Learning Forum

[Monta]

I am modeling two phase bubbly gas flow in pipe. I have following questions regarding Inlet BC.
1. In the literature the entrance length for turbulent flow is 4.4*Re^(1/6)*D. This will cause extra numerical computation. Is it possible to take simply the estimation L = 6* D instead?
2. The flow should be fully developed, so instead of creating an entrance length I defined a UDF velocity profile for the liquid phase. In this case how can I define the gas phase? (No mass flow rate in velocity BC so maybe veloctiy as Mass flow rate /(section * density)?)
3. If I want to distribute the bubbles at the inlet according to a distribution-function. Is this realisable? If yes any thoughts about that?

Thanks in advance ?
Monta.

[Rob]

If the inlet is bubbly then the mass fraction will vary with time, and you'd need to allocate position to the bubble phase to see the bubbles. That won't work with VOF as the model doesn't allow for that. Multifluid VOF (an Eulerian model option) will give more flexibility, but the boundary condition won't be trivial. 

Upstream length needs to be sufficient to prevent the inlet value forcing the solution at the point of interest. With bubbly flow that could be further upstream than you think as the phase regime might try and change in the pipe. Have a look at turbulence damping as that could be important in this case. 

Bubbles aren't distributed as such, you need to set the phase value with location and time. That's probably going to need a UDF, and is going to get complicated. 

 

[Monta]

I am using mixture model. So it is probably better to define a developed turbulent velocity profile at inlet and figure out how to define the gas fraction. Ovoiding the entrance length will reduce computational cost and ovoid an expected flow change along it. Right?

[Rob]

Except with a mix of gas and liquid you may not have a constant velocity on the inlet either. 

[Monta]

So what's from your perspective the simplest, yet efficient, way to define an inlet condition for liquid-gas bubbly turbulent flow (for example water with air bubbles where gas amount is 5%).  

 

[Rob]

So the bubbles are small relative to the cross section? And you're not expecting regime change? 

[Monta]

I assume in a first step that all the bubbles have a size of 0.5mm which ich very small compared to the cross section. The flow stays bubbly. I want only see how gas volume in liquid affects the heat transfer.  

[Rob]

Have a look at the DPM model too. 

[Monta]

I had a look at DPM and I tried it also. Some points are not clear to me: 

1. the surface injection of bubbles from inlet. Are the particles considered as inert? 
2. Point properties: how to specify velocity and mass flow rate? Is for example drift flux model a way to estimate their values? 
3.    steady and unsteady tracking is not well explained in the manual. When can I use the unsteady one?

 

[Rob]

Particles are inert if they don't react/disolve etc. If your bubbles remain as small bubbles (ie no collision) then they're inert. 

DPM particles/bubbles/droplets are injected with a speed and mass flow. Have a look at the options, and pick what makes sense. In your system have a look at a surface injection too. 

Steady tracking will result in a particle track, ie a line showing the flight path of the particle. Transient particles will trigger an injection every particle time step and then show spheres/points of where the particle is. With unsteady particles & steady flow the assumption is that the flow isn't altering with time but you want to see the particle positions. With that you also need to ensure you've run enough particle time steps for everything to settle down and/or reach the state you want to study. 

[Monta]

 

I don’t know exactly what you mean by options. As you can see here I have to input values for velocity and mass flow rate. That’s why I asked about empirical models (like DFM) to estimate both values. Another questions to start and stop time. Is is it just the begin and end of simulation time for example?

 

[Rob]

Time is often zero to a large number: it's more useful when injections are only wanted for short periods. You will know the mass flow of spray/particles/bubbles and for a surface using the inlet velocity is sensible. 

[Monta]

I tried the injection only at t=0s. It works but it seems not realistic since the bubbly flow enters the pipe contiuously with new bubbles. Moreover I want to know how does Fluent compute the number of tracked particles. 

[Rob]

So you need time 0

[Monta]

How about the number of tracked particles. How does fluent compute it? Is there a formula based using flow rate, bubble size/properties and velocity? 

[Rob]

Weird, I posted a lot more text. 

Injection will be 0 < t < 3600 or so, ie bubbles are injected every particle time step for a continuous injection. 

For a surface injection you get one parcel stream per facet. The parcel speed is based on the values you put into the panel. The parcel mass is injection mass divided by the number of parcel streams. Leave the parcel definitions alone until you understand what the changes will do. 

 

[Monta]

Update + question: 

@Rob

I carried out a DPM-Simulation with continuous injection so that I can have approximately a constant amount of gas in my domain. By comparing the convective heat flux from the pipe to the outside with a single phase flow I did not find any difference. Does DPM take into account the effect of gas fraction on convective heat transfer. If yes what did I probably miss to consider? 

[Rob]

DPM is a point mass, but bubbles/particles/droplets do carry heat so can effect the heat transfer. Read the definition of DPM Concentration and then plot that on the outer wall. You did run DPM with "interaction with continuous phase" on?  Also consider how much/little heat will be carried given the bubble volume fraction. 

[Monta]

I took into account the interacation with continuous phase. Besides there is a " particle-wall heat exchange" check box under wall BC. In the ansys documentation there is nothing much said about it.  

[Rob]

Looks sufficient  https://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v231/en/flu_th/flu_th_sect_dpm_p-w_heat_transf.html   How does the concentration plot look?

[Monta]

The heat transfer theory is described for liquid droplets. Can it be applicable also for gas bubble? 

[Rob]

I suspect the solver will use it for all "particles" if you turn the model on. Having had a quick look, I now have coefficients to allow the Weber Number to be calculated for anthracite.