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

2d Airfoil simulation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 8, 2015, 12:24
Exclamation 2d Airfoil simulation
  #1
New Member
 
Join Date: Jan 2015
Posts: 10
Rep Power: 2
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, 12:33
Default
  #2
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 672
Rep Power: 13
LuckyTran will become famous soon enough
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, 12:26
Default
  #3
New Member
 
Join Date: Jan 2015
Posts: 10
Rep Power: 2
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, 06:29
Default
  #4
AHF
New Member
 
amirhossein
Join Date: Jul 2014
Posts: 4
Rep Power: 3
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, 07:12
Default
  #5
New Member
 
Join Date: Jan 2015
Posts: 10
Rep Power: 2
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, 12:06
Default
  #6
New Member
 
Join Date: Mar 2015
Posts: 12
Rep Power: 2
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, 05:17
Default
  #7
New Member
 
Join Date: Mar 2015
Posts: 12
Rep Power: 2
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, 09:49
Default
  #8
New Member
 
Join Date: Jan 2015
Posts: 10
Rep Power: 2
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, 09:53
Default
  #9
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 672
Rep Power: 13
LuckyTran will become famous soon enough
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, 12:56
Default
  #10
New Member
 
Join Date: Jan 2015
Posts: 10
Rep Power: 2
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, 13:07
Default
  #11
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,948
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
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, 09:31
Default
  #12
New Member
 
Join Date: Jan 2015
Posts: 10
Rep Power: 2
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

Reply

Tags
2d simulation, airfoil, mesh independency, turbulence

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
Problem with airfoil shape optimization robyTKD SU2 Shape Design 6 June 13, 2013 19:13
Problem with restart solution in shape_optimization.py robyTKD SU2 Shape Design 21 May 29, 2013 09:26
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 CD-adapco 9 June 21, 2006 10:47


All times are GMT -4. The time now is 20:12.