|
[Sponsors] |
July 1, 2021, 21:19 |
localEuler possible for chtMultiRegionFoam?
|
#1 |
Senior Member
Charles
Join Date: Aug 2016
Location: Vancouver, Canada
Posts: 151
Rep Power: 10 |
I've tested that LTS can be used by buoyantPimpleFoam. But I failed when I used it for chtMultiRegionFoam. It gave the following error message.
Code:
request for volScalarField rDeltaT from objectRegistry
__________________
Charles L. |
|
July 2, 2021, 05:22 |
|
#2 |
Senior Member
|
Tangentially related to the question you raise are:
http://www.tfd.chalmers.se/~hani/kur...rt_Jan2017.pdf and Which solver should I use when I have multiple solids and fluid regions? Possibly this helps. |
|
July 2, 2021, 11:24 |
LTS in multiregionReactingFoam
|
#3 | |
Member
Eric Daymo
Join Date: Feb 2015
Location: Gilbert, Arizona, USA
Posts: 56
Rep Power: 12 |
Hello,
Maybe multiregionReactingFoam will help, since it includes LTS. You can get this solver at: https://github.com/TonkomoLLC/multiRegionReactingFoam I didn't update the code to OpenFOAM-v8 (the latest version on the repo is for OpenFOAM v7). Also the readme file in the repo has the following note that you should be aware of: Quote:
Best regards, Eric Daymo http://www.tonkomo.com |
||
July 2, 2021, 11:51 |
|
#4 |
Senior Member
Charles
Join Date: Aug 2016
Location: Vancouver, Canada
Posts: 151
Rep Power: 10 |
Thanks Domenico for your message.
My original problem is a ventilation in a room with a floor heated by radiation. I want to know the steady state result. I tried setting ddtSchemes to steadystate. But it is very easy to diverge as many posts, such as PIMPLE fvSchemes, indicates it is intrinsically unstable and suggests to use LTS (localEuler). I checked the solver code this morning and saw that LTS is not implemented. In bouyantPimpleFoam, it includes rhoPimpleFoam and includes LTS feature. So, the only solution left is to run simulation in transient for a long time. But this takes a lot computation resources. I have already reduced solid floor density and heat capacity so to make solid part converge faster. Any helps on accelerating fluid side computation are appreciated. While I was writing this post, Eric posted his help. Really appreciate! I will download the code and test it today. I noticed that the version number does not follow that of openfoam.org, e.g. v7 or v8, hope this is not a problem.
__________________
Charles L. |
|
July 2, 2021, 12:02 |
|
#5 |
Member
Eric Daymo
Join Date: Feb 2015
Location: Gilbert, Arizona, USA
Posts: 56
Rep Power: 12 |
Hi, Charles. in the repo you'll find solvers for various versions of OpenFOAM. The OpenFOAM-7 version is here http://https://github.com/TonkomoLLC...onReactingFoam
In other words, just git clone the entire repo and compile only the version you need. Hopefully this works out for you. Best regards, Eric Daymo http://www.tonkomo.com |
|
July 2, 2021, 12:07 |
|
#6 |
Senior Member
Charles
Join Date: Aug 2016
Location: Vancouver, Canada
Posts: 151
Rep Power: 10 |
Ahh, I see. Sorry for missing that. Thanks again, Eric. I've already clone the whole package and will test it out today.
__________________
Charles L. |
|
July 2, 2021, 12:15 |
|
#7 |
Member
Eric Daymo
Join Date: Feb 2015
Location: Gilbert, Arizona, USA
Posts: 56
Rep Power: 12 |
Hi, Charles,
In thinking about the problem at hand, if you have buoyancy effects multiregionReactingFoam may not be appropriate. Although I did implement a gravity field, the pressure equation is based on that of reactingFoam, not the p_rgh implementation found in buoyantPimpleFoam. This may be especially problematic if the room you're simulating is closed, for example. Basically, if multiRegionReactingFoam does not work for you because of something with the pressure equation, the same programming ideas that i used to implement LTS in multiRegionReactingFoam should be possible to implement in a modified version of chtMultiRegionFoam. Let's see what happens with your initial tests, though. Best regards, Eric Daymo http://www.tonkomo.com |
|
July 2, 2021, 12:55 |
|
#8 |
Member
Eric Daymo
Join Date: Feb 2015
Location: Gilbert, Arizona, USA
Posts: 56
Rep Power: 12 |
Hi, Charles,
Your posting here prompted me to update multiRegionReactingFoam to OpenFOAM-8. You can "git pull" the repo again and find the new OF8 solver here: http://https://github.com/TonkomoLLC...onReactingFoam I did a quick test of the solver with a counterflow flame tutorial in with both the Euler transient ddt scheme and the localEuler (LTS) ddtScheme. The new tutorial cases are posted here: http://https://github.com/TonkomoLLC...als-OpenFOAM-8 Best regards, Eric Daymo http://www.tonkomo.com |
|
July 2, 2021, 13:26 |
|
#9 |
Senior Member
Charles
Join Date: Aug 2016
Location: Vancouver, Canada
Posts: 151
Rep Power: 10 |
Thank you Eric. I will get the latest version and test it out.
__________________
Charles L. |
|
July 3, 2021, 04:10 |
|
#10 |
Senior Member
|
Sincere thanks to Eric and Charles for getting in touch. Very insightful to read.
I have three questions to Eric. 1/ In your experience, what are typical gains in CPU time when comparing LTS and non-LTS versions of the solver? 2/ Does the LTS strategy extend from the fluid into the solid domain. I.e., is the time step in the solid domain governed by LTS as well? 3/ what is your view on decoupling the time step in the fluid and solid domain as proposed by students at Chalmers? Thx. Domenico. |
|
July 3, 2021, 12:04 |
|
#11 | |||
Member
Eric Daymo
Join Date: Feb 2015
Location: Gilbert, Arizona, USA
Posts: 56
Rep Power: 12 |
Dear Domenico,
I am very happy to learn that this discussion is helpful to you. With respect to your three questions. Quote:
Quote:
On a related noted, it is also possible in some cases to achieve steady state faster by setting a larger but constant time step for the entire simulation (all regions). This may be a way to achieve the steady state solution faster if the steadyState ddt scheme is not stable, and LTS is not available in the solver (e.g., the default version of chtMultiRegionFoam). Quote:
I hope this reply is helpful and I welcome other's perspectives. Best regards, Eric |
||||
October 15, 2024, 02:07 |
|
#12 |
Senior Member
Desh
Join Date: Mar 2021
Location: Sydney
Posts: 118
Rep Power: 5 |
Hi,
commenting on an old thread but, the latest version OF12 allows this without any modifications. Cheers, Dasith |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Running localEuler ddt on transient case | sufjanst | OpenFOAM Running, Solving & CFD | 4 | February 18, 2019 04:27 |
localeuler timediscretization | xshmuel | OpenFOAM Running, Solving & CFD | 5 | June 22, 2018 07:53 |
multiphaseInterFoam & localEuler | kaaja | OpenFOAM Running, Solving & CFD | 3 | June 15, 2018 08:37 |
Incompressible solver able to use localEuler? | petr.f. | OpenFOAM Running, Solving & CFD | 0 | April 23, 2014 13:34 |
wavetransmissive localEuler | Henning86 | OpenFOAM Running, Solving & CFD | 0 | November 19, 2013 05:48 |