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

OpenFOAM 6, chtMultiRegionFoam residualcontrol for steady state not working

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

Like Tree4Likes
  • 2 Post By Robin.Kamenicky
  • 1 Post By qtruong
  • 1 Post By Robin.Kamenicky

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 28, 2018, 10:45
Default OpenFOAM 6, chtMultiRegionFoam residualcontrol for steady state not working
  #1
New Member
 
Join Date: Mar 2018
Posts: 4
Rep Power: 4
qtruong is on a distinguished road
Hi,

Since chtMultiRegionSimpleFoam was removed in OpenFOAM 6, I tried running a steady state case with chtMultiRegionFoam, with a residualcontrol (shown below). But it does not stop when converged. Has anyone tested if residualcontrol works in the new chtMultiRegionFoam?

Code:
PIMPLE
{
     residualcontrol
     {
          U     1e-4;
     }
}
qtruong is offline   Reply With Quote

Old   September 2, 2018, 07:46
Default
  #2
Member
 
Robin Kamenicky
Join Date: Mar 2016
Posts: 65
Rep Power: 7
Robin.Kamenicky is on a distinguished road
Hi qtruong,

could you try
Code:
residualControl
instead of
Code:
residualcontrol
Kind regards,
Robin
Robin.Kamenicky is offline   Reply With Quote

Old   September 3, 2018, 11:48
Default
  #3
New Member
 
Join Date: Mar 2018
Posts: 4
Rep Power: 4
qtruong is on a distinguished road
Quote:
Originally Posted by Robin.Kamenicky View Post
Hi qtruong,

could you try
Code:
residualControl
instead of
Code:
residualcontrol
Kind regards,
Robin
thank you for the response.

Sorry, it was my typo while writing the post. It was actually "residualControl" in the code, and it's confirmed by the log file:

Code:
PIMPLE: Region gas
PIMPLE: Convergence criteria found
             U:    tolerance  0.0001
Otherwise, with lower "c", there would be "no convergence criteria found".

Nonetheless, the convergence is reached, but chtMultiRegionFoam keeps running until my endTime.
qtruong is offline   Reply With Quote

Old   September 3, 2018, 14:04
Default
  #4
Member
 
Robin Kamenicky
Join Date: Mar 2016
Posts: 65
Rep Power: 7
Robin.Kamenicky is on a distinguished road
Hi qtruong,

Quote:
Originally Posted by qtruong View Post
Nonetheless, the convergence is reached, but chtMultiRegionFoam keeps running until my endTime.
the chtMultiRegionFoam should run till the endTime. It is transient solver not steady-state as chtMultiRegionSimpleFoam.

The residualControl allows to exit PIMPLE outer loops when the residual criteria are fulfilled. Then it continues with next time step.

Kind regards,
Robin
Robin.Kamenicky is offline   Reply With Quote

Old   September 4, 2018, 12:47
Default
  #5
New Member
 
Join Date: Mar 2018
Posts: 4
Rep Power: 4
qtruong is on a distinguished road
Quote:
Originally Posted by Robin.Kamenicky View Post
Hi qtruong,


the chtMultiRegionFoam should run till the endTime. It is transient solver not steady-state as chtMultiRegionSimpleFoam.

The residualControl allows to exit PIMPLE outer loops when the residual criteria are fulfilled. Then it continues with next time step.

Kind regards,
Robin
Is there then a way to solve steady state conjugate heat transfer in OpenFoam 6 ?
ordinary likes this.
qtruong is offline   Reply With Quote

Old   September 4, 2018, 13:12
Default
  #6
Member
 
Robin Kamenicky
Join Date: Mar 2016
Posts: 65
Rep Power: 7
Robin.Kamenicky is on a distinguished road
Hi qtruong,
Quote:
Originally Posted by qtruong View Post
Is there then a way to solve steady state conjugate heat transfer in OpenFoam 6 ?
There is no solver for steady state conjugated heat transfer in OpenFoam6. However, if your problem is steady state problem, the transient solver will converge to steady state.

Eventually you can try to use local time stepping (localEuler time derivative approximation).

Another possibility is to use OpenFoam5 and chtMultiRegionSimpleFoam. If I understand right, the difference between OpenFoam5 and OpenFoam6 is only in usability for conjugated heat transfer solvers.

Hope it helps,
Robin
ordinary likes this.
Robin.Kamenicky is offline   Reply With Quote

Old   March 2, 2019, 10:37
Default
  #7
Member
 
julien givernaud
Join Date: Dec 2018
Posts: 42
Rep Power: 3
julieng is on a distinguished road
Hello,


I try to result a CHT steady state case with openfoam 6 and chtMultiRegionFoam. I am not able to solve it, it crashes after few time steps.

chtMultiRegionSimpleFoam done the job with Openfoam 5, I obtained good accuracy with analytical solutions.



I read your post Robin.Kamenicky, you wrote :


Code:
There is no solver for steady state conjugated heat transfer in  OpenFoam6. However, if your problem is steady state problem, the  transient solver will converge to steady state.

What is the reason to have give up the steady state solver in openfoam 6 ?


Best regards
julieng is offline   Reply With Quote

Old   March 2, 2019, 11:53
Default
  #8
Member
 
Robin Kamenicky
Join Date: Mar 2016
Posts: 65
Rep Power: 7
Robin.Kamenicky is on a distinguished road
Hi julieng,

Actually, I have been mistaken. The official documentation of OF6 for chtMultiRegionFoam tells:
Code:
Solver for steady or transient fluid flow and solid heat conduction, with
     conjugate heat transfer between regions, buoyancy effects, turbulence,
     reactions and radiation modelling.
What was the error?

Kind regrads,
Robin
Robin.Kamenicky is offline   Reply With Quote

Old   March 2, 2019, 12:00
Default
  #9
Member
 
Robin Kamenicky
Join Date: Mar 2016
Posts: 65
Rep Power: 7
Robin.Kamenicky is on a distinguished road
Hi julieng,

according to tutorials. You can setup scheme for time derivative to
Code:
steadyState
Kind Regards,
Robin
Robin.Kamenicky is offline   Reply With Quote

Old   March 4, 2019, 08:15
Default
  #10
Member
 
julien givernaud
Join Date: Dec 2018
Posts: 42
Rep Power: 3
julieng is on a distinguished road
Hello Robin,

Yes it works for stationary cases, I have test it. I have same results than openfoam v5.

I try the new functionnality
"wallHeatTransferCoeff"

I read on the Openfoam 6 release:
Data Processing: function objects for individual regions in a multi-region simulation [ commit a5a034 ]; wallHeatTransferCoeff function object to calculate the wall heat transfer coefficient [ commit 99841e ]; in wallHeatFlux, improved efficiency of heat flux calculation [ commit 6584fa ] and corrected contribution of radiative heat flux [ commit 396259 ].

But I see that it works only for incompressible fluids… cht is for compressible fluids. Maybe someone knows how to modify the file.


I see the post of bloerb
https://www.cfd-online.com/Forums/op...ing-print.html

But I Don't know how to do. I am a total beginner in function object.

Best regards
julieng is offline   Reply With Quote

Old   December 18, 2019, 03:24
Default
  #11
Member
 
Join Date: Nov 2014
Posts: 90
Rep Power: 8
hokhay is on a distinguished road
Quote:
Originally Posted by julieng View Post
Hello Robin,

Yes it works for stationary cases, I have test it. I have same results than openfoam v5.

I try the new functionnality
"wallHeatTransferCoeff"

I read on the Openfoam 6 release:
Data Processing: function objects for individual regions in a multi-region simulation [ commit a5a034 ]; wallHeatTransferCoeff function object to calculate the wall heat transfer coefficient [ commit 99841e ]; in wallHeatFlux, improved efficiency of heat flux calculation [ commit 6584fa ] and corrected contribution of radiative heat flux [ commit 396259 ].

But I see that it works only for incompressible fluids… cht is for compressible fluids. Maybe someone knows how to modify the file.


I see the post of bloerb
https://www.cfd-online.com/Forums/op...ing-print.html

But I Don't know how to do. I am a total beginner in function object.

Best regards
Do you need to change the anything in fvSolution and controlDict too? Such as relaxationFactors or Courant number.

Thank you
hokhay is offline   Reply With Quote

Reply

Tags
chtmultiregionfoam, heat transfer

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
Current state of conjugate heat transfer in OpenFOAM Dreoasteh OpenFOAM 1 June 27, 2017 07:15
OpenFOAM Training Jan-Jul 2017, Virtual, London, Houston, Berlin CFDFoundation OpenFOAM Announcements from Other Sources 0 January 4, 2017 07:15
Suggestion for a new sub-forum at OpenFOAM's Forum wyldckat Site Help, Feedback & Discussions 20 October 28, 2014 10:04
Calculation of the Governing Equations Mihail CFX 7 September 7, 2014 07:27
error message cuteapathy CFX 14 March 20, 2012 07:45


All times are GMT -4. The time now is 01:57.