hi

i am working on CFD simulation of air-water flow in vertical pipe, where water is entering the pipe from the bottom and air is entered through a separate pipe of smaller diamter into the larger pipe near the base .................. the boundary conditions i have set air-water with velocity at the two inlets define (vw 1.5 m/s & va 0.25 m/s) and pressure outlet the top of the exit. the bubble diamter 0.5 mm.

I am using Mixture model (along with SKE) but will eventually switch to Euler after some initial results. I tired running mixture and euler model before with different set of higher velocities but i was not able to get converge soltuion for the steady state but rather residual appearing as oscillating, i checked my grid and its appears to be fine. however after reading many manuals and CFD online replies i swicted to transient calulcations but i still haveing same problem all the residuals (although still oscillating)goes to below 10-5 except void fraction and continuity oscillating in 10-3 and 10-4 showing oscillating behaviour.

I am in need of help and advice to identify where i am doing wrong.

at http://www.learningcfd.com/ you can find a tutorial dealing with a water-air flow in a pipe. if you have problems with the download i can send you a short pdf describing problem setup and solution. the model does not accout for the bubble breakup and coalescence. you will need an add-on module wich is sold seperatly by fluent inc if you are interested in bubble size distributions.

good luck with you project rom

Simulating your flow with a steady solver is not the proper approach, because in most cases multiphase flows are not steady.

In the unsteady calculation, it's not a problem if you notice oscillation in the residuals, if they reduce at least at 10^-3.

Just do a check: try to simulate your system setting the convergence criterion for all variables to 10^-3 (the default in FLUENT). At the end of the calculation, check if the mass balance is respected (Use the Report -> Fluxes function). If so, the solution should be acceptable.

If your continuity residuals oscillates around 10^3, try to increase to 0.5 or 0.6 the under relaxation factor of the pressure and to reduce to 0.4 the under relaxation factor of the momentum.

Best regards, ap

Couple things need clarfication here. Firstly, I beg differ from the comment by ap:

"...in most cases multiphase flows are not steady...."

Well, yes and NO. The sentence is very well phrased indeed. And it is true as well, the "in most cases" part especially.

However, for vertical pipe flow in the bubbly regime, the flow is inherently steady in nature. Although, if one desired not to resolve any transient behavior, he/she can do an unsteady state simulation with 3-5 iterations per time step. But all said and done, you can check for yourself that in both cases the results will be the same.

Regarding the oscillation/convergence issues, here is my feedback. It is not a good idea to judge convergence only using the residuals. In most cases, it is more important to monitor relevant physical quantities at the cross section of interest and judge convergence when:

a) They level off at a steady value. b) They exhibit repeated oscillations about a steady value.

For instance, in vertical bubbly flows, one could monitor the area weighted average of the dispersed phase volume fraction at the outlet and run the simulations until the area weighted average levels off. The reason for this is because, sometimes although Fluent may report that convergence has been reached when residuals touch the 1e-4 limit, this may not represent true "physical convergence". What has happened is that the residuals have dropped to the level as set in the panel. That's all.

Usually, I set the residuals for continuity to an impossible value (say around 10e-13) and prefer to monitor the convergence using the relevant flow quantities (volume fraction across a section, velocity magnitude at a point, etc.).

There is an excellent tutorial solved using Fluent by Dr. Troshko for Turbulent vertical air-water upflows in a pipe available at: http://www.fluentusers.com/fluent6/d...id/node188.htm

which even considers the effect of custom Drag and Lift forces using User-Defined functions.

Hope this Helps...

Best Regards, Srinath Madhavan

You can choose to model a gas-solid flow as a steady flow if the volume fraction is low and the gas doesn't significantly influence the behaviour of the liquid main phase, but I would consider it as a simplification of the real case.

If you want to consider the real phenomena which could happen, it's not a good idea to make such an hypothesis, even if it would dramatically reduce computational time.

For example, the gas phase could induce oscillation in the flow and also bubbles may give origin to coalescence and break-up phenomena, which can't be considered steady at all. Also, I wouldn't consider the exchange of turbulence properties between phases as a steady phenomena.

Regards, ap

Wholly agree, but given the condition that one neglects bubble breakup and coalescence (which essentially introduces population balance concepts - not very easy to implement although there is some level of support in one of the Intermediate Tutorials for Fluent) and keeping in mind that vertical pipe upflows are hydrodynamically simple in nature (walls being the main source of turbulence if we do not consider bubble-induced turbulence and say even Turbulence modulation/modification; Also turbulence characteristics of the continuous phase are well investigated in pipe flows), I do not see any harm in simulating the flow as being steady in nature even at reasonably high holdups. The beauty here is restricted to the constraint that we assume that we are in the Bubbly flow regime.

On the other hand, if we talk of buoyancy driven flows such as bubble columns and/or Airlift reactors, we are talking of definite unsteady characteristics even if the flow is bubbly in nature. Additionally the flow cannot be considered Axisymmetric anymore

Using the mixture model is a good approach to start with in pipe flows. However, the Eulerian model is better suited to the case at hand (vertical pipe upflows). The ability to be able to define custom drag/lift expressions and incorporate Turbulent dispersion effects (if necessary) really makes the Eulerian approach more flexible and realistic in nature when compared to the ASMM.

The main reason for emphasizing steady solution is that it introduces lesser complexity in the problem definition. You do not have to worry about time stepping and other parameters to start with. One of the ways to determine whether your flow can be treated as steady or not is to refer to experiments. Gas-Liquid bubbly pipe flows in particular have been explored for years and generic conclusions support the idea that the flow is axisymmetric, steady and fully developed given enough pipe length and time. As you being to understand the nature of the flow it becomes way easier to see why solving in steady state makes more sense.

But as you put it rightly, once Population balance enters the picture, things start to go a little awry and certain assumptions are no longer valid I apologize for being a little verbose and drifting off the topic.

Best Regards,

Srinath Madhavan

I agree, but, if I'm not wrong, Aly's domain is something like this:


| |
| |
| |
| |
| |
| |
| |
| |___
| <--- air inlet
| ___
| |
\
\____ water inlet


So, it's not axisymmetric due to the air inlet, and I'm not sure the lateral inlet will keep the steady behaviour.

Regards,
ap

Oops, sorry. I was talking all the while keeping in mind the Fluent Tutorial. I apologize.

No prob. You dind't tell annything wrong and you seem very expert in the gas-liquid flow field, which actually isn't my main field of investigation. I work moreover on gas-solid systems (mainly fludized beds).

Best Regards, ap

[sanbhat]

I needed some clarity on the u-relaxation setting.
Why is that, the pressure factor is increased and momentum factor increased in order to get a quick convergence, if we see that the continuity residuals are oscillating near 10^-3?

[EYITAYOAFOLABI]

can you kindly send me this tutorial?
l am finding it difficult downloading it from the web quoted.
my email i d is
elizamos2001@yahoo.com