CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   homogeneous free surface flow with phase change. (http://www.cfd-online.com/Forums/cfx/126620-homogeneous-free-surface-flow-phase-change.html)

 Niru November 21, 2013 13:23

homogeneous free surface flow with phase change.

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

 ghorrocks November 21, 2013 17:53

Can you post an image of what you are doing?

 Niru November 21, 2013 19:56

1 Attachment(s)
Attached a image of Liquefied Natural Gas (liquid phase) spreading on water.

 ghorrocks November 22, 2013 05:41

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.

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.

 Niru November 22, 2013 11:45

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.

 ghorrocks November 23, 2013 05:46

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.

 Niru November 24, 2013 14:33

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.

 ghorrocks November 24, 2013 17:12

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?

 Niru December 24, 2013 21:49

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?

 ghorrocks December 25, 2013 05:28

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.

 Niru December 25, 2013 14:21

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.

 ghorrocks December 26, 2013 00:11

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.

 kiwishall December 26, 2013 05:24

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.

 Niru December 26, 2013 11:27

@Ghorrocks- thankyou for replying. I will give it a try.
@kiwiall- I modelled LNG as pure cmponent -methane.

 All times are GMT -4. The time now is 07:37.