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

Need help with CFX simulation for airfoil

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 20, 2009, 20:41
Default
  #41
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,796
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
Originally Posted by Arti View Post
I did a mesh test for 50K 60K and 80K plus cells of my setup. Am now using the 80K cell as my choice. Am trying to do the lift and drag curves to confirm it with the experimental results i have. I think im getting it. Some settings were slightly off. Will try again. Thanks for the advice.
Hi,

I would be very surprised if you have achieved mesh convergence with a mesh of this size. The differences between your meshes is not enough to get meaningful results. Generally you half the element edge lengths, so you will get around 4 times as many elements per refinement in a 2D simulation or 8 times as many elements in a 3D simulation.

Until you have a mesh converged solution then there is no way your results are accurate.

Glenn Horrocks
ghorrocks is offline   Reply With Quote

Old   May 21, 2009, 02:41
Default
  #42
New Member
 
Join Date: Apr 2009
Posts: 26
Rep Power: 8
Arti is on a distinguished road
hmmm Not sure whats wrong with my software.. I can now get a better grid size with the required wall distance than those i got before. But just to ensure im going the right way.
I hope you can tell me that the way of mesh refinement that im doing is correct. The smallest number of element points i have on the airfoil is 60 top 70 bottom without any errors.
So i would have about 59 cells top and 69 cells bottom right? So refinement is done by halving the 59 cells which makes 118 and so on till i have a converged result. Is this what you mean?

Last edited by Arti; May 21, 2009 at 11:00.
Arti is offline   Reply With Quote

Old   May 21, 2009, 19:23
Default
  #43
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,796
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Hi,

Yes, halving the mesh element edge length is the usual increment for mesh sensitivity studies. Refer to "Computational Fluid Dynamics" by Roache for a detailed discussion on this. It has also been implemented as an editorial policy by Journal of Fluids Engineering, see http://journaltool.asme.org/Template...umAccuracy.pdf

So if your mesh has 60 elements on the top face of the foil, ideally I would then use 120 and 240 and so on. As a minimum (as discussed in the JFE reference) you should increase by a factor of 1.3, so 60, then 80 then 100 but bigger steps are desireable.

Glenn Horrocks
ghorrocks is offline   Reply With Quote

Old   May 22, 2009, 13:00
Default
  #44
New Member
 
Join Date: Apr 2009
Posts: 26
Rep Power: 8
Arti is on a distinguished road
ah I get it now. Thanks for the information.

Was wondering does setting a specific boundary condition work for all situations for example in an airfoil simulation can setting the boundary condition for one angle of attack be used for the remaining ones.
It seems like im having problem with some angles even with the same boundary. Am trying to collect data to see if my mesh convergence has reached.
Arti is offline   Reply With Quote

Old   May 26, 2009, 10:52
Default
  #45
LSC
Member
 
LSC
Join Date: May 2009
Posts: 58
Rep Power: 8
LSC is on a distinguished road
Hi,

currently I have managed to get my CL within 7% error and 60% error for CD (more or less expected). This was done with SST k-omega and intermittency-ReTheta transition model at default values. I did a CF plot and found that transition was predicted further upstream when compared with experimental (therefore resulting in large drag error). Are there any best known methods on tuning the transition model coefficients?
LSC is offline   Reply With Quote

Old   May 26, 2009, 19:02
Default
  #46
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,796
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Hi,

Before you tune the coefficients, are you sure you have the inlet turbulence level correct? Also what about surface roughness - does your model properly account for surface roughness?

Glenn Horrocks
ghorrocks is offline   Reply With Quote

Old   May 27, 2009, 05:57
Default
  #47
LSC
Member
 
LSC
Join Date: May 2009
Posts: 58
Rep Power: 8
LSC is on a distinguished road
Hi, the turbulence intensity was calculated based on the width and height of the wind tunnel geometry given in the journals where the authors did an experiment on the airfoil which I am simulating as well. However, I did the calculations based on a rectangular cross section wheresa the actual wind tunnel cross section is octagonal. In fact, one of my main objective is to look into the effects of surface roughness on airfoil but currently I am in the midst of getting the clean airfoil data first and subsequently add roughness on the surface. Currently looking into tuning the transition model coefficient to reduce the CD error. Please advise
LSC is offline   Reply With Quote

Old   May 28, 2009, 00:20
Default Cfd 3d airfoil
  #48
Member
 
sivaramakrishnaiah
Join Date: Mar 2009
Location: india,pondicherry
Posts: 74
Rep Power: 8
sivarama1 is on a distinguished road
Send a message via MSN to sivarama1 Send a message via Yahoo to sivarama1 Send a message via Skype™ to sivarama1
Hi all,
yes,i am also doing same type of problem,I create model in I Gambit and meshed,but that is 2d model,how to export to CFX-11.
IS IT POSSIBLE TO EXPORT TO CFX-11(2D GEOMETRY IN GAMBIT)
__________________
sivaramakrihnaiah
sivarama1 is offline   Reply With Quote

Old   May 28, 2009, 03:35
Default
  #49
New Member
 
Join Date: Apr 2009
Posts: 26
Rep Power: 8
Arti is on a distinguished road
Please read a few post back. About how to simulate a 2D effect for Airfoil. There is NO actual 2D simulation for CFX u will have to extrude it to 3D.
Arti is offline   Reply With Quote

Old   May 28, 2009, 07:06
Default 2d export to CFX-11
  #50
Member
 
sivaramakrishnaiah
Join Date: Mar 2009
Location: india,pondicherry
Posts: 74
Rep Power: 8
sivarama1 is on a distinguished road
Send a message via MSN to sivarama1 Send a message via Yahoo to sivarama1 Send a message via Skype™ to sivarama1
I am new in this field,
what i am analyzing
1) first i was taken one airfoil in that i was done 2D mesh in GAMBIT,That i should export to solver means CFX-11,but CFX-11 most i was used in 3D simulations only,2D mesh not imported in cfx-11.
if dont mind your MSN ID,I SHOULD CONTACT.
Thanking you.
__________________
sivaramakrihnaiah
sivarama1 is offline   Reply With Quote

Old   May 28, 2009, 11:39
Default
  #51
New Member
 
Join Date: Apr 2009
Posts: 26
Rep Power: 8
Arti is on a distinguished road
As i was saying. Extrude (or use the sweep function in Gambit) your 2D mesh into 3D and u would have solve your problem. Cant be simpler than that.
Arti is offline   Reply With Quote

Old   May 30, 2009, 01:11
Default
  #52
LSC
Member
 
LSC
Join Date: May 2009
Posts: 58
Rep Power: 8
LSC is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Hi,

Before you tune the coefficients, are you sure you have the inlet turbulence level correct? Also what about surface roughness - does your model properly account for surface roughness?

Glenn Horrocks
Hi Glenn,

you are right! I made a mistake in the inlet turbulence level..The CD and CL error are greatly reduced. Really appreciate your invaluable advice and many many thanks!!
LSC is offline   Reply With Quote

Old   July 14, 2009, 13:23
Default
  #53
New Member
 
Join Date: Jun 2009
Posts: 2
Rep Power: 0
meow55 is on a distinguished road
hi there, currently i'm having a problem with my simulation. i had done a simulation with 0 angle of attack, but when my angle of attack increases, the error percentage gets larger n larger. But when i'm doing 0 angle of attack , my errors are less than 1% for both lift n drag. I'm using mesh transformation to perform the angle of attack. Can anyone advise on this issue? thanks
meow55 is offline   Reply With Quote

Old   July 14, 2009, 13:30
Default
  #54
New Member
 
Join Date: Jun 2009
Posts: 2
Rep Power: 0
meow55 is on a distinguished road
hi there, currently i'm having a problem with my simulation. i had done a simulation with 0 angle of attack, but when my angle of attack increases, the error percentage gets larger n larger. But when i'm doing 0 angle of attack , my errors are less than 1% for both lift n drag. I'm using mesh transformation to perform the angle of attack. Can anyone advise on this issue? thanks
meow55 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
Pros and Cons for CFX, CFdesign, COMSOL Val Main CFD Forum 3 June 10, 2011 02:20
nucleate boiling simulation in CFX Anil CFX 3 August 25, 2010 14:18
PhD using CFX Rui CFX 9 May 28, 2007 05:59
2D simulation - ICEM meshing for CFX question Ben Makhal CFX 5 April 11, 2007 08:44
Simulation of turbine cascade in CFX. Jonas Pedro Caumo CFX 0 December 9, 2006 14:54


All times are GMT -4. The time now is 05:00.