CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM (
-   -   Help needed in specifying BC for superconic intake simulation (

mecbe2002 October 25, 2012 07:21

Help needed in specifying BC for superconic intake simulation
1 Attachment(s)
Hi all,

I am trying to simulate an axi-symmetric ramjet intake. Plz find the geometry & BC in the attached image.

I am specifying
  1. Velocity, static pressure & static pressure for the inlet
  2. static pressure at the outlet
  3. slip for the wall - since i am doing inviscid flow simulation
  4. inletOutlet for the freestream boundary

i am using rhoCentralFoam solver.
I ran the simulation for few time steps and then calculated the "Total pressure" using "ptot" utility at the inlet, but its not matching with the inlet condition. But the Mach number is matching. How?

i.e. @ Inlet specified
static P = 28,562 Pa
static T = 153.81 K
velocity = 542 m/s
(The above values are calculated using isentropic relations)

calculated Total Pressure = 123,343 Pa, but actual value is 296,000 Pa. But the Mach number is matching 2.18


kmooney October 25, 2012 12:13

Is it possible that specifying both a pressure drop and velocity inlet boundary condition is over specifying the problem? Maybe try just the pressure drop and see what U field evolves to meet it. I'm no expert in compressible flows so I may be way off on this.

cnsidero October 25, 2012 16:08

For supersonic flows you specify all values at inlet and no values at outlet. You can refer to one of the many compressible flow CFD books that show this to be true by examining the characteristic wave propagation.

For subsonic flows you specify all values but one and at the outlet only one value. This is why it is quite common for subsonic flows to specify all the velocity components (or velocity magnitude and direction, which is the same thing) but not pressure at the inlet and only pressure at the outlet.


mecbe2002 October 25, 2012 23:45

I figured out the problem.

The "ptot" utility is using Bernoulli's equation to calculate the total pressure. So this is for incompressible flows.

I used ParaView calculator to calculate the total pressure and the value matched :)

All times are GMT -4. The time now is 00:49.