I am solving a fluid flow problem with one inlet and two outlets. The simulation does not converge. I tried a problem with one inlet and one outlet. It works.

My question is: If I have two outlets, what restriction or anything I should do about the two outlets? Do I have to specify the ratio of flow rate at the two outlets? Thanks!!

Ming

Ming,

I have solved several problems where there is a single inlet and multiple outlets. In one typical case there are one inlet and 6 outlets (and 2 more outlets which are modeled as inlets with negative flux). they all converge nicely.

So, please explain your problem a bit more

1. is the flow compressible or incompressible

2. is the flow laminar or turbulent, if turbulent what kind of turbulence model are you using and what kind of mesh

3. what kind of boundary condition are you specifying at the inlet (fixed velocity? total pressure?)?

4. what is the purpose of the simulation; what are you trying to solve?

5. what do you know about the condition at the exit boundaries

6. what are you using as your initial guess?

7. what kind of solver are you using?

and perhaps many more such questions.

I don't think there is anything wrong in having multiple outlets. There has to be some other explanation, perhaps hidden in the problem setup.

For multiple outlets, you need to specify the flow ratio for each outlet so that the total outflow can be balanced by inflow.

For multiple inlets, depending on your inlet boundary conditions, you can use Neumann boundary conditions for all variables (extrapolation condition, for viscous flow). You can set the pressure at one outlet, and use extrapolation for all other inlets. Inflow/outflow mass flux matching is needed explicitly in the program anyway.

Be careful accidentially not to set a pressure difference somewhere in the domain by the boundary conditions. This would be the case if you used pressure boundary conditions both at the inlet and the outlet (even a single outlet) or if you set the pressure at two outlets.

regards

DML

Hi,

Let me try to learn something here:

1) the original question is about convergence problems with a case with multiple outlets. So is your comment

"Be careful accidentially not to set a pressure difference somewhere in the domain by the boundary conditions. This would be the case if you used pressure boundary conditions both at the inlet and the outlet (even a single outlet) or if you set the pressure at two outlets. "

related to convergence problem. Or is it an advice to get getting the real solution.

The reason I am asking is because I have run several iteratons of a problem where I have one inlet and several outlets (as I stated in the first response to the original question). All these outlets exit the air into a chamber. I thought it be a relistic condition to impose same fixed pressure boundary codition at all the outlets. Thus the simulation predicts the distribution of flow into various ducts. I did not have any convergence problems. I also had a solution that compared excellently with testing (measurements). But it is still possible that I might have done something wrong but still got reasonable annswer.

can you please explain why I should not impose the same pressure condition at all the exits (that exit into the same chamber or into the ambient). I am simulation incompressible turrbulent flow.

Often times the goal of such simulations is to predict the ratio (not to specify it). I have done it and the results showed excellent comparison with the measurements. I was solving incompressible turbulent flow.

I don't know what is the purpose of this simulatoin though.

(1). It is really an interesting question, and a confusing one. (2). I think, it has a lot to do with the formulation itself, whether it is incompressible or compressible formulation. (3). In the incompressible formulation, the pressure can be decoupled from the Navier-Stokes equations, and the velocity field can be obtained independent of the pressure field. So, assuming that you have the exact velocity field in incompressible flow, there is only one pressure unknown you can specify, that is you can specify the pressure only at one point. The rest of the pressure field can then be obtained from the velocity field. (4). But like the solution to the boundary layer equation, one can input the pressure distribution and obtain the solution, you are free to specify the pressure field also. If the pressure field is constant, then, you can set it to a constant value, and the pressure terms will drop out from the Navier-Stokes equations. (5). But then, I am sure that you will not find the pressure loss in the constant pressure field solution, even if the solution of the velocity field exists. In the case of the boundary layer equation, the pressure distribution is given, so there is no way one can change it in the solution. (you specify the solution as the input there). (6). If you try to use the real world experience in air, then it is a completely different story, because it is in the compressible flow domain, even though the Mach number effect is small at low speed. The mechanism in compressible flow is not the same as that in incompressible flow. (7). I can only say that it is a confusing issue. The only thing I can say is: you are free to specify the pressure field, but then what you obtained may not be the solution you are looking for. But if the condition is close to the test condition, then the solution would be close enough.

My comment was related to both convergence problems and getting a correct (real) solution. Most of the issues were already touched by J.Chien in his reply.

For incompressible calculations, one is free to specifiy static pressure at any number of points and no matter where the points are located (boundary or inner elements). It is allowed only if the pressure gradients imposed by the setting are correct. If one knew the entire static pressure field, why not to use it?

Now, if you specify static pressure at two points and this setting results in wrong pressure gradients, then either your program will have hard time to converge or you will get a wrong solution (perhaps not really a converged one). Your case is a special one where the physics says what kind of boundary conditions you should use at the outlets. Your outlets are really at atmospheric pressure, so what you do is OK.

Different example, staying with air flows, could be an analysis of a ventilation duct which branches into two legs of different cross-sections. One cuts out the calculation domain from the duct. One sets the inlet well before the branch and two outlets after the branch (on each leg one outlet). For this example, static pressure will perhaps be quite different at the two outlet planes. Although you can still specify static pressure at more than one point (inlet, outlets,... whatever), this may be a hard task unless you have some measurements.

The original message did not say exactly what was the physical case to be modeled. That is why I could not be more precise in my response.

DML

one approach that is often useful is use a simplified 1-D model to estimate your flow splits. Then depending on your solution assumption (compressible or incompressible) you can use the results of this analysis to help set boundary conditions according to what your code allows.