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

flue gas condensation

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 31, 2020, 07:42
Default flue gas condensation
  #1
New Member
 
Jay
Join Date: Mar 2020
Posts: 3
Rep Power: 3
fluid_dynamics_learner is on a distinguished road
Problem statement:
A flue gas is flowing inside a horizontal tube with certain mass flow rate and temperature. Cold air with a certain temperature is passed over tube in cross flow arrangement.

Desired output:
Variation of condensate mass flow rate over the entire length of tube.

Inputs:
Gas inlet temperature, gas mass flow rate, mass fraction of different species.
Length of tube, diameter of tube.
Cold air inlet temperature.

My setup:
1.Multiphase model: Eulerian , (3Phases)
2.Viscous model-k-epsilon, standard and enhanced wall treatment.
3.Species Transport: ON
4.Coupled interfaces.
5.Boundary Conditions: Inlet: Temperature and mass flow rate of gas and air
Outlet: Pressure -outlet.
6.Domains : 1-Inlet gas domain
2-Outlet air domain
3-Tube wall
7. Phases : 1- phase1 - Mixture
2- phase2- Water-liquid
3- phase3- Air

8.Phase interaction : Phase1 (vapor species) to Phase 2(water-liquid); evaporation-condensation



Problem facing :
1.In cell zone condition mixture is being defined at inner domain as well as outer domain, but i want only air in outer domain.
2.The solution diverges after 50 iteratios and" floating point error" arrises.

It would be helpful if you would guide me through the setup for this problem.


:
fluid_dynamics_learner is offline   Reply With Quote

Old   April 1, 2020, 04:20
Default Multiphase Modeling
  #2
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 33
vinerm will become famous soon enough
Fluent does not allow choosing a material for a cell zone when Multiphase model is used. It is mixture everywhere, however, you can restrict it to a particular phase and a particular specie of that phase by initializing with that value. So, if you have air and vapor as one phase and water as second phase, initialize with volume fraction of 1 and mass fraction of 1 for air in the outer domain. This way, you will only have air. You can fix the value of mass fraction to 1 to ensure that it stays so.

You do not need to add air as third phase.
__________________
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   April 16, 2020, 10:31
Default Flue gas condensation
  #3
New Member
 
Jay
Join Date: Mar 2020
Posts: 3
Rep Power: 3
fluid_dynamics_learner is on a distinguished road
Thank you for the clarification of the doubt.

Further i am facing another problem. I know the gas will not condense immediately throughout the tube, first it will reach the dew point temperature, and then it will loose its sensible heat.
I have achieved the desired results of variation of mass flow rate with respect to length via coding, but with fluent i am facing following problems:

Patching: I assigned water-liquid volume fraction as "0" in the domain.

1. The volume fraction of water-liquid should increase continuously, but in case of fluent simulation, its volume fraction increases for certain length and then decreases to 0.

2.1. The volume fraction of gas mixture should decrease continuously, but in case of fluent simulation, its volume fraction increases for certain length and then increases to 1.
fluid_dynamics_learner is offline   Reply With Quote

Old   April 16, 2020, 10:39
Default Evaporation-Condensation
  #4
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 33
vinerm will become famous soon enough
The phase change model you are using is thermal model, i.e., everything depends on temperature. If the temperature starts rising again due to any reason, the liquid will evaporate again. Also note that densities of water-liquid and water-vapor have a ratio close to 2000, i.e., if vapor condenses, only 1/2000th of the originally occupied volume is required to keep water. If vapor is being modeled as incompressible, it cannot expand to fill the space, hence, leading to pressure reduction, which could lead to re-evaporation if you have provided saturation temperature as a function of pressure. So, vapor or vapor-air mixture, whichever you are using, must be modeled as ideal gas.
__________________
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   April 21, 2020, 07:56
Default
  #5
New Member
 
Jay
Join Date: Mar 2020
Posts: 3
Rep Power: 3
fluid_dynamics_learner is on a distinguished road
Thankyou so much sir for your reply.
I implemented the same and now the mass transfer rate and VOF are showing the actual trend as per the analytical solution.

But the only problem i am facing is the mixture temeprature is changing by only 2K, where it decreases from 300K to 285K.
Whereas inlet Temperature of the mixture is 473K.

I have triend 2-D steady state and transient simulation also.
Their also i am facing the same problem.

Expected Problem: It is taking the same temperature with wich it is being initialized that is 300K

I am using Hybrid initialization, with patching of Volume fraction of "0",inside the domain.

It would be helpful if you clarify the initialisation and patching technique to be used for such problems.
fluid_dynamics_learner is offline   Reply With Quote

Old   April 21, 2020, 08:16
Default Initial Condition
  #6
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 33
vinerm will become famous soon enough
You need to ensure that there is at least a very small amount of vapor initially. So, each phase should have a positive volume fraction. If ideally you want it to be all liquid, start with liquid volume fraction of 0.99999 but vapor of 0.00001 but not 1 and 0.
__________________
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

Tags
condensation, condensation model, multiphase flow, multiphase modelling, species tranport

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
Domain Reference Pressure and mass flow inlet boundary AdidaKK CFX 75 August 20, 2018 05:37
Setting the height of the stream in the free channel kevinmccartin CFX 10 July 9, 2015 21:36
error message cuteapathy CFX 14 March 20, 2012 06:45
condensation flue gas Marc FLUENT 0 November 30, 2006 11:44
Gas pressure question Dan Moskal Main CFD Forum 0 October 24, 2002 22:02


All times are GMT -4. The time now is 19:27.