[fatchang]

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 anybody there?

[A CFD free user]

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.

[fatchang]

Thanks for your reply! I will try it today.

[A CFD free user]

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.

[fatchang]

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

[A CFD free user]

Originally Posted by fatchang

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.

[fatchang]

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.

[A CFD free user]

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.

[fatchang]

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.

[A CFD free user]

Originally Posted by fatchang

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!!!

[fatchang]

Oh, I see....

[fatchang]

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.

[pchoopanya]

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


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

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:
http://www.cfd-online.com/Forums/flu...imulation.html

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

[beehuah]

Hi all,
Hope that someone is still available here. I'm simulating PEMFC with fluent using the fuel cell module. I also got the zero water saturation result and I realize that during iteration calculation, my uds-2 which is the water saturation has no calculation at all. The uds-2 remain zero throughout my calculation till almost 100 iteration.
Do anyone has any idea of whats wrong?
I have ensure that specified value for all inlet in water saturation and i have also check on the cell zone condition for channel and gdl the water content is zero.
Hope that someone can help me on this matter. thanks in advance.

[navidamin]

Originally Posted by beehuah

Hi all,
Hope that someone is still available here. I'm simulating PEMFC with fluent using the fuel cell module. I also got the zero water saturation result and I realize that during iteration calculation, my uds-2 which is the water saturation has no calculation at all. The uds-2 remain zero throughout my calculation till almost 100 iteration.
Do anyone has any idea of whats wrong?
I have ensure that specified value for all inlet in water saturation and i have also check on the cell zone condition for channel and gdl the water content is zero.
Hope that someone can help me on this matter. thanks in advance.

You can use this tutorial:
http://s000.tinyupload.com/index.php...70361651896302
Check these three with the tutorial:
1. Under relaxation factors
2. Multigrid settings
3. Inlet Conditions

[beehuah]

hi navidamin,

thanks for the reply and tutorial. I have check the tutorial and my setting for the three criteria that you stated are the same with tutorial. the water saturation iteration is still zero.

thanks

[kobe bryant]

Originally Posted by fatchang

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.

hello,Mr chang.Have you solved this problem?I meet also this problem:water saturation is approximately zero.How can you solve that?
hope your reply.

[kobe bryant]

Originally Posted by beehuah

Hi all,
Hope that someone is still available here. I'm simulating PEMFC with fluent using the fuel cell module. I also got the zero water saturation result and I realize that during iteration calculation, my uds-2 which is the water saturation has no calculation at all. The uds-2 remain zero throughout my calculation till almost 100 iteration.
Do anyone has any idea of whats wrong?
I have ensure that specified value for all inlet in water saturation and i have also check on the cell zone condition for channel and gdl the water content is zero.
Hope that someone can help me on this matter. thanks in advance.

Hello,have you solved this problem?water saturation is zero even anode and cathode RH is 100% in my simulation.Can you tell me ?thank you very much,hope to get your reply.

[sabrina sabi]

Originally Posted by kobe bryant

Hello,have you solved this problem?water saturation is zero even anode and cathode RH is 100% in my simulation.Can you tell me ?thank you very much,hope to get your reply.

please sir can you tell me how input relative humidity fuel cell in fluent please explain for me how