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

No liquid water exist in my Fuel Cell simulation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 26, 2014, 17:52
Default No liquid water exist in my Fuel Cell simulation
  #1
New Member
 
Join Date: Feb 2014
Posts: 8
Rep Power: 3
fatchang is on a distinguished road
Hi guys,

I am using the PEMFC module to simulate a pemfc with the single serpentine flow field. In the figures, the water saturation and water content in channels and gdls are 0, which means there is no liquid water and water vapor. However, the mass fraction of water is bigger than 0. So, I am confused.

I have done these things:

1. enable the multiphase in PEMFC panel;

2. set the Realitve Humidity to 100% by adjusting the species mole fraction at the inlets.

3. set the solution zones of UDS 2 and 3 as all zones, which enables the water saturation and water content for simulation.

pic1: Contours of Static Pressure. (channel_cathode)
pressure of ch_c.jpg

pic2: Contours of mass fraction of H2O.(channel_cathode)
mass fraction of water ch_cathode.jpg

pic3: Contours of water saturation. (channel_cathode)
water saturation of ch_c.jpg

pic4: Contours of water content. (gdl_cathode)
water content of gdl_c.jpg

pic5: Contours of mass fraction of H2O (gdl_cathode)
mass fraction of water gdl_c.jpg

My first question is whether I set the parameters incorrectly. Then, you can see that the mass fraction of water is bigger than 0 (pic.5), but the water content is 0(pic.4). Is it possible that I set the contours for UDS incorrectly?
The third question is what else I need to do if I want to get liquid water(water saturation>0) in the channel and gdl.

Look forward to your reply!

Qichang
fatchang is offline   Reply With Quote

Old   February 27, 2014, 11:54
Default
  #2
New Member
 
Join Date: Feb 2014
Posts: 8
Rep Power: 3
fatchang is on a distinguished road
Is anybody there?
fatchang is offline   Reply With Quote

Old   February 27, 2014, 19:37
Default
  #3
Senior Member
 
A CFD free user's Avatar
 
A-A Azarafza
Join Date: Jan 2013
Posts: 187
Rep Power: 4
A CFD free user is on a distinguished road
Hi fatchang,
I suppose, you should set the value of water saturate(not flux) in both inlets zero. The value of water content in both GDL and channels must be zero as well. Fix it using cell zone condition. Try this and tell me if it works.
__________________
Regard yours
A CFD free user is offline   Reply With Quote

Old   February 27, 2014, 19:38
Default
  #4
New Member
 
Join Date: Feb 2014
Posts: 8
Rep Power: 3
fatchang is on a distinguished road
Thanks for your reply! I will try it today.
fatchang is offline   Reply With Quote

Old   February 27, 2014, 19:58
Default
  #5
Senior Member
 
A CFD free user's Avatar
 
A-A Azarafza
Join Date: Jan 2013
Posts: 187
Rep Power: 4
A CFD free user is on a distinguished road
One more thing, generally, water content is not defined in GDL zones. I mean that water content is defined for membrane and catalyst layers. So, you shouldn't expect of existing saturate water in GDLs. Another thing usually some guys forget while making contour is that they check "global range", Uncheck it and see how it goes.
__________________
Regard yours
A CFD free user is offline   Reply With Quote

Old   February 27, 2014, 21:10
Default
  #6
New Member
 
Join Date: Feb 2014
Posts: 8
Rep Power: 3
fatchang is on a distinguished road
I check my case file just now. In my former simulation, I have set the value of water saturate(not flux) in both inlets as zero. And the default value of water content in both GDL and channels was fixed to zeros in cell zone condition. So I do not change anything in my case file actually.

For the contours, I also uncheck the "Global Range" and make contours for catalyst and membrane. Er, I cannot upload the figures in quick reply. The value of water content in catalyst layers and membrane is none zero. However, the value of water saturation is still zero. I don't know why.

One more question, if the temperature of all the inlets and outlets is 353K, how to set the temperature in Solution Initialization? I want to know what's the mechanism that make the water vapor condense into liquid water in catalyst and membrane.

Thanks for your help,

Qichang
fatchang is offline   Reply With Quote

Old   February 28, 2014, 07:50
Default
  #7
Senior Member
 
A CFD free user's Avatar
 
A-A Azarafza
Join Date: Jan 2013
Posts: 187
Rep Power: 4
A CFD free user is on a distinguished road
Quote:
Originally Posted by fatchang View Post
I check my case file just now. In my former simulation, I have set the value of water saturate(not flux) in both inlets as zero. And the default value of water content in both GDL and channels was fixed to zeros in cell zone condition. So I do not change anything in my case file actually.

For the contours, I also uncheck the "Global Range" and make contours for catalyst and membrane. Er, I cannot upload the figures in quick reply. The value of water content in catalyst layers and membrane is none zero. However, the value of water saturation is still zero. I don't know why.

One more question, if the temperature of all the inlets and outlets is 353K, how to set the temperature in Solution Initialization? I want to know what's the mechanism that make the water vapor condense into liquid water in catalyst and membrane.

Thanks for your help,

Qichang



Initialize energy equation with temperature 353 (the value you already used in inlets). When the energy equation is solved, the temperature distribution will be different form the value you used in initialization. Respecting to the mechanism which turns water vapor into liquid (condensation), I think, the answer is the difference between water vapor pressure (Pwv) and the pressure of saturate vapor (Psat).
P.s. which operating voltage are you working? Maybe you'd better change the operating voltage and examine the results again. Did you check the multiphase option in define fuel cell model box already? How about the contact angle in both anode and cathode CL? I'm quite sure you ignored one thing. Be in touch and keep me updated. Are you really solving saturate water equation? Have a look at the " solution controls" and see if the water saturate equation is highlighted.
__________________
Regard yours
A CFD free user is offline   Reply With Quote

Old   February 28, 2014, 14:46
Default
  #8
New Member
 
Join Date: Feb 2014
Posts: 8
Rep Power: 3
fatchang is on a distinguished road
I understand the mechanism now. Thanks, you are so nice.
The operation voltage is 0.5V now. I have try other values already, the results are similar to this one. If you are talking about the Models->PEMFC->model panel->Multiphase, I have check this option already. The contact angle of Catalyst and GDLs in both anode and cathode is 110. Is anything wrong with this value? Do I need to remain the value of Catalysts as 0?
For the equations of water saturation and water content in "Solution Control", they are highlighted.
Er, could you give me an effective sample case file, or help me check my case file? If you are willing to check my file, I can share a link on dropbox. Thus, you can download it directly.
fatchang is offline   Reply With Quote

Old   March 1, 2014, 16:09
Default
  #9
Senior Member
 
A CFD free user's Avatar
 
A-A Azarafza
Join Date: Jan 2013
Posts: 187
Rep Power: 4
A CFD free user is on a distinguished road
First, thanks for the positive words.
Well, regarding case file, there are many case studies you can find in the literature. But, the tutorial provided by Fluent is the first one which anyone who wants to start it's way in PEMFC uses first. Respecting to if I'm able to check your results, I will send you a private email. Please check it.
__________________
Regard yours
A CFD free user is offline   Reply With Quote

Old   March 1, 2014, 16:25
Default
  #10
New Member
 
Join Date: Feb 2014
Posts: 8
Rep Power: 3
fatchang is on a distinguished road
Yes, I also built the case file in the tutorial as you mentioned. I followed every step. When the voltage is 0.75V, the current density is 0.24A/cm2. It is almost 25% different from the 0.324A/cm2 in the tutorial. I checked the file for many times, however, I did not find the way to solve the problem.

Look forward to your private email.
fatchang is offline   Reply With Quote

Old   March 1, 2014, 16:32
Default
  #11
Senior Member
 
A CFD free user's Avatar
 
A-A Azarafza
Join Date: Jan 2013
Posts: 187
Rep Power: 4
A CFD free user is on a distinguished road
Quote:
Originally Posted by fatchang View Post
Yes, I also built the case file in the tutorial as you mentioned. I followed every step. When the voltage is 0.75V, the current density is 0.24A/cm2. It is almost 25% different from the 0.324A/cm2 in the tutorial. I checked the file for many times, however, I did not find the way to solve the problem.

Look forward to your private email.
Oh Oh, that's the point you're making wrong. I'm quite sure that if you had gone the correct way, you should've received a value equal to 0.324 or something near to it. I can't recall the fourth digit right now. I did this part many times, so, I know what the final value should be!!!
__________________
Regard yours
A CFD free user is offline   Reply With Quote

Old   March 1, 2014, 16:39
Default
  #12
New Member
 
Join Date: Feb 2014
Posts: 8
Rep Power: 3
fatchang is on a distinguished road
Oh, I see....
fatchang is offline   Reply With Quote

Old   March 5, 2014, 12:30
Default
  #13
New Member
 
Join Date: Feb 2014
Posts: 8
Rep Power: 3
fatchang is on a distinguished road
I get some new results these days. The IV curve, water content, water saturation and pressure distribution seem reasonable. However, the velocity is too high. I will send you private message right now, please check it.
fatchang is offline   Reply With Quote

Old   March 19, 2014, 07:28
Default
  #14
New Member
 
Join Date: Aug 2011
Posts: 13
Rep Power: 5
pchoopanya is on a distinguished road
Hello Qichang and Everyone,

My apologies for not replying promptly. I hardly come to this site and log in to check my inbox.

Regarding your question, have you sorted it out?

Personally, I would say, do not be confused with WATER MASS FRACTION and WATER SATURATION and WATER CONTENT

First, mass fraction of water only applies to water VAPOUR, yes! I had the same problem until I figured it out. According to the species transport equation, what you see for the X_h20 is the water vapour, not liquid water

So, in your case... the non-zero mass fraction of water (vapour) does not contradict to the zero water saturation...

Because the water saturation applies to the LIQUID water, it tells you how much the space in the pore is occupied by the liquid water. Your result only suggests that there is water vapour in the channel but the condition may not be appropriate for these water vapour to condense into liquid water... (the conditions can be the water vapour pressure reaches its maximum which is the saturation pressure). We can check this by referring to the WATER ACTIVITY... lower than 1 indicates VAPOUR while greater than 1 indicates LIQUID water

So now you have a hint of the first two, let's move on to the WATER CONTENT... this is also the LIQUID water, but they are the water in the membrane... the higher value, the better protonic conductivity and hence higher current. It is nothing to do with liquid water in the channel so you can just ignore it.

If you wanna see the liquid water, yes, you were on the right track to increase the RH%. One thing I would suggest is to decrease the voltage (hence increase the reaction), say, 0.3V? You could see that the water vapour condense to form liquid water.... You can prove this by looking at WATER ACTIVITY contour... the area with higher than 1 indicates there is some liquid water condensed from vapour.

Regarding modelling the two phase flow in the channel, do you mean you wanna see and show the liquid water accumulating on, for example, the channel walls? I saw one paper they modelled this but they do not use the PEMFC model. They did not include the electrochemical reaction, what they did was they just input the liquid water as a SOURCE term within the GDL so they emerged into the channel. The liquid water was then visualised or tracked by the interface between liquid water and gas phase using Volume of Fraction (VOF) model - check this out, I'm sure it's in FLUENT as I replicated their study once.... Interesting, but still lacking some reality.

So, to summarise, I think all you have to do is to decrease the voltage and then visualise the liquid water by looking at WATER ACTIVITY. This is all we can do as far as I know as PEMFC add-on module does not include the VOF model. By combining them, of course would be awesome which I don't know the possibility of this. Someone has a clue?

My personal experience suggests that the water saturation level is very very low though you are using 100% RH% for both gases and at low operating voltage. I do not know why either. Ironically, our flow-field design is far too effective so that the water removal ability is soooooo great and no liquid water left!?!! I am trying to see whether the GDL pore is blocked by liquid water as well - by looking at the water saturation, but this is too low to believe that the pore is blocked. Any suggestion?

PL - I am replying this in your original thread because I think it would be more useful as everyone can see and discuss to further our understanding.

Please feel free to correct me! I really need it! and give me answer to my question also.



Regards,

Pattarapong


================================================== ===========


Quote:
Originally Posted by fatchang
Hi pchoopanya,

How are you?

I find your discussions on PEMFC on the CFD Online forum. I am using the PEMFC module to simulate a pemfc with the single serpentine flow field. However, I meet some problems and can not solve them until now. Could you give me some advises?

In the contours, the water saturation and water content in channels and gdls are 0, which means there is no liquid water and water vapor. However, the mass fraction of water is bigger than 0. So, I am confused.

I have done these things:
1. enable the multiphase in PEMFC panel;
2. set the Realitve Humidity to 100% by adjusting the species mole fraction at the inlets.
3. set the solution zones of UDS 2 and 3 as all zones, which enables the water saturation and water content for simulation.

Because I cannot send pictures by the website, you can check the pictures of results through the link:
No liquid water exist in my Fuel Cell simulation

From your experience, What I need to do if I want to get liquid water in the channels and gdls, means make the multiphase module work?

Look forward to your reply!

Sincerely,
Qichang
pchoopanya is offline   Reply With Quote

Reply

Tags
water content, water saturation

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
modeling empirical fuel in liquid fuel combustion Hayder Mohammed FLUENT 0 August 7, 2013 03:06
Displying interface of liquid water using VoF model pchoopanya FLUENT 2 March 15, 2013 17:42
PEM fuel cell simulation pchoopanya Mesh Generation & Pre-Processing 0 March 11, 2013 14:22
Cells with t below lower limit Purushothama CD-adapco 2 May 31, 2010 21:58
Help! Warnings on liquid fuel combustion Julie CD-adapco 0 August 31, 2004 10:58


All times are GMT -4. The time now is 02:46.