-
|
Has anyone encountered an issue where the simulation consistently stops or becomes stuck just before the activation of a water mist system? |
Beta Was this translation helpful? Give feedback.
Replies: 7 comments 17 replies
-
|
If you are not running the current release of FDS, try your case with the current release. If it is not working with the current release please post your input file. |
Beta Was this translation helpful? Give feedback.
-
|
I'll try your case. As a note you are not getting any significant runtime benefit with the coarser meshes. The runtime is going to be driven by the two 200x22 meshes. You might as well just use the same resolution throughout. |
Beta Was this translation helpful? Give feedback.
-
|
Thank you very much for your assistance. I will take your suggestions into account and standardize the mesh configuration accordingly. |
Beta Was this translation helpful? Give feedback.
-
|
A couple other notes now that I have looked at your geometry in smokeview: You have redefined GVEC which means a purely horizontal tunnel will behave like a tunnel on a slope; however, you have also created a geometry that is sloped. It seems like you are double counting the slope. Along with that is you have a lot of solid cells below the tunnel floor and gas cells above the tunnel ceiling in each mesh. These are sucking up computing time and resources without any impact on flow in the tunnel. |
Beta Was this translation helpful? Give feedback.
-
|
It stalled for me and I see the issue. Your sprinklers are at the minumum y side of the tunnel and you have set ORIENTATION=0,-1,0 which is pointing at the minimum y side. When a sprinkler operates, FDS picks a random location to insert a drop using the ORIENTATION and OFFSET. If that is in a solid, it tries again. In your case it is always in a solid and you are stuck in an inifinite loop. Change to 0,1,0. You also have a wall at y=0.5. Move the sprinklers a little bit toward the tunnel center to make sure they are in the gas. |
Beta Was this translation helpful? Give feedback.
-
|
If I reduce the number of gas cells and solid cells, and adjust the gravity
settings, would that help resolve the issue with my water mist/sprinkler
system not activating properly?
Jason Floyd ***@***.***>於 2025年12月16日 週二，下午11:21寫道：
… A couple other notes now that I have looked at your geometry in smokeview:
You have redefined GVEC which means a purely horizontal tunnel will behave
like a tunnel on a slope; however, you have also created a geometry that is
sloped. It seems like you are double counting the slope.
Along with that is you have a lot of solid cells below the tunnel floor
and gas cells above the tunnel ceiling in each mesh. These are sucking up
computing time and resources without any impact on flow in the tunnel.
—
Reply to this email directly, view it on GitHub
<#15728 (reply in thread)>,
or unsubscribe
<https://github.com/notifications/unsubscribe-auth/B3TC73N73IGBVJ6W4JSD4I34CAPN7AVCNFSM6AAAAACPGORGDCVHI2DSMVQWIX3LMV43URDJONRXK43TNFXW4Q3PNVWWK3TUHMYTKMRXGA2TENQ>
.
You are receiving this because you authored the thread.Message ID:
***@***.***>
|
Beta Was this translation helpful? Give feedback.
-
|
In fact, in addition to the water mist issue, I have encountered another
problem during the simulation that I have not yet been able to resolve.
Whenever the simulation reaches around 200–300 seconds, a warning appears
stating:
“WARNING: Minimum density, 0.120 kg/m³ clipped in mesh,”
and eventually the simulation stops with the error message:
“ERROR: Numerical Instability.”
Could you advise on how this issue might be resolved?
The simulation output (.out) file is attached for reference.
Jason Floyd ***@***.***> 於 2025年12月16日週二 下午11:47寫道：
… It stalled for me and I see the issue. Your sprinklers are at the minumum
y side of the tunnel and you have set ORIENTATION=0,-1,0 which is pointing
at the minimum y side. When a sprinkler operates, FDS picks a random
location to insert a drop using the ORIENTATION and OFFSET. If that is in a
solid, it tries again. In your case it is always in a solid and you are
stuck in an inifinite loop. Change to 0,1,0. You also have a wall at y=0.5.
Move the sprinklers a little bit toward the tunnel center to make sure they
are in the gas.
—
Reply to this email directly, view it on GitHub
<#15728 (reply in thread)>,
or unsubscribe
<https://github.com/notifications/unsubscribe-auth/B3TC73KFTFR6NPX2XI2W4PD4CASQBAVCNFSM6AAAAACPGORGDCVHI2DSMVQWIX3LMV43URDJONRXK43TNFXW4Q3PNVWWK3TUHMYTKMRXGA3TOMQ>
.
You are receiving this because you authored the thread.Message ID:
***@***.***>
|
Beta Was this translation helpful? Give feedback.
-
|
See if this helps: 
|
Beta Was this translation helpful? Give feedback.
-
|
As prerviously noted all the cells below the floor of the tunnel are consuming computing resources with no impact on the vehicle tunnel. The same is true for the cells above the vehcile tunnel. While there is a void space above the tunnel, it is seperated from the vehicle portion by 20 cm of concrete which has a thermal penetration time measured in hours. You also do not need to specify OBST for the exterior boundaries of the MESH. You can just use VENT. This saves a plane of grid cells on all faces. You only have 13 cells across the height of the tunnel. By removing the portions of the domain not actually participating in region with the fire you could apply those cells to increasing the resolution eslewhere. You are using WIND which is meant for outdoor flows. Either DYNAMIC_PRESSSURE on the VENT or a SURF with VEL depending on what exactly it is you are trying to do. You have a high MW fuel with no specified properties (see the guide chapter on defining species). This case ran to completion. It is your input minus domain not particpating in the vehicle tunnel, DEVC, and uneeded RAMP lines (Last two just done to make it easier to review the file). The grid size is halved and DYNAMIC_PRESSURE is used (tuned to give ~2.5 m/s with no fire). The case took about 2 days running on 20 cores. &HEAD CHID='f01'/ &MESH ID='Mesh01', IJK=200,40,26, XB=100.0,150.0,0.5,10.5,20.5,27,MULT_ID='M'/ &SPEC ID='REAC_FUEL',FORMULA='C7H12.8',SPECIFIC_HEAT=1.5/ &REAC ID='Reaction1', &MATL ID='CONCRETE', &SURF ID='CONCRETE_SURFACE', &OBST ID='CARObstruction', XB=574.5,584.5,6.0,9.0,24.5,25.0, SURF_ID='CONCRETE_SURFACE', TEXTURE_ORIGIN=0.0,5.0,0.0/ &VENT ID='L-OPEN', SURF_ID='OPEN', XB=100.0,100.0,0.5,10.5,20.5,27.0,DYNAMIC_PRESSURE=10.5,PRESSURE_RAMP='P'/ &SLCF QUANTITY='VELOCITY', PBY=5.5,VECTOR=T/ &TAIL / |
Beta Was this translation helpful? Give feedback.
-
|
I have a question about your code. &OBST ID='fire', XB=577.5,584.0,6.5,8.5,23.5,24.0, BULK_DENSITY=550.0, SURF_IDS='wood2','PLASTIC2','wood2'/ The geometric thickness of the obstruction is 0.5 m (24.0 − 23.5). 2 × 0.06 m + 0.02 m = 0.14 m What am I misunderstanding? |
Beta Was this translation helpful? Give feedback.
-
|
That is not what the SURF_IDS input means; it is not describing a set of layers. Please review the User's Guide for both SURF_IDS and BULK_DENSITY. |
Beta Was this translation helpful? Give feedback.
-
|
Thank you for your valuable suggestions. The space above the tunnel is intentionally reserved for a smoke exhaust duct, with exhaust openings on both sides of the duct. In this case, would it still be appropriate to omit the OBST definition? In addition, would modeling the domain with a single MESH affect the simulation results? |
Beta Was this translation helpful? Give feedback.
-
|
Single mesh vs. multiple meshes should have equivalent results. A single mesh in a domain this size is going to take a long time. For the exhaust shaft, do you care about what happens inside the shaft or do you just care about the impact of exhaust on the conditions inside the vehicle tunnel? |
Beta Was this translation helpful? Give feedback.
-
|
My main concern is the use of VENTs to model the smoke exhaust duct.
Specifically, I need to create openings on the VENT plane to allow smoke to
be drawn into the exhaust duct, and I am uncertain whether this approach
can properly represent the intended flow behavior. Moreover, the exhaust
duct has an irregular geometry, as in my original design.
Jason Floyd ***@***.***>於 2025年12月29日 週一，下午8:35寫道：
… Single mesh vs. multiple meshes should have equivalent results. A single
mesh in a domain this size is going to take a long time.
For the exhaust shaft, do you care about what happens inside the shaft or
do you just care about the impact of exhaust on the conditions inside the
vehicle tunnel?
—
Reply to this email directly, view it on GitHub
<#15728 (reply in thread)>,
or unsubscribe
<https://github.com/notifications/unsubscribe-auth/B3TC73OGJ6HK5WTJNKEJUKD4EENXNAVCNFSM6AAAAACPGORGDCVHI2DSMVQWIX3LMV43URDJONRXK43TNFXW4Q3PNVWWK3TUHMYTKMZWGQ4DSMQ>
.
You are receiving this because you commented.Message ID:
***@***.***>
|
Beta Was this translation helpful? Give feedback.
-
|
Do you need to know the conditions inside the exhaust duct, or do you just need to know the conditions inside the tunnel? If you need to know the detailed conditions inside the exhaust duct then you will need to resolve the flow in the duct which is going to require significantly more grid resolution than you currently have. If there is some aspect about conditions in the exhaust duct, then consider how could those objectives be met, For example, would the FDS HVAC model suffice? |
Beta Was this translation helpful? Give feedback.
-
|
In fact, I already know the exhaust flow rate required for the smoke
exhaust duct. I plan to place EXHAUST vents on both sides of the duct to
achieve this. However, my concern is that I need to create several openings
in the ceiling so that smoke can enter the exhaust duct, and I am not sure
whether this can be achieved using VENTs.
Jason Floyd ***@***.***>於 2025年12月29日 週一，下午9:08寫道：
… Do you need to know the conditions inside the exhaust duct, or do you just
need to know the conditions inside the tunnel? If you need to know the
detailed conditions inside the exhaust duct then you will need to resolve
the flow in the duct which is going to require significantly more grid
resolution than you currently have.
If there is some aspect about conditions in the exhaust duct, then
consider how could those objectives be met, For example, would the FDS HVAC
model suffice?
—
Reply to this email directly, view it on GitHub
<#15728 (reply in thread)>,
or unsubscribe
<https://github.com/notifications/unsubscribe-auth/B3TC73OEFI6F5U5AQOWZXP34EERVZAVCNFSM6AAAAACPGORGDCVHI2DSMVQWIX3LMV43URDJONRXK43TNFXW4Q3PNVWWK3TUHMYTKMZWGUZDMNA>
.
You are receiving this because you commented.Message ID:
***@***.***>
|
Beta Was this translation helpful? Give feedback.
-
|
I suggest you create a simple test case and use that to develop the inputs you need. |
Beta Was this translation helpful? Give feedback.
-
|
Is it not possible to use the model you provided, create the smoke exhaust
duct above the tunnel using VENTs, and then make openings to allow the
smoke to enter the duct?
Jason Floyd ***@***.***>於 2025年12月29日 週一，下午9:14寫道：
… I suggest you create a simple test case and use that to develop the inputs
you need.
—
Reply to this email directly, view it on GitHub
<#15728 (reply in thread)>,
or unsubscribe
<https://github.com/notifications/unsubscribe-auth/B3TC73NBW77MZWL2C3QE4YD4EESLTAVCNFSM6AAAAACPGORGDCVHI2DSMVQWIX3LMV43URDJONRXK43TNFXW4Q3PNVWWK3TUHMYTKMZWGUZTGNQ>
.
You are receiving this because you commented.Message ID:
***@***.***>
|
Beta Was this translation helpful? Give feedback.
-
|
Your current input is a large model which takes a long time to run. I would recommend you determine what is needed for your exhaust duct by creating a much simple test case in much smaller domain. I don't know what your specific ojectives are or what is or is not acceptable to your stakeholders. It is up to you to decide the most appropriate apporach and verify that it is doing what you want. |
Beta Was this translation helpful? Give feedback.
-
|
I would also appreciate your help in identifying which aspects of my simulation setup may be causing the recurring numerical instability. |
Beta Was this translation helpful? Give feedback.
It stalled for me and I see the issue. Your sprinklers are at the minumum y side of the tunnel and you have set ORIENTATION=0,-1,0 which is pointing at the minimum y side. When a sprinkler operates, FDS picks a random location to insert a drop using the ORIENTATION and OFFSET. If that is in a solid, it tries again. In your case it is always in a solid and you are stuck in an inifinite loop. Change to 0,1,0. You also have a wall at y=0.5. Move the sprinklers a little bit toward the tunnel center to make sure they are in the gas.