CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   simple model, difficult outlet (

Eric December 24, 2006 20:03

simple model, difficult outlet
Dear Friends,

My model is a cylinder: 2.8 mm in diameter, 7.35 mm in length. One end of the cylinder is inlet and the other is out. At inlet, velocity = 311.4 m/s; how to set the boundary condition at Out? If I set the pressure at OUT as 1 atm, maybe not good, could you give me some advice?

Thank you in advace.


Manu December 25, 2006 11:32

Re: simple model, difficult outlet
Preessure Outlet Relative Pressure : 0

Sameer December 28, 2006 10:31

Re: simple model, difficult outlet
Hi Eric !

In your problem velocity is very high ( 311.4 m/s ), flow must be highly turbulent and undevloped. I think you should try with mass flow rate at inlet and outlet as a opening.

Robin December 29, 2006 13:31

Re: simple model, difficult outlet
It depends on what is downstream of your outlet that you have not included in your model. Keep in mind that a boundary condition is an approximation of what the external conditions may be.

Since you are modelling a pipe and have specified the flow at the inlet, a pressure outlet would be appropriate. I wouldn't bother with an opening unless you really expect reversed flow.

There are two options for the pressure: average static pressure or "static pressure".

The Average Static Pressure option will allow the pressure value to vary locally, but maintain the area averaged for pressure at the value you specify, thus allowing the profile to develop naturally. This is appropriate if the flow continues along the pipe beyond your boundary condition.

The "Static Pressure" option will maintain a constant static pressure at the outlet. This would approximate the conditions occurring when the pipe exits into a large plenum. In such a case, the static pressure would be roughly constant across the pipe.

If the fluid is liquid and you are not including cavitattion, it really doesn't matter what pressure you set. The solution will be the same relative to the outlet.

If flow is compressible, you need to consider the conditions more carefully. If you don't know the outlet pressure and flow is entering your domain from a large plenum, you would probably be better off specifying a total pressure at your inlet equal to the static pressure of your plenum (if the velocity is sufficiently low in the plenum, the Ptotal=Pstatic) and a mass flow rate at the outlet.

Again, there are some options as to how the static pressure will vary at the mass flow outlet; Scale Mass Flows, Shift Pressure, and Constant Flux.

The default is mass flow update option "Scale Mass Flows" and does the equivalent of the Average Static Pressure, allowing the local mass flow rate to vary naturally but maintaining the total flow rate specified.

Shift Pressure allows you to enter a relative pressure profile which the solver will match by shifting up or down to get your mass flow rate. If you put a constant value in here, you will get a constant static pressure at the outlet, which as before will approximately represent the conditions at a sudden expansion.

The last option, Constant Flux, is not physically realistic for this case as it will force the mass flux to be constant everywhere.

Finally, if you only know the pressure conditions at the inlet and outlet, you can set it up with a total pressure at the inlet and a static pressure at the outlet, in which case the mass flow rate will be determined.

Regards, Robin

Eric December 29, 2006 22:16

Re: simple model, difficult outlet
Dear Friends,

Happy new year.

Thank you for your helping and I will try as you said.

Mang thanks


Ashwin k May 22, 2014 02:32

inlet boundary conditions
hello guys,
i have seen ur above comments regarding wat boundary conditions should be specified at inlet and outlet. from above i concluded that for outlet pressure condition should be given and for inlet velocity condition should be given.
in my problem i m using a cylinder with diameter of 8mm with inlet and outlet port diameters 7mm and 2.8mm respectively distance from inlet to outlet port is 32mm. pump operates at 400bar. so now how do i find velocity at the inlet.

thank u in advance

sans May 23, 2014 04:44

Do you know the flow?

ghorrocks May 23, 2014 08:13

Sans is right - the boundary conditions you apply are the flow conditions you know about the flow. It oculd be flow rate or pressure.

You mention 400 bar - remember that this should be just used as the reference pressure, the important thing for the simulation is the pressure rise/drop, so the pressure difference between the inlet and outlet.

All times are GMT -4. The time now is 21:09.