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

Residual Control for Continuity

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 13, 2023, 05:34
Default Residual Control for Continuity
  #1
New Member
 
Osman Özdemir
Join Date: Feb 2021
Posts: 3
Rep Power: 5
osmanveysel is on a distinguished road
Hello,

I would like to set a residual control for continuityGlobal as a convergence criteria. There are options to set a residual control for velocity, pressure, turbulence properties etc., however I could not find an appropriate setting for continuity. If there is any idea would be great.

Thanks.
osmanveysel is offline   Reply With Quote

Old   August 19, 2023, 21:09
Default
  #2
Member
 
yijin Mao
Join Date: May 2010
Location: Columbia, MO
Posts: 64
Rep Power: 16
alundilong is on a distinguished road
Setting criteria for velocity and pressure is equivalent to continuity as solving velocity and pressure is the same as solving the continuity.
Quote:
Originally Posted by osmanveysel View Post
Hello,

I would like to set a residual control for continuityGlobal as a convergence criteria. There are options to set a residual control for velocity, pressure, turbulence properties etc., however I could not find an appropriate setting for continuity. If there is any idea would be great.

Thanks.
alundilong is offline   Reply With Quote

Old   August 27, 2023, 14:42
Default
  #3
New Member
 
Osman Özdemir
Join Date: Feb 2021
Posts: 3
Rep Power: 5
osmanveysel is on a distinguished road
Thanks for your answer. But when I set my residualControl to 1e-5 for p, U, k and omega, solution stops when they decrease under 1e-5. However globalContinuity may stay above 1e-4, 1e-3. So I am looking for something like in Fluent, it is possible to set a residualControl for continuity seperately. How can I do same kind of thing in OpenFOAM?


Quote:
Originally Posted by alundilong View Post
Setting criteria for velocity and pressure is equivalent to continuity as solving velocity and pressure is the same as solving the continuity.
osmanveysel is offline   Reply With Quote

Old   August 27, 2023, 21:17
Default
  #4
Member
 
Tatsuya Shimizu
Join Date: Jul 2012
Posts: 42
Rep Power: 14
LongGe is on a distinguished road
Hello Osman

Wouldn't a combination of runTimeControl and continuityError in functionObject accomplish what you want to do? This writing style will work with OpenFOAM-v2212.


functions
{
continuityError1
{
type continuityError;
libs (fieldFunctionObjects);
phi phi;
}


runTimeControl1
{
type runTimeControl;
libs (utilityFunctionObjects);
conditions
{
condition1
{
type minMax;
functionObject continuityError1;
fields (cumulative);
value 1e-02;
mode minimum;
}
}
satisfiedAction end;
}
}
__________________
Our Work: https://www.idaj.co.jp/product/ennovacfd/openfoam_gui/
Powered by Ennova : https://ennova-cfd.com/
Ennova's Channel Partners : http://www.wolfdynamics.com/
LongGe is offline   Reply With Quote

Old   August 28, 2023, 04:34
Default
  #5
New Member
 
Osman Özdemir
Join Date: Feb 2021
Posts: 3
Rep Power: 5
osmanveysel is on a distinguished road
I just changed cumulative to local, it worked and it gave what I need. I guess I will add other criterias like U, p, turbulence etc. here to have a compact convergence criterion.
Thank you.


Quote:
Originally Posted by LongGe View Post
Hello Osman

Wouldn't a combination of runTimeControl and continuityError in functionObject accomplish what you want to do? This writing style will work with OpenFOAM-v2212.


functions
{
continuityError1
{
type continuityError;
libs (fieldFunctionObjects);
phi phi;
}


runTimeControl1
{
type runTimeControl;
libs (utilityFunctionObjects);
conditions
{
condition1
{
type minMax;
functionObject continuityError1;
fields (cumulative);
value 1e-02;
mode minimum;
}
}
satisfiedAction end;
}
}
osmanveysel is offline   Reply With Quote

Reply

Tags
continuity, openfoam, residual control

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[solidMechanics] Support thread for "Solid Mechanics Solvers added to OpenFOAM Extend" bigphil OpenFOAM CC Toolkits for Fluid-Structure Interaction 686 December 22, 2022 09:10
Maximum number of iterations exceeded chtmultiregionsimpleFoam Moncef OpenFOAM Running, Solving & CFD 28 July 13, 2020 14:26
Free surface issues with interDyMFoam for hydroturbine oumnion OpenFOAM Running, Solving & CFD 0 October 6, 2017 14:05
simpleFoam error - "Floating point exception" mbcx4jc2 OpenFOAM Running, Solving & CFD 12 August 4, 2015 02:20
Micro Scale Pore, icoFoam gooya_kabir OpenFOAM Running, Solving & CFD 2 November 2, 2013 13:58


All times are GMT -4. The time now is 02:10.