Why the initial residual is not zero？

chaochaoyoyo · April 9, 2016, 02:47

Hi All:

I 'm trying to solve transient buoyant-driven flow in a 2D cavity by my own solver. What makes me confused is when temperature field is uniform, the initial residual of temperature is not zero, which equals to 0.000188696!

The temperature of top and bottom wall are set equal to internal field, and the two side wall are zeroGradient. Besides, phi is zero, lambda and cv are dimensionedscalar (constant).

Any suggestion will be appreciated.

Code:

	

fvScalarMatrix TEqn
(
    fvm::ddt(rho, T)
  + fvm::div(phi, T)
  - fvm::laplacian(lambda/cv, T)	  
);

Tobi · April 12, 2016, 06:39

Hi,

we are doing iterative modeling. Think about that. You get numerical errors, discretization errors, interpolation errors and much more. Also if we simulate a flow in a simple pipe with inlet outlet and converged solution we could obtain p in the last iteration like 1e-4 that is actually not even zero too.

In your case it is clear for us that it should be zero but in the numerical point of view not really. Normally if you did everything correct you should get 0 of course (hex mesh and everything is well done). You can check that out with scalarTransportFoam. If you set U to zero -> phi = 0, set T initial and boundary to the same value you will get:

Code:

DILUPBiCG:  Solving for S, Initial residual = 0, Final residual = 0, No Iterations 0
Time = 0.0002

But here we are solving for incompressible flow:

Code:

            solve
            (
                fvm::ddt(S)
              + fvm::div(phi, S)
              - fvm::laplacian(DT, S)
             ==
                fvOptions(S)
            );

So I think you get the non zero values due to your time derivation. Which is at last:
$\frac{\partial}{\partial t} ( \rho S ) = \rho \frac{\partial S} {\partial t} + S \frac{\partial \rho} {\partial t}$

$\rho \frac{\partial S} {\partial t} + S \frac{\partial \rho} {\partial t} = \rho^o \frac{S^n - S^o} {\Delta t} + S^0 \frac{\rho^n - \rho^o} {\Delta t}$

Rho is calculated by thermodynamics and could return numerical errors. That would be the reason in your case. You can try to fix rho to a const value. Then each term should vanish and you should end up with zero.

chaochaoyoyo · April 24, 2016, 11:45

Quote:

Originally Posted by Tobi

Hi,

we are doing iterative modeling. Think about that. You get numerical errors, discretization errors, interpolation errors and much more. Also if we simulate a flow in a simple pipe with inlet outlet and converged solution we could obtain p in the last iteration like 1e-4 that is actually not even zero too.

In your case it is clear for us that it should be zero but in the numerical point of view not really. Normally if you did everything correct you should get 0 of course (hex mesh and everything is well done). You can check that out with scalarTransportFoam. If you set U to zero -> phi = 0, set T initial and boundary to the same value you will get:

Code:

DILUPBiCG:  Solving for S, Initial residual = 0, Final residual = 0, No Iterations 0
Time = 0.0002

But here we are solving for incompressible flow:

Code:

            solve
            (
                fvm::ddt(S)
              + fvm::div(phi, S)
              - fvm::laplacian(DT, S)
             ==
                fvOptions(S)
            );

So I think you get the non zero values due to your time derivation. Which is at last:
$\frac{\partial}{\partial t} ( \rho S ) = \rho \frac{\partial S} {\partial t} + S \frac{\partial \rho} {\partial t}$

$\rho \frac{\partial S} {\partial t} + S \frac{\partial \rho} {\partial t} = \rho^o \frac{S^n - S^o} {\Delta t} + S^0 \frac{\rho^n - \rho^o} {\Delta t}$

Rho is calculated by thermodynamics and could return numerical errors. That would be the reason in your case. You can try to fix rho to a const value. Then each term should vanish and you should end up with zero.

Thank you for your reply. After using relative temperature rather than absolute temperature, this problem is solved! I think it is mainly caused by machine accuracy. Your reply has given me a lot of inspiration.

Tobi · July 4, 2016, 09:51

Dear all,

to clear the topic... the above equation is only valid if we solve explicit. As we can see from the implementation, we solve implicit. That means that we create a matrix that has to be solved. Solving the algebraic set of equations will result in numerical errors that would lead to the initial error here (:

bbita · November 22, 2017, 10:49

Dear Foamers,

I am facing the same problem in different solvers. The density is not the reason as I tried to remove density from the equation and the same thing happened. Using relative parameter (e.g. zero instead of 300K for temperature) solved the issue. My problem is if I have some variation in my system, even if when my temperature become steady, I have some initial residual and my simulation is not speeding up. Any idea?

April 9, 2016, 02:47	Why the initial residual is not zero？	#1
chaochaoyoyo New Member Zhanchao Hu Join Date: Apr 2016 Posts: 8 Rep Power: 10	Hi All: I 'm trying to solve transient buoyant-driven flow in a 2D cavity by my own solver. What makes me confused is when temperature field is uniform, the initial residual of temperature is not zero, which equals to 0.000188696! The temperature of top and bottom wall are set equal to internal field, and the two side wall are zeroGradient. Besides, phi is zero, lambda and cv are dimensionedscalar (constant). Any suggestion will be appreciated. Code: fvScalarMatrix TEqn ( fvm::ddt(rho, T) + fvm::div(phi, T) - fvm::laplacian(lambda/cv, T) );

April 12, 2016, 06:39		#2
Tobi Super Moderator Tobias Holzmann Join Date: Oct 2010 Location: Bad Wörishofen Posts: 2,711 Blog Entries: 6 Rep Power: 52	Hi, we are doing iterative modeling. Think about that. You get numerical errors, discretization errors, interpolation errors and much more. Also if we simulate a flow in a simple pipe with inlet outlet and converged solution we could obtain p in the last iteration like 1e-4 that is actually not even zero too. In your case it is clear for us that it should be zero but in the numerical point of view not really. Normally if you did everything correct you should get 0 of course (hex mesh and everything is well done). You can check that out with scalarTransportFoam. If you set U to zero -> phi = 0, set T initial and boundary to the same value you will get: Code: DILUPBiCG: Solving for S, Initial residual = 0, Final residual = 0, No Iterations 0 Time = 0.0002 But here we are solving for incompressible flow: Code: solve ( fvm::ddt(S) + fvm::div(phi, S) - fvm::laplacian(DT, S) == fvOptions(S) ); So I think you get the non zero values due to your time derivation. Which is at last: $\frac{\partial}{\partial t} ( \rho S ) = \rho \frac{\partial S} {\partial t} + S \frac{\partial \rho} {\partial t}$ $\rho \frac{\partial S} {\partial t} + S \frac{\partial \rho} {\partial t} = \rho^o \frac{S^n - S^o} {\Delta t} + S^0 \frac{\rho^n - \rho^o} {\Delta t}$ Rho is calculated by thermodynamics and could return numerical errors. That would be the reason in your case. You can try to fix rho to a const value. Then each term should vanish and you should end up with zero. SamPrabhu likes this. __________________ Keep foaming, Tobias Holzmann

July 4, 2016, 09:51		#4
Tobi Super Moderator Tobias Holzmann Join Date: Oct 2010 Location: Bad Wörishofen Posts: 2,711 Blog Entries: 6 Rep Power: 52	Dear all, to clear the topic... the above equation is only valid if we solve explicit. As we can see from the implementation, we solve implicit. That means that we create a matrix that has to be solved. Solving the algebraic set of equations will result in numerical errors that would lead to the initial error here (: __________________ Keep foaming, Tobias Holzmann

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
simpleFoam error - "Floating point exception"	mbcx4jc2	OpenFOAM Running, Solving & CFD	12	August 4, 2015 03:20
Unstabil Simulation with chtMultiRegionFoam	mbay101	OpenFOAM Running, Solving & CFD	13	December 28, 2013 14:12
pimpleFoam: turbulence->correct(); is not executed when using residualControl	hfs	OpenFOAM Running, Solving & CFD	3	October 29, 2013 09:35
calculation stops after few time steps	sivakumar	OpenFOAM Running, Solving & CFD	7	March 17, 2013 07:37
Orifice Plate with a fully developed flow - Problems with convergence	jonmec	OpenFOAM Running, Solving & CFD	3	July 28, 2011 06:24

November 22, 2017, 10:49		#5
bbita Member Join Date: May 2017 Posts: 44 Rep Power: 9	Dear Foamers, I am facing the same problem in different solvers. The density is not the reason as I tried to remove density from the equation and the same thing happened. Using relative parameter (e.g. zero instead of 300K for temperature) solved the issue. My problem is if I have some variation in my system, even if when my temperature become steady, I have some initial residual and my simulation is not speeding up. Any idea?