed Abdul Majeed
Join Date: May 2012
Posts: 72
Rep Power: 5
hamed.majeed is on a distinguished road
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
hamed.majeed is offline   Reply With Quote

Old   July 10, 2012, 19:26
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   July 10, 2012, 22:40
Default
  #6
Member
 
Hamed Abdul Majeed
Join Date: May 2012
Posts: 72
Rep Power: 5
hamed.majeed is on a distinguished road
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
hamed.majeed is offline   Reply With Quote

Old   July 12, 2012, 11:52
Default Verification of the results
  #7
Member
 
Hamed Abdul Majeed
Join Date: May 2012
Posts: 72
Rep Power: 5
hamed.majeed is on a distinguished road
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.



Results for 5 x refined grid in x direction


hamed.majeed is offline   Reply With Quote

Old   July 12, 2012, 11:54
Default mesh refining needed for mesh independency
  #8
Member
 
Hamed Abdul Majeed
Join Date: May 2012
Posts: 72
Rep Power: 5
hamed.majeed is on a distinguished road
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.
Meshing for flat plate immersed solid
Thank you.

Regards
Hamed
hamed.majeed is offline   Reply With Quote

Old   July 12, 2012, 12:18
Default
  #9
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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.
hamed.majeed likes this.
Far is offline   Reply With Quote

Old   July 12, 2012, 18:45
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
hamed.majeed likes this.
ghorrocks is offline   Reply With Quote

Old   July 14, 2012, 00:43
Default
  #11
Member
 
Hamed Abdul Majeed
Join Date: May 2012
Posts: 72
Rep Power: 5
hamed.majeed is on a distinguished road
Thank you.
Please could you help me out with the following mesh requirement for flat plate.
Meshing for flat plate immersed solid
I am using the cfx mesh.

Regards
Hamed
hamed.majeed is offline   Reply With Quote

Old   July 14, 2012, 02:34
Default
  #12
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,098
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
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.
flotus1 is offline   Reply With Quote

Old   February 4, 2015, 06:55
Default
  #13
New Member
 
Nazanin Ansari
Join Date: Sep 2013
Posts: 4
Rep Power: 3
ansari.nazanin is on a distinguished road
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!
ansari.nazanin is offline   Reply With Quote

Old   February 4, 2015, 07:00
Default
  #14
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ansari.nazanin likes this.
ghorrocks is offline   Reply With Quote

Old   February 4, 2015, 08:07
Default
  #15
New Member
 
Nazanin Ansari
Join Date: Sep 2013
Posts: 4
Rep Power: 3
ansari.nazanin is on a distinguished road
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?
Attached Files
File Type: docx Beleg-Englisch.docx (73.3 KB, 13 views)
ansari.nazanin is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Importing or Creating 2D Flat Surfaces into CFX Sam CFX 5 March 30, 2013 12:11
k-omega-SST model (OF 1.6) - turbulent flat plate cboss OpenFOAM Running, Solving & CFD 23 November 13, 2011 02:28
laminar flow on flat plate AmirFluid Main CFD Forum 7 June 22, 2010 05:49
CFX vs. Fluent for coupling analysis aspirany CFX 3 January 21, 2010 00:25
Free convection flow over vertical flat plate Polly Main CFD Forum 1 February 11, 2003 14:25


All times are GMT -4. The time now is 21:51.