CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT > Fluent Multiphase

air water flow

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 27, 2020, 09:52
Default air water flow
  #1
New Member
 
hella
Join Date: Dec 2019
Location: Tunisia
Posts: 10
Rep Power: 2
hellaadouni is on a distinguished road
Hello everyone,

I have two questions:

1.I'm working on a horizontal air-water confined flow, and I got the slug flow. The problem is when the slug hits the upper part of the channel and blocks the air, this air must return as I think. But it doesn't. Do you have an explanation for this?
I'm sure that the air doesn't return because the air BC is velocity inlet, but I really want to understand where did the air goes once a slug blocks its passage to the outlet?

2. Since I'm working with two incompressible flows, is it wrong that I didn't use "operating density"? (Im working with VOF Model).


I'll be grateful if you help me.

Thanks
hellaadouni is offline   Reply With Quote

Old   January 29, 2020, 05:05
Default Details
  #2
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
Hi

Since the scenario is not very clear to me from the description, could you share more details, may be a couple of images of the domain?
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   January 29, 2020, 09:43
Default
  #3
New Member
 
hella
Join Date: Dec 2019
Location: Tunisia
Posts: 10
Rep Power: 2
hellaadouni is on a distinguished road
Quote:
Originally Posted by vinerm View Post
Hi

Since the scenario is not very clear to me from the description, could you share more details, may be a couple of images of the domain?
hello,
thank you for your response.
So the domain is like this:
Rectangular channel with two inlets: one for water and the other for air.
I keep raising the air velocity while the water velocity is fixed until a slug appears.
For this critical air velocity (where slug appears), the water blocks the passage of air. The air keeps pushing the slug until it leaves the channel.
My problem is, at the time that we have the water blocking the air, physically the air must return, but it doesn't..So I don't understand what's happening at that moment.
config.PNG

slug.PNG
hellaadouni is offline   Reply With Quote

Old   January 29, 2020, 09:56
Default Suggestions
  #4
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
There are two important points here

1. Operating density and operating pressure have to be set as 0
2. Air has to be modeled as ideal gas

There is another important point, which may be relevant. If air is pushed back because it hits water wave, then water has to be modeled as compressible as well using compressible liquid density model. There are a few phenomena that are based on specific properties and if those are not included, phenomena are not observed in CFD. E.g., water hammer cannot be observed without modeling water as compressible liquid, shock wave cannot be observed without modeling gas as ideal or real gas, Joule-Thomson cannot be observed until gas is modeled as real gas (ideal gas never heats up or cools down).
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   January 29, 2020, 10:42
Default
  #5
New Member
 
hella
Join Date: Dec 2019
Location: Tunisia
Posts: 10
Rep Power: 2
hellaadouni is on a distinguished road
Quote:
Originally Posted by vinerm View Post
There are two important points here

1. Operating density and operating pressure have to be set as 0
2. Air has to be modeled as ideal gas

There is another important point, which may be relevant. If air is pushed back because it hits water wave, then water has to be modeled as compressible as well using compressible liquid density model. There are a few phenomena that are based on specific properties and if those are not included, phenomena are not observed in CFD. E.g., water hammer cannot be observed without modeling water as compressible liquid, shock wave cannot be observed without modeling gas as ideal or real gas, Joule-Thomson cannot be observed until gas is modeled as real gas (ideal gas never heats up or cools down).
I'm modeling both fluids as incompressible, so you think this is wrong?
And concerning the operating density, by putting zero you mean to disable it? please see attached photos and bear with me, thank youair.PNG

water.PNG

operationg conditions.PNG
hellaadouni is offline   Reply With Quote

Old   January 29, 2020, 10:48
Default Compressibility is important here
  #6
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
Value of 0 does not disable these. Rather Fluent starts using pressure values as absolute values; default is gauge. Operating density is used to determine the buoyancy. For the time being, let water be as it is. But for gas, select ideal gas. You may disable the energy equation and assume that water and air are at same temperature. With incompressible gas, you may not observe what you are expecting. The downstream pressure has to increase beyond the upstream for air to return. That can happen only when pressure is real pressure, i.e., using ideal gas law.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   January 29, 2020, 10:51
Default
  #7
New Member
 
hella
Join Date: Dec 2019
Location: Tunisia
Posts: 10
Rep Power: 2
hellaadouni is on a distinguished road
Quote:
Originally Posted by vinerm View Post
Value of 0 does not disable these. Rather Fluent starts using pressure values as absolute values; default is gauge. Operating density is used to determine the buoyancy. For the time being, let water be as it is. But for gas, select ideal gas. You may disable the energy equation and assume that water and air are at same temperature. With incompressible gas, you may not observe what you are expecting. The downstream pressure has to increase beyond the upstream for air to return. That can happen only when pressure is real pressure, i.e., using ideal gas law.
Thank you so much
So i'll only change the gas as ideal and see what happens?
I'll keep the operating density as it is?
hellaadouni is offline   Reply With Quote

Old   January 29, 2020, 10:55
Default Settings
  #8
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
You have to set operating density and operating pressure to 0. Along with that, set 101325 Pa as pressure at the outlet and inlet.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
icoReactingMultiphaseInterFoam air on water stratified flow tonnykz OpenFOAM Verification & Validation 0 August 20, 2019 13:31
No liquid water exist in my Fuel Cell simulation fatchang FLUENT 19 October 15, 2018 14:27
CFD analaysis of Pelton turbine amodpanthee CFX 31 April 19, 2018 18:02
Simulation of air flow in a chamber Issa CFX 3 November 23, 2009 17:16
Two-phase air water flow problems by activating Wall Lubrication Force challenger85 CFX 5 November 5, 2009 05:44


All times are GMT -4. The time now is 07:54.