LES Pool fire simulation for a circular pool

[harshad lalit]

Hello,

My name is Harshad Lalit and I am a student of Purdue University. I am trying to run an LES simulation for a 30 cm diameter liquid toluene pool fire with a flame height of approximately 1.2 m. 

1) I started by running the validation case of a 1m square methanol pool fire (methanol_1_m.fds) set up in the /Validation/Pool_Fires/ folder. I have attached a picture of the domain and the .fds file herewith. I would like to know how I can change the geometry of the pool to incorporate a circular pool and provide the mass flow rate/velocity for the liquid pool.  

2) I also had a question regarding the end time for a simulation of a pool fire. Are there any technical things to note to set a particular end time and the averaging time for a pool fire LES ? I ask because in the methanol_1_m.fds file, the end time has been set as 400 s.

Any help with the above will be deeply appreciated.

Thanks,

Best Regards

Harshad Lalit 

[Randy McDermott]

Hi Harshad,

First, thank you for using the discussion forum! :)

1) We do not currently have capability to generate circular OBST.  As you probably know, you could use RADIUS if the VENT can but put on the boundary.  But this will not capture any lip effects.  The only alternatives are (a) write a script to generate the pool or (b) use a third party tool (e.g., PyroSim or Blender).

2) If you are dealing with a real pool of a specified mass of methanol, then you would have to capture the burn out time.  For time averaging, I would play with your averaging window (both size and position) to check sensitivity of your statistics to these parameters.

Randy

--
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/c20264b2-d802-4ff6-957b-43676111de6e%40googlegroups.com.
For more options, visit https://groups.google.com/d/optout.

[harshad lalit]

Hello Randy,

Thanks for your reply.

Could you elaborate on what you meant by writing a script to generate a pool. How can this script be integrated with the FDS input file ?

Regarding the 2nd question, if I have a circular VENT with gas inflow instead of a real pool, then is the averaging time decided by the number of flow through's (Length_of_domain/Inlet_velocity) ? If this is the case then for a fire with a large flame length, the computational expense will be enormous. 

Best Regards

Harshad Lalit 

[Randy McDermott]

Attached is a script you can use to generate OBST lines that can be cut and pasted into an FDS input file (you can also write the script to simply generate the input file if you want).

The computational expense is not at bad as you are imagining.  There are numerous examples in our validation suite.  These calculations are doable.

To view this discussion on the web visit https://groups.google.com/d/msgid/fds-smv/1f048d88-7dcd-4441-9b23-6f3daa2e9095%40googlegroups.com.

[harshad lalit]

Thanks for the help. I will look into this. 

[harshad lalit]

Hi,

I have a conceptual question regarding pool fires.

To start of, I am simulating toluene gas coming out of a circular VENT, instead of a liquid toluene pool. Can the Mass Burning Rate of the liquid pool (which is specified in literature) be equated to the mass flow rate of the gas coming out of the VENT ?

Thanks,

Best Regards

Harshad Lalit 

[Randy McDermott]

Assuming pure toluene, yes.

To view this discussion on the web visit https://groups.google.com/d/msgid/fds-smv/0079240e-231a-4d38-a6fd-a856cd0af832%40googlegroups.com.

[harshad lalit]

Hello,

I tried to simulate a 30 cm diameter liquid Toluene pool fire by first assuming it as pure gas and creating a circular VENT as the mass flow inlet. The domain size was 0.7 x 0.7 x 1.2 m in the X, Y and Z directions. The mesh was 70, 70 and 60 cells in the X, Y and Z directions. 

Attached are the FDS input file and the plots of the mean temperature and radial velocity compared with experiments of Klassen & Gore, 24th Symposium, 1992 at different Z locations above the burner exit. 

Seems like I am terribly over-predicting both the radial velocity and the temperature. Is this because of a very coarse mesh chosen or is there anything wrong with my FDS input file or assumption of a gas based flow for a liquid pool fire ?

[Randy McDermott]

There are several parameters in your input file that do not make sense.  Probably the biggest one was INITITAL_UNMIXED_FRACTION=0, this will make the temps high; plus you had SUPPRESSION as FALSE and your RADIATIVE_FRACTION was too low.  Further, you had several numerical and physical parameters different from the default values.  You should have a good reason for changing these.  Here is a corrected input file.  See if this helps.

To view this discussion on the web visit https://groups.google.com/d/msgid/fds-smv/c7022874-f132-4e22-95b1-a846c0f20888%40googlegroups.com.

[harshad lalit]

Thanks for the corrections. However, I tried running the simulation with the file you gave and the temperature field after 40 s gave me just uniform temperature of 288 K throughout (I have attached the image)

I was using the 7p1_cm_methane_4mm file from the "Purdue_Flames" validation folder and the settings of the INITIAL_UNMIXED_FRACTION = 0 and SUPRESSION = FALSE were present in the file by default. Now that INITIAL_UNMIXED_FRACTION =1, it is not combusting because it is behaving like a nonpremixed flame. How can I change this ?

Also, I would like to know if modeling it as a gaseous burner is a crude assumption and would I be better off running a liquid pool as done in the experiment

Thanks,

Harshad 

[Randy McDermott]

Harshad,

Please submit an Issue.  Thanks.

Randy

To view this discussion on the web visit https://groups.google.com/d/msgid/fds-smv/6305ade2-6dd3-493a-939a-5d60082f7f4d%40googlegroups.com.

[Randy McDermott]

There is a bug in the current code related to CONVERT_VOLUME_TO_MASS.  Take out this parameter and your case should run.

[harshad lalit]

Okay, I will try this out before sending the issue. Thanks ! 

[Randy McDermott]

Actually, by reading the user guide (novel idea) I discovered that this was more of a "feature" than a bug---you have to specify TMP_FRONT if you use CONVERT_VOLUME_TO_MASS.  I added an error flag to the latest source to catch this in the future.

To view this discussion on the web visit https://groups.google.com/d/msgid/fds-smv/658763fe-e0c4-43f2-a4c8-e6fd90ecc86b%40googlegroups.com.

[harshad lalit]

So I ran the simulation with the corrections to my input file. The temperature does come down which was good, but the computed radial velocities are still overpredicted by as much as a factor of 2 (attached are the figures and the input file). 

Is there any further changes that I should incorporate into the input file ?

[Randy McDermott]

Well, I suspect, given the results, the answer is yes.  But let's continue this off line until we get things sorted out.

To view this discussion on the web visit https://groups.google.com/d/msgid/fds-smv/bdb3a26a-6f4d-45d2-9be3-21f8fa4482c7%40googlegroups.com.

[fde]

Speaking of this function, what is the benefit of it and where is it appropriate to use it?

Thank you.

[Randy McDermott]

There can be confusion over mass flux boundary conditions.  The safe bet is to always use MASS_FLUX.  But some users have expected to be able to set VEL and MASS_FRACTION and get that specified mass flux (without accounting for the diffusive flux).  I think I discuss this in the guide.  But when you specify VEL, this is a VOLUME flow rate out the SURF.  If you prefer to use that bc and you want it to represent a specific MASS_FLUX then you would add this CONVERT_VOLUME_TO_MASS option.  This is discussed in detail in Sec. 9.1.6 of the user guide.

To unsubscribe from this group and stop receiving emails from it, send an email to fds-smv+unsubscribe@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/8c0728e3-75d6-41af-a9ca-04b18b18645d%40googlegroups.com.