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

homogeneous free surface flow with phase change.

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 21, 2013, 13:23
Default homogeneous free surface flow with phase change.
  #1
Member
 
niru
Join Date: Apr 2012
Posts: 51
Rep Power: 5
Niru is on a distinguished road
I am trying to model an transient open(external) flow of cryogenic liquid on water.
I have modeled water as a rough wall with specific heat transfer coefficient.
I have also specified a 'specified mass transfer' to account the phase change from cryogenic liquid to vapor upon contact with wall.
My output would be the thickness of cryogenic liquid on water with time, its velocity and the amount of phase change with time.

1. In output, I am not able to get values for fluid pair models - mass transfer from cryogenic liquid to vapor. I see the variable in CFX-post, but no values.
What should I do to get the values with respect to time.
2. Is it enough if I specify the wall heat transfer coeff/heat flux/temp?
Should I add any additional variables to take into account the heat from water to cryogenic liquid?
3. How to get the thickness of cryogenic liquid in post processing.

my smallest mesh size is 0.1m, fluid domain size is 10x6.4x2.2 m.
time step -0.01
Niru is offline   Reply With Quote

Old   November 21, 2013, 17:53
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Can you post an image of what you are doing?
ghorrocks is offline   Reply With Quote

Old   November 21, 2013, 19:56
Default
  #3
Member
 
niru
Join Date: Apr 2012
Posts: 51
Rep Power: 5
Niru is on a distinguished road
Attached a image of Liquefied Natural Gas (liquid phase) spreading on water.
Attached Images
File Type: jpg Poolspreading.jpg (32.9 KB, 27 views)
Niru is offline   Reply With Quote

Old   November 22, 2013, 05:41
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
This is a very complex problem. Do I read correctly that you are assuming the water can be modelled as a rough wall boundary with heat transfer? This does not sound very accurate to me.

But ignoring these details and just answering your questions:
1) Are you sure you actually have any phase change taking place?
2) Are you asking whether this is an accurate assumption? Before you can answer this the key question is - "How accurate do you want the results of this simulation to be?" The more accurate you want it the more careful you need to be to include the correct physics.
3) Once you have a region of liquid LNG then you can plot this easily in CFD-Post, get the height at a XY location, get total volumes of liquid and all sorts of things. You think of a way of measuring the height and there will be a way of implementing it.
ghorrocks is offline   Reply With Quote

Old   November 22, 2013, 11:45
Default
  #5
Member
 
niru
Join Date: Apr 2012
Posts: 51
Rep Power: 5
Niru is on a distinguished road
But ignoring these details and just answering your questions:
1) Are you sure you actually have any phase change taking place?
Yes ,phase change is taking place. The fluid region is covered with vapor when I do post processing with vapor.
I track the temperature through monitor points too.
2) Are you asking whether this is an accurate assumption? Before you can answer this the key question is - "How accurate do you want the results of this simulation to be?" The more accurate you want it the more careful you need to be to include the correct physics.
I want the amount of LNG converting with vapor with respect to time.I have given a specific value for mass flux in CFX-Pre. This changes with time,and I need to track it. Tracking these in experiments is also quite tough.

3) Once you have a region of liquid LNG then you can plot this easily in CFD-Post, get the height at a XY location, get total volumes of liquid and all sorts of things. You think of a way of measuring the height and there will be a way of implementing it.
I find out the volume of LNG and then divide by areaAve of LNG in the water.
Will that account for height?

there is a variable called Bulk transfer LNG|LNGvapor
This doesnot have values. I dunno the reason.
Niru is offline   Reply With Quote

Old   November 23, 2013, 05:46
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
2) You missed the point of my question - can you put a % value on how accurate you want to be? If you are happy with 50% or 1% error will lead to entirely different simulations as the more accurate simulation will require much more physics.

3) Then just do a volumeInt of the LNG liquid fraction for the volume, and if you want the average height you can divide by the areaInt of the LNG liquid faction on the water surface. This is an average height which is one measurement of depth. There are many others - such as depth at a point, max/min depth, etc.
ghorrocks is offline   Reply With Quote

Old   November 24, 2013, 14:33
Default
  #7
Member
 
niru
Join Date: Apr 2012
Posts: 51
Rep Power: 5
Niru is on a distinguished road
2) You missed the point of my question - can you put a % value on how accurate you want to be? If you are happy with 50% or 1% error will lead to entirely different simulations as the more accurate simulation will require much more physics.

75% accuracy is something that I am aiming at.
Few of the physics cannot be captured when water is modelled as a wall.

If this works, I will try try a multifluid vof where air and water are 2 phases and LNG and LNG vapor are another pair of phases.
Niru is offline   Reply With Quote

Old   November 24, 2013, 17:12
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
For this level of accuracy you do not need to catch all the exact physics but only the main effects.

How does the LNG behave when it is sitting on water? I suspect there will be some important interactions there (but I am not sure, I am not an expert in this area).

Can you accurately model LNG boiling with no water present? Do you have a benchmark result to compare against?
ghorrocks is offline   Reply With Quote

Old   December 24, 2013, 21:49
Default
  #9
Member
 
niru
Join Date: Apr 2012
Posts: 51
Rep Power: 5
Niru is on a distinguished road
when LNG spreads on water, two forces are dominating. Gravitational forces push the LNG outward and inertial forces offer resistance to the flow.
Currently there are no good benchmark data. But there have been few experiments done before. The file size is big and I am not able to attach one.
the file size is around 1000KB.


Also , I have one more question regarding .
I get a courant number < 0.5
but my acoustic courant number is very high (RMS- 139.05 and MAX-365.95)
What does this mean?
Niru is offline   Reply With Quote

Old   December 25, 2013, 05:28
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
What does this mean?
Not very much. CFX is an implicit solver and does not have a Courant number time step limitation. If you have done a time step independance check and that is OK then you are fine. You have done a time step independance check, haven't you?

If you are doing a simulation with no benchmark data to check your modelling accuracy you need to be very careful. You need to find the closest benchmarks you can and make sure you can model them.
ghorrocks is offline   Reply With Quote

Old   December 25, 2013, 14:21
Default
  #11
Member
 
niru
Join Date: Apr 2012
Posts: 51
Rep Power: 5
Niru is on a distinguished road
No, I havent done a timestep independence test. Are you refering to grid independence test?

I thought of doing it after one successful run in CFX.
Niru is offline   Reply With Quote

Old   December 26, 2013, 00:11
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You should do a sensitivity test on ALL tunable parameters. Mesh density is one, but time step size and convergence criteria are two others which need to be checked. You may also have others, such as boundary proximity or some aspect of your physical model.

But you are correct - get the physics working correctly (but inaccurately) on a coarse mesh first. Once the physics is working correctly then the next step is getting it accurate by checking the sensitivity of all the parameters.
ghorrocks is offline   Reply With Quote

Old   December 26, 2013, 05:24
Default
  #13
New Member
 
Lee
Join Date: Oct 2012
Posts: 26
Rep Power: 4
kiwishall is on a distinguished road
Hi! I have been modelling a expander of LNG. And the problem of defining the material troubled me more. So could you tell me how you define the LNG or just simplify it with methane?
Thanks.
kiwishall is offline   Reply With Quote

Old   December 26, 2013, 11:27
Default
  #14
Member
 
niru
Join Date: Apr 2012
Posts: 51
Rep Power: 5
Niru is on a distinguished road
@Ghorrocks- thankyou for replying. I will give it a try.
@kiwiall- I modelled LNG as pure cmponent -methane.
Niru is offline   Reply With Quote

Reply

Tags
free surface, homogeneous, phase change, rough wall

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
Free Surface Flow with Sediment Transport M. Riffai CFX 3 September 5, 2013 09:45
free surface flow in non-inertial reference frame Tiedingg FLOW-3D 1 February 26, 2009 20:51
Pls. help about Free surface flow AT CFX 0 May 29, 2008 00:10
Free surface vortex flow Guillaume CFX 3 August 25, 2005 20:52
CFX 4.4 New free surface option Viatcheslav Anissimov CFX 0 April 3, 2002 06:27


All times are GMT -4. The time now is 20:30.