Convection-diffusion in 1D : wrong solution for a large Delta x

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

 June 4, 2010, 09:09 Convection-diffusion in 1D : wrong solution for a large Delta x #1 Senior Member   Emanuele Join Date: Mar 2009 Posts: 110 Rep Power: 10 Sponsored Links Hi, i wrote a solver to solve a convection-diffusion equation on a 1D mesh fvScalarMatrix noUEqn ( fvm::div(v,noU) == fvm::laplacian(d1,noU) ); where v is a constant value surfaceScalarField (value is 4), d1 is a constant value surfaceScalarField (value is 0.1) and noU is a volScalarField Mesh: 1 m x 1 m x 1m [10 x 1 x 1] -> Delta x = 0.1 Boundary condition : inlet: noU=0 outlet: noU=1 Using UPWIND scheme on div(v,noU) i obtain a wrong noU field : all values are negative (the only positive value remains at the outlet like boundary condition says)!! If i reduce Delta x to 0.01 i obtain a positive noU field according to analitical solution. I printed noUEqn.H() and noUEqn.A() and they are like the values manually computed with a simple spreadsheet. How can i fix it?? Why at lower resolution it gives me negative values? Thanks in advance Regards Emanuele Last edited by nuovodna; June 7, 2010 at 09:42.

 June 7, 2010, 09:45 #2 Senior Member   Emanuele Join Date: Mar 2009 Posts: 110 Rep Power: 10 If i use UPWIND scheme on div, I have this noU cell values: Code: ``` -3.41333e-07 -2.38933e-06 -1.26293e-05 -6.38293e-05 -0.000319829 -0.00159983 -0.00799983 -0.0399998 -0.2 -1``` These values are totally different from analytical solution: they should be positive

 June 18, 2010, 05:47 #3 Senior Member   Emanuele Join Date: Mar 2009 Posts: 110 Rep Power: 10 I invert the matrix manually and it returns the same negative value. Perhaps, the effect of boundary is dominant

 July 1, 2010, 13:25 #4 Senior Member     Santiago Marquez Damian Join Date: Aug 2009 Location: Santa Fe, Santa Fe, Argentina Posts: 430 Rep Power: 17 Emanuele: are you inverting the noUEqn matrix Code: ```fvScalarMatrix noUEqn ( fvm::div(v,noU) == fvm::laplacian(d1,noU) );``` inmediately after it is assembled or once solve is called?. Before calling solve noUEqn doesn't include the BC contribution. Regards. __________________ Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC) - CONICET/UNL Tel: 54-342-4511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe - Argentina. http://www.cimec.org.ar

 July 2, 2010, 05:45 #5 Senior Member   Emanuele Join Date: Mar 2009 Posts: 110 Rep Power: 10 I printed the noU values in this way fvScalarMatrix noUEqn ( fvm::div(v,noU) == fvm::laplacian(d1,noU) ); solve(noUEqn); OFstream outCellValues("outCellValues.dat"); forAll(mesh.cells(), celli) { outCellValues << mesh.C()[celli].component(0) << " " << noU[celli] << endl; }

 July 2, 2010, 11:48 Typical behaviour I guess #6 Senior Member   Antonio Martins Join Date: Mar 2009 Location: Porto, Porto, Portugal Posts: 112 Rep Power: 10 I believe you are getting the typical behaviour. If DeltaX is too high and using upwind you will get to much numerical dispersion, that disapear if you define a lower value of deltaX. Consult Versteeg for more information. Regards, Antonio Martins

 October 2, 2010, 18:47 #7 Senior Member     Santiago Marquez Damian Join Date: Aug 2009 Location: Santa Fe, Santa Fe, Argentina Posts: 430 Rep Power: 17 Emanuele, I had forgotten this thread until a few days ago when I started to have the same issues with a similar problem, I reported them into the FOAM bug tracker and in the bug section of this forum: http://www.cfd-online.com/Forums/ope...ssembling.html problems seems to be related to the way of upwind scheme is implemented in FOAM. Could post some info related to your problem, including books and papers where it is analyzed? Regards. __________________ Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC) - CONICET/UNL Tel: 54-342-4511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe - Argentina. http://www.cimec.org.ar

 October 2, 2010, 19:56 #8 Member   Ovie Doro Join Date: Jul 2009 Posts: 99 Rep Power: 10 Hi, I know this isnt related exactly to the problem in this thread, but bears some similarities nonetheless. My question is: has anyone tried to implement InterFOAM in 1-D. I am trying to simulate Stefan problems using interFoam and apparently it looks like the solution in 1-D makes no sense while 2-D formulation appears to influence the results somewhat due to the additional boundary conditions. If anyone has any ideas it would be nice. Thanks.

 October 2, 2010, 23:07 #9 Senior Member     Santiago Marquez Damian Join Date: Aug 2009 Location: Santa Fe, Santa Fe, Argentina Posts: 430 Rep Power: 17 Ovie, I've tried an 1D example of interFoam in order to study how compressive term works. It's a very interesting case because, momentum equation vanishes and only non-linear equation for phase is solved really. It allowed me to compare interFoam results with simple Matlab/Octave code. I'll be working on that again next weeks. Maybe you can start a new thread about this topic to share some results. Regards. __________________ Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC) - CONICET/UNL Tel: 54-342-4511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe - Argentina. http://www.cimec.org.ar

 October 2, 2010, 23:40 #10 Member   Ovie Doro Join Date: Jul 2009 Posts: 99 Rep Power: 10 Thanks Santiago, As it is, I wasnt sure if my point had any merit to it thats why I was reluctant to start a new thread. But on your suggestion, I might just consider doing that to see if others with similar challenges can report their findings. Thanks for your response all the same.

October 3, 2010, 00:59
#11
Member

Ovie Doro
Join Date: Jul 2009
Posts: 99
Rep Power: 10
Quote:
 Originally Posted by santiagomarquezd Ovie, I've tried an 1D example of interFoam in order to study how compressive term works. It's a very interesting case because, momentum equation vanishes and only non-linear equation for phase is solved really. It allowed me to compare interFoam results with simple Matlab/Octave code. I'll be working on that again next weeks. Maybe you can start a new thread about this topic to share some results. Regards.

But I am curious. How did you formulate the problem? I mean the mesh and what boundary conditions did you impose on patches? I have tried a simple approach of declaring only inlet and outlet patches for a 1-D rectangular block but when I run the computation, it is just completely useless results I get. So I would really like to see how you managed to pull this off...

Thanks

October 4, 2010, 05:53
one dimensional convection-diffusion results
#12
Senior Member

Emanuele
Join Date: Mar 2009
Posts: 110
Rep Power: 10
Hi Santiago, these are my results.

Equation:

fvm::div(v,U) == fvm::laplacian(d,U)

with
d= 0.001
v = 1
U(0) = 0
U(1) = 1

Four schemes combination on div :
-) Gauss linear on div + Gauss linear corrected on laplacian (in figure as CDS)
-) Gauss upwind on div + Gauss linear corrected on laplacian (UPWIND)
-) Gauss linearUpwind cellMDLimited Gauss linear 1 on div + Gauss linear corrected on laplacian (LIMITERS)
-) Gauss limitedLinear 1 on div + Gauss linear corrected on laplacian (limitedLinear)

Classified according to Peclet number:

Pe = v * Delta x / d

Regards

Emanuele
Attached Images
 Diffusione_Convezione_1D_UPWIND.png (4.2 KB, 45 views) Diffusione_Convezione_1D_linearLimited.png (4.6 KB, 42 views) Diffusione_Convezione_1D_LIMITERS.png (4.6 KB, 37 views) Diffusione_Convezione_1D_CDS.png (7.6 KB, 41 views)

Last edited by nuovodna; October 4, 2010 at 06:42. Reason: errors on schemes definition

 October 4, 2010, 07:29 What is the value of the time increment #13 Senior Member   Antonio Martins Join Date: Mar 2009 Location: Porto, Porto, Portugal Posts: 112 Rep Power: 10 Hi, What is the value of the value increment? According to the figures, it looks you have a larger courant than allowed by stability requirements. Also, try to use more precise interpolation methods, such as gamma, minmod, or SFCD. Although non limited, they are much more precise than upwind... Also, more information on this problem can be found in the book of Malaskera. Regards, António Martins

 October 4, 2010, 07:58 #14 Senior Member     Santiago Marquez Damian Join Date: Aug 2009 Location: Santa Fe, Santa Fe, Argentina Posts: 430 Rep Power: 17 Emanuele. your results seems as I expected, particularly for Central Difference and Upwind. In CD the oscillations are normal due large Pe, this scheme is unstable for Pe>1. With respect of upwind it should be stable in all range of Pe numbers, but in FOAM it is not the case due the form of divergence assembling (check the link I posted a few days ago). Respect of limited schemes I would have expected a bounded behavior but it seem to have the same problems. Could you post a paper o book in which this problem is shown? I'm searching too, but the only references I've got are for FEM. Regards. __________________ Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC) - CONICET/UNL Tel: 54-342-4511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe - Argentina. http://www.cimec.org.ar

 October 4, 2010, 08:18 expected results #15 Senior Member   Emanuele Join Date: Mar 2009 Posts: 110 Rep Power: 10 Hi Santiago, i read your bug report and my results correspond to your alert on fvm::div assembling. This problem is described here Finite Volume Method for Convection-Diffusion Problems and in famous book like Peric or Veersteg

 October 20, 2010, 13:36 #16 Senior Member     Santiago Marquez Damian Join Date: Aug 2009 Location: Santa Fe, Santa Fe, Argentina Posts: 430 Rep Power: 17 Emanuele, Professor Tung gives the right answer in slide 47 as you said, the explanation is taken from Versteeg. Thx. __________________ Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC) - CONICET/UNL Tel: 54-342-4511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe - Argentina. http://www.cimec.org.ar

 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 CFD_student Main CFD Forum 0 March 19, 2007 13:04 Suman Kumar Main CFD Forum 7 July 15, 2003 14:05 Matt Umbel Main CFD Forum 14 January 12, 2001 15:34 Z.Zeng Main CFD Forum 8 October 22, 1999 09:06 Abhijit Tilak Main CFD Forum 6 February 5, 1999 02:16

All times are GMT -4. The time now is 06:09.