January 3, 2023 at 2:04 pmMontaSubscriber
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 🙂
January 3, 2023 at 3:14 pmRobAnsys Employee
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.
January 3, 2023 at 4:07 pmMontaSubscriber
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?
January 3, 2023 at 4:17 pmRobAnsys Employee
Except with a mix of gas and liquid you may not have a constant velocity on the inlet either.
January 4, 2023 at 1:04 pmMontaSubscriber
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%).
January 4, 2023 at 4:11 pmRobAnsys Employee
So the bubbles are small relative to the cross section? And you're not expecting regime change?
January 5, 2023 at 6:45 amMontaSubscriber
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.
January 5, 2023 at 10:04 amRobAnsys Employee
Have a look at the DPM model too.
January 12, 2023 at 1:44 pmMontaSubscriber
I had a look at DPM and I tried it also. Some points are not clear to me:
- the surface injection of bubbles from inlet. Are the particles considered as inert?
- Point properties: how to specify velocity and mass flow rate? Is for example drift flux model a way to estimate their values?
- steady and unsteady tracking is not well explained in the manual. When can I use the unsteady one?
January 12, 2023 at 1:55 pmRobAnsys Employee
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.
January 12, 2023 at 2:50 pmMontaSubscriber
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?
January 12, 2023 at 4:08 pmRobAnsys Employee
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.
January 13, 2023 at 8:58 amMontaSubscriber
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.
January 13, 2023 at 9:41 amRobAnsys Employee
So you need time 0
January 13, 2023 at 9:56 amMontaSubscriber
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?
January 13, 2023 at 11:07 amRobAnsys Employee
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.
- You must be logged in to reply to this topic.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Suppress Fluent to open with GUI while performing in journal file
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2023 Copyright ANSYS, Inc. All rights reserved.