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

Enthalpy Residuals remains constant even though Temperature is converged

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

Like Tree1Likes
  • 1 Post By pss47

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 4, 2018, 07:09
Default Enthalpy Residuals remains constant even though Temperature is converged
  #1
New Member
 
Sudarshan Padubidre
Join Date: May 2018
Posts: 14
Rep Power: 8
pss47 is on a distinguished road
Hi all,

I am performing steady state vehicle cabin simulations using buoyantSimpleFoam solver. The geometry is complex but I got pretty good mesh which has 3 nonOrthogonal Faces with Max nonOrthogonality = 73 degrees.


The boundary conditions are simple for now, Velocity and Temperature are specified at inlet. All walls are adiabatic.



The internal field is reaching the inlet temperature but still the 'h' residuals are almost constant throughout the simulation. I have attached the related images with the post. I don't know what is the reason for this issue. Any help is appreciated.



Code:

//Temperature 



dimensions      [0 0 0 1 0 0 0];

internalField   uniform 300;

boundaryField
{

    #includeEtc "caseDicts/setConstraintTypes"

    "Wall_.*"
    {
        type            zeroGradient;
    }

    "Inlet_.*"
    {
        type            fixedValue;
        value           uniform 280;
    }

    "Outlet_.*"
    {
        type            inletOutlet;
        inletValue      uniform 280;
        value           uniform 280;
    }

}
Code:
//Velocity

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField

{
#includeEtc "caseDicts/setConstraintTypes"
    "Wall_.*"
    {
        type         noSlip;
    }

    "Inlet_.*"
    {
        type            surfaceNormalFixedValue;
            refValue        uniform -2;

//        type                flowRateInletVelocity;
//            volumetricFlowRate  0.0035;
//            value               (0 0 0);

    }

    "Outlet_.*"
    {
        type            inletOutlet;
            inletValue      uniform (0 0 0);
            value           uniform (0 0 0);
    }
}
Temperature.png

Residuals.png

CaseFiles.zip
pss47 is offline   Reply With Quote

Old   November 4, 2018, 09:31
Default
  #2
Senior Member
 
Peter Baskovich
Join Date: Jul 2014
Posts: 127
Rep Power: 12
pete20r2 is on a distinguished road
None of the other fields, except for maybe epsilon are converged either.
I think you need to keep running for more timesteps.
That being said, I think you need to converge the flow fields (U and p_rgh) (also the turbulent quantities) before you can trust the h field.
Depending on what result you are actually trying to quantify from this study, you can choose what level of convergence is acceptable when it becomes clear that the temperature field (at your sensor locations) looks to be stable.
In your T plot the temperatures are clearly still falling (visually), hence there is still a substantial residual.
pete20r2 is offline   Reply With Quote

Old   November 7, 2018, 05:42
Default
  #3
New Member
 
Sudarshan Padubidre
Join Date: May 2018
Posts: 14
Rep Power: 8
pss47 is on a distinguished road
Quote:
Originally Posted by pete20r2 View Post
None of the other fields, except for maybe epsilon are converged either.
I think you need to keep running for more timesteps.
That being said, I think you need to converge the flow fields (U and p_rgh) (also the turbulent quantities) before you can trust the h field.
Depending on what result you are actually trying to quantify from this study, you can choose what level of convergence is acceptable when it becomes clear that the temperature field (at your sensor locations) looks to be stable.
In your T plot the temperatures are clearly still falling (visually), hence there is still a substantial residual.

Hello Peter,


I agree that the flow fields has not yet converged. But, what i don't understand is that why residuals of h field is almost constant even though the temperature is coverging to the required solution(It has to reach 280K according to the BC).



Thank you for your interest on the issue
Sudarshan
pss47 is offline   Reply With Quote

Old   November 7, 2018, 05:55
Default
  #4
Senior Member
 
Peter Baskovich
Join Date: Jul 2014
Posts: 127
Rep Power: 12
pete20r2 is on a distinguished road
The convergence reported by the solver is for the entire field. Since your flow field is not converged there can be no certainty in where the h field is not converged. Constant residual just mean that there is the same difference between solution steps, the solver may still be working towards a converged solution. The difference may not be in the location you are sensing at so it is not showing up in your plot.
Depending on you problem, it is generally recommended to get flow field convergence below 1e-4 to 1e-6 to have consistent results.
pete20r2 is offline   Reply With Quote

Old   November 7, 2018, 06:26
Default
  #5
New Member
 
Sudarshan Padubidre
Join Date: May 2018
Posts: 14
Rep Power: 8
pss47 is on a distinguished road
Quote:
Originally Posted by pete20r2 View Post
The convergence reported by the solver is for the entire field. Since your flow field is not converged there can be no certainty in where the h field is not converged. Constant residual just mean that there is the same difference between solution steps, the solver may still be working towards a converged solution. The difference may not be in the location you are sensing at so it is not showing up in your plot.
Depending on you problem, it is generally recommended to get flow field convergence below 1e-4 to 1e-6 to have consistent results.

The value of Temperature in the entire mesh is below 281 ( initial value being 300) when I check it in the paraview.
pss47 is offline   Reply With Quote

Old   November 13, 2018, 11:45
Default
  #6
New Member
 
Sudarshan Padubidre
Join Date: May 2018
Posts: 14
Rep Power: 8
pss47 is on a distinguished road
I have found the reason for the strange behavior. It is the combination of BC and computation of residuals in OpenFOAM.


According to this source, the errors for the residuals are normalized using the average of the computed variable. When the final solution is completely homogeneous throughout the domain, The mean value is approximately equal to the computed variable which keeps the residual constant.


I changed the boundary condition to get non uniform solution, the residuals started decreasing.


Code:
internalField   uniform 300;

boundaryField
{

    #includeEtc "caseDicts/setConstraintTypes"

    "Wall_.*"
    {
        type            zeroGradient;
    }

    "Wall_Floor_.*"
    {
        type            fixedValue;
        value           uniform 300;
    }

    "Inlet_.*"
    {
        type            fixedValue;
        value           uniform 280;
    }

    "Outlet_.*"
    {
        type            inletOutlet;
        inletValue      uniform 280;
        value           uniform 280;
    }

}
Residuals_new.png
Wowbagger likes this.
pss47 is offline   Reply With Quote

Reply

Tags
buoyantsimplefoam, residuals non convergence, thermophysical model

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
Simple piston movement in cylinder- fluid models arun1994 CFX 4 July 8, 2016 03:54
unexpected constant Temperature on a clip surface Sungki OpenFOAM Running, Solving & CFD 0 August 4, 2015 05:50
Calculation of the Governing Equations Mihail CFX 7 September 7, 2014 07:27
Constant heat flux with uniform temperature Jake Lee FLUENT 2 April 13, 2011 23:08
Two-Phase Buoyant Flow Issue Miguel Baritto CFX 4 August 31, 2006 13:02


All times are GMT -4. The time now is 11:37.