CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

2d Airfoil simulation

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

Like Tree1Likes
  • 1 Post By Far

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 8, 2015, 13:24
Exclamation 2d Airfoil simulation
  #1
New Member
 
Join Date: Jan 2015
Posts: 24
Rep Power: 9
Athos1387 is on a distinguished road
hi,
I'm simulating a NACA0021 with 2ddp FLUENT. I've got some problems and would be happy if anyone could help. the info is as below:
Chord based Re = 120,000
v=25 m/s
AOA = 8 deg.
Turbulence method = k-w SST , transitional flow
till now used both SIMPLE and SIMPLEC for coupling
Pressure - PRESTO!
the rest - 2nd order upwind

so one problem is the refiner my mesh becomes, the amount of Cl and Cd become more different from the experimental data. WHY?!!!
second problem is, my Cl and Cd are 10 times smaller than the experimental data. WHY?!!!
and I would like to know which coupling is better to use. also for pressure and other equations which scheme is better to use.
oh and can anyone tell me the amount of elements in the mesh that are around enough for mesh independency?
thanks.
Athos1387 is offline   Reply With Quote

Old   August 11, 2015, 13:33
Default
  #2
Senior Member
 
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,069
Rep Power: 60
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
I think you should focus on why your drag and lift coefficients are off. Have your checked your reference values?

SIMPLE & SIMPLEC should be ok. SIMPLEC allows higher urf for faster convergence than SIMPLE. The fullly COUPLED algorithm is not a bad choice if you are unsure. PISO is generally for transient calculations where it really outshines the SIMPLE algorithms.

I tend to prefer second order scheme for pressure, but PRESTO is probably better for airfoils.

For advected quantities, 2nd order is ok.
LuckyTran is offline   Reply With Quote

Old   August 12, 2015, 13:26
Default
  #3
New Member
 
Join Date: Jan 2015
Posts: 24
Rep Power: 9
Athos1387 is on a distinguished road
Thank you for the reply LuckyTran,
I set the reference values to compute from inlet. I really don't understand why the lift and drag coef. end up like that. I also check lift and drag convergence through the iteration.
Also I used COUPLED today and it ended way faster than the other two.
Athos1387 is offline   Reply With Quote

Old   August 13, 2015, 07:29
Default
  #4
AHF
Member
 
AHF's Avatar
 
amirhossein
Join Date: Jul 2014
Location: iran
Posts: 81
Rep Power: 10
AHF is on a distinguished road
i prefer to you use Spalart-Allmaras_model
make sure about references parameter
AHF is offline   Reply With Quote

Old   August 13, 2015, 08:12
Default
  #5
New Member
 
Join Date: Jan 2015
Posts: 24
Rep Power: 9
Athos1387 is on a distinguished road
Thank you AHF for the reply.
I set the reference values to be computed from the inlet.
Athos1387 is offline   Reply With Quote

Old   August 13, 2015, 13:06
Default
  #6
New Member
 
Ronald Thompson
Join Date: Mar 2015
Location: Portland, Oregon, USA
Posts: 25
Rep Power: 9
dynamic is on a distinguished road
Quote:
Originally Posted by Athos1387 View Post
Thank you AHF for the reply.
I set the reference values to be computed from the inlet.
Setting the reference values from the inlet is fine, but you manually have to input values for reference length, Area and depth. depth should be equal to 1 as you are doing your calculation in 2d, are and length then depend on the dimensions of your aerofoil.
dynamic is offline   Reply With Quote

Old   August 14, 2015, 06:17
Default
  #7
New Member
 
Ronald Thompson
Join Date: Mar 2015
Location: Portland, Oregon, USA
Posts: 25
Rep Power: 9
dynamic is on a distinguished road
Quote:
Originally Posted by Athos1387 View Post
Thank you AHF for the reply.
I set the reference values to be computed from the inlet.
Setting the reference values from the inlet is fine, but you manually have to input values for reference length, Area and depth. depth should be equal to 1 as you are doing your calculation in 2d, are and length then depend on the dimensions of your aerofoil.
dynamic is offline   Reply With Quote

Old   August 14, 2015, 10:49
Default
  #8
New Member
 
Join Date: Jan 2015
Posts: 24
Rep Power: 9
Athos1387 is on a distinguished road
Thanks dynamic,
I did what you suggested but it ended up in another wrong series of solutions. actually they became totally off.
Athos1387 is offline   Reply With Quote

Old   August 14, 2015, 10:53
Default
  #9
Senior Member
 
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,069
Rep Power: 60
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Quote:
Originally Posted by Athos1387 View Post
Thanks dynamic,
I'll do this, but how do I find the area?
You need to compute somewhere else what the reference area and length is and then specify those reference values in Fluent. The reference area and length are in the definition of the drag and lift coefficients. Depending on the field of study, the reference area and length may be different, so it's very important to the same definition that you are comparing your results to. Usually the reference length is the chord length and reference area is the planform area. Usually...
LuckyTran is offline   Reply With Quote

Old   August 16, 2015, 13:56
Default
  #10
New Member
 
Join Date: Jan 2015
Posts: 24
Rep Power: 9
Athos1387 is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
You need to compute somewhere else what the reference area and length is and then specify those reference values in Fluent. The reference area and length are in the definition of the drag and lift coefficients. Depending on the field of study, the reference area and length may be different, so it's very important to the same definition that you are comparing your results to. Usually the reference length is the chord length and reference area is the planform area. Usually...
Well I found out that since my simulation is 2D, the reference area and depth should be 1. The reference length is the chord C. I changed it in " report --> reference values " from 1 to 0.07 (my chord is 0.07m or 70mm) but nothing changed.
Athos1387 is offline   Reply With Quote

Old   August 18, 2015, 14:07
Default
  #11
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,552
Blog Entries: 6
Rep Power: 52
Far has a spectacular aura aboutFar has a spectacular aura about
Send a message via Skype™ to Far
Quote:
Well I found out that since my simulation is 2D, the reference area and depth should be 1. The reference length is the chord C. I changed it in " report --> reference values " from 1 to 0.07 (my chord is 0.07m or 70mm) but nothing changed.

CL and CD uses the reference density, reference velocity and reference area (0.5 * density * area * velocity^2).

So changing length (not directly) and area will affect them. (reference area = depth of wing * chord length)

Just coming to main point, change your area to 1 * 0.07 = 0.07 m^2 will do the trick...
Far is offline   Reply With Quote

Old   August 21, 2015, 10:31
Default
  #12
New Member
 
Join Date: Jan 2015
Posts: 24
Rep Power: 9
Athos1387 is on a distinguished road
Thanks Far for the reply,
I'll try it and let you know the results. actually I'm busy with something else right now.
Athos1387 is offline   Reply With Quote

Old   August 30, 2015, 09:47
Default
  #13
New Member
 
Join Date: Jan 2015
Posts: 24
Rep Power: 9
Athos1387 is on a distinguished road
Thank you Far,
the problem of the amount of Cd and Cl is solved. but still the other problem remains that the more the mesh elements become, the results have more difference from the experimental results. and I haven't reached mesh independency yet. can you help me there too?!
Athos1387 is offline   Reply With Quote

Old   August 30, 2015, 11:58
Default
  #14
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,552
Blog Entries: 6
Rep Power: 52
Far has a spectacular aura aboutFar has a spectacular aura about
Send a message via Skype™ to Far
Quote:
Originally Posted by Athos1387 View Post
Thank you Far,
the problem of the amount of Cd and Cl is solved.
What was the issue?

Quote:
but still the other problem remains that the more the mesh elements become, the results have more difference from the experimental results. and I haven't reached mesh independency yet. can you help me there too?!
mesh Independence does not imply the accuracy of your results. It is to reduce discretization errors. There are are also more source of errors. Like physical model e.g. turbulence modeling and Y+ is important aspect of this study.

Do you see the error in Cd only or both in Cd and Cl. If both then you need to worry ...
Athos1387 likes this.
Far is offline   Reply With Quote

Old   September 15, 2015, 05:05
Default
  #15
New Member
 
Join Date: Jan 2015
Posts: 24
Rep Power: 9
Athos1387 is on a distinguished road
sorry for replying this late and thank you for your help.
both of them (Cd and Cl) show the same problem. the first mesh G1 with 26600 elements is the most accurate and G4 with 117600 elements has the least accuracy and is way off course. Also G5 with 236000 elements diverges with 2-3 iterations.
i read in a paper that K-omega SST turb. model is the best for these cases, although in that paper the model was 3d but I'm trying to solve a 2d first. about Y+ actually I don't have much info and haven't found anything similar to my problem.
Athos1387 is offline   Reply With Quote

Reply

Tags
2d simulation, airfoil, mesh independency, turbulence

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Problem with airfoil shape optimization robyTKD SU2 Shape Design 7 March 7, 2022 17:18
Problem with restart solution in shape_optimization.py robyTKD SU2 Shape Design 21 May 29, 2013 10:26
Airfoil simulation using moving wall Alejandro NUMECA 9 November 4, 2008 03:00
NO STAGNATION POINT FOR AIRFOIL SIMULATION Rif Main CFD Forum 6 February 4, 2008 08:33
Compressible transonic airfoil RAE2822 simulation Stefano Siemens 9 June 21, 2006 11:47


All times are GMT -4. The time now is 07:53.