[cfd user]

hello people
i have a question about simulation of hydrogen dispersion in partly open space. i try model 3D simulation like in the attached file! i use species transport modeling! there one inlet with hydrogen mole concentration of 1, velocity inlet of 0.02 m/sec. there are two outlet, roof and door vent. the boundery condition of them need to be pressure outlet, in fluent when u choose pressure outlet boundery condtion, he asked u to choose species also. in the room there is ambient air, i dont know what to choose in the roof and door vent, what species, i dont want to force boundery condtion of species in the outlet, all the idea of the simulation is to see the dispersion of the hydrogen, the species in the outlet need to be obtained
alone from the result of the dispersion
if someone know how to refer to the species choice in pressure outlet, it's will help me very much

thank's
cfd-user

[mehulkumar]

Dear friend,

Species tab on Press.Outlet BC is not for fixing up your species at the outlet but to manage flow reversal you can specify the relative (min.) value in that tab.

You can read more on https://www.sharcnet.ca/Software/Flu...ug/node244.htm

Mehulkumar

[ComputerGuy]

CFD User,

mehulkumar is correct. Species outlet conditions in Fluent are used for backflow calculations; that is, if the cells near the outlet have a lower pressure than that of the outlet, one would expect flow to move from the outlet into the domain.

It's not clear to me that under steady state conditions, there should be anything but hydrogen in your domain, as your main "inlet" is pure hydrogen.

As you're modeling dispersion, you can do 2 things:

1) Set the backflow concentration to be 0 for hydrogen. If you have a species "air" or "oxygen," it should automatically be set to 1 by a mass balance. By doing this, the time it takes to fill the whole domain with hydrogen should be a conservative. That is, this is the longest time to fill the domain with hydrogen

2) Set the backflow concentration to be 1 for hydrogen. This is equivalent to having hydrogen "leak" in under backflow/negative pressure conditions. This would be non-conservative.

Hope this helps.

Regards,
ComputerGuy

Originally Posted by cfd user

hello people
i have a question about simulation of hydrogen dispersion in partly open space. i try model 3D simulation like in the attached file! i use species transport modeling! there one inlet with hydrogen mole concentration of 1, velocity inlet of 0.02 m/sec. there are two outlet, roof and door vent. the boundery condition of them need to be pressure outlet, in fluent when u choose pressure outlet boundery condtion, he asked u to choose species also. in the room there is ambient air, i dont know what to choose in the roof and door vent, what species, i dont want to force boundery condtion of species in the outlet, all the idea of the simulation is to see the dispersion of the hydrogen, the species in the outlet need to be obtained
alone from the result of the dispersion
if someone know how to refer to the species choice in pressure outlet, it's will help me very much

thank's
cfd-user

[cfd user]

thank you very much people for the help :-)

i have still problem with the simulation of hydrogen dispersion in partly open space using fluent. i try to model 3D simulation like in the attached file.
i use species transport modeling! there one inlet with hydrogen mole concentration of 1, velocity inlet of 0.02 m/sec. there are two outlet, roof and door vent. the boundery condition of them need to be pressure outlet.
i choose gravity acceleration to get something similear to the result of journal (see one of the result in the file attached)
when i calculate and get species maps in the domain, i see that in the inlet there isn't 1 mole of hydrohen, (the is the boundary condition of the inlet), it's seems that during the calclution he doesn't keep the boundery condition and gave another value small then one mole, something like 0.8 (there is a distrubution in the inlet face and it's suppose to be just pure hydrogen like i gave in the boundery condition) when i choosed without gravity acceleration (in the operating condition) he gave me one mole in inlet during of the calc, but the results doesnt seem like of the journal, it's seems strange! what should i do,
thank u all! in the journal they used the gravity acceleration!!!

[mehulkumar]

Dear friend.
Can you please give the input conditions details.
For getting input details in file go to Report->input summary.
Select all boundary cond. and get on file.

And upload it on site, so I and may be other can check it so your doubt can be clear.

Mehulkumar

[cfd user]

thank You friend, for your help,
i upload the file,
in the simulation there are three main boundery condition,
inlet: velocity inlet of pure hydrogen (1 mass/mole fraction ) with 0.02 m/sec (suppose-laminer).
door vent: pressure outlet (back flow species 0.23 - mass fraction of oxygen)
roof ventressure outlet (back flow species 0.23 - mole fraction of oxygen).
in time of t=0, in the the domain, just air (0.21% oxygen, 79% nitrogen)
Thank you very much

[cfd user]

hi, friend
i upload the fluid details, i hope u meant that. tell me if u need other details . and again, thank you very much for helping me

[mehulkumar]

Dear friend,

I re-check your BC file. I found that at inlet species specification is not done by mole fraction! It's using default specification method.

Please verify it in BC file and FLUENT model also.

Regards,
Mehulkumar Patel