Is OpenFoam really reliable? It is Urgent!!!
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.
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
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. "
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.
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.
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. ;-)
as posted already within the other thread at http://www.cfd-online.com/Forums/ope...tml#post329361: I don't know how you calculated your total pressure, but when I use the isentropic equation
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 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.
The tutorial case
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.
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; 63:1–21, 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, 214–282, 2000.
3) If you think it is a bug, report it in detail on mantis, describing step-by-step how you perform your calculation.
Thanks u all
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
What next thread? :)
|All times are GMT -4. The time now is 01:24.|