CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Initial Residual for p too high!

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

Like Tree10Likes
  • 10 Post By chegdan

Reply
 
LinkBack Thread Tools Display Modes
Old   March 5, 2013, 04:58
Default Initial Residual for p too high!
  #1
Member
 
Nikesh Bhattarai
Join Date: Nov 2011
Location: Daejeon, South Korea
Posts: 70
Rep Power: 4
nikesh is an unknown quantity at this point
Hi all,

I am simulating a simple 2D flat plate flow in OpenFoam using simpleFOAM to validate a new turbulence model that I would like to implement here. This new turbulence model is a slight modification of the kOmegaSST model which includes few new terms into the nut equation.

Results from kOmegaSST model are all OK! However, when I use this new model for the same grid, my initial pressure residuals oscillate around a pretty high value, at around 0.03 while the initial U,k and omega residuals are all at a reasonable convergence criterion, at around 10^-5.

This is not making much sense to me. Because, after some iterations(about 6~7,000) when I extract the results (even without reaching the convergence tolerance) and compare, they don't yet seem so weird or deviating highly from that of the SST's results.

I have checked my code numerous times, doesn't seem to have any problems in there.

Could there be a problem with the solvers I chose?

I am as well wondering how the p-residual is calculated in simpleFOAM.

I would highly appreciate any insights into this!

Thanks!
Nikesh

These are my settings and I've used the same for kOmegaSST (in the pic attached).
Attached Images
File Type: png Screenshot.png (41.3 KB, 144 views)
nikesh is offline   Reply With Quote

Old   March 5, 2013, 05:17
Default
  #2
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,186
Rep Power: 16
immortality is on a distinguished road
hi
Test for one or two order lower p tolernces than U,...
1e-9 or 1e-10
immortality is offline   Reply With Quote

Old   March 5, 2013, 06:23
Default
  #3
Member
 
Nikesh Bhattarai
Join Date: Nov 2011
Location: Daejeon, South Korea
Posts: 70
Rep Power: 4
nikesh is an unknown quantity at this point
Thanks!
Tried, yet not much of a difference.
nikesh is offline   Reply With Quote

Old   March 9, 2013, 16:51
Default
  #4
New Member
 
AndreiCFD
Join Date: Nov 2012
Posts: 27
Rep Power: 4
andrei.cimpoeru is on a distinguished road
Hi


Basically I am having the same problem.... I just want to ask you if you managed to do it in the end. I am simulating the flow over an aerofoil using k omega sst and simpleFoam with wall functions..........
Have you got any ideas?


Thanks

Andrei
andrei.cimpoeru is offline   Reply With Quote

Old   March 10, 2013, 01:35
Default
  #5
Member
 
Nikesh Bhattarai
Join Date: Nov 2011
Location: Daejeon, South Korea
Posts: 70
Rep Power: 4
nikesh is an unknown quantity at this point
Hii Andrei,
Well, I am still stuck with the same problem. Obviously higher p-residual means mass is not being conserved so well somewhere in the cells. You might want to look into your boundary conditions once more. Basically that is what I am trying to do too. And the schemes and type of mesh you are using for airfoil flow.
nikesh is offline   Reply With Quote

Old   March 10, 2013, 07:28
Default
  #6
New Member
 
AndreiCFD
Join Date: Nov 2012
Posts: 27
Rep Power: 4
andrei.cimpoeru is on a distinguished road
Hi

Ok I understand . I am using k omega sst , wall functions and simpleFoam solver ..... I have changed my boundary conditions many times still nothing......for example how you o file looks like and something that I don't understand : how do you calculate
the turbulent kinetic energy K and the rate of dissipation W(omega).......

thanks

Andrei
andrei.cimpoeru is offline   Reply With Quote

Old   March 10, 2013, 10:56
Default
  #7
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 543
Rep Power: 18
chegdan will become famous soon enough
Nick,

There are some strategies that I would try to get these residuals down to something you would like.
  1. Lower your pressure relTol by an order of magnitude compared to U i.e. relTol = 0.001 for P and relTol = 0.01 for U.
  2. Without knowing the mesh you are using you may need to increase the nonorthogonal corrector by 1 or 2. if you are using a tet mesh...then there are many things you can do.
  3. Use first order schemes to start with (you will move to higher order ones later)
  4. Obtain an initital velocity field with potentialFoam
  5. Using simpleFoam, the intial condition from potentialFoam, and first order schemes...turn turbulence OFF and once convergence seems to bottom out, turn turbulence on while the simulation is running
  6. Once a steady-state is obtained, stop the simulation, switch to second order schemes and restart the simulation with turbulence on and see if that helps

There are a lot of other strategies that you can try, but this one might be sufficient. Without knowing more details like divergence schemes; mesh structure and checkmesh results; y+ values; and boundary conditions there is not much to add on my part.

I would look at the thread SimpleFoam convergence problems and then move on to a search of the forum. There are many threads about simpleFoam convergence...but my list of threads is not in front of me right now. good luck.
kiddmax, fumiya, Alhasan and 7 others like this.
__________________
Dan

Find me on twitter @dancombest and LinkedIn

Last edited by chegdan; March 10, 2013 at 19:01. Reason: spelling
chegdan is offline   Reply With Quote

Old   March 15, 2013, 05:17
Default
  #8
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,186
Rep Power: 16
immortality is on a distinguished road
how can decrease the initial residuals for p in unsteady problems when relaxations are not applicable?
immortality is offline   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
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
pimpleFoam: turbulence->correct(); is not executed when using residualControl hfs OpenFOAM Running, Solving & CFD 3 October 29, 2013 09:35
SLTS+rhoPisoFoam: what is rDeltaT??? nileshjrane OpenFOAM Running, Solving & CFD 4 February 25, 2013 05:13
pisoFoam with k-epsilon turb blows up - Some questions Heroic OpenFOAM Running, Solving & CFD 26 December 17, 2012 04:34
Convergence moving mesh lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 15:09


All times are GMT -4. The time now is 19:03.