|
[Sponsors] |
August 13, 2023, 05:34 |
Residual Control for Continuity
|
#1 |
New Member
Osman Özdemir
Join Date: Feb 2021
Posts: 3
Rep Power: 5 |
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. |
|
August 19, 2023, 21:09 |
|
#2 | |
Member
yijin Mao
Join Date: May 2010
Location: Columbia, MO
Posts: 64
Rep Power: 16 |
Setting criteria for velocity and pressure is equivalent to continuity as solving velocity and pressure is the same as solving the continuity.
Quote:
|
||
August 27, 2023, 14:42 |
|
#3 |
New Member
Osman Özdemir
Join Date: Feb 2021
Posts: 3
Rep Power: 5 |
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?
|
|
August 27, 2023, 21:17 |
|
#4 |
Member
Tatsuya Shimizu
Join Date: Jul 2012
Posts: 42
Rep Power: 14 |
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/ |
|
August 28, 2023, 04:34 |
|
#5 | |
New Member
Osman Özdemir
Join Date: Feb 2021
Posts: 3
Rep Power: 5 |
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:
|
||
Tags |
continuity, openfoam, residual control |
Thread Tools | Search this Thread |
Display Modes | |
|
|
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 |