# Advice-bc for low speed airfoil

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

 April 29, 2005, 12:54 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.

 April 30, 2005, 04:12 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.

 April 30, 2005, 04:40 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

 May 2, 2005, 03:08 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.

 May 2, 2005, 03:13 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.

 May 2, 2005, 03:17 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

 May 2, 2005, 12:34 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.

 May 2, 2005, 22:31 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.

 May 3, 2005, 03:04 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

 May 3, 2005, 14:17 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.

 May 3, 2005, 15:37 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.

 May 4, 2005, 02:18 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).

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Bogey Jammer Main CFD Forum 0 September 29, 2009 17:06 Frank Main CFD Forum 1 April 21, 2008 18:36 MSc Student Siemens 2 August 9, 2006 13:49 Quarkz Main CFD Forum 2 January 6, 2006 11:56 Sawa FLUENT 3 January 14, 2003 02:10

All times are GMT -4. The time now is 13:47.