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

chtMultiRegionFoam natural convection negative initial temperature

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

Like Tree4Likes
  • 1 Post By Tobi
  • 2 Post By keitaro7_14
  • 1 Post By saidc.

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 8, 2021, 06:09
Post chtMultiRegionFoam natural convection negative initial temperature
  #1
Member
 
Said CATALBAS
Join Date: Feb 2020
Location: Türkiye
Posts: 43
Rep Power: 3
saidc. is on a distinguished road
Hi,

I'm trying to do turbulent natural convection heat transfer case with chtMultiRegionFoam. The geometry is here. By the way geometry is 3D. The sphere that is at the origin of the coordinate system is 1023.15 K and the fluid (helium) is 523.15K.
  • It starts well to run but after few iterations initial temperature value decreasing. Although the decrease is small, the initial temperature value eventually becomes negative. I first thought it might be because of the mesh, so i refined the mesh but result was the same. Then i tried temperature limits on fvOptions, but this didn't work either.
  • Another problem is the results aren't looks like LES. I've researched similar cases and if we were to compare, my results are disgusting, behave like laminar.

For curiosity I changed my case to cavity and made all boundaries wall (adiabatic bc) and it works much better than inlet-outlet one. Unfortunately I want to do this with patches.

I think i'm doing something wrong on boundary conditions but i can't figure it out. What should I change, what should I try? I am open to any suggestions. Files are attached.

Kind regards,
Said.

For quick look:
Code:
fluid/T

internalField   uniform $Tinitial;
boundaryField
{
    inlet
    {
        type            fixedValue;
        value           uniform $Tinitial;
    }
    outlet
    {
        type            inletOutlet;
        inletValue      uniform $Tinitial;
        value           uniform $Tinitial;
    }
	wall
    {
        type           zeroGradient;
    }
    fluid_to_sphere
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        neighbourFieldName T;
        kappa           kappa;
        Tnbr            T;
        value           uniform $Tinitial;
    }	
}
Code:
fluid/p_rgh

internalField   uniform $pInitial;
boundaryField
{
    outlet
    {
        type            fixedValue;
        value           uniform $pInitial;
    }
    inlet
    {
        type            fixedFluxPressure;
        gradient        uniform 0;
        value           uniform $pInitial;
    }
    wall
    {
        type            fixedFluxPressure;
        gradient        uniform 0;
        value           uniform $pInitial;
    }	
    fluid_to_sphere
    {
        type            fixedFluxPressure;
        gradient        uniform 0;
        value           uniform $pInitial;
    }
}
Code:
fluid/p

internalField   uniform $pInitial;
boundaryField
{
    outlet
    {
        type            calculated;
        value           uniform $pInitial;
    }
    inlet
    {
        type            calculated;
        value           uniform $pInitial;
    }
    wall
    {
        type            calculated;
        value           uniform $pInitial;
    }
    fluid_to_sphere
	{
        type            calculated;
        value           uniform $pInitial;	
	}
}
Code:
fluid/U

internalField   uniform (0 0 0);
boundaryField
{
    inlet
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    outlet
    {
        type        pressureInletOutletVelocity;
        inletValue      uniform (0 0 0);
        value           uniform (0 0 0);
    }
    wall
    {
        type 	fixedValue;
	value 	uniform (0 0 0);		
    }	
    akiskan_to_kure
    {
        type 	fixedValue;
	value   uniform (0 0 0);	
    }
}
Attached Files
File Type: zip hotSphereNaturalConvectionLES.zip (152.0 KB, 3 views)
saidc. is offline   Reply With Quote

Old   February 8, 2021, 07:35
Default
  #2
Senior Member
 
Domenico Lahaye
Join Date: Dec 2013
Posts: 346
Blog Entries: 1
Rep Power: 10
dlahaye is on a distinguished road
What do mean by "Then i tried temperature limits on fvOptions, but this didn't work either." ?
dlahaye is offline   Reply With Quote

Old   February 8, 2021, 07:58
Default
  #3
Member
 
Said CATALBAS
Join Date: Feb 2020
Location: Türkiye
Posts: 43
Rep Power: 3
saidc. is on a distinguished road
Quote:
Originally Posted by dlahaye View Post
What do mean by "Then i tried temperature limits on fvOptions, but this didn't work either." ?
Hi dlahaye,

When i add temperature limit for fluid region, solver stops iteration after like 200 iterates. I mean 0 iteration, all parameters are stay same. For example, first 200 iteration initial temperature value decreasing but still positive, after 200 iteration initial temperature is becomes negative, after last iteration parameteres never change.

kind regards,
Said.
saidc. is offline   Reply With Quote

Old   February 8, 2021, 09:17
Default
  #4
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Augsburg
Posts: 2,597
Blog Entries: 6
Rep Power: 47
Tobi has a spectacular aura aboutTobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Check out your fluid field in the domain? The negative temperature should occur in e.g. some cell or due to unphysical values for p and U. A work-around to fix your problem is to start with another solver (without your sphere). E.g., rhoSimpleFoam/rhoPimpleFoam. I supose that there is a problem somewhere else and the outcome destroyes your energy equation. You can also test with "incompressiblePerfectGas".
saidc. likes this.
__________________
Keep foaming,
Tobias Holzmann
Tobi is offline   Reply With Quote

Old   February 8, 2021, 12:59
Default
  #5
New Member
 
JuanMi
Join Date: Nov 2017
Posts: 26
Rep Power: 6
keitaro7_14 is on a distinguished road
Please attach a runnable example if you want us to help you, with the corresponding scripts (Allrun, etc.). You uploaded a case which is not directly runnable.

A priori your case does not seem too complicated.
Tobi and saidc. like this.
keitaro7_14 is offline   Reply With Quote

Old   February 8, 2021, 15:11
Post
  #6
Member
 
Said CATALBAS
Join Date: Feb 2020
Location: Türkiye
Posts: 43
Rep Power: 3
saidc. is on a distinguished road
Quote:
Originally Posted by keitaro7_14 View Post
Please attach a runnable example if you want us to help you, with the corresponding scripts (Allrun, etc.). You uploaded a case which is not directly runnable.

A priori your case does not seem too complicated.
Hi Tobi and Juan,

Case file is 85 mb so i can't upload here. link, this is github download link. Rar file has everything you need, just download and type ./Allrun.

Also i'll try Tobi's advice as soon as possible.

kind regards,
Said.
Tobi likes this.
saidc. is offline   Reply With Quote

Old   February 9, 2021, 07:14
Default
  #7
Senior Member
 
Peter Hess
Join Date: Apr 2011
Location: Austria
Posts: 228
Rep Power: 13
peterhess is on a distinguished road
Hello Sadic

In:

templates\0\fluid

p_rgh is overall 0.

This is not allowed and should be 1.013e5 (if zou have atmospharic pressure).

That is the main resion for the negative temperature in this solver.

Regards

Peter
peterhess is offline   Reply With Quote

Reply

Tags
chtmultiregionfoam, heat tranfer, les, natural convectin

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
[solidMechanics] Support thread for "Solid Mechanics Solvers added to OpenFOAM Extend" bigphil OpenFOAM CC Toolkits for Fluid-Structure Interaction 633 November 29, 2021 17:00
chtMultiRegionSimpleFoam turbulent case Aditya Patil OpenFOAM Running, Solving & CFD 6 April 24, 2017 23:13
Floating point exception error lpz_michele OpenFOAM Running, Solving & CFD 53 October 19, 2015 03:50
Micro Scale Pore, icoFoam gooya_kabir OpenFOAM Running, Solving & CFD 2 November 2, 2013 14:58
Upgraded from Karmic Koala 9.10 to Lucid Lynx10.04.3 bookie56 OpenFOAM Installation 8 August 13, 2011 05:03


All times are GMT -4. The time now is 10:42.