Initialization error

cprasad111 · June 8, 2011, 04:12

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

ghorrocks · June 8, 2011, 07:43

It sounds like everything is a liquid. This means it is not a multiphase model. Why did you choose a multiphase model?

cprasad111 · June 8, 2011, 08:50

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.

ghorrocks · June 8, 2011, 09:00

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?

cprasad111 · June 8, 2011, 09:08

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.

ghorrocks · June 8, 2011, 21:54

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.

cprasad111 · June 9, 2011, 02:06

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 · June 9, 2011, 02:21

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

ghorrocks · June 9, 2011, 07:50

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.

cprasad111 · June 9, 2011, 08:05

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

June 8, 2011, 04:12	Initialization error	#1
cprasad111 New Member Churamani Prasad Join Date: May 2011 Posts: 16 Rep Power: 15	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

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[OpenFOAM] Native ParaView Reader Bugs	tj22	ParaView	270	January 4, 2016 12:39
Accessing phi from a fvPatchField at same patch	johndeas	OpenFOAM	1	September 13, 2010 21:23
checking the system setup and Qt version	vivek070176	OpenFOAM Installation	22	June 1, 2010 13:34
Problem with compile the setParabolicInlet	ivanyao	OpenFOAM Running, Solving & CFD	6	September 5, 2008 21:50
user defined function	cfduser	CFX	0	April 29, 2006 11:58

June 8, 2011, 07:43		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,872 Rep Power: 144	It sounds like everything is a liquid. This means it is not a multiphase model. Why did you choose a multiphase model?

June 8, 2011, 08:50		#3
cprasad111 New Member Churamani Prasad Join Date: May 2011 Posts: 16 Rep Power: 15	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.

June 8, 2011, 09:00		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,872 Rep Power: 144	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?

June 8, 2011, 09:08		#5
cprasad111 New Member Churamani Prasad Join Date: May 2011 Posts: 16 Rep Power: 15	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.

June 8, 2011, 21:54		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,872 Rep Power: 144	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.

June 9, 2011, 02:06		#7
cprasad111 New Member Churamani Prasad Join Date: May 2011 Posts: 16 Rep Power: 15	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.

June 9, 2011, 02:21		#8
cprasad111 New Member Churamani Prasad Join Date: May 2011 Posts: 16 Rep Power: 15	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

June 9, 2011, 07:50		#9
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,872 Rep Power: 144	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.

June 9, 2011, 08:05		#10
cprasad111 New Member Churamani Prasad Join Date: May 2011 Posts: 16 Rep Power: 15	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