CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   Repeating boundary condition (

Marco83 January 6, 2010 18:06

Repeating boundary condition
Hi all,

I would like to know how to set up a repeating boundary condition in CFX. To understand my problem, you can imagine to have a geometry with one inlet and one outlet. This geometry is an elementary cell that gets repeated an ungodly large number of times in reality.

My goal is to set inlet and outlet pressures and require the velocity profiles at the inlet and outlet to be identical.

The tedious way of doing it is to set an arbitrary inlet, solve, take the outlet and use it as the inlet over and over again. Since I have to run 100+ simulations varying a few parameters, doing it manually is not exactly an option.

Any suggestion?

Tristan January 6, 2010 19:27

So you want a periodic boundary condition, right?


Marco83 January 7, 2010 09:14

I am not sure if a repeating boundary condition is exactly what I am looking for (I mean it; I am not too familiar with this type of BC and I may be missing the right way to use it).

I still want a pressure gradient between inlet and outlet, but the velocity profile has to be the same.

How would you implement this condition in CFX?

kingjewel1 January 7, 2010 09:19

If you're wanting the same profiles, set your inlet in CEL or otherwise... and then set your outlet by CEL to be the same as your inlet:
eg you want your inlet profile to be x^2-3/2x+9, then you can make this a CEL function and attatch it to the outlet too.
or in my experience i set inlet to be velocity and then do outlet:=ave(Velocity)@Inlet

Marco83 January 7, 2010 09:33

The point is that I don't know the shape of the velocity profile. If I were to code this problem, I would use an iterative approach, setting an arbitrary inlet profile, getting an outlet profile and feeding it back at the inlet over and over, until the difference between the two becomes small enough.

Tristan January 7, 2010 17:58

For fully developed turbulent channel flow simulations, they use periodic boundary conditions at the inlet and outlet. Since the pressure can't be periodic (it drops along the channel) they add a source term to the streamwise momentum equation to include the non-periodic part of the pressure and the solver is therefore only finding the periodic part of the pressure. So your source term is something like -(Pout-Pin)/L and the inlet/outlet velocity profiles will adjust together since you have a periodic boundary condition. Your "true" pressure is the solver computed perdiodic part plus a linearly decaying (Pin at inlet, Pout at outlet) non-periodic part.


All times are GMT -4. The time now is 20:53.