# Mixture model - pipe flow

 Register Blogs Members List Search Today's Posts Mark Forums Read

 March 30, 2005, 11:01 Mixture model - pipe flow #1 Aly Guest   Posts: n/a 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.

 March 31, 2005, 03:51 Re: Mixture model - pipe flow #2 rom Guest   Posts: n/a 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

 March 31, 2005, 14:50 Re: Mixture model - pipe flow #3 ap Guest   Posts: n/a 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

 April 1, 2005, 14:58 Re: Mixture model - pipe flow #4 pUl| Guest   Posts: n/a 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

 April 1, 2005, 18:32 Re: Mixture model - pipe flow #5 ap Guest   Posts: n/a 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

 April 1, 2005, 20:45 Re: Mixture model - pipe flow #7 ap Guest   Posts: n/a 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

 April 1, 2005, 20:48 Re: Mixture model - pipe flow #8 pUl| Guest   Posts: n/a Oops, sorry. I was talking all the while keeping in mind the Fluent Tutorial. I apologize.

 April 2, 2005, 14:30 Re: Mixture model - pipe flow #9 ap Guest   Posts: n/a 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

 May 7, 2009, 09:34 #10 New Member   Sandeep Join Date: Mar 2009 Location: Blacksburg, US Posts: 3 Rep Power: 10 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?

 June 21, 2010, 13:50 #11 New Member   EYITAYO AFOLABI Join Date: Apr 2009 Posts: 10 Rep Power: 10 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

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Munni Main CFD Forum 6 December 7, 2015 12:33 achaokaoyan Main CFD Forum 0 July 10, 2010 10:52 vismech STAR-CCM+ 1 August 11, 2009 10:38 dongye Main CFD Forum 0 October 1, 2007 22:23 Abhi Main CFD Forum 12 July 8, 2002 09:11

All times are GMT -4. The time now is 00:26.