CFD Online URL
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

OF Compressible equations SIMPLE/PISO

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   April 17, 2010, 13:41
Default OF Compressible equations SIMPLE/PISO
  #1
Member
 
Ngoc-Minh Truong
Join Date: Feb 2010
Location: Toulouse, France
Posts: 42
Rep Power: 6
truong_nm is on a distinguished road
Send a message via MSN to truong_nm
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 pressure-velocity 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 pressure-velocity coupling.
Can someone help me on this point ?
Thanks a lot
truong_nm is offline   Reply With Quote

Old   April 18, 2010, 04:05
Default
  #2
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,890
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
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,
mm.abdollahzadeh likes this.
__________________
Alberto

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.
GeekoCFD 32bit - The 32bit edition of GeekoCFD.
GeekoCFD text mode - A smaller version of GeekoCFD, text-mode only, with only OpenFOAM. Available in a variety of virtual formats.
alberto is offline   Reply With Quote

Old   April 19, 2010, 06:29
Default
  #3
Member
 
Ngoc-Minh Truong
Join Date: Feb 2010
Location: Toulouse, France
Posts: 42
Rep Power: 6
truong_nm is on a distinguished road
Send a message via MSN to truong_nm
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 pseudo-transient simulations (as rhoPimple make) and CFL notions (if there is no deltaT, no CFL can be calculated ).
Basically, my problems are steady-state. 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
truong_nm is offline   Reply With Quote

Old   April 19, 2010, 11:31
Default
  #4
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,890
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by truong_nm View Post
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.
rhoCentralFoam is also for viscous flows (I'm looking at 1.6.x). See the "if (!inviscid) ...".

Quote:
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 pseudo-transient simulations (as rhoPimple make) and CFL notions (if there is no deltaT, no CFL can be calculated ).
simpleFoam uses the SIMPLE algorithm, under-relaxing the solution.

Best,
__________________
Alberto

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.
GeekoCFD 32bit - The 32bit edition of GeekoCFD.
GeekoCFD text mode - A smaller version of GeekoCFD, text-mode only, with only OpenFOAM. Available in a variety of virtual formats.
alberto is offline   Reply With Quote

Old   April 19, 2010, 11:49
Default
  #5
Member
 
Ngoc-Minh Truong
Join Date: Feb 2010
Location: Toulouse, France
Posts: 42
Rep Power: 6
truong_nm is on a distinguished road
Send a message via MSN to truong_nm
Quote:
Originally Posted by alberto View Post
rhoCentralFoam is also for viscous flows (I'm looking at 1.6.x). See the "if (!inviscid) ...".

simpleFoam uses the SIMPLE algorithm, under-relaxing the solution.

Best,
Well, thanks for your reply. I took a look at the code for rhoCentralFoam. To me, Kurganov and Tadmor are designed for hyperpolic equations, i.e. Euler equations. Moreover, when I read the code, there is indeed "if (!inviscid)" but after that, no 'turbulence -> correct()' term.
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 under-relaxing factors, even very low ones (1e-2,1e-3)

Let the show go on
truong_nm is offline   Reply With Quote

Old   April 19, 2010, 12:57
Default
  #6
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,890
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by truong_nm View Post
Well, thanks for your reply. I took a look at the code for rhoCentralFoam. To me, Kurganov and Tadmor are designed for hyperpolic equations, i.e. Euler equations.
Turganov and Tadmor schemes are basically Riemann-free schemes were developed also for convection-diffusion equations

Kurganov, A; Tadmor, E, New high-resolution central schemes for nonlinear conservation laws and convection-diffusion equations, J. Comp. Phys, Vol. 160, Issue 1, pp 241-282.
Quote:
Moreover, when I read the code, there is indeed "if (!inviscid)" but after that, no 'turbulence -> correct()' term.
For sure, that confirms your reply concerning that equations are no more Euler equations but NS equations without turbulence model .
Yes. rhoCentralFoam solves the N-S equations without turbulence model.

Quote:
Concerning rhoSimpleFoam, my computation crashes almost immediately when 'transonic' is off and waits for crash whan 'transonic' is on ... Even with under-relaxing factors, even very low ones (1e-2,1e-3)
What case? Flow conditions? Solver configuration?

Best,
__________________
Alberto

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.
GeekoCFD 32bit - The 32bit edition of GeekoCFD.
GeekoCFD text mode - A smaller version of GeekoCFD, text-mode only, with only OpenFOAM. Available in a variety of virtual formats.
alberto is offline   Reply With Quote

Old   April 19, 2010, 15:59
Default
  #7
Member
 
Ngoc-Minh Truong
Join Date: Feb 2010
Location: Toulouse, France
Posts: 42
Rep Power: 6
truong_nm is on a distinguished road
Send a message via MSN to truong_nm
My case(s) is(are):

2D Airfoil RAE2822 Mach .75, non-zero angle of attack (when 'transonic' boolean is true, Mach .6 otherwise, Reynolds about 6M)
Turbulence model: Spalart Allmaras.
truong_nm is offline   Reply With Quote

Old   April 24, 2010, 12:33
Default
  #8
Member
 
Ngoc-Minh Truong
Join Date: Feb 2010
Location: Toulouse, France
Posts: 42
Rep Power: 6
truong_nm is on a distinguished road
Send a message via MSN to truong_nm
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
truong_nm is offline   Reply With Quote

Old   May 14, 2010, 08:46
Default
  #9
Member
 
Florian Ettner
Join Date: Mar 2009
Location: Munich, Germany
Posts: 40
Rep Power: 7
dohnie is on a distinguished road
Alberto,
mentioning Ferziger's textbook, I suppose you were referring to the Rhie-Chow 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?
dohnie is offline   Reply With Quote

Old   May 14, 2010, 11:15
Default
  #10
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,890
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
Hello,
no, I was referring to pressure-based 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 density-based 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

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.
GeekoCFD 32bit - The 32bit edition of GeekoCFD.
GeekoCFD text mode - A smaller version of GeekoCFD, text-mode only, with only OpenFOAM. Available in a variety of virtual formats.
alberto is offline   Reply With Quote

Old   May 14, 2010, 11:23
Default
  #11
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,890
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by truong_nm View Post
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
Technically if rhoPisoFoam converges, rhoSimpleFoam should too. Usually in steady simulations what might kill your run are the first iterations, because the solution can change very steeply.

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

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.
GeekoCFD 32bit - The 32bit edition of GeekoCFD.
GeekoCFD text mode - A smaller version of GeekoCFD, text-mode only, with only OpenFOAM. Available in a variety of virtual formats.
alberto is offline   Reply With Quote

Old   May 17, 2010, 10:40
Default
  #12
Member
 
Ngoc-Minh Truong
Join Date: Feb 2010
Location: Toulouse, France
Posts: 42
Rep Power: 6
truong_nm is on a distinguished road
Send a message via MSN to truong_nm
Thanks Alberto, I'll do what you recommend and I'll let you know
truong_nm is offline   Reply With Quote

Old   May 17, 2010, 11:05
Default
  #13
Member
 
Florian Ettner
Join Date: Mar 2009
Location: Munich, Germany
Posts: 40
Rep Power: 7
dohnie is on a distinguished road
Thank you, Alberto, I'll have a look at the publication.
dohnie is offline   Reply With Quote

Old   May 17, 2010, 11:34
Default
  #14
Member
 
Ngoc-Minh Truong
Join Date: Feb 2010
Location: Toulouse, France
Posts: 42
Rep Power: 6
truong_nm is on a distinguished road
Send a message via MSN to truong_nm
This is what happened:
1. Following your advice for relaxation factors and keywords in the SIMPLE sub-dictionary, 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
truong_nm is offline   Reply With Quote

Old   May 17, 2010, 14:13
Default
  #15
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,890
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
It looks like there is some problem in the setup, but it's hard to say without having the case :-)

Good luck
__________________
Alberto

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.
GeekoCFD 32bit - The 32bit edition of GeekoCFD.
GeekoCFD text mode - A smaller version of GeekoCFD, text-mode only, with only OpenFOAM. Available in a variety of virtual formats.
alberto is offline   Reply With Quote

Old   May 18, 2010, 04:42
Default
  #16
Member
 
Ngoc-Minh Truong
Join Date: Feb 2010
Location: Toulouse, France
Posts: 42
Rep Power: 6
truong_nm is on a distinguished road
Send a message via MSN to truong_nm
I tried another setup: rhoPisoFoam + local time in order to reproduce pseudo-transient computations that can be found in paying CFD softs. It seems that computations run
Do you think this technique is a good alternative ?
truong_nm is offline   Reply With Quote

Old   May 18, 2010, 10:52
Default
  #17
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,890
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
Yes. You can do pseudo-transient runs with rhoPimpleFoam too, which should allow larger Co numbers, maybe with your local time stepping.

Best,
__________________
Alberto

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.
GeekoCFD 32bit - The 32bit edition of GeekoCFD.
GeekoCFD text mode - A smaller version of GeekoCFD, text-mode only, with only OpenFOAM. Available in a variety of virtual formats.
alberto is offline   Reply With Quote

Old   May 18, 2010, 11:06
Default
  #18
Member
 
Ngoc-Minh Truong
Join Date: Feb 2010
Location: Toulouse, France
Posts: 42
Rep Power: 6
truong_nm is on a distinguished road
Send a message via MSN to truong_nm
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 sub-iterations (nOuterCorrectors) do you recommend to me ?

Thanks
truong_nm is offline   Reply With Quote

Old   May 18, 2010, 11:17
Default rhoSimpleFoam
  #19
Member
 
Sylvain Martel
Join Date: Apr 2009
Location: University of Sherbrooke/Quebec/Canada
Posts: 51
Rep Power: 7
smart is on a distinguished road
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 under-relaxing factors, even very low ones (1e-2,1e-3)"

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 steady-state critical flow in a nozzle.

Have you progressed with this task?

Sylvain
smart is offline   Reply With Quote

Old   May 18, 2010, 11:40
Default
  #20
Member
 
Ngoc-Minh Truong
Join Date: Feb 2010
Location: Toulouse, France
Posts: 42
Rep Power: 6
truong_nm is on a distinguished road
Send a message via MSN to truong_nm
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.
truong_nm is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Guide: Writing Equations in LaTeX on the CFD Online Forums pete Site Help, Feedback & Discussions 13 December 9, 2014 07:38
Grid generation and Compressible Euler equations oe Main CFD Forum 7 September 8, 2008 22:28
trying to solve 2d compressible euler equations dave Main CFD Forum 4 July 16, 2003 10:08
Navier-Stokes equations in compressible flow GACEM Hatem Phoenics 1 June 3, 2001 06:30
3d discretisation of compressible NS equations sanku Main CFD Forum 1 January 30, 2000 22:01


All times are GMT -4. The time now is 20:56.