H2 Leak dispersion

[Vanillama]

Hello FDS community,

I am trying to model a H2 leak within a compartment and I am trying to make a comparison between VOLUME_FLOW and MASS_FLUX.

I wrote two different computation txt files and run them separately but I get different results (VOLUME_FLOW leads to greater leakage) and I do not understand why.

Below the two different lines which should, as far as I understand the guide, give the same results (but which do not, so I am wrong somewhere)

Case 1

&SURF ID = 'H2_SUPPLY_ELZ1_1', SPEC_ID(1) = 'HYDROGEN', MASS_FRACTION(1) = 1.0, VOLUME_FLOW = -0.1639, TMP_FRONT = 80.0 / 
&VENT XB = 15.0, 45.0, 0.4, 4.6, 2.6, 2.6, SURF_ID = 'H2_SUPPLY_ELZ1_1', COLOR = 'RED' / 

Case 2

&SURF ID = 'H2_SUPPLY_ELZ1_1', SPEC_ID(1) = 'HYDROGEN', MASS_FLUX(1) = 0.000117, TMP_FRONT = 80.0 / 
&VENT XB = 15.0, 45.0, 0.4, 4.6, 2.6, 2.6, SURF_ID = 'H2_SUPPLY_ELZ1_1', COLOR = 'RED' / 

In order to calculate the MASS_FLUX / VOLUME_FLOW , I did the following calculation:

H2 Leak [kg/s] = 0.01474 kg/s
Surface [m2] = 126 m2 (calculated on the basis of the corresponding VENT)
H2 density [kg/m3] = 0.08988 kg/m3

VOLUME_FLOW = 0.01474 / 0.08988 = 0.1639
MASS_FLUX = 0.01474 / 126 = 0.000117

If I understand correctly MASS_FLUX (which run with &SPEC ID = 'HYDROGEN', MASS_FRACTION_0 = 0.0 /), I should have the same result but that's not the case.

Do you know where I am wrong in the calculation ?

Below the two FDS file in case of need (MFR is the case with MASS_FLUX).
FDS_2VentsTop_MultMeshes_20cm_MFR.txt
2VentsTop_MultMeshes_20cm.txt

Thank you by advance for your help
Regards

[drjfloyd]

Read 10.1.6 in the User's Guide

[Vanillama]

I am sorry.

I already spent the whole day reading this paragraph. I can't see why I am wrong here :/

Could you point out the part of the line where the parameter is wrong please ?

[Vanillama]

I feel like both &SURF lines are correctly implemented but maybe the problem is somewhere else. Maybe with the interaction of the MASS_FLUX / VOLUME_FLOW with the assocciate VENT.

I am not sure

[drjfloyd]

Make sure your calculations are correct for the H2 density at 1 atmosphere and 80 C.

For the wall you have three boundary conditions: temperature, species mass fraction, and velocity. Temperature and species (along with the pressure inside the domain) define the density. How much mass of a species enters follows the species transport equation. That has two transport terms an advective term and a diffiusive term.

When you specifiy the velocity the mass the enters is the mass from the velocity plus an diffusion if there is a gradient between the wall BC and the gas cell. This can result in more or less mass than expected.

When you specify mass flux, the wall BC for velocity and species is set to guarantee the mass flux.

[Vanillama]

Indeed, the calculation for H2 density at 80 °C is not perfectly good and should be modified to 0,06957.

But, in that respect, it makes things worse as it leads to an increasing of the H2 VOLUME_FLOW entering the model from 0.1639 to 0.2118 and so the velocity.

For the rest, I totally understand the explaination provided. It was what I understood so far about how the model works.
I know the question can be silly. But, I really had huge deviation (I am talking about ten / 20 percents H2 volume fraction deviation / as well as huge deviation in terms of velocity).

[Vanillama]

I found this old reply on the former FDS forum and I think it can answer my issue.

[https://groups.google.com/g/fds-smv/c/7duLnLEG4I4]

In that topic, Sir David Sheppard says that it has concerned regarding the use of VOLUME_FLOW to introduce flow into a domain as he found massive errors when running its simulations in general (the topic is 11 years old so I am not sure that the answers are still relevant).
On the contrary, it recommends to use MASS_FLUX as it seems to provide the correct answer (message posted on the 31 March 2014).

You already replied this issue with the same explaination

I also noted in the User's guide paragraph this line
"Note that specifying a combination of VEL and MASS_FRACTION can lead to inaccurate results if the specif ied velocity is small because diffusion will dominate the mass transport. To obtain an accurate species mass f lux at a boundary, use MASS_FLUX." --> In my case, the velocity is definitely low as the VOLUME_FLOW is low. I thought it was only applicable to VEL but considering your reply, I guess it is also applicable to VOLUME_FLOW as well (as both are the same thing in the end).

To be faire, I would have thought that in the case of pure gas diffusion (no fire), this BC would not have lead to any issueas there are no temperature variation and therefore imposing a constant volume should not lead to such deviation comparing with MASS_FLUX.

Finally, can you confirm me that in the case of such a model, it is better to use MASS_FLUX as it is the keyword which allow a proper representation of my problem ?

Thank you by advance

[drjfloyd]

As the guide says "To obtain accurate species mass flux at a boundary, use MASS_FLUX."

[Vanillama]

Could you also confirm that it is still possible to use VOLUME_FLOW to model AIR insertion into the model through &VENT ?

I have also AIR Vent and I am concerned about how I should modelled them. As far as I understand, background species insertion at &VENT boundary is fine with VOLUME_FLOW

Thank you for the explaination.

Regards

[drjfloyd]

Any time you have the possibility of diffusive transport contributing to the mass flux, you will wind up with a different mass flux than just determined by the velocity.