CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   CFX problems with supersonic inlet condition - Inlet values in CFX-Post are wrong (

jannnesss February 22, 2011 17:43

CFX problems with supersonic inlet condition - Inlet values in CFX-Post are wrong

I am setting up a 2D-simulation in CFX 12.01 with an supersonic inlet and supersonic outlet boundary condition.
I need to simulate the supersonic flow in a 2D-channel with a ramp.
I specified p, T and u at the inlet. The calculation works fine, no errors or something else.

But when I check the results in CFX post (or tecplot) I can see some problems at the inlet. For example: When I use the functionCalculator in post, the static temperature calculated at the inlet is the value I gave CFX as boundary condition (when I calculate it hybrid). But when I calculate the temperature "conservative" the value is not the same I gave CFX as boundary condition.

For those who don't know the calculator in post.
The temperature at the cell face is correct like I said CFX as boundary condition. But when I check the temparature one cell further in the domain (free slip walls for the first cells in the domain) the static temperature is approximately 10 K higher than the value I gave CFX as boundary conditon. The same for the Mach number.

Please help me, because it looks more or less like a bug because the calculation itself works fine and the flowfield is also okay!!! The only thing which is wrong, is that the the "real" inlet condition is wrong because of the effect I described above....

best regards and thanks a lot!!!!!

ghorrocks February 22, 2011 18:16

Are you sure your boundary is correct? Usually this sort of effect is the solver establishing equilibrium to account for boundary specification errors.

jannnesss February 22, 2011 19:07

Well, I think everything should be allright.
The Mach number, static temperature and static pressure is given...
I used the NASA-Format from CFX to calculate the corresponding specific heat capacitiy in order to calculate from the Mach number the velocity (u=sqrt(kappa*R*T)*Ma). After one calculation I used for the next one the specific heat capacity calculated from CFX post at the inlet.

The only value which could be incorrect is in my opinion the velocity at the inlet. I forgot to mention above, the same effect as for the temperature occurs for the velocity and pressure.

The temperature increases about 10 K
The pressure increases about 500 Pa
The velocity decreases about 10 m/s

And this gap occurs in the first cell!!!
Maybe it is because of an inaccuracy in the specific heat capacity (-> kappa)

CycLone February 23, 2011 10:24

Is the passage expanding? Is the solution converged?

Check the total conditions at both locations. Your total pressure and temperature should be about the same. An increase in static temperature and pressure are consistent with a decrease in velocity. If the total conditions are the same, look for why the velocity is decreasing. An expanding passage would explain this.

RossFS February 23, 2011 17:00

You will get a significant difference between hybrid and conservative boundaries near a boundary/wall based on the difference in how they are calculated (its a finite volume thing - look them up in xref.pdf provided in the ANSYS installation somewhere).

Also, this thread might be of use as I was modelling a similar flow and encountered a number of problems along the way (still unresolved) including T and P issues like you have mentioned:

jannnesss February 25, 2011 17:24

Hey guys!!!

thanks for your advice!!!!

Now I know the problem, and it might help you (RossFS) as well.
The problem in my case was the turbulence model. I used the EARSM model, but this was not the problem. The main problem was the CFX option "medium intensity" for the turbulence boundary condition at the inlet.
Because of the high inlet velocity the kinetic turbulent energy was overestimated by CFX. I tried two options, zero gradient and a fixed value for the turbulent kinetic energy & turbulent eddy dissipation. Both worked...

I am not sure if the explenation is correct, but I think the high turbulent kinetic energy (which is a boundary condition) gets his energy from the free stream...maybe something like an energy transfer which looks like an compression (T up, p up, u down)

Thanks for you advice....the best method is definitely to simplify the model!! (new test geometry, laminar, ideal air and so on....)

best regards,


All times are GMT -4. The time now is 06:19.