
[Sponsors] 
April 17, 2010, 12:41 
OF Compressible equations SIMPLE/PISO

#1 
Member

Dear Foamers,
I am currently investigating on OF abilities with compressible flows. Basically, three cases: strictly subsonic flow (Mach .6) then shockwave (Mah .725, .75) on an airfoil. In order to choose the solver I will use, I decided to open the source code I found that OF uses PISO/SIMPLE algorithms for compressible flows! Why ? I am quite sure that PISO/SIMPLE are pressurevelocity coupling methods for incompressible flows because NS PDE system (continuity, momentum) does not include pressure equation but pressure gradient. On the contrary, for compressible flows, the NS PDE system includes continuity, momentum, energy and the coupling equation is the equation of state. So no need for pressurevelocity coupling. Can someone help me on this point ? Thanks a lot 

April 18, 2010, 03:05 

#2 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
You should refer to the literature to learn the details. A good starting point could be the book: Ferziger, Peric, Computational Methods for Fluid Dynamics, Springer. This should give you the information you're looking for.
To make it short: SIMPLE and PISO can be applied also to compressible flows, with the due changes (basically the addition of the energy equation and the incorporation of compressibility effects in the pressure equation) compared to their incompressible formulation. You might want to take a look at rhoCentralFoam and rhopSonicFoam for your cases. Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

April 19, 2010, 05:29 

#3 
Member

Thanks for your reply Alberto, I will certainly take a look at the reference.
I went on my investigations. I saw that both solvers you mentioned are Euler solvers ? I need NS Solvers beause I want to capture the boundary layer. Therefore, NS solvers adapted to aerodynamics include: rhoPimpleFoam, rhoPisoFoam, , rhoSimpleFoam, sonicFoam. Only one solver is steady, rhoSimpleFoam. When I analyze its source code, it seems that OF consider steady state as d/dt = 0. How can it be possible to solve with stability such equations ? I am thinking of pseudotransient simulations (as rhoPimple make) and CFL notions (if there is no deltaT, no CFL can be calculated ). Basically, my problems are steadystate. It would be very expensive to compute my 2D airfoil with an unsteady solver, right (of course, depending on my mesh) ? Thanks for your help, hope my question aren't too dummy 

April 19, 2010, 10:31 

#4  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Quote:
Quote:
Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

April 19, 2010, 10:49 

#5  
Member

Quote:
For sure, that confirms your reply concerning that equations are no more Euler equations but NS equations without turbulence model . Finally, none of the tutorials have turbulenceProperties file with them. Concerning rhoSimpleFoam, my computation crashes almost immediately when 'transonic' is off and waits for crash whan 'transonic' is on ... Even with underrelaxing factors, even very low ones (1e2,1e3) Let the show go on 

April 19, 2010, 11:57 

#6  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Quote:
Kurganov, A; Tadmor, E, New highresolution central schemes for nonlinear conservation laws and convectiondiffusion equations, J. Comp. Phys, Vol. 160, Issue 1, pp 241282. Quote:
Quote:
Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

April 19, 2010, 14:59 

#7 
Member

My case(s) is(are):
2D Airfoil RAE2822 Mach .75, nonzero angle of attack (when 'transonic' boolean is true, Mach .6 otherwise, Reynolds about 6M) Turbulence model: Spalart Allmaras. 

April 24, 2010, 11:33 

#8 
Member

Any idea ?
I succeeded in running my cases with sonicFoam, rhoPisoFoam and rhoPimpleFoam with their own settings. But still failed with rhoSimpleFoam. Case: Mach .6 on 2D Airfoil RAE2822 U: "freestream" inlet/outlet, "zerogradient" wall P: "freestream" inlet/outlet, "zerogradient" wall T: "freestream" inlet, "zerogradient" outlet/wall Numerical schemes: I tried different settings for every sections: Gauss linear, upwind for convection even Minmod. I stayed with Gauss linear for gradient and laplacian. Thanks for your reply 

May 14, 2010, 07:46 

#9 
Member
Florian Ettner
Join Date: Mar 2009
Location: Munich, Germany
Posts: 41
Rep Power: 9 
Alberto,
mentioning Ferziger's textbook, I suppose you were referring to the RhieChow interpolation. However, if it is true that we need this (as OpenFOAM uses collocated grids), then I don't understand why a solver like rhoSonicFoam works. Its formulation is completely density based, p is gained from the ideal gas equation, and there is no PISO loop or anything comparable. Can you enlighten me, please? 

May 14, 2010, 10:15 

#10 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Hello,
no, I was referring to pressurebased compressible algorithm they describe, in reply to the first question on the use of PISO and SIMPLE algorithms for compressible flows. You can also take a look at the paper Demirdzic, I., Lilek, Z., Peric, M., A collocated finite volume method for predicting flows at all speeds, International Journal for Numerical Methods in Fluids, Vol. 16, 1029  1050, 1993 which contains the detailed explanation of the same approach explained in the book. In a densitybased approach you clearly do not have a pressure equation, and you use directly the continuity equation for the density, relying on the equation of state to compute the pressure. Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

May 14, 2010, 10:23 

#11  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Quote:
Did you try to set pMin, rhoMin and rhoMax at appropriate values in the SIMPLE subdictionary? In general, the relaxation should not be so strong (I use: p: 0.6, U: 0.4, rho: 0.05, 0.4 for all the rest, or, alternatively p:0.3, U:0.7, but the first usually converges much faster. Of course you might need smaller values than these, but 10^3 seems too small :)). If you need that, you've probably something wrong somewhere else in the problem setup. Simply take the pimpleFoam case that converges, change name to the PIMPLE dictionary into SIMPLE, add the limitation on rho in the same dictionary, and try. Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

May 17, 2010, 09:40 

#12 
Member

Thanks Alberto, I'll do what you recommend and I'll let you know


May 17, 2010, 10:05 

#13 
Member
Florian Ettner
Join Date: Mar 2009
Location: Munich, Germany
Posts: 41
Rep Power: 9 
Thank you, Alberto, I'll have a look at the publication.


May 17, 2010, 10:34 

#14 
Member

This is what happened:
1. Following your advice for relaxation factors and keywords in the SIMPLE subdictionary, the computation crashes quite immediately. 2. When I add the 'transonic' keyword, the computation makes about 800 steps but the 'cumulative error' dramatically grows up and then the computation crashes. 3. Even with low relaxation factors. That is to say that these relaxation factors (in this case) only delay the crash. Thanks for your suggestion and the investigations go on 

May 17, 2010, 13:13 

#15 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
It looks like there is some problem in the setup, but it's hard to say without having the case :)
Good luck
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

May 18, 2010, 03:42 

#16 
Member

I tried another setup: rhoPisoFoam + local time in order to reproduce pseudotransient computations that can be found in paying CFD softs. It seems that computations run
Do you think this technique is a good alternative ? 

May 18, 2010, 09:52 

#17 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Yes. You can do pseudotransient runs with rhoPimpleFoam too, which should allow larger Co numbers, maybe with your local time stepping.
Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

May 18, 2010, 10:06 

#18 
Member

rhoPisoFoam + SLTS local time step technique works very well. But with rhoPimpleFoam, density increases dramatically (relaxation factor at .05 as you suggested) and the computation finally crashes. How many subiterations (nOuterCorrectors) do you recommend to me ?
Thanks 

May 18, 2010, 10:17 
rhoSimpleFoam

#19 
Member
Sylvain Martel
Join Date: Apr 2009
Location: University of Sherbrooke/Quebec/Canada
Posts: 51
Rep Power: 9 
Hi, in previous post, you said:
"Concerning rhoSimpleFoam, my computation crashes almost immediately when 'transonic' is off and waits for crash whan 'transonic' is on ... Even with underrelaxing factors, even very low ones (1e2,1e3)" Do you have to define transonic "on" or "off" condition? I would like to switch from OF 1.5 to 1.6 to try solving steadystate critical flow in a nozzle. Have you progressed with this task? Sylvain 

May 18, 2010, 10:40 

#20 
Member

Basically, this option appears in the source code of the solvers (rhoSimple, rhoPimple or rhoPiso) [transonic is actually a boolean and its default value is false]. After reading the source code and a post on CFDOnline (Question about rhoSimpleFoam "if (transonic)"), I tried. For the moment, I did not succeed in using this option. All my successful computations ran with transonic as false.


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Guide: Writing Equations in LaTeX on the CFD Online Forums  pete  Site Help, Feedback & Discussions  20  June 16, 2015 13:52 
Grid generation and Compressible Euler equations  oe  Main CFD Forum  7  September 8, 2008 21:28 
trying to solve 2d compressible euler equations  dave  Main CFD Forum  4  July 16, 2003 09:08 
NavierStokes equations in compressible flow  GACEM Hatem  Phoenics  1  June 3, 2001 05:30 
3d discretisation of compressible NS equations  sanku  Main CFD Forum  1  January 30, 2000 22:01 