Two Phase Flow inside a Header
 

Dear friends,

I have been trying to simulate the fluid flow inside a header which has an inlet and four outlets for a couple of days. The inlet condition is as below;
gas volume fraction=0.8612, massFlow(inlet)=41 kg/s

First of all, I used homogeneous free surface model and in the next simulation I used in-homogeneous free surface method (Drag coefficient 0.44 and h=500 w/m2K and 4.5 dyne/cm surface tension coefficient for the interface)

My question: when I use in-homogeneous method, the simulation does not converge well and the results are not trustworthy at all. Could you tell me which method is the best for my simulation? (I need to make sure about mass flow rates and Gas mass fraction in each branch, according to the results)

I appreciate your attention

The choice of multiphase model options depends on the fluid you are trying to model.

You only use the homogenous model if both phases share a variable (usually velocity). This usually only makes sense for free surface models. So if your flow does not have a distinct free surface then the homogenous model is not suitable.

There are various non-homogenous models depending on whether it is drops, bubbles, slugs, foam, and so on. I don't know what your fluid state is so cannot say what is suitable.

Thanks Glenn for your response.

There are two fluids
1. Gas, Density 28.98 [kg/m3], Cp=3474 [J/kgK], Dynamic Viscosity=0.017 cp
2. Liquid, Density 549.39[kg/m3], Cp=3238 [J/kgK], Dynamic Viscosity=0.0888 cp

Inlet Condition: MassFlow 41 [kg/s], T=347 [C], Gas Volume Fraction=0.8612

I suppose that there is no bubbles or particles and I think that there are just two continuous fluids.

Please let me know if there are other parameters which are important for making decision about the model (homogeneous or inhomogeneous) that should be implemented.

Your inlet is at the bottom, where liquid and gas enter simultaneously in a mixed way. So, given this configuration you need a inhomogeneous model. Period.

Then in the horizontal pipe with the 4 branches, the gas and liquid might separate to form a free surface, if you are lucky. But that depends on the velocity, aggregation, etc. Given the velocity of 7 m/s, I won't give a penny for it.

Moreover, you won't be able to get a good prediction of the distribution over the 4 branches, if you don't know the spatial distribution and the aggregation of the gas and liquid (bubbles in liquid or droplets in gas??). Unless you know this, you can get any answer you like. Do you now assume a homogeneous distribution with a certain length scale? Are you sure about this?

Sometimes, these things are just unknown, then it is better to put your inlet further downstream or to a point where you know or can estimate what you have......

Thanks Gert-Jan
You know, that is a part of a piping system which is supposed to enter a burner and warm up the gas. However, in this part there is no heat flux from the surroundings.
I mean, I just need to know how much flow rate is passing through each branch and what the gas mass fraction is in each branch. So, I guess that there would not be any evaporation or condensation and no droplets or bubbles would take shape. Please let me know if you disagree with me.

I just had surface tension coefficient and I have no idea about length scale. So, I switched off mass transfer and interphase transfer.

Please give me more hints about your perspective.

I don't know your system at all.

I don't know the length scale, but given this mass flows, I would expect that the size is large enough to ignore surface tension. So, untick surface tension in Pre, and your results will be much better.

Thanks a lot

Could you give me some hints about specifying Drag coefficient when we are using In-homogeneous method?

What hint are you looking for?

But before we look into this parameter, you say you are looking at an inhomogenous flow. Why did you choose this? Also, there are three types of inhomogenous flow - particle model, mixture model and free surface. Which of these models is appropriate?

You need to choose the appropriate multiphase model before you start thinking about the parameters that model requires.

Dear Glenn

I tried to gain more information about this simulation.
Frankly speaking, I have no idea about the fluid flow in this case, in reality and I don't have any experimental results about my case. I mean, I am not sure about the presence of bubbles or droplets. Also, I have no information about bubble diameters if there are bubbles. Besides, I have no idea about drag coefficient if I want to go for Inhomogeneous model. I just know that there is no heat flux and the fluid flow seems Incompressible since the velocity is low enough.
All in all, I suppose that it is better to opt for the homogeneous model and free surface modelling and I will try to use a refined mesh in order to resolve more details.

Please give me your idea if you disagree with me.

I refer to my first post:

"Moreover, you won't be able to get a good prediction of the distribution over the 4 branches, if you don't know the spatial distribution and the aggregation of the gas and liquid (bubbles in liquid or droplets in gas??). Unless you know this, you can get any answer you like. Do you now assume a homogeneous distribution with a certain length scale? Are you sure about this?

Sometimes, these things are just unknown, then it is better to put your inlet further downstream or to a point where you know or can estimate what you have......"

Bottomline, you can get out anyhing from you CFD simulation, but not a free surface. Your velocities are way too high.
I would look for a point upstream where you know what you have, or can estimate it better,

Good luck. You might need it (a lot).

Just a heads up have a look at the GENTOP (Generalized Two Phase Flow) work the Dresden Helmholtz Centre have done. They've released models for this exact kind modelling situation.


Guess what? Helmholtz developed the framework in CFX but Ansys released it on Fluent. Idiots! (Ansys, not Helmholtz)