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

rhoCentralFoam (6) DOES NOT read fvOptions

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 25, 2019, 04:38
Default rhoCentralFoam (6) DOES NOT read fvOptions
  #1
New Member
 
Join Date: Nov 2016
Posts: 8
Rep Power: 6
LennyZ is on a distinguished road
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.]

Last edited by wyldckat; August 26, 2019 at 16:24. Reason: see "Moderator note:"
LennyZ is offline   Reply With Quote

Old   August 25, 2019, 10:37
Default
  #2
Senior Member
 
Join Date: Aug 2015
Posts: 474
Rep Power: 11
clapointe is on a distinguished road
rhoCentralFoam is not coded to use fvOptions, hence it is not read (and therefore not a bug).

Caelan
clapointe is offline   Reply With Quote

Old   August 26, 2019, 03:08
Default
  #3
New Member
 
Join Date: Nov 2016
Posts: 8
Rep Power: 6
LennyZ is on a distinguished road
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')
LennyZ is offline   Reply With Quote

Old   August 26, 2019, 04:53
Default
  #4
Senior Member
 
Carlo_P
Join Date: May 2019
Location: Italy
Posts: 177
Rep Power: 4
Carlo_P is on a distinguished road
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.
Carlo_P is offline   Reply With Quote

Old   August 26, 2019, 13:21
Default
  #5
New Member
 
Join Date: Nov 2016
Posts: 8
Rep Power: 6
LennyZ is on a distinguished road
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
LennyZ is offline   Reply With Quote

Old   August 26, 2019, 16:34
Default
  #6
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,962
Blog Entries: 45
Rep Power: 123
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
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:
    Quote:
    Originally Posted by Carlo_P View Post
    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.
__________________
wyldckat is offline   Reply With Quote

Old   January 25, 2021, 02:09
Default
  #7
New Member
 
Matus Cvengros
Join Date: May 2018
Posts: 3
Rep Power: 4
bluecore is on a distinguished road
If that is the case, how come that official user guide advertises fvOptions?
https://www.openfoam.com/documentati...ntralFoam.html
bluecore is offline   Reply With Quote

Old   January 25, 2021, 03:07
Default
  #8
Senior Member
 
Join Date: Dec 2019
Posts: 138
Rep Power: 3
shock77 is on a distinguished road
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
shock77 is offline   Reply With Quote

Old   January 25, 2021, 03:32
Default
  #9
New Member
 
Matus Cvengros
Join Date: May 2018
Posts: 3
Rep Power: 4
bluecore is on a distinguished road
Quote:
Originally Posted by shock77 View Post
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?
bluecore is offline   Reply With Quote

Old   January 25, 2021, 03:43
Default
  #10
Senior Member
 
Join Date: Dec 2019
Posts: 138
Rep Power: 3
shock77 is on a distinguished road
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.
shock77 is offline   Reply With Quote

Old   March 24, 2021, 06:55
Default
  #11
Member
 
Join Date: Dec 2018
Posts: 34
Rep Power: 4
hbulus is on a distinguished road
Delete this comment please
hbulus is offline   Reply With Quote

Reply

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
Configuration of boundary conditions and fvOptions file Raza Javed OpenFOAM Running, Solving & CFD 16 May 3, 2019 16:35
[mesh manipulation] Importing Multiple Meshes thomasnwalshiii OpenFOAM Meshing & Mesh Conversion 18 December 19, 2015 18:57
Parallel Error in ANSYS FLUENT 12 zeusxx FLUENT 25 July 17, 2015 04:40
[Commercial meshers] fluentMeshToFoam multidomain mesh conversion problem Attesz OpenFOAM Meshing & Mesh Conversion 12 May 2, 2013 10:52
999999 (../../src/mpsystem.c@1123):mpt_read: failed:errno = 11 UDS_rambler FLUENT 2 November 22, 2011 09:46


All times are GMT -4. The time now is 23:39.