CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Initialization error

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 8, 2011, 03:12
Exclamation Initialization error
  #1
New Member
 
Churamani Prasad
Join Date: May 2011
Posts: 16
Rep Power: 5
cprasad111 is on a distinguished road
Multiphase model

Geometry is simple. A rectangle divided into two domains 1 and 2 seprated by an interface.

Two mixtures are created "kerosene phase" having components "kerosene" n "aceticacid" AND "water phase" having components "water" n "aceticacid".

Initial Condition:
In domain 1: there is only kerosene phase with known acetic acid mass fraction. (kerosene is contraint)
In domain 2: there is only water phase with known acetic acid mass fraction. (water is constraint)

CFX initialization i have done:
DOMAIN1:

SELECTED KEROSENE PHASE
kerosene phase-volume fraction :1
acetic acid-mass fraction:0.009
kerosene-constraint

SELECTED WATER PHASE
water phase-volume fraction:0
acetic acid -mass fraction:0
water-constraint

now when i monitored mass fraction of water of water phase in domain 1 its showing 1 and not 0.

Although i have specified water phase volume fraction to be 0, the mass fraction of water is being calculated from the constraint i.e. 1-acetic acid mass fraction(=0) which gives 1.But i want water mass fraction in domain 1 to be 0.

I must be doing some mistakes.

plz help
cprasad111 is offline   Reply With Quote

Old   June 8, 2011, 06:43
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,150
Rep Power: 73
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
It sounds like everything is a liquid. This means it is not a multiphase model. Why did you choose a multiphase model?
ghorrocks is offline   Reply With Quote

Old   June 8, 2011, 07:50
Default
  #3
New Member
 
Churamani Prasad
Join Date: May 2011
Posts: 16
Rep Power: 5
cprasad111 is on a distinguished road
water phase and kerosene phase are immiscible, so, i am using multiphase model. And initially acetic acid is present only in kerosene phase which by diffusion transfers to the water phase.
cprasad111 is offline   Reply With Quote

Old   June 8, 2011, 08:00
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,150
Rep Power: 73
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
And the boundary between the domains - do the kerosene and water mix, or are they kept separate?

Are you using a free surface model or some other eularian model for the kerosene/water mixture?
ghorrocks is offline   Reply With Quote

Old   June 8, 2011, 08:08
Default
  #5
New Member
 
Churamani Prasad
Join Date: May 2011
Posts: 16
Rep Power: 5
cprasad111 is on a distinguished road
kerosene and water does not mix. I am using free surface model.

Earlier I tried it as single phase model, and the boundary between domains were specified as wall, such that water and kerosene does not mix. For acetic acid, mass transfer was forced by adding source terms subdomain.This worked but the concentration of acetic acid changes in the whole domain at once. But this model does not allow natural diffusion of acetic acid from kerosene to water neither convetion diffusion in the domain.

I also tried adding source terms to the domain-boundary instead but this did not work.
cprasad111 is offline   Reply With Quote

Old   June 8, 2011, 20:54
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,150
Rep Power: 73
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Does the interface between the water and kerosene move?

Your comment about the source term - then just apply the source term to the interface/boundary. Obviously you cannot apply the source term to the whole domain.
ghorrocks is offline   Reply With Quote

Old   June 9, 2011, 01:06
Default
  #7
New Member
 
Churamani Prasad
Join Date: May 2011
Posts: 16
Rep Power: 5
cprasad111 is on a distinguished road
Interface does not move.

I tried applying source term to the boundary/interface, but in that case the result is not good its weired. I'll try that again and see what is the result.
cprasad111 is offline   Reply With Quote

Old   June 9, 2011, 01:21
Default
  #8
New Member
 
Churamani Prasad
Join Date: May 2011
Posts: 16
Rep Power: 5
cprasad111 is on a distinguished road
for the boundary source i have two options, which do you think should be used

1. k*((ave(reactant.molconc)@Boundary 1)-(ave(reactant.molconc)@Boundary 2))*reactant.mw

2. k*((ave(reactant.molconc)@Domain1)-(ave(reactant.molconc)@Domain2))*reactant.mw

k is some appropriate term

Domain 1 is the left part of the rectangle and domain 2 is the right half. The common boundary has between the domains has boundary 1 in domain 1 and boundary 2 in domain 2
cprasad111 is offline   Reply With Quote

Old   June 9, 2011, 06:50
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,150
Rep Power: 73
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If the boundary does not move then do not use a multiphase approach. Use two single phase domains (there is an expert parameter to allow you to put different fluids in separate domains, do a search of the forum to find it), and connect them with an interface. Turn off the p/mom interface, but define your own mass fraction equation. Then you do not need multiphase models.

For your transfer equation why are you using average concentrations? Surely the important thing is the local concentration at either side of the interface. You will have to use some sort of mass fraction interface to do this I think.
ghorrocks is offline   Reply With Quote

Old   June 9, 2011, 07:05
Default
  #10
New Member
 
Churamani Prasad
Join Date: May 2011
Posts: 16
Rep Power: 5
cprasad111 is on a distinguished road
Thankyou very much for you reply

I tried with the source term to the interface (the 1st choice from my previous reply) and its working almost fine. I also found out why it did not work earlier(probably due to wrong i.e. very high k value)

Now, to make the model better, I will try to find that expert parameter and other usefuls tips as metioned by you.

Thanks once again
cprasad111 is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Native ParaView Reader Bugs tj22 OpenFOAM Paraview & paraFoam 263 November 24, 2013 10:55
Accessing phi from a fvPatchField at same patch johndeas OpenFOAM 1 September 13, 2010 20:23
checking the system setup and Qt version vivek070176 OpenFOAM Installation 22 June 1, 2010 12:34
Problem with compile the setParabolicInlet ivanyao OpenFOAM Running, Solving & CFD 6 September 5, 2008 20:50
user defined function cfduser CFX 0 April 29, 2006 10:58


All times are GMT -4. The time now is 08:43.