vent with volume flux/velocity

[Evangelos Tzanidis]

Hello everyone,

I am replicating a scenario of an atrium fire in FDS6.0.1.

At the top of my domain (rectangular atrium 20m x 20m x 20m) I have two square exhaust vents (0.54m x 0.54m each) with fans producing a volume flux of 3.8m^3/s.

In order to achieve the required flow, I applied VOLUME_FLUX on a SURF line and used it as an input to my VENTs.

In my results, the velocity at the centre of the exhaust (found by using a DEVC) is around 10m/s, thus resulting in a volume flux of 2.9m^3/s (VOLUME_FLUX=u*A) instead of 3.8m^3/s.

I have aligned the vent with the mesh so there is no error in the area. Furthermore, the reduced exhaust flow is also proven by a very big smoke layer, compared to experiments.

I also attempted to assign velocity (13 m/s) as an input, instead of a volume flux, but it gave me the same results.

What could explain this?

Thank you in advance,

Evangelos

p.s. I have attached the input file

[Randy McDermott]

You should use the wall output quantity 'VOLUME FLOW WALL', see sec 16.9.11 (end) for a discussion.  You will see that your volume flow is correct (I checked it)---there may be other reasons for your problems with the smoke layer.  The gas phase quantities are subject to interpolation error, which is large on your coarse grid.  You should also tighten your velocity tolerance.  You have errors of nearly 10 cm/s near your burner mesh boundary.

&PRES VELOCITY_TOLERANCE=1.E-3, MAX_PRESSURE_ITERATIONS=100/

&DEVC ID='Vol Flow', XB= 1.35, 1.89,-0.27, 0.27, 18.35, 18.35, QUANTITY='VOLUME FLOW WALL', IOR=-3 /

--
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/2a9aedb1-7d21-46a7-9ebb-4ba3fbf66660%40googlegroups.com.
For more options, visit https://groups.google.com/groups/opt_out.

[Evangelos Tzanidis]

Thank you very much for your immediate response!!

I just noticed the velocity tolerance problem, it must have had a major impact on my simulation's accuracy.

Regarding the volume flow through the vent, I changed the QUANTITY to 'VOLUME FLOW WALL' and it gave me the following error:

ERROR: DEVC QUANTITY VOLUME FLOW WALL not found

forrtl: error (78): process killed (SIGTERM)

I couldn't find the quantity in the user manual either. Could it be that you did a typo?

Best Regards,

Evangelos

[Randy McDermott]

This is a pretty new feature.  I thought it was in 6.0.1, but maybe not.  It will be in the next release, though, 6.1.0, or you can compile the latest SVN.

To view this discussion on the web visit https://groups.google.com/d/msgid/fds-smv/10f76efe-de4a-403d-980e-49e3b96b8849%40googlegroups.com.

[Evangelos Tzanidis]

Hello,

I am sorry to disturb you again guys but it seems like my problems with this scenario are continuing to persist.

I am trying to replicate the results of an experimental study* in FDS6. When I compared my predictions to the results of the study I found out that my smoke layer thickness grows very rapidly and the final smoke layer height falls much lower than expected. That indicates either that:

 

1. too much smoke is produced by the fire or that 

2. not enough smoke is extracted through the exhaust vents on the roof.

The HRR of the fire appears to be correct (in the csv file) and I think that the soot and CO yields are correctly assigned, so my guess is that the problem is in the vents.

So, I placed DEVCs to measure the VOLUME FLUX through the exhaust vents and obtained 3.26 m3/s instead of 3.8 m3/s, which was the value that I assigned.

Therefore, I think that the under-performing exhaust vents cause my problem. Could you possibly have a look at my most recent input file (attached) and tell me how to fix the volume flux of the exhausts?

Thank you very much for the help!

*Gutiérrez-Montes C, Sanmiguel-Rojas E, Viedma A, Rein G. Experimental data and numerical modelling of 1.3 and 2.3 MW fires in a 20 m cubic atrium. Building and Environment 2009;44(9)  1827-1839

[dr_jfloyd]

or 

3) meshing needs improvement

Meshes are solved independently and then stitched together. You have a large number of meshes with only a handful of grid cells across them.  I would not recommend this.

Your fire resolution is over 0.4 m.  This is a very coarse grid for a 1 or 2 MW fire.  The paper you refer to recommended D*/dx = 10 to 15 and you have 2 to 3

4)considering experimental error

examples:

the paper states the estimated error on the fan flow measurement is 10 %.

the paper states that the fire heat release was not directly measured but was scaled based on a much smaller pool (paper estimates the error of this at 15 %)

5) inputs vs. experiment description

examples:

the paper estimates the burning efficiency of the heptane was 85 %.  Your inputs give an efficiency of 97 %

the real building has a prismatic roof with a total height of 20 m.  Your inputs are for a flat roof with a  total height of 18.6 m.

[David Sheppard]

I would be very critical of any results that used VOLUME_FLUX to introduce flow into a domain.  I found massive errors when using VOLUME_FLUX to model a gas leak.   

 

Run the same scenario using MASS_FLUX and compare your results.  I know that MASS_FLUX provides the correct answer because I ran a series of models and integrated the results.

[dr_jfloyd]

Dave,

Your issue was you were trying to use volume_flux to inject a specific flux of a species. This is prone to diffusive errors which is why we state in the user's guide to use massflux when trying to do this. You had the correct volume flow but not species due to diffusion. If you were just injecting the background species, volume_flux would have worked. In this case the user is removing a volumetric flow, so your comment does not apply.

[David Sheppard]

I would still run a case with MASS_FLUX to see if FDS provides the same answer.  The explanation as to why FDS cannot introduce a species with VOLUME_FLUX and it can when using MASS_FLUX does not make sense to me.  I hope that FDS has been modified to not allow SPECIES with a VOLUME_FLUX since it provides bad results. 

[dr_jfloyd]

For a simulation with a fire, MASS_FLUX and VOLUME_FLUX for an outlet flow are not equivalent boundary conditions.  VOLUME_FLUX imposed a constant wall velocity that does not change with temperature.  Therefore, as the fire size increases, the temperature will increase, the density will decrease, and while the volume flow will be constant the mass flow will decrease due to the reduction in density.  MASS_FLUX maintains a constant mass flow, but does this by changing the wall velocity.  Because of this, running M. Tzanidis's input with VOLUME_FLUX and MASS_FLUX would be expected to result in similar but not identical simulations.  

[Evangelos Tzanidis]

Dear dr_jfloyd

Thank you for your immediate and thorough response.

1. You are absolutely right about the mesh quality, but my problem insists throughout all my meshes (my finest mesh has D*/dx=10). 

So I think that the source of the problem lies elsewhere.

2. Regarding the experimental errors, I did not consider them and that was a big mistake of mine. 

I am thinking of performing a sensitivity analysis on the volume flux and HRR, so that I can quantify their effect and identify whether my predictions improve for any of the cases.

Do you think this would be  good idea?

3. Regarding the geometry, there is another study by the same people*, which indicated that approximating the roof as a flat plate does not cause any deterioration in the predictions, as long as the volume of the atrium is kept constant.

4. I could not find any information on how to calculate the soot and CO yields from the combustion efficiency. The values that I have used in my simulations are those for a well ventilated Heptane fire (obtained from SFPE handbook of fire protection engineering). Can you suggest a better way of estimating these values?

5. Regarding the volume flux errors (3.2 instead of 3.8 m3/s), do you think that they are caused by some of the above or could they be another separate problem?

Thank you for all the help!

Evangelos

*Ayala P, Cantizano A, Gutierrez-Montes C, Rein G. Influence of atrium roof geometries on the numerical predictions of fire tests under natural ventilation conditions. Energy and Buildings 2013;65  382-390

[dr_jfloyd]

2. Generally a good idea to have some understanding of how uncertainty can impact your calculation.  Consider looking at NFPA 92B's calculation approach for atrium smoke control.  In a few minutes with the correlations you should be able to estimate the impact on layer height given the uncertainty in exhaust and fire size.  

4.  combustion efficiency is actual heat release rate divided by the maximum possible heat release rate (e.g. complete combustion).  Any carbon that goes to soot or CO represents unrealized heat release rate and the more of each you make the lower your combustion efficiency.  

5. If you want to measure volume flux, use a VOLUME FLOW device rather than a VELOCITY device.  Extrapolating a single point velocity measurement over a larger area will have error.

[Brad Casterline]

Brian, the example jet_fan, in the Flowfields folder, shows you how to do that.
Brad

[fde]

As far as I understand VOLUME FLOW WALL is used for measuring volume flow of a gas that passes through an object surface (inlet or outlet). What is the main reason to introduce this different DEVC ID? Why cannot the regular DEVC be used for walls as well? 

[Randy McDermott]

VOLUME FLOW is a GAS PHASE OUTPUT, whereas VOLUME FLOW WALL is a SOLID PHASE OUTPUT.  The former may snap to the wrong face and have an O(DX) error for the velocity component.  If you want to ensure you get the correct WALL value, use VOLUME FLOW WALL.

On Tue, Sep 12, 2017 at 3:52 AM, fde <yilmaz....@gmail.com> wrote:

As far as I understand VOLUME FLOW WALL is used for measuring volume flow of a gas that passes through an object surface (inlet or outlet). What is the main reason to introduce this different DEVC ID? Why cannot the regular DEVC be used for walls as well? 

--

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+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/c23dfdcd-331e-472f-b0e2-dd77f1baf872%40googlegroups.com.
For more options, visit https://groups.google.com/d/optout.

[fde]

So the whole idea is just a prevention of snapping and the wrong use.  IOR is a must in all WALL outputs, also I understand. 

Thank you.  

On Tuesday, September 12, 2017 at 12:32:32 PM UTC+2, Randy McDermott wrote:

VOLUME FLOW is a GAS PHASE OUTPUT, whereas VOLUME FLOW WALL is a SOLID PHASE OUTPUT.  The former may snap to the wrong face and have an O(DX) error for the velocity component.  If you want to ensure you get the correct WALL value, use VOLUME FLOW WALL.

On Tue, Sep 12, 2017 at 3:52 AM, fde

As far as I understand VOLUME FLOW WALL is used for measuring volume flow of a gas that passes through an object surface (inlet or outlet). What is the main reason to introduce this different DEVC ID? Why cannot the regular DEVC be used for walls as well?