CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Is OpenFoam really reliable? It is Urgent!!!

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

Like Tree2Likes
  • 1 Post By tomf
  • 1 Post By alberto

Reply
 
LinkBack Thread Tools Display Modes
Old   October 31, 2011, 13:10
Exclamation Is OpenFoam really reliable? It is Urgent!!!
  #1
New Member
 
Min Thaw Tun
Join Date: Mar 2011
Location: Kaluga, Russia
Posts: 19
Rep Power: 6
Technoyoungman is on a distinguished road
Send a message via Yahoo to Technoyoungman
Hi Dear Foamers!!
I've found some strange behaviors of OpenFoam simulation. I'm now very confused. Is OpenFoam really reliable? Well I will tell what I found out. When I run the tutorial case "Wedge15M5"in the rhoCentralFoam, the result of pressure, temperature and velocity seems very satisfactory. You can look details in the master thesis dissertation "Simulation and validation of compressible flow in nozzle geometries and validation of OpenFOAM for this application" by Benjamin Wuthrich. But these results are only static parameters. We must check the total (stagnation) parameters.
According to the normal shock wave and oblique shock wave theory, the stagnation pressure must drop after shock. But OpenFoam gives the fault result. You can see them in the attachments. I made no modification to the tutorial. So the result should be reliable. As u can see in the attachment, stagnation pressure rises dramatically after shock. Even there are slight total temperature rises.
T*=T+U^2/(2*Cp);

So Dear Foamers, if I made mistake, please tell me what should I do. I want to hear your advices or discussions or any suggestion. Please!! I think that it is important for all of the foamers.

PS: I can't calculate the total pressure and temperature according to compressible equation due to very high value of lambda (velocity/critical speed).
P/P*=(1-(k-1)/(k+1)*lambda^2)^(k/k-1) ----------- k= gamma = 1.4
U can also check other solver, rhopSonicFoam

static_p.jpg

vel.jpg

ptot.jpg

Ma.jpg

Stag_T.jpg

REF: Normal Shock Wave by NASA
" For compressible flows with little or small flow turning, the flow process is reversible and the entropy is constant. The change in flow properties are then given by the isentropic relations (isentropic means "constant entropy"). But when an object moves faster than the speed of sound, and there is an abrupt decrease in the flow area, the flow process is irreversible and the entropy increases. Shock waves are generated which are very small regions in the gas where the gas properties change by a large amount. Across a shock wave, the static pressure, temperature, and gas density increases almost instantaneously. Because a shock wave does no work, and there is no heat addition, the total enthalpy and the total temperature are constant. But because the flow is non-isentropic, the total pressure downstream of the shock is always less than the total pressure upstream of the shock; there is a loss of total pressure associated with a shock wave. The ratio of the total pressure is shown on the slide. Because total pressure changes across the shock, we can not use the usual (incompressible) form of Bernoulli's equation across the shock. The Mach number and speed of the flow also decrease across a shock wave. "

Last edited by Technoyoungman; October 31, 2011 at 13:29.
Technoyoungman is offline   Reply With Quote

Old   November 2, 2011, 06:13
Default
  #2
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Delft, Netherlands
Posts: 226
Rep Power: 10
tomf is on a distinguished road
Send a message via MSN to tomf Send a message via Skype™ to tomf
Dear Min Thaw Tun,

I have seen a similar behavior when investigating a converging-diverging channel. Either in an expansion fan or across a shock the total temperature varied. Also the total pressure behavior was incorrect although the static pressure and temperature, velocity, density and Mach number showed correct behavior (qualitatively at least). I have tried many different schemes, meshes, turbulence models.

So unfortunately I can not help you, just confirm that I have spotted the same behavior and still interested if someone has performed a correct simulation.

Kind regards,
Tom
Technoyoungman likes this.
tomf is offline   Reply With Quote

Old   November 2, 2011, 06:26
Arrow
  #3
New Member
 
Min Thaw Tun
Join Date: Mar 2011
Location: Kaluga, Russia
Posts: 19
Rep Power: 6
Technoyoungman is on a distinguished road
Send a message via Yahoo to Technoyoungman
Quote:
Originally Posted by tomf View Post
Dear Min Thaw Tun,

I have seen a similar behavior when investigating a converging-diverging channel. Either in an expansion fan or across a shock the total temperature varied. Also the total pressure behavior was incorrect although the static pressure and temperature, velocity, density and Mach number showed correct behavior (qualitatively at least). I have tried many different schemes, meshes, turbulence models.

So unfortunately I can not help you, just confirm that I have spotted the same behavior and still interested if someone has performed a correct simulation.

Kind regards,
Tom

Dear Tom,
Thanks you for ur reply. I've been longing for a response. Actually I'm going to submit a term paper with OpenFoam. I would like to check the total pressure loss from shock wave and compare with theory. Because of this reult I don't know what to do. It shouldn't be like this because this is the very basic of supersonic flow. OpenCFD should take responsibility for these. I'm just thinking.
Technoyoungman is offline   Reply With Quote

Old   November 3, 2011, 02:14
Default
  #4
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Did you take a look at the literature (Kurganov and Tadmor schemes) and at the paper where the solver was described?

Also, if you can provide a small case reproducing the problem, you can report the problem to the developers, if you believe it is a bug and it does not depend on your setup.

P.S. Adding "Urgent" to a title of a post is an invitation *not* to read it. ;-)
Technoyoungman likes this.
__________________
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 open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   November 3, 2011, 06:56
Default
  #5
ndr
New Member
 
Join Date: Aug 2009
Location: Stuttgart, Germany
Posts: 20
Rep Power: 8
ndr is on a distinguished road
Hi,

as posted already within the other thread at No shock in airfoil 0012 case despite of Mach number exceeds 1: I don't know how you calculated your total pressure, but when I use the isentropic equation

p_{tot}=p\cdot(1+\frac{\gamma-1}{2}Ma^{2})^{\frac{\gamma}{(\gamma-1)}}

I obtain different results. A contour plot is attached to this post and when compared to the analytical solution it looks quite reasonable.
I did a quick calculation and if I didn't miss something the analytical solution gives a Mach number behind the shock of around 3.65 (approx. 3.6 in the OF solution). The total pressure ratio p_{t,1}/p_{t,0} should be slightly above 0.6 and OF delivers approx. 0.66.

So unless I miscalculated the analytical part maybe you could check your total pressure calculation, I'm not sure if this is really an issue of OpenFoam.

Regards

Nils
Attached Images
File Type: jpg Wedge.jpg (16.9 KB, 70 views)

Last edited by ndr; November 3, 2011 at 09:43.
ndr is offline   Reply With Quote

Old   November 5, 2011, 04:24
Default sonicFoam
  #6
Member
 
Join Date: May 2009
Posts: 31
Rep Power: 8
KrisT is on a distinguished road
The tutorial case

compressible/sonicFoam/laminar/shockTube

also give erroneous results (at least up to 1.6). Speed of shock is wrong. Maybe scheme is not conservative?

IF it has not been fixed in later versions it would be better to remove that particular tutorial case.

To my experience rhoCentralFoam gives the expected results.
KrisT is offline   Reply With Quote

Old   November 5, 2011, 13:31
Default
  #7
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Hi,

1) The validation of the procedure is published: C. J. Greenshields, H. G. Weller, L. Gasparini, J. M. Reese, Implementation of semi-discrete, non-staggered central schemes in a colocated, polyhedral, finite volume framework, for high-speed viscous flows, Int. J. Numer. Meth. Fluids 2010; 63:121, 2009, DOI: 10.1002/fld.2069.

2) The original description of the schemes can be fouind here: A. Kurganov, E. Tadmor, New High-Resolution Central Schemes for Nonlinear Conservation Laws and Convection-Diffusion Equations, J. Comp. Phys., 160, 214282, 2000.

3) If you think it is a bug, report it in detail on mantis, describing step-by-step how you perform your calculation.

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 open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   November 9, 2011, 15:00
Talking Thanks u all
  #8
New Member
 
Min Thaw Tun
Join Date: Mar 2011
Location: Kaluga, Russia
Posts: 19
Rep Power: 6
Technoyoungman is on a distinguished road
Send a message via Yahoo to Technoyoungman
Hi Dear Foamers!!
Thank u for all ur discussion.
I've checked the stagnation pressure. Now I didn't use ptot postprocessor utility.
I used the stagnation pressure equation
p_{tot}=p\cdot(1+\frac{\gamma-1}{2}Ma^{2})^{\frac{\gamma}{(\gamma-1)}}

p_stag1.jpg
rhoCentralFoam (tutorial)


p_stag2.jpg
rhoPsonicFoam (tutorial)


p_stag.jpg
rhoPsonicFoam (with 100 kPa, 1735m/c (M=5), 300K)
Tutorial are normal. Do me a favor . Well I will post my problem in next thread.
Technoyoungman is offline   Reply With Quote

Old   November 9, 2011, 23:41
Default
  #9
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
What next thread?
__________________
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 open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Reply

Tags
openfoam, shock wave, total pressure

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
Superlinear speedup in OpenFOAM 13 msrinath80 OpenFOAM Running, Solving & CFD 18 March 3, 2015 06:36
New OpenFOAM Forum Structure jola OpenFOAM 2 October 19, 2011 06:55
Cross-compiling OpenFOAM 1.7.0 on Linux for Windows 32 and 64bits with Mingw-w64 wyldckat OpenFOAM Announcements from Other Sources 3 September 8, 2010 06:25
Modified OpenFOAM Forum Structure and New Mailing-List pete Site News & Announcements 0 June 29, 2009 05:56
Adventure of fisrst openfoam installation on Ubuntu 710 jussi OpenFOAM Installation 0 April 24, 2008 14:25


All times are GMT -4. The time now is 04:08.