SimScale CAE Forum

Boundary conditions in pipe with two outlets CFD simulation


I’ve got a question on setting up boundary velocity and pressure conditions for pipe system with several outlets. Imagine we have a pipe system with one fixed velocity inlet and we want to find velocity at the each of two outlets.

For example if I change inlet-2 BC in this case to outlet-2 boundary condition, what type of pressure BC I should use (inlet-outlet, zero gradient)?


not sure if I understand correctly, but you’re interested in a setup with

  • 1 inlet (fixed velocity)
  • 2 outlets

right? The easiest set up would be

  • 1 inlet: “Velocity inlet
  • 2 outlets: “Pressure outlet

So for an incompressible flow simulation, this is inlet:

this is outlet:

The Velocity inlet fixes velocity, but puts pressure to a zero-gradient. The Pressure outlet fixes pressure at a specific value and makes velocity zero gradient. Find out more about each boundary condition here:


Thank you for quick response.

You’ve understood me correctly. Does this set-up work for the buoyant flow as well (fixed velocity inlet and fixed real pressure outlets)?

So as I see, if I make two outlets there is no difference in boundary set-up for the second outlet. But I thought that there are two different pressure values at the different outlets (pressure drop between different inlet-outlets). And when I put the same pressure value for different outlets I suggest that they have the same pressure drop. In this case it should work only for symmetrical systems, when flow separates equally, like this. But it’s not clear for me what we do to simulate non-symmetrical systems, like I mentioned before, when we don’t know exact pressure values at the outlets.

Thank you again.

@varsey @dheiny, I’ll jump in if I may.

Firstly, this setup would work for buoyant flow and other analysis types as well. As a side note, there are several ways to use this combination, each bringing certain benefits (but that’s a different topic).

Regarding the second paragraph, there are two issues. The more obvious is that, if you know the values of pressure at the two outlets, you could specify those values at Pressure outlet definition. This will result in a valid setup with, in the special case of the simulation you provided, different mass flows at the outlets.

The less trivial case, as you mentioned, is when the exact pressure values are not known at the outlets. If you replace outlet conditions with Set gradient to zero for both velocity and pressure (you should use Custom BC for that), you will see the simulation crashes at the first iteration. Since no pressure values are defined in the domain, the incompressible solver cannot fully constrain the system of equations.

To move forward, you could assume the flow conditions are fully known at the inlet, i.e. both pressure and velocity. Use a Custom BC to set fixed values for both at the inlet, and leave outlets to be zero gradient. Now the system is well-constrained, and your simulation will successfully run. Mass flow at the outlet now depends on the features of your geometry.

@gholami, @varsey,

good point with fixing both quantities at the inlet and leaving them both open. @varsey - would be great to have such a project as a public project. Is it by any chance a public one you’re working on?

@dheiny @gholami Thank you for replies!

I’ve read in different places that fixing both quantities at the inlet and leaving them both open is not a good practice as it can lead to unreliable results (for example, slide 49 here), so I never tried it yet. But it worth a shot.

I’m dealing with non-trivial geometry case with different outlets, so I have to test this problem on less sophisticated configuration as pipe with several outlets on my PC to be sure BC setup works fine. I guess in case of success it’ll be no problem to upload simple pipe test on Simscale when I done.

@varsey, this is not always the case. Specifically in your incompressible scenario, where no information is provided at the outlets, assuming fully-developed conditions would help (in fact, it is not a strong assumption. It can still be used if little influence is expected on the domain).

With all that said, there are several cases where this is not a good definition of bc: compressible/variable-densit y flows, mutiphase flows, turbulent flows, and recirculation/reentry at outlet are a few. So, in the end it really depends. I would suggest that you carry on with the simulation to see if it works out. In any case, it would be nice to have your simulation on SimScale.

@gholami @dheiny ,
I did simulation of pipe with several outlets using BC we discussed and it doesnt seem to work well - project link.
May be it’s geometry configuration which is to fancy. And may be I did something wrong in setup.

Could you please give a look at project? Thank you.


I had a quick look. There is a small issue with one of the boundary conditions (assigned twice), but that should not be the cause of the problem. I will have a more detailed look and maybe try a few things. We discussed that this kind of bc definition is not always a good choice. Let’s see how it is in this case.

Hi @varsey

To me it works. And unless you plan something out of this world :wink: I think you overcomplicated this problem.

Here is the link and let me know if it’s what you were looking for:

(With y+ you have to play yourself – I don’t have that much time.)


@Maciek Thank you ever so much for your help. I see now it does work pretty good.

Thanks to all the contributors of this thread as well.