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

Advice-bc for low speed airfoil

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 29, 2005, 12:54
Default Advice-bc for low speed airfoil
  #1
Vincent
Guest
 
Posts: n/a
Hi,

I want to simulate a low reynold number (around 50000) and low speed (5m/s) flow around a very thin airfoil in sea level conditions of standard atmosphere at 0 angle of attack. The grid I use is a C structured grid. But I don't know what bc I should use for farfield. I tried pressure_far_field but it gives me a density of 2kg/m3 which is far from 1.225 and I assume the flow is not compressible for this range of velocities. In this case of bc, the calculation converges very well. So I think the grid is good. But I also tried velocity_inlet, which gives me the right density, and then the calculation doesn't converge at all. Therefore I guess the lack of convergence is du to the choice of bc. So I am wondering what bc I should use to have a convergence in this case of flow. I hope someone can help me. Thank you in advance.

Vincent.
  Reply With Quote

Old   April 30, 2005, 04:12
Default Re: Advice-bc for low speed airfoil
  #2
Peter Gasparovic
Guest
 
Posts: n/a
Use velocity_inlet on all boundaries. Make sure your grid has radius atleast (~20 x airfoil chord) around airfoil, otherwise use UDF imposing velocity circulation on boundary. Air: use constant density and set operating pressure location upwind, close to boundary. Solver: never use coupled solvers for such small velocities. I made the same mistake and always had divergence problems.
  Reply With Quote

Old   April 30, 2005, 04:40
Default Re: Advice-bc for low speed airfoil
  #3
Luca
Guest
 
Posts: n/a
Are you sure you have set the rigth operating pressure?it's strange you have a difference on far-field density. Luca
  Reply With Quote

Old   May 2, 2005, 03:08
Default Re: Advice-bc for low speed airfoil
  #4
Vincent
Guest
 
Posts: n/a
Hi,

Thank you for the answer. Actually what I tried after posting my question on friday was to use velocity inlet and pressure outlet on the right boundary and used enhanced wall treatment in the k-epsilon model options (with coupled implicit). I was surprised it had a very good convergence when running the calculation.

I will try velocity_inlet, and segregated solver though, as you told me, tomorrow as soon as I go back to work. Yet what do you mean by grid radius ? And why should it work better when using a segregated solver ?

Thanks again, Vincent.
  Reply With Quote

Old   May 2, 2005, 03:13
Default Re: Advice-bc for low speed airfoil
  #5
Vincent
Guest
 
Posts: n/a
Hi,

It is strange for me too. But I did set the right pressure, ie 101325 Pa. The temperature is T=296, and it gives me around 2 kg/m3. I have to set a lower pressure if I want to have a density of around 1.2kg/m3, ie the one I'd like ! I haven't had time yet to look in the manual of Fluent how the density is calculated but it may give the explanation. I am also wondering if it couldn't be the very low Mach number (0.015) that creates such a problem in the far_field_pressure calculation.

Thanks for considering my problem, Vincent.

  Reply With Quote

Old   May 2, 2005, 03:17
Default Re: Advice-bc for low speed airfoil
  #6
Luca
Guest
 
Posts: n/a
Have you set the rigth mach number? to use the far field bc you have to use the ideal gas model. So pressure is determined by the law p=rho * R *T_static. Ho far is your far.field bc form the profile?Luca
  Reply With Quote

Old   May 2, 2005, 12:34
Default Re: Advice-bc for low speed airfoil
  #7
Vincent
Guest
 
Posts: n/a
I set the right mach number, in regards to my parameters. But I think I understand my mistake. I have to set 0 in the pressure gauge in the setting of the pressure_far_field bc panel. Now it gives me the right density. I didn't know it was a local relative pressure.

Thank you for everything !

Vincent.
  Reply With Quote

Old   May 2, 2005, 22:31
Default Re: Advice-bc for low speed airfoil
  #8
Riaan
Guest
 
Posts: n/a
Carefull - because you are now solving an internal flow vs. a external flow (i.e far-field)....make sure your walls are faaaaaaaar away.

  Reply With Quote

Old   May 3, 2005, 03:04
Default Re: Advice-bc for low speed airfoil
  #9
Luca
Guest
 
Posts: n/a
Yes, that's rigth...the pressure you use are all gauge except fot the pressure in the operating pressure panel. Luca
  Reply With Quote

Old   May 3, 2005, 14:17
Default Re: Advice-bc for low speed airfoil
  #10
Peter Gasparovic
Guest
 
Posts: n/a
1) as to grid radius and velocity_inlet:

For external flows I always use cylinder as a grid boundary. It's good for any angle of attack. You can set velocity_inlet BC on whole boundary. Faces where exists outflow during computation are automatically assumed as pressure_outlets.

2) as to segregated solver:

I made the similar mistake (see: Re: flat plate transition: SST k-omega divergence) and I was told that coupled-implicit solver is primarily aimed at M>0.6, and often diverges for very low speeds.
  Reply With Quote

Old   May 3, 2005, 15:37
Default Re: Advice-bc for low speed airfoil
  #11
Vincent
Guest
 
Posts: n/a
Hi,

Thank you for the advice. Just in case, do you know if there is a rule concerning how far the external boundary should be from the airfoil ? Should I take into account the size of the airfoil, the speed, or both ? Also, does the cylinder as a grid boundary work in 3D ?

Regards, Vincent.
  Reply With Quote

Old   May 4, 2005, 02:18
Default Re: Advice-bc for low speed airfoil
  #12
Peter Gasparovic
Guest
 
Posts: n/a
I everywhere read values 15~20 times chord. Maybe you can lower it to 10, but why? There is only few cells on the boundary, so there is no reason to lower this radius.

I am sure it work in 3D too. However I use sphere. So you can simply change yaw angle on whole boundary.

I think the pressure (airfoil thickness, speed) has to do little with grid radius (there is only small error). Most important is to dissipate velocity circulation around airfoil on sufficient large scale, otherwise you get too big pressure drag (inclined local velocity vector).
  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
[FloWorks] Request advice for an airfoil calculation problem Bogey Jammer Main CFD Forum 0 September 29, 2009 17:06
Airfoil boundary condition Frank Main CFD Forum 1 April 21, 2008 18:36
Simulation of transonic flow over NACA0012 airfoil MSc Student CD-adapco 2 August 9, 2006 13:49
Simulating flow past airfoil with different AOA Quarkz Main CFD Forum 2 January 6, 2006 11:56
High speed flow problems Sawa FLUENT 3 January 14, 2003 02:10


All times are GMT -4. The time now is 03:27.