
[Sponsors] 
April 5, 2006, 05:36 
Hi,
at present I'm try to de

#1 
New Member
Richard Larson
Join Date: Mar 2009
Posts: 4
Rep Power: 10 
Hi,
at present I'm try to develop a pressure based algorithm for compressible fluid flow. Following the state of the art for this kind of algorithm, I formulate pressure equation in term of pressure correction equation. Thus I add a convective transport term in pressure correction equation to take in account density correction at high Mach flow. Well I've several problems with boundary condition for pressure correction. For example for subsonic flow in 2D tube with inlet velocity boundary and outlet pressure boundary what kind of boundary I have to impose? I try zero gradient for pressure correction at inlet and fixed value for pressure correction at outlet but it doesn't work. For very low Mach value the algorithm works properly. Please help me! Best regards Richard Larson 

April 5, 2006, 06:23 
This is textbook stuff: you pr

#2 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,802
Rep Power: 24 
This is textbook stuff: you problem is that the correct definition of the boundary conditions changes with the Mach number.
Basics first: 1) The boundary condition on the pressure equation is the same as on the pressure, but the value of pressure correction on the fixedValue boundary is zero 2) Altogether, you have 3 boundary conditions to specify: rho (call it p), U and T 3) The method of characteristics tells you how to do it. On each boundary, figure out how many characteristics point into the domain  this is how many b.c.s you are allowed to specify. In short: supersonic inlet: 3 characteristics pointing inwards supersonic outlet: 0 characteristics going in subsonic inlet: 2 going in subsonic outlet 1 going in Thus: supersonic inlet + supersonic outlet: specify everything at the inlet subsonic inlet + supersonic outlet: not allowed (not enough b.c. can be given) supersonic inlet + subsonic outlet: not allowed (overspecified) subsonic inlet + subsonic outlet: specify U and T at the inlet and p at the outlet For you, it seems that subsonic in + subsonic out works (good); for supersonic flow throughout, specify everything at the inlet. (Can I have a piccie of the solution as a reward?) :) Enjoy, Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

April 5, 2006, 07:48 
Thanks for the answer.
I ag

#3 
New Member
Richard Larson
Join Date: Mar 2009
Posts: 4
Rep Power: 10 
Thanks for the answer.
I agree with you, I've formulated only pressure correction equation: p(N) = p(N1) + pcoor fvm::laplacian(srho*srUA, pcorr)  fvm::div(phiD,pcorr) == fvc::div(phi) where fvm::laplacian(srho*srUA, pcorr) is the same as in incompressible formulation, "phiD" is the flux "U*psi", where "U" is the velocity, "psi" is the compressibility [s^2/m^2] and "phi" is the mass flux. I'm not sure if Mach = 1 is the borderline condition for the characteristics of this equation. Can you tell me somethig about it?! Best regards Richard Larson 

April 5, 2006, 10:18 
'm not sure if Mach = 1 is the

#4  
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,802
Rep Power: 24 
Quote:
Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

April 5, 2006, 11:27 
The doubt raises since that th

#5 
New Member
Richard Larson
Join Date: Mar 2009
Posts: 4
Rep Power: 10 
The doubt raises since that the pressure correction is a "quasiphysical" quantity... I'm sorry.
Thus, what kind of boundary conditions for pressure correction do you suggest me?!? I try zerogradient at inlet velocity patch and fixedvalue 0.0 at outlet pressure. It works only for very low mach number 0.005 while for mach number 0.1 and up the calculation fails. I think that this type of boundary conditions for pressure correction are right only if the convetive term in pressure correction equation become much smaller than diffusive term. I've no idea which is the solution at the problem. The test case is a 2D duct with inlet velocity, pressure outlet and no slip wall and a inlet temperature of 300K. I really need help Best regards RL 

April 5, 2006, 14:22 
Being learner throught reading

#6 
New Member
Javier Ros
Join Date: Mar 2009
Posts: 8
Rep Power: 10 
Being learner throught reading, and not an expert in presure not in numerics, thinking at a physical level I think you are using wrong conditions.
In an incompresible flow with one inlet and one outlet, if the velocity is fixed in the inlet, the flow and therefore the presure drop gets mainly defined. Perhaps with the exception of the neighborhood of the oulet. Especifiying a zero gradient condition at outlet may be an apropiate way to have realistic fields in the mentioned neighborhood. But still presure is undetermined (only presure drop gets determined) so it seems reasonable to eliminate that undetermination througt a boundary condition at the inlet that specifies presure as a constant. So I think you have to exchaNge your presure boundary conditions at inlet and outlet. Javier Ros 

April 6, 2006, 02:18 
Just I've rereaded my post, an

#7 
New Member
Javier Ros
Join Date: Mar 2009
Posts: 8
Rep Power: 10 
Just I've rereaded my post, and I don't agree with myself.
Consider my sugestion as a different posibility. With the same reasoning it seems that the BCs that you are using are apropiate (not wrong as I have said). Javier Ros 

April 6, 2006, 03:24 
Thank you very much Javier and

#8 
New Member
Richard Larson
Join Date: Mar 2009
Posts: 4
Rep Power: 10 
Thank you very much Javier and Hrv, for your suggestions.
Perhaps the problem are not boundary conditions, but it could be the flux "phiD" in the convective term of the pressure correction equation. It has the form of Ma^2/U. It isn't a mass flux and then is not conservative, maybe this can leads problems?!? What do you think about it?!? RL 

October 30, 2008, 09:48 
Hi, Richard,
Did you figure o

#9 
Member
Ivan Lau
Join Date: Mar 2009
Location: Hong Kong
Posts: 56
Rep Power: 10 
Hi, Richard,
Did you figure out what is wrong with your problem? I have a similar problem. Please advise if you have a solution for this problem. Regards, iL 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
pressure correction  George  Main CFD Forum  2  May 21, 2005 12:47 
pressure correction and absolure pressure  George  Main CFD Forum  5  March 22, 2005 07:10 
pressure correction in fem  Oscar Link  Main CFD Forum  0  October 19, 2004 03:40 
pressure driven flow by pressure correction method  justentered  Main CFD Forum  0  December 30, 2003 00:52 
a problem about pressure correction method  tommewang  Main CFD Forum  2  May 15, 2003 21:18 