Auto-Ignition Temperature issue

[Jesus Alberto Mejias Tuni]

Hi,

I am simulating a pool fire, by using a vent and imposing the MLRPUA in it, the issue is without using the auto ignition temperature it returns a HRR of 65.8kW as an average after 100 seconds burning, but adding the auto ignition temperature, and some minor changes in the mesh and ignitor temp, the HRR increases a lot, going beyond the 200kW, which goes way beyond the 65.3 that the pool is supposed to give, by multiplying the area the MLRPUA and the heat of combustion. So that is my issue, i am using the auto ignition temperature because my next step would be to use a mist sprinkler for extinguishing the fire, and for what i have read in the User guide is recommended to use the auto ign. temperature for this cases.

the actual mesh is 2.5cm in the inner 0.6x0.6x1.2 m, and 5cm beyond, with AIT and a mix of 5 and 10cm without AIT

That is my main issue, i also would like to know if using one mesh inside the other is advisable, like im doing here, if it is advisable to reduce the heat of combustion to achieve a lower efficiency, similar to real results where there is aprox. a 0.8 to 0.9 efficiency, at least in a case exposed in the validation guide. And if a vent is recommended for this case over using a liquid surface. 

Thank you in advance for your assistance and for any feedback you can provide, have a nice day

[Kevin]

The files should be EXACTLY the same except for the appearance of AIT in one and not the other. Otherwise, it is very difficult to diagnose a problem with AIT.

[Jesus Alberto Mejias Tuni]

Ok i modified the file without the AIT and made then the same, being the AIT the only difference and simulated it, making an average on the HRR from second 100 to 300 the HRR's are 65.6kW without AIT and 263kW with the AIT.

Regarding the first 100 seconds, the average is 64.7kW without AIT and 85.9 with the AIT, the HRR with the AIT remains low for the first 50 seconds (approximatelly lower than 15kW, and then it increases) i included the HRR file for the AIT simulation because it might be useful, thank you for your time and have a nice day

[Kevin]

I'll take a look at these. I assume you are using FDS 6.2.0, the latest version?

[Jesus Alberto Mejias Tuni]

Yes, that is correct i am using fds 6.2.0, thank you very much

El ago 31, 2015 7:20 PM, "Kevin" <mcgr...@gmail.com> escribió:
>
> I'll take a look at these. I assume you are using FDS 6.2.0, the latest version?
>

>t

[Kevin]

I suggest that you not use two meshes as you have done. The fine mesh gets boundary conditions from the coarse mesh, but the coarse mesh does not see the fine mesh at all. Thus, FDS is doing two combustion calculations -- one on the coarse mesh and one on the fine mesh. The coarse mesh calculation is so crude that the temperatures drop below the AIT and the room slowly fills with unburned fuel. This will eventually burn, giving you the high HRR.

If you want to study fire dynamics, restrict the fire to one mesh.

[Jesus Alberto Mejias Tuni]

I understand, but still the heat output is even 4 times the expected, and it shouldn't keep a heat output so high for 200 seconds if it only stocks up in fuel for 50 to 100 seconds. Anyway i will follow your recommendation and make the calculations with only one mesh and see how it works out. thanks.

[Jesus Alberto Mejias Tuni]

Pardon me, if i, may would you advise the usage of the vent and the mass flux rate, like it is applied in the script, or of a liquid surface, imposing the boiling temperature and the such, for a problem of this kind, because for me right now, in my inexperience, is really hard to prefer one over the other with a firm basis, thank you for your time. 

El lunes, 31 de agosto de 2015, 21:47:38 (UTC+2), Kevin escribió:

[Kevin]

There are some examples of pool fires in the FDS Validation Guide. The input files are here

https://github.com/firemodels/fds-smv/tree/development/Validation/Pool_Fires/FDS_Input_Files

[Kevin]

I told you that FDS was not designed to do this. Use a single mesh spanning the fire and do not overlap two meshes over the fire.

[Randy McDermott]

I want to make a clarification regarding the use of a "single mesh spanning the fire", lest this becomes lore.

FDS is not designed for overlapping meshes.  We have left this capability functional for development of embedded mesh methods and debugging mpi routines.  It should probably be disallowed until embedded mesh methods are operational.

But this does not mean that you cannot have a mesh boundary inside a fire.  I do this routinely and it works fine.  As with any mesh interface, you must monitor the velocity error and ensure you have a tight enough tolerance.  Additionally, it is probably a bad idea to have a coarse-fine mesh interface inside the fire simply because there are errors associated with a refinement boundary.

--
You received this message because you are subscribed to the Google Groups "FDS and Smokeview Discussions" group.
To unsubscribe from this group and stop receiving emails from it, send an email to fds-smv+u...@googlegroups.com.
To post to this group, send email to fds...@googlegroups.com.
To view this discussion on the web visit https://groups.google.com/d/msgid/fds-smv/42f33c94-2ac3-47d6-8e49-45f7e77f812d%40googlegroups.com.

For more options, visit https://groups.google.com/d/optout.