# 3D Separation Model using K-Omega SST Divergence

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

February 12, 2013, 01:27
3D Separation Model using K-Omega SST Divergence
#1
New Member

Join Date: Oct 2012
Posts: 7
Rep Power: 7
Hey guys,

I'm trying to model a 3-D wing in Fluent to study the effects of boundary restabilisation via Vortex Generators.

I started by using the k-e model, before realising that this was inappropriate for the high angles of attack I would be studying. I have now tried to switch to k-Omega SST to better capture boundary layer separation, and refined my mesh (50 layers of inflation, first off wall thickness of 1e-06 due to a fairly high Reynolds number of ~ 10^5). My domain is about 20 chord lengths radius (I have a cylinder) of my wing, and I'm using a pressure-far-field condition.

My solution doesnt last too long before it starts to diverge, and I have no clue why. I have been searching all over the forums for a good two days trying to solve this issue, but without any luck.
Any ideas?

-------------------------------------------------------------------------
Also, here are some of the parameters that I have set (just to reference):

1) Pressure Based, Steady
2) Energy - On, SST k-omega
3) Air - ideal gas (for pressure-far-field condition)
4) Velocity - 13.44 m/s
5) Courant # of 5

Attached is a picture of part of my mesh.

Thank you for your help
Attached Images
 1.jpg (103.1 KB, 65 views)

Last edited by TempestCFD; February 12, 2013 at 08:32.

 February 12, 2013, 08:47 #2 Senior Member   Join Date: Mar 2011 Location: Germany Posts: 431 Rep Power: 13 A common problem, not a big issue. Jut reduce your courant number to 1 at the start of solution and slowly increase it. By doing so, I hope your problem will be solved. mrenergy likes this.

February 12, 2013, 13:22
Progress but a new fault
#3
New Member

Join Date: Oct 2012
Posts: 7
Rep Power: 7
cfd seeker, thank you for your reply.

The initialisation now works, however the solution begins to diverge soon after, giving new errors (see screenshot attached).

I'm curious about the behavior of the continuity residuals at the beginning as well (staying at exactly 1 initially)?

I will try reducing my courant number further, but am open to other ideas as well.

Frustrated but still determined,

TempestCFD
Attached Images
 output.jpg (94.3 KB, 77 views)

 February 13, 2013, 12:57 #4 Senior Member   Join Date: Mar 2011 Location: Germany Posts: 431 Rep Power: 13 what is the mach no? in which sotware you made your mesh? what is the minimum qulity of your mesh? also trying with 1st order upwind for all equztions at the start of the solution.

 February 13, 2013, 13:24 #5 New Member   Join Date: Oct 2012 Posts: 7 Rep Power: 7 The mach number is low (M = 0.0386). I meshed the setup in Ansys Mesher. My elements are fairly good quality and I have a fine mesh of about 6.5 million elements. Anything specific you want to know? Skewness ect? I re-ran the simulation with a courant number of 0.1 and relaxed the energy from 1 -> 0.9 and the solution runs okay. The continuity residuals seem to flat line at 10e-02 though which is not satisfactory in my eyes. I'm going to look at improving the elements near the trailing edge of the airfoil as its sharp and not a great transition to the tet elements behind that section. Any additional concepts or ideas would be greatly appreciated. Thank you

 February 14, 2013, 08:35 #6 Senior Member   Join Date: Mar 2011 Location: Germany Posts: 431 Rep Power: 13 Continuity convergence is very slow and secondly courant no and convergence are directly propotional, so let the solution run as it is and check the convergence of global parameters like CL,CD,CM etc.

 February 14, 2013, 08:39 #7 New Member   Join Date: Oct 2012 Posts: 7 Rep Power: 7 I tried running the solution with a velocity inlet and pressure outlet instead, and the continuity went down to 10e-04. Much better. My Cl and Cd seem exceptionally high however. I can't seem to find any issues with my reference values that would cause this. Thank you for your guidence by the way, it is greatly appreciated.

February 15, 2013, 14:21
#8
Senior Member

Join Date: Mar 2011
Location: Germany
Posts: 431
Rep Power: 13
Quote:
 My Cl and Cd seem exceptionally high however
Have you resolved the boundary layer properly? what's the range of wall y+ ?
Have you scaled the mesh after importing it in Fluent?

 February 15, 2013, 14:29 #9 New Member   Join Date: Oct 2012 Posts: 7 Rep Power: 7 My boundary layer (in my opinion) has been resolved well, even too well. My y+ is ~ 0.15 - 0.89 What do you mean by "scaling the mesh after importing it into fluent" ?

 February 15, 2013, 15:10 #10 Senior Member   Join Date: Mar 2011 Location: Germany Posts: 431 Rep Power: 13 Wall y+ 0.15 - 0.89 Wow it's great...what is the total mesh size? How much RAM does you machine have.... What is the units in which you created geometry and then meshed it? If it's other than "meters" then you have to scale it in Fluent, follow Mesh>Scale

 February 15, 2013, 15:25 #11 New Member   Join Date: Oct 2012 Posts: 7 Rep Power: 7 Total mesh size is huge (about 5.5 million elements), 12 GB of ram, lol. It lags a bit Everything was done in metres

 February 16, 2013, 08:44 #12 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,352 Blog Entries: 6 Rep Power: 45 Why energy is on? Are you using pressure based -coupled solver?

 February 16, 2013, 18:33 #13 New Member   Join Date: Oct 2012 Posts: 7 Rep Power: 7 Sorry, I forgot to mention, I switched energy off, switching from pressure-far-field condition to a velocity-inlet/pressure-outlet setup. Yes, pressure based, coupled.

 Tags divergence, diverges, sst k-omega

 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 TedBrogan Main CFD Forum 0 January 23, 2013 01:00 kenan Main CFD Forum 0 January 17, 2013 07:14 Attesz CFX 7 January 5, 2013 04:32 dancfd OpenFOAM Pre-Processing 0 June 9, 2011 23:25 swe704 Main CFD Forum 0 February 5, 2010 09:36

All times are GMT -4. The time now is 13:59.

 Contact Us - CFD Online - Privacy Statement - Top