Time Step

[Seto]

Hi all users and developers,

My colleague is using FDS to model the flow of methane into a space
and then monitoring the volume fraction of methane. This is her input
file:

&HEAD CHID='EXPLOSION_DUMMY', TITLE='EXPLOSION_DUMMY' /

&MESH IJK=64,64,120, XB=-1.6,1.6,-1.6,1.6,0.0,6.0 /

&TIME T_END=1.0 /

&SPEC ID='METHANE' /

&SURF ID='WIND',VEL=-9.0,TMP_FRONT=34., PROFILE='ATMOSPHERIC' /
&VENT MB='XMIN', SURF_ID='WIND' /
&VENT MB='XMAX' ,SURF_ID='OPEN' /
&VENT MB='YMIN' ,SURF_ID='OPEN' /
&VENT MB='YMAX' ,SURF_ID='OPEN' /

&SURF ID='LEAK', MASS_FLUX(1)=4000, RAMP_MF(1)='leak_ramp' /
&RAMP ID='leak_ramp', T= 0., F=1.0 /
&RAMP ID='leak_ramp', T= 0.5, F=0.868 /
&RAMP ID='leak_ramp', T= 1., F=0.0 /

&VENT XB= 0.0,1.0,0.0,1.0,0.0,0.0, SURF_ID='LEAK', COLOR='RED' /

&DUMP MASS_FILE=.TRUE. /

&SLCF PBY=0.0, QUANTITY='METHANE' /
&SLCF PBY=0.1, QUANTITY='METHANE' /

&TAIL /

Now, the file runs normally but it takes a very long time to finish
the calculations. The time step for each calculation is 0.00000 s
(from the out file). Although the result can be shown if we stop the
run in the middle.
To try and get the finished results sooner, we tried defining the time
step to a larger number 0.001 s by adding the line:

DT = 0.001, LOCK_TIME_STEP=.TRUE.

The file runs normally but when it's finished, the methane
concentration won't show. The slice file will just show a blank slate.

Is this because of the time step? Is there a way to show the results?

Thank you very much,

Seto

[F-Sim.de]

Seto,
the small timestep is caused by the combination of relatively high velocities and a very small gridsize. Increasing the timestep seems not to be a good idea to me. It could lead to numerical instabilities.
If you need your results faster, I would suggest using the OpenMP-version on a system with a multicore.

Boris

[Marion Meinert]

Hi Seto,

I think you can't use FDS to model a mass flow of that amount.
Your injection of 4000 kg/sm² methane, calculated with a density of 0,72kg/m³, would cause a velocity of more than 5000 m/s (conservation of mass).
FDS is not appropriate for such high velocities.

Regards,

Marion

[Seto]

Hi Boris,

Thank you for your input. I made the gridsize very small as it is the
size of the vent. If I make it any smaller, I wouldn't be able to
specify the vent. Since your post, I tried using the OpenMP-version
but cannot get it to work. I currently use a quadcore system. So
everytime I use FDS it's only using 25% of the CPU power. When I run
the input file on the OpenMP version, the CPU usage goes up to around
60% but the calculation terminates shortly after (before finishing).
Have you used the OpenMP version succesfully?

Marion,

Thank you for telling me. I've checked and sure enough, the flowrate
is too large. We've since stopped this simulation and use other
softwares.

Thank you all for the help.

Seto.

[Robert Taylor]

Dear Seto, I often use FDS for the kind of problem you describe. However, it is not possible to calculate the first part of the release, which will be a supersonic jet. The approach I use is to calculate the first part of the release using a standard momemntum jet model such as that of Long, for the first part of the jet. The velocity falls inversely with the distance along the jet, so that you can determine the location  at which the assumpttions made in FDS become applicable Then a supply is modeled in FDS, equivalent to a cross section of the jet selected so that the gas velocity is not large.

 

FDS seems to accept velcities of as much as 40 m/s quite well - I investigated convergence for a series of locations for the representative cross section, and at velocities up to this level the results were fairly consistent.

 

I could validate the form of the jets and resulting plumes for outdor conditions by comparing with photographs, and with hand held gas monitors at the fire ground, though only at lower pressure releases.

 

The only problem with this approach is that you cannot take obstructions in the path of the jet into account. I think that at present you would need a different type of CFD program to model this, though we are gradually building up a library of simple impingement models to supplement the free jet models like that of Long.

 

With kind regards, Robert Taylor.

 

 

--
You received this message because you are subscribed to the Google Groups "FDS and Smokeview Discussions" group.
To post to this group, send email to fds...@googlegroups.com.
To unsubscribe from this group, send email to fds-smv+u...@googlegroups.com.
For more options, visit this group at http://groups.google.com/group/fds-smv?hl=en.

[Randy McDermott]

Not sure which version you are using, but I think you need

&SLCF PBY=0, QUANTITY='MASS FRACTION', SPEC_ID='METHANE' /

See, for example, section 14.3.13 of User Guide.