# Natural convection over a single tube

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

 May 1, 2013, 14:18 Natural convection over a single tube #1 Member   ankur Join Date: May 2012 Location: India Posts: 50 Rep Power: 6 Hey Guys, I am simulating a single tube of 325 mm length and 25 mm diameter kept inside a closed box of 2 m X 2 m X 2 m dimensions filled with air. I am simulating air as the perfect gas (compressible model). The tube is kept at 350 K temperature and air is at 300 K. I am using buoyantPimpleFoam solver in Openfoam 2.0.0. The pressure is atmospheric at the tube and at the walls of the container, the velocity is no slip everywhere. The problem is with the convergence, I am getting a fluctuating residuals for velocity and pressure. The residuals varies from 1e-02 to 1e-04, but it is not converging. The velocity vectors seems ok everywhere but the temperature range is showing 299.97 to 350 K, which should not go below 300 K (ideally). I am taking a time step of 1e-05, and the meshing is tetrahedral (unstructured). I am using k-epsilon model as well as have tried SSTkOmega. Please help me if you have any idea about this, I have tried every boundary conditions I could. Thanks in advance

 May 3, 2013, 11:07 nonOrthogonalCorrector #2 Senior Member   Fabian Roesler Join Date: Mar 2009 Location: Germany Posts: 210 Rep Power: 10 Hi How many nonOrthogonalCorrectors do you apply? With tetrahedral mesh you probably have to increase them. Could you post your fvSolution dict? Regards Fabian

 May 3, 2013, 13:40 #3 Member   ankur Join Date: May 2012 Location: India Posts: 50 Rep Power: 6 Hey Thanks for your reply, I am posting my fvSolutions /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.0.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { "rho.*" { solver PCG; preconditioner DIC; tolerance 0; relTol 0; } p_rgh { solver GAMG; tolerance 1e-09; relTol 0.001; smoother GaussSeidel; cacheAgglomeration true; nCellsInCoarsestLevel 20; agglomerator faceAreaPair; mergeLevels 1; minIter 1; } p_rghFinal { solver GAMG; tolerance 1e-09; relTol 0.001; smoother GaussSeidel; cacheAgglomeration true; nCellsInCoarsestLevel 20; agglomerator faceAreaPair; mergeLevels 1; minIter 1; } h { solver GAMG; tolerance 1e-08; relTol 0.01; smoother GaussSeidel; cacheAgglomeration true; nCellsInCoarsestLevel 20; agglomerator faceAreaPair; mergeLevels 1; minIter 1; } R { solver PBiCG; preconditioner DILU; tolerance 1e-08; relTol 0.01; } U { solver smoothSolver; smoother GaussSeidel; nSweeps 2; tolerance 1e-07; relTol 0.01; } k { solver smoothSolver; smoother GaussSeidel; nSweeps 2; tolerance 1e-07; relTol 0.01; } omega { solver smoothSolver; smoother GaussSeidel; nSweeps 2; tolerance 1e-07; relTol 0.01; } "(U|k|omega|h|R)Final" { \$U; relTol 0; } } PIMPLE { momentumPredictor yes; nOuterCorrectors 1; nCorrectors 2; nNonOrthogonalCorrectors 0; } { p 0.5; U 0.3; T 0.5; k 0.5; omega 0.5; nut 0.5; R 0.5; nuTilda 0.5; } In one of the cases I had some fins on the same tube, I used nNonOrthogonalCorrectors = 4 and air as incompressible fluid, but in that case velocity was converging but p_rgh was not converging. Plz have a look at it. // ************************************************** *********************** // Last edited by Ank; May 3, 2013 at 13:56.

May 4, 2013, 03:46
#4
Senior Member

T Chourushi
Join Date: Jul 2009
Location: India
Posts: 319
Blog Entries: 1
Rep Power: 10
Quote:
 Originally Posted by Ank Hey Thanks for your reply, I am posting my fvSolutions /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.0.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { "rho.*" { solver PCG; preconditioner DIC; tolerance 0; relTol 0; } p_rgh { solver GAMG; tolerance 1e-09; relTol 0.001; smoother GaussSeidel; cacheAgglomeration true; nCellsInCoarsestLevel 20; agglomerator faceAreaPair; mergeLevels 1; minIter 1; } p_rghFinal { solver GAMG; tolerance 1e-09; relTol 0.001; smoother GaussSeidel; cacheAgglomeration true; nCellsInCoarsestLevel 20; agglomerator faceAreaPair; mergeLevels 1; minIter 1; } h { solver GAMG; tolerance 1e-08; relTol 0.01; smoother GaussSeidel; cacheAgglomeration true; nCellsInCoarsestLevel 20; agglomerator faceAreaPair; mergeLevels 1; minIter 1; } R { solver PBiCG; preconditioner DILU; tolerance 1e-08; relTol 0.01; } U { solver smoothSolver; smoother GaussSeidel; nSweeps 2; tolerance 1e-07; relTol 0.01; } k { solver smoothSolver; smoother GaussSeidel; nSweeps 2; tolerance 1e-07; relTol 0.01; } omega { solver smoothSolver; smoother GaussSeidel; nSweeps 2; tolerance 1e-07; relTol 0.01; } "(U|k|omega|h|R)Final" { \$U; relTol 0; } } PIMPLE { momentumPredictor yes; nOuterCorrectors 1; nCorrectors 2; nNonOrthogonalCorrectors 0; } { p 0.5; U 0.3; T 0.5; k 0.5; omega 0.5; nut 0.5; R 0.5; nuTilda 0.5; } In one of the cases I had some fins on the same tube, I used nNonOrthogonalCorrectors = 4 and air as incompressible fluid, but in that case velocity was converging but p_rgh was not converging. Plz have a look at it. // ************************************************** *********************** //
Hello,

Do, something like this and let us know about the convergence.

PIMPLE
{
momentumPredictor yes;
nOuterCorrectors 1;
nCorrectors 2;
nNonOrthogonalCorrectors 1;
pRefCell 0;
pRefValue 0;
}

relaxationFactors
{
fields
{
}
equations
{
"(U|T|k|epsilon|R)" 1;
"(U|T|k|epsilon|R)Final" 1;
}
}

You can also have a look at the tutorial/case folder of other heat transfer problems.

Also, try varying the "nNonOrthogonalCorrectors" upto 1 & 2. If still you are not getting the convergence then try to make quality (skewness for unstructured < 0.7) mesh.

 May 4, 2013, 07:30 outerCorrectors and relaxation #5 Senior Member   Fabian Roesler Join Date: Mar 2009 Location: Germany Posts: 210 Rep Power: 10 Right. These settings look good for me too. Check your mesh quality. If you still have problems you could increase your outer correctors and give some relaxation factors. Regards Fabian

 May 4, 2013, 13:51 #6 Member   ankur Join Date: May 2012 Location: India Posts: 50 Rep Power: 6 Hey Thanks alot for your replies. I have updated my fvSolution accordingly in an already running case. The velocity residual is 1e-05 and pressure residual is 0.054, pressure residual is coming down with time. Hope to have it converged in some more time. I will post you accordingly after some time. Once again thanks a lot for the help. One more thing I would like to ask, what is the significance of the outer correctors and non orthogonal correctors. Ankur

May 6, 2013, 07:13
#7
Senior Member

T Chourushi
Join Date: Jul 2009
Location: India
Posts: 319
Blog Entries: 1
Rep Power: 10
Quote:
 Originally Posted by Ank Hey Thanks alot for your replies. I have updated my fvSolution accordingly in an already running case. The velocity residual is 1e-05 and pressure residual is 0.054, pressure residual is coming down with time. Hope to have it converged in some more time. I will post you accordingly after some time. Once again thanks a lot for the help. One more thing I would like to ask, what is the significance of the outer correctors and non orthogonal correctors. Ankur

 May 6, 2013, 07:30 Nice Page #8 Senior Member   Fabian Roesler Join Date: Mar 2009 Location: Germany Posts: 210 Rep Power: 10 Nice, didn't know that page. Thanks. Any news Ankur? Regrads Fabian

May 7, 2013, 02:05
#9
Senior Member

T Chourushi
Join Date: Jul 2009
Location: India
Posts: 319
Blog Entries: 1
Rep Power: 10
Quote:
 Originally Posted by fabian_roesler Nice, didn't know that page. Thanks. Any news Ankur? Regrads Fabian
You are welcome, even it is mentioned in the user guide of OF by Sir H. Jasak.

 May 7, 2013, 02:32 #10 Member   ankur Join Date: May 2012 Location: India Posts: 50 Rep Power: 6 Hey Sorry I got busy in some other work. I have seen that page..not fully understood though. I will read it again and will let you know. The case of tube having fins is now converging, the pressure has gone to 0.02 from 0.5..the convergence is slow. The grid quality is the problem I think, because the grid number is 1600000, mesh is tetra, and the skewness is around 1.1. I am using Gmsh 2.3.0 and I am not able to decrease the skewness below this value. I am very thankful to both of you for your valuable suggestions and time. I will post back as soon as possible with further updates.

May 7, 2013, 03:05
#11
Senior Member

T Chourushi
Join Date: Jul 2009
Location: India
Posts: 319
Blog Entries: 1
Rep Power: 10
Quote:
 Originally Posted by Ank Hey Sorry I got busy in some other work. I have seen that page..not fully understood though. I will read it again and will let you know. The case of tube having fins is now converging, the pressure has gone to 0.02 from 0.5..the convergence is slow. The grid quality is the problem I think, because the grid number is 1600000, mesh is tetra, and the skewness is around 1.1. I am using Gmsh 2.3.0 and I am not able to decrease the skewness below this value. I am very thankful to both of you for your valuable suggestions and time. I will post back as soon as possible with further updates.

Sometimes quality mesh really have an impact on results, may be with skewness of around 1.1 you may not get good results. Actually, order of >1 means you need to re-mesh your geometry.
So, it is usually advisable to keep skewness upto <0.8. For, that you need to really try hard in meshing. Spend sometime reading the same.
At last, the CFD solution depends on "Geometry meshing + solution algorithms" methods. So, you need to keep a balance between these, knowing only one method may cause problems in the results.

 May 7, 2013, 03:13 #12 Member   ankur Join Date: May 2012 Location: India Posts: 50 Rep Power: 6 Hey Tushar Thanks for the suggestion. I have tried a lot to decrease the skewness, and you are right I should try harder to make it good. I am going to do it first. I will let you know once I am done with it. Ankur

 June 3, 2013, 04:10 #13 Member   ankur Join Date: May 2012 Location: India Posts: 50 Rep Power: 6 Hey tushar I am a little late for the reply. I have completed the CFd simulations of a cylinder without fins successfully. I got good results. In some time I will also simulate it with fins, hopefully It will also be done. This reply is just to let you that its done and thanks for the help. I am facing some other problem wich I am going to post today on forum. Thanks

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Ank OpenFOAM 2 February 20, 2013 23:56 are_if Main CFD Forum 0 January 30, 2012 09:22 jorien CFX 0 October 14, 2011 09:26 Stephan FLUENT 0 November 10, 2006 14:07 Ravi FLUENT 3 November 7, 2005 11:28

All times are GMT -4. The time now is 15:16.