[Sideshore]

Hello

I'm trying to simulate a pipeflow with 2 inflow boundary conditions and 1 outflow boundary condition using simpleFoam.

I tried using a fixedValue boundary condition for the velocity at the outflow. But the simulation didn't converged and I got disturbances at the outflow. Which is expected because the flow is not uniform when it approaches the outflow boundary.

I would like to define the velocity with zeroGradient at the inflow and the massflow or average velocity at the outflow. And the pressure with fixedValue at the inflow and zeroGradient at the outflow.

How can I set the massflow or the average velocity at the outflow boundary?

Any suggestions are appreciated!!

[gschaider]

Originally Posted by Sideshore

Hello

I'm trying to simulate a pipeflow with 2 inflow boundary conditions and 1 outflow boundary condition using simpleFoam.

I tried using a fixedValue boundary condition for the velocity at the outflow. But the simulation didn't converged and I got disturbances at the outflow. Which is expected because the flow is not uniform when it approaches the outflow boundary.

I would like to define the velocity with zeroGradient at the inflow and the massflow or average velocity at the outflow. And the pressure with fixedValue at the inflow and zeroGradient at the outflow.

How can I set the massflow or the average velocity at the outflow boundary?

Any suggestions are appreciated!!

So you want a boundary condition that keeps the velocity at the outlet the same but only rescales it to satisfy the prescribed mass flow. I'm not aware of such a BC (which doesn't mean that there is none).

If I had to do such a thing I'd use groovyBC (basically using an expression for the value like "U*mfTarget/mfCurrent" - the two mfs being specified/calculated). Note that probably to get this stable you'll have to make it a bit more complicated: at least some kind of underrelaxation to avoid trouble during the startup-phase and you'll have to decide whether you allow backflow (because that would be accelerated by the scaling too). And of course there is the general problem of specifying the massflow at the outlet ....

[wouter]

hello,

If you have two inlets and one outlet. I think the best thing to do is set the two inlet velocities (fixed value). Calculate the velocities from the ratio of flows through the inlet and the area of the inlets by hand and let simpleFoam calculate the outlet flow, what being an incompressible steady state should result in the asked for massflow.

hope this helps

Wouter

[Sideshore]

Thank you both for your reply!

Ansys CFX does have a massflow boundary condition, could be a very nice addition to OPENFOAM!

If I had to do such a thing I'd use groovyBC (basically using an expression for the value like "U*mfTarget/mfCurrent" - the two mfs being specified/calculated).

GroovyBC sounds interesting! But as you said it might be a struggle to get a stable solution. I'm going to look into groovyBC thanks!

If you have two inlets and one outlet. I think the best thing to do is set the two inlet velocities (fixed value). Calculate the velocities from the ratio of flows through the inlet and the area of the inlets by hand and let simpleFoam calculate the outlet flow, what being an incompressible steady state should result in the asked for massflow.

Prescribing the inflow velocity at both inlets does not give an accurate result. Because when you prescribe the inflow velocity normally you also prescribe the fixed pressure at the outlet. Therefore you end up with a pressure difference between both inlets. Which is not the case I would like to simulate.

Of course you could iterate between inlet velocities to end up with a similar pressure at both inlets.

[wouter]

hello Jan Willem,

Maybe you can use my suggestion as a stable start for the simulation with groovyBC

Best
Wouter

[akidess]

I think the fixedMean boundary condition works nicely for such a case.

[mOHAMMAD SADIK]

Hello i am trying to solve the same problem in Ansys fluent , how do i check if momentum is conserved?