[Slurm]

Good morning everyone,

As the title says, I am trying to create a turbulent pipe flow on a square channel.

I see that Converge sets the tools for imposing a synthetized turbulence field for the LES data, but I don't know how to impose a periodic boundary.

What I have tried so far is to input both "INLET" and "OUTLET" as matching periodic boundaries, but setting them like that, removes the option to input a velocity at the INLET. Then if simulated (with initialized velocity), the flow slows down to zero-velocity.

Am I doing something wrong or the "Periodic" boundaries in Converge are not thought to do this kind of simulations?

Kind regards

[yli]

Hi,
We don't have a direct way to set a periodic inflow/outflow. But we can realize this by adding momentum source.
Is your case a single-phase flow or multiphase flow? If it is single phase flow, you can set the inflow /outflow as "periodic" boundary->stationary-translational.

Then go to "physical models", enable "source modeling", choose momentum source, and select source units as momentum/m^3.s (momentum per unit volume per unit time, or kg/(m2.s2) ). Notice this momentum source has same unit as pressure gradient, so basically you are enforce a pressure gradient over your geometry to drive the flow. The momentum source direction is the same direction as your primary flow.

If you have test data of pressure gradient, you can directly put it here. Other wise if you have mean velocity, then you can tune the momentum source value to match your mean flow velocity.

Thanks and let us know if you need further help.

[yli]

Another easier way to do it is using hidden inputs to specify pressure jump across periodic faces:
In Studio, go to "adavanced parameters" and turn on "hidden inputs" and add "periodic_jump" as hidden variables and specify the value based on
pressure_jump=dP/dx*length.

[Abubakar123]

Hi Yanheng Li, I have tried to do this but it didn't work. Can you help with this?