
[Sponsors] 
December 20, 2010, 08:12 

#81 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21 
Why don't you just write a direction mixed boundary condition which has got a separate refValue, refGrad and valueFraction for the convection and diffusion part? Each operator does its own matrix assembly anyway and you have 4 separate functions for the coefficient:
virtual tmp<Field<Type> > valueInternalCoeffs virtual tmp<Field<Type> > valueBoundaryCoeffs virtual tmp<Field<Type> > gradientInternalCoeffs() const virtual tmp<Field<Type> > gradientBoundaryCoeffs() const Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

December 20, 2010, 09:29 

#82 
Member
George Pichurov
Join Date: Jul 2010
Posts: 39
Rep Power: 6 
Thanks Santiago for the help. I have a debugger, I only need to figure out where to supply the above commands.
Thanks Hrv for your help too, I have to figure out for myself the meaning of this . Could anybody please provide little more info on how to use the lines suggested by hrv? These are virtual templated functions? Lets say I have a patch called "outlet" and a variable called LMA. What should I do to enquire the coefficients (and possibly change them) in the near outlet cells of the variable LMA? Anybody ? Last edited by jorkolino; December 21, 2010 at 11:40. 

December 20, 2010, 13:44 

#83  
Member
George Pichurov
Join Date: Jul 2010
Posts: 39
Rep Power: 6 
Quote:
What is the correct precedence in the code (cause I've seen it both ways): first solve then relax or vice versa? I noticed relaxation factor of unity has huge impact on results when linear div scheme is used, in comparison to when no relaxation is used. I would expect relaxation factor of 1 to have no impact on the solution. That happens to a well defined parameter: fixed inlet value and zerogradient outlet value in 1D. It is almost certain that there is a problem with Foam not only with certain BC, but also with the precedence of relaxation. URF of 1 should not change the behavior at all. Last edited by jorkolino; December 21, 2010 at 03:53. 

December 21, 2010, 14:24 

#84 
New Member
David Huckaby
Join Date: Jul 2009
Posts: 21
Rep Power: 7 
George,
from your discussion, its seems for your equation you are trying to advect information from the outlet into the domain using the negative of the velocity. As such it would seem that you would want to use "phi" within your divergence operator, e.g. div(phi, LMRA). Dave 

December 21, 2010, 15:58 

#85  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26 
Quote:
yourEqn = ...; yourEqn.relax(); yourEqn.solve(); If you see the relax() method applied to a field (like p in simple algorithm), you are explicitly relaxing the variable. You typically relax the equation before solving the equation. In the SIMPLE algorithm, you explicitly relax the pressure after the solution of the pressure equation and the flux correction, but before the velocity correction. Quote:
What you see is due to something else (can your solution converge with URF = 1?) About the directioMixed BC, it is basically an extended Robin condition (a*U + b*dU = c), which allows you to specify a different "fraction" of fixedGradient / fixedValue in each direction (Sorry for the horrible wording ). There are a couple of BC's to look at, which are derived from the directionMixed BC:  outletStabilised, which applies upwind differencing to outlets  pressureInletOutletVelocity (see header for description) Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image. OpenQBMM  An opensource implementation of quadraturebased moment methods Last edited by alberto; December 21, 2010 at 15:59. Reason: clarified 

December 22, 2010, 05:46 

#86  
Member
George Pichurov
Join Date: Jul 2010
Posts: 39
Rep Power: 6 
Quote:
I appreciate your help. If you could please briefly outline the steps I need to follow. I imagine it should be like this: 1. First I define a new class inheriting from fvFixedValuePatch, similar to the example oscillatingFixedValueFvPatchField.H (http://foam.sourceforge.net/doc/Doxy...8H_source.html). 2. Then I need to define my inlets(outlets) in the dictionary file to reflect this new BC. 3. I should print(and modify later on) the 4 contributions to the coefficients using the 4 functions above. Is it correct? Thanks for your help. 

December 22, 2010, 05:59 

#87 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21 
Nope, but you are on the right track. Shall we make a deal  I will help you do this and we'll then include it into Extend?
This is what you do:  take a mixed condition and make a new one, call it doubleMixed or valueGradMixed. Be creative with the name, I don't mind  we need two copies of: // Value field Field<Type> refValue_; // Normal gradient field Field<Type> refGrad_; // Fraction (01) of value used for boundary condition scalarField valueFraction_; You can call them valueRefValue valueRefGrad valueValueFraction gradientRefValue gradientRefGrad gradientValueFraction  pull them through constructors, mapping, access functions, autoMap and rMap,  we have 2 functions which become a BIG problem; we will leave them for later. They are: snGrad() and evaluate(). For the moment, use the value entries and we'll figure them out later. Now you have 4 "impact" functions: // Return the matrix diagonal coefficients corresponding to the // evaluation of the value of this patchField with given weights virtual tmp<Field<Type> > valueInternalCoeffs ( const tmp<scalarField>& ) const; // Return the matrix source coefficients corresponding to the // evaluation of the value of this patchField with given weights virtual tmp<Field<Type> > valueBoundaryCoeffs ( const tmp<scalarField>& ) const; AND // Return the matrix diagonal coefficients corresponding to the // evaluation of the gradient of this patchField virtual tmp<Field<Type> > gradientInternalCoeffs() const; // Return the matrix source coefficients corresponding to the // evaluation of the gradient of this patchField virtual tmp<Field<Type> > gradientBoundaryCoeffs() const; In the valueInternalCoeffs and valueBoundaryCoeffs you will use the valueRefValue valueRefGrad valueValueFraction and in gradientInternalCoeffs() and gradientBoundaryCoeffs() you will use the gradientRefValue gradientRefGrad gradientValueFraction. The formulae are the same, it's just that in the value and gradient entries you allow a separate mix of fixedValue to fixedGradient, because you have 6 controls now. I think you've now got the drift; it remains to sort out the snGrad and evaluate, but I guess the genii who claim this is physical behaviour will tell me what to do. Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

December 22, 2010, 06:19 

#88  
Member
George Pichurov
Join Date: Jul 2010
Posts: 39
Rep Power: 6 
Quote:
I calculate a SS problem on a transient solver (scalarTransportFoam) with ddt set to SteadyState. It converges on several time steps rather slowly with URF=1, because it does a single iteration per time step on the calculated variable. Instead I would expect it to iterate until the final solution is reached on the first time step. Maybe I have to use explicit relaxation here. Thanks, I think I can make use of the first one. But I still need a method to remove the diffusive part at inlets for my second parameter, so I need to search for way to do that.I have asked two posts above wether my suggestion is correct. 

December 22, 2010, 10:08 

#89  
Member
George Pichurov
Join Date: Jul 2010
Posts: 39
Rep Power: 6 
Quote:
Quote:
l attach the header and source files, together with Make files to create a libraby. Now everything compiles well. I've used dummy expressions in the snGrad and evaluate functions, just to pass the compile stage. I still need your help on how to split the effect of value and grad in those functions. Last edited by jorkolino; December 28, 2010 at 04:26. 

December 22, 2010, 12:11 

#90  
Member
George Pichurov
Join Date: Jul 2010
Posts: 39
Rep Power: 6 
Quote:
thanks for reply. Mathematically the expression above seems to me equivalent to div(phi,LMRA), which is originally used. But I may try your suggestion anyway. The big problem now is how to set up B.C. such that to ensure stable matrix, and also how to disable diffusive contribution at inlets when using fixedValue B.C at inlets. Regards 

December 27, 2010, 13:54 

#91 
Member
George Pichurov
Join Date: Jul 2010
Posts: 39
Rep Power: 6 
Hi there,
I am posting the boundary condition which uses upstream value for the representation of the convection term. I have tested it for upwind scheme and can confirm that solution stays bounded for any value of Peclet. On the contrary, the basic fixedValue B.C. oscillated under same conditions when Pe>2. The problem that I solve requires that the outlet value is fixed, but the inlet is unknown. When using zeroGradient for inlet I have problems with both the standard fixedValue and the atttached B.C. They create instability in case when source terms are present. So, I was thinking on the following. After integration of the PDE for the last cell, there is no mathematical restriction on how many B.C will be defined for that last cell. In other words, I can apply fixed value and fixed gradient on the resulting integral equation, thus creating two discrete equations. So, why not generate two equations for the nearboundary cell, and skip an equation for the, lets say, the first cell? The matrix will be solvable, and the values in all cells will emerge as far as No of equations is equal to No of cells. Any ideas how can this be done with OF? Last edited by jorkolino; January 19, 2011 at 04:50. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Warning: Dynamic zone with wrong CG using 6DOF  Manoj Kumar  FLUENT  1  August 11, 2012 04:03 
BuoyantBoussinesqSimpleFoam and axialsymmetric results wrong mass flow  Thomas Baumann  OpenFOAM  6  December 21, 2009 11:31 
udf error  srihari  FLUENT  0  February 9, 2009 10:00 
Pressure contour seems wrong???  Harry Qiu  FLUENT  1  June 29, 2001 05:53 
What's wrong with my UDF?  olivia  FLUENT  1  June 23, 2001 17:06 