Residual problem of 2D airfoil simulation

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

 April 10, 2010, 11:28 Residual problem of 2D airfoil simulation #1 Member   tom Join Date: Feb 2010 Posts: 46 Rep Power: 8 Hi all I met a puzzle when I am doing a 2d airfoil in different AOA, the reynolds number is 30000, boundary condition is pressure far field, chord length is 1m. solver is implicit density based, viscous model is sparart-allmaras. when the simulation ran in a smal AOA, residual pattern oscillated in a small region, but the lift, drag and momentum coefficient converge easily. by increasing the AOA, result become worse, residual, lift, drag and momentum coefficient oscillated widely. can sb give me a clew for that, is there something wrong with my mesh or boundary condition. I put 4 pics into the attachment( two of them are residual and cd figure in 5 degree, the others are figures taken under the 90 degree) Regards Han 1.jpg 2.jpg 3.jpg 4.jpg

 April 10, 2010, 20:38 #2 Senior Member   Join Date: Nov 2009 Posts: 411 Rep Power: 11 What is your mesh size (how many chords around the airfoil in all directions) ? I suspect you need to use a larger computational domain for large AOA. Do

April 11, 2010, 05:31
Hi do
#3
Member

tom
Join Date: Feb 2010
Posts: 46
Rep Power: 8
Quote:
 Originally Posted by DoHander What is your mesh size (how many chords around the airfoil in all directions) ? I suspect you need to use a larger computational domain for large AOA. Do
how can I check the chords around the airfoil, by the way, my computational domain is 20 times of the chord length, is it big engough? I will try a bigger domain for large AOA and see what will be happened. Thank you fou your reply

Han

 April 13, 2010, 01:01 #4 Senior Member   Chris Join Date: Jul 2009 Location: Ohio, USA Posts: 169 Rep Power: 9 You're probably getting reflections off of the boundaries. You should move your boundaries out, like DoHander said, and also make sure your really stretch the grid as you move out to the far-field. By stretching the grid, you'll damp (hopefully most of) the waves before they get to the boundary, so then they can't be reflected back to the airfoil. edit: I should say that you might be getting reflections. There could be other problems, but this is the first thing I would try.

April 13, 2010, 08:20
#5
Member

tom
Join Date: Feb 2010
Posts: 46
Rep Power: 8
Quote:
 Originally Posted by Chris D You're probably getting reflections off of the boundaries. You should move your boundaries out, like DoHander said, and also make sure your really stretch the grid as you move out to the far-field. By stretching the grid, you'll damp (hopefully most of) the waves before they get to the boundary, so then they can't be reflected back to the airfoil. edit: I should say that you might be getting reflections. There could be other problems, but this is the first thing I would try.
Hi Chris
Thank you for you reply, now I expand my domain, it is 40 times of the chord length, but still the result oscillates, does it mean the domain is still not big enough? I have nothing to do with that now. I post my mesh here, wish you can help me solve the problem.

Thank you
Han
Attached Images
 1.jpg (98.2 KB, 56 views)

 April 13, 2010, 11:55 #6 Senior Member   Chris Join Date: Jul 2009 Location: Ohio, USA Posts: 169 Rep Power: 9 It looks like you're not stretching the grid enough. The point is to stretch it so that the waves you are trying to push out of the domain become unresolved near the boundary. This will cause them to be taken out by the inherent dissipation of the numerical scheme. If the waves are taken out before they get to the boundary, then they won't be reflected back from the boundary. Try a growth rate of 1.2 or more once you're sufficiently far from the airfoil, with a domain of 20c. Make sure you stretch it in a smooth manner, or the code might blow up. Also, what AoA are you running? For high AoA's the problem becomes unsteady, which could be what the oscillations are telling you. See this youtube video: http://www.youtube.com/watch?v=Ti5zUD08w5s&NR=1

April 13, 2010, 12:08
#7
Member

tom
Join Date: Feb 2010
Posts: 46
Rep Power: 8
Quote:
 Originally Posted by Chris D It looks like you're not stretching the grid enough. The point is to stretch it so that the waves you are trying to push out of the domain become unresolved near the boundary. This will cause them to be taken out by the inherent dissipation of the numerical scheme. If the waves are taken out before they get to the boundary, then they won't be reflected back from the boundary. Try a growth rate of 1.2 or more once you're sufficiently far from the airfoil, with a domain of 20c. Make sure you stretch it in a smooth manner, or the code might blow up. Also, what AoA are you running? For high AoA's the problem becomes unsteady, which could be what the oscillations are telling you. See this youtube video: http://www.youtube.com/watch?v=Ti5zUD08w5s&NR=1
Hi Chris
Thank you so much, I would try to stretch the grid with 20c domain, by the way, my AOA is 90 degree, does the big AOA cause the oscillation and have nothing to do with the mesh?

 April 13, 2010, 12:55 #8 Senior Member   Chris Join Date: Jul 2009 Location: Ohio, USA Posts: 169 Rep Power: 9 Yeah, I would think that would be an issue. At that point, I don't think it can be solved as a steady problem anymore. However, you'll still want to stretch the grid. How are you setting the AoA? I can't tell from the picture if the grid is with AoA = 0 or 90. If it's 0, then are you changing the velocity vector in FLUENT? If so, then, from the picture you showed, your grid won't really be aligned with the flow anymore.

April 13, 2010, 14:36
#9
Member

tom
Join Date: Feb 2010
Posts: 46
Rep Power: 8
Quote:
 Originally Posted by Chris D Yeah, I would think that would be an issue. At that point, I don't think it can be solved as a steady problem anymore. However, you'll still want to stretch the grid. How are you setting the AoA? I can't tell from the picture if the grid is with AoA = 0 or 90. If it's 0, then are you changing the velocity vector in FLUENT? If so, then, from the picture you showed, your grid won't really be aligned with the flow anymore.
yes, I set the AOA by changing the velocity vector, if I rotate the airfoil and let it become vertically with the grid not horizontally, is it better than changing the velocity vector in boundary condition?

April 13, 2010, 16:03
#10
Senior Member

Chris
Join Date: Jul 2009
Location: Ohio, USA
Posts: 169
Rep Power: 9
Quote:
 Originally Posted by caohan yes, I set the AOA by changing the velocity vector, if I rotate the airfoil and let it become vertically with the grid not horizontally, is it better than changing the velocity vector in boundary condition?
Either way, you'll end up with the same thing. You'll get this:

airfoil-grid.jpg

Changing the velocity vector works for low AoA, but I don't think it's a good idea for high AoA. Your grid wouldn't be aligned with the flow anymore, which I think would cause you some problems with you solution. Also, from the perspective of the rotated grid, the far field boundaries are actually pretty close to the airfoil, which could explain the oscillations in the residuals.

I would suggest using a different grid for high AoA. Build a C-grid around an airfoil at a high AoA, like 80 deg or so. That way, you'll be able to align the grid with the flow. Then, if you want to run a range of AoA, changing the velocity vector by ten degrees (i.e., from either 80 deg to 70, or 80 deg to 90) won't be such a big deal.

 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 nedved OpenFOAM Running, Solving & CFD 14 Yesterday 02:51 msrinath80 OpenFOAM Running, Solving & CFD 18 March 3, 2015 06:36 basneb OpenFOAM 15 June 7, 2010 00:54 sivakumar OpenFOAM Pre-Processing 9 September 9, 2008 12:53 braennstroem OpenFOAM Running, Solving & CFD 16 May 15, 2006 02:23

All times are GMT -4. The time now is 21:04.