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

3D Separation Model using K-Omega SST Divergence

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

Like Tree1Likes
  • 1 Post By cfd seeker

Reply
 
LinkBack Thread Tools Display Modes
Old   February 12, 2013, 01:27
Question 3D Separation Model using K-Omega SST Divergence
  #1
New Member
 
Join Date: Oct 2012
Posts: 7
Rep Power: 4
TempestCFD is on a distinguished road
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
File Type: jpg 1.jpg (103.1 KB, 48 views)

Last edited by TempestCFD; February 12, 2013 at 08:32.
TempestCFD is offline   Reply With Quote

Old   February 12, 2013, 08:47
Default
  #2
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
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.
cfd seeker is offline   Reply With Quote

Old   February 12, 2013, 13:22
Default Progress but a new fault
  #3
New Member
 
Join Date: Oct 2012
Posts: 7
Rep Power: 4
TempestCFD is on a distinguished road
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.


Thanks in advance.


Frustrated but still determined,


TempestCFD
Attached Images
File Type: jpg output.jpg (94.3 KB, 53 views)
TempestCFD is offline   Reply With Quote

Old   February 13, 2013, 12:57
Default
  #4
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
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.
cfd seeker is offline   Reply With Quote

Old   February 13, 2013, 13:24
Default
  #5
New Member
 
Join Date: Oct 2012
Posts: 7
Rep Power: 4
TempestCFD is on a distinguished road
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
TempestCFD is offline   Reply With Quote

Old   February 14, 2013, 08:35
Default
  #6
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
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.
cfd seeker is offline   Reply With Quote

Old   February 14, 2013, 08:39
Default
  #7
New Member
 
Join Date: Oct 2012
Posts: 7
Rep Power: 4
TempestCFD is on a distinguished road
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.
TempestCFD is offline   Reply With Quote

Old   February 15, 2013, 14:21
Default
  #8
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
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?
cfd seeker is offline   Reply With Quote

Old   February 15, 2013, 14:29
Default
  #9
New Member
 
Join Date: Oct 2012
Posts: 7
Rep Power: 4
TempestCFD is on a distinguished road
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" ?
TempestCFD is offline   Reply With Quote

Old   February 15, 2013, 15:10
Default
  #10
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
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
cfd seeker is offline   Reply With Quote

Old   February 15, 2013, 15:25
Default
  #11
New Member
 
Join Date: Oct 2012
Posts: 7
Rep Power: 4
TempestCFD is on a distinguished road
Total mesh size is huge (about 5.5 million elements), 12 GB of ram, lol. It lags a bit

Everything was done in metres
TempestCFD is offline   Reply With Quote

Old   February 16, 2013, 08:44
Default
  #12
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Why energy is on? Are you using pressure based -coupled solver?
Far is offline   Reply With Quote

Old   February 16, 2013, 18:33
Default
  #13
New Member
 
Join Date: Oct 2012
Posts: 7
Rep Power: 4
TempestCFD is on a distinguished road
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.
TempestCFD is offline   Reply With Quote

Reply

Tags
divergence, diverges, sst k-omega

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
Scaling omega in SST turbulence model TedBrogan Main CFD Forum 0 January 23, 2013 01:00
k - omega SST turbulence model with wall functions kenan Main CFD Forum 0 January 17, 2013 07:14
Water subcooled boiling Attesz CFX 7 January 5, 2013 04:32
Boundary Conditions for k omega SST dancfd OpenFOAM Pre-Processing 0 June 9, 2011 23:25
SST model swe704 Main CFD Forum 0 February 5, 2010 09:36


All times are GMT -4. The time now is 21:44.