for compressible flows, how to set stagnation pressure boundary conditions?

As stated in the library case of no. 234:

** The prescription of the stagnation pressure at the nozzle inlet is obtained from the following relationship between the stagnation pressure and the inlet values of Mach number and density: p0=rhoin*[1+0.5*(gamma-1)*Min**2]**[gamma/(gamma-1)]. When the inlet mass-flow per unit area is made the subject of this equation, the familiar co & val form results:

rhoin*uin=co*(val-pP), where,

co=2*gamma/[uin*(gamma-1)], val=p0*rhoin/rho0.

For this case, the inlet velocity which appears in co ie. uin is assumed known. Strictly speaking this quantity is a function of the calculation, and should hence be re-calculated in GROUND as the calculation ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~ ~~ proceeds.

can anyone tell me how to calculate it in ground??

A commonly-used approximation is to use val=SAME for the velocity in the COVAL statement, which means that the in-cell velocity will be used for the incoming velocity.

Strictly, you will have to set VAL=GRND for the velocity, and then compute VAL in group 13 section 12 of ground.for from continuity. It will probably be necessary to relax the inlet velocity so as to maintain numerical stability.

Thanks for your help.

your know when set the stagnation pressure boundary condition, one should set the Co of pressure to negative value of flow density, and in the FAQ, it told me that the Co of pressure can't be set to access the ground.for, so how to set the Co of pressure,when the inlet density isn't constant (beacuse of the temperature at the inlet isn't constant).

another question is how to set the inlet boundary conditions when the inlet static pressure is lower than the ambient static pressure. this question is commonly encountered when you do some simulation of overexpanded jet.

can you tell me more detail about the stagnation pressure conditions.

The -ve coefficient is a flag for phoenics to apply a stagnation condition for incompressible flow. The option is not relevant for compressible flow.

For inlet conditions, etc, it is best to look at library cases n111, n112 (transonic flow in a nozzle) and n113 (underexpanded free jet). These and other cases using PHOENICS, including an overexpanded free jet, were reported in the following papers:

Palacio A, Malin MR, Proumen N & Sanchez L Numerical computations of steady transonic and supersonic flow fields International Journal of Heat Mass Transfer, Vol. 33, No 6, pp 1193-1204, 1990. (CHAM Ref 90/25 )

Palacio A, Malin MR, Proumen N & Sanchez L Flowfield predictions of transonic and supersonic problems Proceedings of the 3rd PHOENICS User Conference-Dubrovnk. The PHOENICS Journal of Computational Fluid Dynamics and Its Applications Vol. 2, No 2, pp 202-218 1989. Published by CHAM 1989 (CHAM Ref 89/29).

Further advice can be obtained from your local agent CHAM Shanghai (email: phoenics@public8.sta.net.cn). The contact name is Dr JinLong Fan.

thanks for you help.

but I can't get the correct shock structure yet. the numerical dissipation seems too strong, and results show the first shock wave (mach disc) is obvoius, but the following shock is too small and the number of the shock is only three. I had used the high-order scheme and results is similar. the difference is that the strength of the first shock is enhanced.

I had seen the same problem handled by FLUENT software, it is clearly different from my results which were got by the PHOENICS whether Is it software problem or did I handle it incorrect? I really don't know why?

my problem is as following: A supersonic argon plasma jet discharge into low-pressure environment, the inlet static pressure, velocity, and temperature are given. the plasma properties are dependent on the pressure and temperature. the static pressure is about 48Kpa, and the ambient pressure is 10Kpa, so the plasma jet is underexpanded. the LTE model is used in this step, next step I want to use the non-LTE model to handle it.

I really need your help to overcome the obstacle, if not, i can't carry out the following work.

thanks advance.

hi, I think the idea of using stagnation pressure for capturing shock isnt good. Why not use mass flow inlet and pressure outlet but the problem that i am facing in fluent is that it modifies the boundary condition itself and not showing any pressure rise as much as wanted.. How come it is modifying the boundary condition it must be rigid on that part by incorporating some shock.. Acoording to mine predigament theres shud be shock and its reflection in a supersonic shock duct flow..

kamlesh