[LennyZ]

Dear Foamers -- looks like a bug:

rhoCentralFoam (6) DOES NOT read fvOptions upon solver execution. It does not read from /constant not from /system. Checked with rhoSimpleFoam -- no problem there.
It is as if the file (fvOptions) is simply not there .. like file with this name does not exist.


Thanks for looking into it.

[Moderator note: Moved from the Bugs subforum to the CFD Solving forum.]

[clapointe]

rhoCentralFoam is not coded to use fvOptions, hence it is not read (and therefore not a bug).

Caelan

[LennyZ]

Thanks! Suspected that. Would you happen to know a quick workaround to limit temperature or pressure in rhoCentralFoam? (sorry for posting in a 'bug thread')

[Carlo_P]

Hey,
you can limit pressure or temperature in fvSolution.
Check this file: https://github.com/OpenFOAM/OpenFOAM...tem/fvSolution

Instead of rhoMin and rhoMax you can use temperatureMin and temperatureMax and other variables.
I think that the new version would like to have rhoMinFactor or something like this.

[LennyZ]

Hi!

Appreciate that. This is for rhoCentralFoam and I wonder where to place something like minTemperature or minPressure in fvSolution and what these variables actually are. I can start looking into the code, but that is after I make sure nobody has a quick answer (not obvious from Google). Normally, I would limit the temperature in fvOptions which is not available under rhoCentralFoam.


L 08/29/19

[wyldckat]

Quick notes:

1. rhoCentralFoam uses an equation implementation which will likely require special handling of source terms; I say this due to first post on this thread: Adding source terms to rhoCentralFoam
2. Limiting density only works on solvers that implement it. For example, if you use this search page: https://github.com/OpenFOAM/OpenFOAM...ressureControl - it's already configured to look for "pressureControl" and lists the files that mention it. You can find this way which solvers use this method.
   You can also look for "rhoMin" or "rhoMax" for other examples.
3. Take a look into the files where the class "pressureControl" is implemented and you will see how the "rhoMin" and "rhoMax" values are used.
4. This:
   

   Originally Posted by Carlo_P

   Instead of rhoMin and rhoMax you can use temperatureMin and temperatureMax and other variables.

   is false regarding the possibilities to use other field names, at least in OpenFOAM 6, it's only available for "rho" and it depends on whether it was implemented/used or not.
5. In order to limit in rhoCentralFoam, you will likely have to create a custom version of this solver, either to at least use "fvOptions.constrain" or to enforce a min-max value on temperature... if it even makes sense, in case it only handles energy.

[bluecore]

If that is the case, how come that official user guide advertises fvOptions?
https://www.openfoam.com/documentati...ntralFoam.html

[shock77]

Hi,


I had the same problem and updated the solver with just a few lines and recompiled it. Its all described in this post:


Sudden Increase of residuals

[bluecore]

Originally Posted by shock77

Hi,


I had the same problem and updated the solver with just a few lines and recompiled it. Its all described in this post:


Sudden Increase of residuals

Thanks! That's exactly what I was searching for. However, there are 2 inviscid checks in the rhoCentralFoam.C code. Did you just add an additional statement at the end of the file? Since it's not included in the original code, can you please explain where does the inclusion of "EEqnRCF" come from?

[shock77]

Hi,


I am not sure what you mean with "additional statement". You have to include fvOptions in rhoCentralFoam.C, so you need the statement: #include "fvOptions.H.


EEqnRCF is just a name I made up. RCF = rhoCentralFoam. This is just to use constrain and correct functionality.

[hbulus]

Delete this comment please