[Marpole]

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.

request for volScalarField rDeltaT from objectRegistry

I'm using openFOAM v8. I'm wondering if LTS is implemented in chtMultiRegionFoam?

[dlahaye]

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.

[edaymo]

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:

LTS is based on a one fluid region (region 0). Therefore, if there are multiple fluid regions, LTS time steps will be chosen based on the characteristic times of the fluid assigned to region 0. Therefore, in a multiple fluid region application where LTS will be used, one may wish to assign the most "time step sensitive" fluid region to fluid region 0 (e.g., by placing the name of this more sensitive fluid region first in under "fluid" in constant/regionProperties.

I hope this helps you move forward with your work.

Best regards,

Eric Daymo
http://www.tonkomo.com

[Marpole]

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.

[edaymo]

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

[Marpole]

Ahh, I see. Sorry for missing that. Thanks again, Eric. I've already clone the whole package and will test it out today.

[edaymo]

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

[edaymo]

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

[Marpole]

Thank you Eric. I will get the latest version and test it out.

[dlahaye]

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.

[edaymo]

Dear Domenico,

I am very happy to learn that this discussion is helpful to you.

With respect to your three questions.

1/ In your experience, what are typical gains in CPU time when comparing LTS and non-LTS versions of the solver?

The speed up with LTS really depends, but it is usually significantly faster than the non-LTS solution. As an example, on my older laptop, I can run the OpenFOAM-8 counterFlowFlame2D example in non-LTS mode (1 core) in 63 sec, but in LTS mode in just 39 sec. I don't have other examples readily available to share speed-up data, but such speedup is often seen when LTS is enabled.

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?

In the way I implemented LTS for the solver I discussed with Charles, no, LTS does not extend to the solid region. There, Euler or steadyState discretization is used. The LTS method in OpenFOAM sets the local time step size based on the characteristic time for flow, heat release, and reaction rates. These physics do not exist in the solid phase. Thus, to implement LTS in the solid phase, one would need to develop an algorithm to set the local time step based on the characteristic time of diffusion heat transfer in the solid. Or some other method to set the solid region time step, like the one proposed in the referenced Chalmer's paper is needed. I personally have run successful simulations setting the solid region time discretization to "steadyState" even though the fluid region time discretization is LTS.

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).

3/ what is your view on decoupling the time step in the fluid and solid domain as proposed by students at Chalmers?

I think this decoupling of the time step size in the fluid and solid domains is fine based on my own experience with utilizing different time step sizes in different regions of a multi-region case.


I hope this reply is helpful and I welcome other's perspectives.

Best regards,

Eric

[dasith0001]

Hi,

commenting on an old thread but, the latest version OF12 allows this without any modifications.

Cheers,
Dasith