# Fluent multiphase

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

 March 3, 2010, 12:14 Fluent multiphase #1 New Member   Join Date: Mar 2010 Posts: 5 Rep Power: 7 Hi, I am modelling an a microchannel evaporator. I know that i have two phases but i dont know the flow pattern if it is bubbly flow or droplet flow. So based on an article i chose the air as the primary phase and the water as the secondary one. I tried the opposite case and i had different resultats. I used the eulerian model per phase, K-E standard. Can u help me to know on which bases we choose the primary and the secondary phase. Thank you

 March 4, 2010, 04:55 #2 Senior Member   Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 12 Why do you use standard k-e for a microchannel? Flow in microchannels is generally laminar. Furthermore, what are mass and volume fractions of the both phases you mention? rgd likes this.

 March 4, 2010, 05:45 #3 New Member   Join Date: Mar 2010 Posts: 5 Rep Power: 7 Flow in my case can be laminar or turbulent depending on the velocity. In fact before entering the microchannel the flow passes in a distributor. To calculat ethe volume fraction, i supposed a vapor quality (for ex x= 0,3) and based on a correlation of calculation of void fraction i've calculated the void fraction. In all my cases (using air and water as the two phases), the volulme fraction >0,9. But the problem in a microchannel evaporator we cant know for sure the flow patter ( bubbly or mist flow or ..) But what i cant undertsand is the contradition in results when i permute the primary and secondary phase.

March 5, 2010, 15:06
MP Modeling - different results
#4
Senior Member

CFDtoy
Join Date: Mar 2009
Location: United States
Posts: 145
Blog Entries: 2
Rep Power: 8
Let me quote you "But what i cant undertsand is the contradition in results when i permute the primary and secondary phase.[/QUOTE]"

Basically would you agree if a liquid droplet in a gas phase and a gas bubble in a liquid differ in their nature?? if so why? Density ratio and the ability of one phase to buoyantly move within the continuous part. This exactly what the modeling does !

You send the liquid as continuous and vapor to be the dispersed (ideal scenario), the drag calculations are based on the dispersed phase and not the continuous phase !! So, you will get different results when you move around the phases in the eulerian two fluid model !!! (FLUENT is black box yes..but this is what is going on ...)

Choose liquid to be continuous, air - dispersed, (second phase), choose laminar (or turbulent if you see that the distributor does a lot of mixing) and your solution will just be fine !!

If you need additional help in modeling or numerics related to multiphase flows, kindly let us know.

Best regards,

CFDtoy

Quote:
 Originally Posted by sm.ensmp Flow in my case can be laminar or turbulent depending on the velocity. In fact before entering the microchannel the flow passes in a distributor. To calculat ethe volume fraction, i supposed a vapor quality (for ex x= 0,3) and based on a correlation of calculation of void fraction i've calculated the void fraction. In all my cases (using air and water as the two phases), the volulme fraction >0,9. But the problem in a microchannel evaporator we cant know for sure the flow patter ( bubbly or mist flow or ..) But what i cant undertsand is the contradition in results when i permute the primary and secondary phase.
__________________
CFDtoy

 March 6, 2010, 12:03 #5 New Member   Join Date: Mar 2010 Posts: 5 Rep Power: 7 of course i know that but i what i didnt know how fluent functions and if it takes all these factors in consideration. I found an article where they took air as the primary phase and they confirmed their fluent results with the experimentations. At first i did what u said but after i read this article i inverted the phases. Anyways i count on doind experimental tests and then i will compare with the simulations. Thank you

March 7, 2010, 11:40
inverting phases
#6
Senior Member

CFDtoy
Join Date: Mar 2009
Location: United States
Posts: 145
Blog Entries: 2
Rep Power: 8
The drag coefficients often implemented are functions available in literature such as those of ISHII etc...or Syamlal's for solid etc. Basically, drag function models are available as a function of particle (gas bubble or liquid droplet) diameter in a continuous media.

Just to make sure, drag Cd for gas bubble not the same as liquid droplet drag in air => Any software will use this criteria to model the drag sink terms not only FLUENT.

The experiments, may have dispersed phase 1 in 2 with a given % ...which will tell the user which assumption to use while modeling multiphsae. If the % of the droplets in air is around 10% or lower you can use dilute assumption and do a DPM model ..but for gas bubbles in liquid, one can use eulerian mp with reduced bubble size diameter consideration (increased surface area for interaction with liquid).

For bubble columns, (with gravity), the ability of the bubbles to follow gravity or "stick" to a region will depend on the drag terms modeled in the solution.

Best wishes,

CFDtoy

Quote:
 Originally Posted by sm.ensmp of course i know that but i what i didnt know how fluent functions and if it takes all these factors in consideration. I found an article where they took air as the primary phase and they confirmed their fluent results with the experimentations. At first i did what u said but after i read this article i inverted the phases. Anyways i count on doind experimental tests and then i will compare with the simulations. Thank you
__________________
CFDtoy

 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 Hossam CFX 1 November 3, 2010 07:57 ivanbuz FLUENT 11 March 10, 2010 16:13 L3munoz FLUENT 10 August 26, 2009 04:59 Marcin FLUENT 1 March 4, 2005 12:41 TOM FLUENT 6 July 15, 2002 03:24

All times are GMT -4. The time now is 19:00.