Pressure rise induced by fires in tunnels

[Matteo Pachera]

Dear users,

I'm currently trying to model a simple tunnel with a fire in the center of it, but I found some odd results when I looked at the pressure distribution. 

In my model I used a single mesh for the discretization of the domain to reduce the spurious fluctuations of the pressure. To induce the longitudinal flow in the tunnel I imposed different pressures at the portals. I ran my model with two different grids resolutions and I compared the results. The fine grid has cubic cells of 0.25 m size and the coarse one had cubic cells of 0.50 m size. I attach the input file I used for the simulations from which I deleted several outputs, for sake of simplicity.

I attach the profiles of the pressure and temperature along the tunnel and the velocity and the pressure as function of time. The velocity and the temperatures show the same trend in both simulations, but the pressure profiles show much larger differences. I lowered the convergence criteria for both pressure and velocity errors and in both cases the simulations converged to the imposed criteria, so I don't expect any error due to divergence of the results.

I'm wondering if these pressure profiles have a physical meaning of if they are only consequence of numerical effects and eventually how can I improve my results.

Thanks a lot

Matteo

[Kevin]

I would not consider these pressure fluctuations "spurious". Fluctuations on the order of 10 Pa are normal in a fire scenario.

[Matteo Pachera]

I agree with your that these fluctuations are relatively small, but what made me suspicious about the solution is the rising pressure in the first part of the tunnel. I expected the pressure to decrease upstream the fire as the air flows in the tunnel from left to right. 

[Randy McDermott]

Have you plotted the mean x velocity?

--
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/1336f700-1940-4cfe-a1a7-2e3e9847b973%40googlegroups.com.

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

[Matteo Pachera]

I plotted the average velocity at the inlet of the tunnel. I calculated that as volume flow divided by the area of the tunnel's cross section.

On Friday, 25 August 2017 14:49:18 UTC+2, Randy McDermott wrote:

Have you plotted the mean x velocity?

On Fri, Aug 25, 2017 at 8:39 AM, Matteo Pachera <matteo.p...@gmail.com> wrote:

I agree with your that these fluctuations are relatively small, but what made me suspicious about the solution is the rising pressure in the first part of the tunnel. I expected the pressure to decrease upstream the fire as the air flows in the tunnel from left to right. 

On Friday, 25 August 2017 14:29:56 UTC+2, Kevin wrote:

I would not consider these pressure fluctuations "spurious". Fluctuations on the order of 10 Pa are normal in a fire scenario.

On Friday, August 25, 2017 at 7:56:37 AM UTC-4, Matteo Pachera wrote:

Dear users,

I'm currently trying to model a simple tunnel with a fire in the center of it, but I found some odd results when I looked at the pressure distribution. 

In my model I used a single mesh for the discretization of the domain to reduce the spurious fluctuations of the pressure. To induce the longitudinal flow in the tunnel I imposed different pressures at the portals. I ran my model with two different grids resolutions and I compared the results. The fine grid has cubic cells of 0.25 m size and the coarse one had cubic cells of 0.50 m size. I attach the input file I used for the simulations from which I deleted several outputs, for sake of simplicity.

I attach the profiles of the pressure and temperature along the tunnel and the velocity and the pressure as function of time. The velocity and the temperatures show the same trend in both simulations, but the pressure profiles show much larger differences. I lowered the convergence criteria for both pressure and velocity errors and in both cases the simulations converged to the imposed criteria, so I don't expect any error due to divergence of the results.

I'm wondering if these pressure profiles have a physical meaning of if they are only consequence of numerical effects and eventually how can I improve my results.

Thanks a lot

Matteo

--
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.

[Randy McDermott]

Matteo,

At the moment, the best I can do is to point you to Eq. (4.70) in the FDS Tech Guide.  The DYNAMIC_PRESSURE sets \tilde{p}_{ext} in this equation.

I am not sure if you trying to do this, but a key point is that DYNAMIC_PRESSURE cannot be used as a static pressure drop in the tunnel.  If you had no losses in a tunnel or duct (set FREE_SLIP=T on walls), and no fire, then if you specify 50 Pa as the DYNAMIC_PRESSURE at the inlet to the domain the volume flow will adjust to give a velocity of 0.5*U^2 = 50/1.2 or U = 9.1 m/s.  But the static pressure drop in the duct would be zero (no losses, no pressure drop).

I've mentioned this in posts before, but if you know the volume flow, then that is the bc you should set for inflow.  If you do this for your case, you will see the PRESSURE decease along the tunnel as you expect.  This should be the correct physical pressure (relative to the pressure at the outlet).

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/2f9f3da6-acfc-4faf-afdf-db9a23ef503a%40googlegroups.com.

[Matteo Pachera]

I chose my boundary conditions because I expected that a total pressure inlet and a static pressure outlet will guarantee the maximum stability to the calculation. As well setting the pressure at the portals I expected to limit the fluctuations along the tunnel.

I will try a similar case and I will send you the results as soon as they are ready.

Regards

Matteo

[Matteo Pachera]

I simulated the same case imposing the velocity at the inlet and the pressure at the outlet. Now the results look much better but I would like to have similar results also using the pressure boundary condition. When I simulate a tunnel I often impose atmospheric pressure at the portals, so I don't really impose the velocity in the simulation.

[Randy McDermott]

Matteo,

I am working on a fix for this.  My current theory is that the freedom we give to an "OPEN" boundary create fluctuations at the inlet that eventually settle out (pressure recovers).  By specifying the velocity directly we take more control over the normal and tangential velocity components at the inlet.  In theory, we can do the same when we impose a pressure boundary condition.  But this will require some surgery.

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/57419dfc-862e-449e-8040-bd0372758305%40googlegroups.com.

[Matteo Pachera]

Thanks for your support

[Matteo Pachera]

Dear Randy, I forgot to ask you if this issue is going to be fixed in the next minor release? And eventually when are you planning to release it?

Thanks again

Matteo

[Randy McDermott]

Sorry, I got sidetracked. But the current state of affairs is that with a coarse grid the pressure loss with dynamic inlet behaves closer to the velocity inlet.  With fine grid resolution we see H climbing.  I don't quite have my arms around the problem.  For now, we have to assume using velocity (or volume) inlet is the preferred method.

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/79260b2d-b602-4a03-954a-97ba5c7afdb9%40googlegroups.com.

[Matteo Pachera]

I made some further simulations with my basic setup changing the power of the fire and the grid size. The results show that with some low values of HRR (3 MW) the simulation runs smoothly also with a refined mesh (0.25 m grid size, Mesh 3), but when the fire power rises the pressure shows a strange profile. I tried to increase the grid size (0.5 m, Mesh 2 and 1 m, Mesh 1) and I compared the results with those obtained in the previous case. For the mesh with 0.5 m cells the pressure is still reasonable up to 9 MW, but for higher values the pressure rises again. For the coarse grid with 1 m cells the pressure shows a good trend for all the values of HRR up to 15 MW, but the results, comparing the longitudinal velocity, are not mesh independent, so I wouldn't rely on them so much.

I attach some of the results I obtained: the velocity along the tunnel for different fire powers and grids sizes, the pressure along the tunnel for different grid's sizes and the temperature. 

Is there any parameter on which I would work in order to attenuate the pressure rise? Moreover I would like to know how can I obtain the same longitudinal velocities for mesh 2 and mesh 3 even if the pressure gradient in the tunnel are so different? I have another small question about the possibility to calculate the mass averaged temperature in the tunnel, now I'm using the simple area average temperature but it is not so correct. Is there any statistics parameter I could use to evaluate the mass averaged value of a variable?

Thanks again for your support,

Matteo

[Randy McDermott]

You could use

STATISTICS=’MASS INTEGRAL’

but the temperature is already the Favre-filtered temperature (local mass average), so you would be double counting the mass.

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/70e52600-58cf-4fbe-aab3-06b233d0e213%40googlegroups.com.

[Matteo Pachera]

So just to check if I understood correctly: the MEAN temperature evaluated by FDS is calculated as the integral over the area of the local mass flow times the temperature divided by the total mass flow. 

[Randy McDermott]

Favre averaging is discussed in the tech guide.  In short, a Favre averaged field is locally int(rho*T)/int(rho), where int is the integral over the cell volume.  This is what FDS stores in TMP(I,J,K).  If you want further spatial or temporal averaging, use the STATISTICS outputs discussed in 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/4d3de6cd-c937-4c36-96dc-64bab46e79ae%40googlegroups.com.

[Matteo Pachera]

I read that section but I didn't realised the effect of the Favre averaging. I think I will need something different that the simple Favre average because I would like to calculate the temperature as int(rho*cp*T*u)/int(rho * u *cp).

[Randy McDermott]

This is a velocity weighting applied to the enthalpy.  Understand that the "int" is implicit, since we do not actually have the resolved fields.  All in all, I really don't see any benefit over just taking MEAN of TMP.

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/facda9b6-c4ee-4bb9-a4f8-912c937e1602%40googlegroups.com.

[Matteo Pachera]

Honestly at the moment I'm working with the MEAN temperature, but sometimes for comparison with other models I would like to calculate the mass average temperature or velocity weighted enthalpy. But this was just a secondary question, more a doubt I had. 

The main issue I'm facing is regarding the pressure in the tunnel, apparently with a really poor mesh I obtain pressure profiles that have a more reasonable trend than those which I obtain with refined grids. I would like to understand a bit better what are the parameters influencing this effect and how could I limit it? I know that the problem cannot be solved at the moment but maybe there are some ways to go around it.

[Randy McDermott]

I can just reiterate my current observations and thoughts.

1. I believe the momentum equation is balanced.  The mean H field is rising and this is most likely being balanced by a fluctuation, DUDT, at the inlet.  This is why prescribing velocity (volume flow) works.  It is a Neumann condition for pressure (H), whereas when you specify dynamic pressure you are specifying a Dirichlet condition for H and this allows DUDT/=0.

2. It appears that higher fire powers exacerbate this effect, which makes some sense to me.

3. Coarse grids have higher turbulent viscosity, which I think helps dampen the fluctuations.

I also think there is an inconsistency in what FDS means by "dynamics pressure" as a boundary condition.  Let's define total pressure p as p_s (static) + p_dyn (dynamic).  DYNAMIC_PRESSURE is really treated like a static pressure in the code.  My question to you is: which do you really mean to implement?  Because if you know the dynamic pressure (1/2)u^2, then you are just as well to specify the velocity or volume flow---problem solved.  But if you really mean static pressure, then I think you do not know exactly what this is because it varies in time, given a static pressure of 0 at the outlet (this is what OPEN implements) and the fluctuations of the fire.

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/e5d292ef-5251-473b-8e84-e1b43274195b%40googlegroups.com.

[Matteo Pachera]

I think I need to read a bit to understand your first point, but the other two make sense to me as well. 

Regarding the implementation of my boundary conditions, usually I don't know the value of the volume flow or the velocity. If I simulate a tunnel I set the pressure at the portals at the atmospheric value and I install some ventilation device to evaluate their capability to confine the smoke and the longitudinal velocity. The simplified case which I proposed here is just an example where I imposed an overpressure at the inlet in order to investigate the pressure distribution along the tunnel. 

[Randy McDermott]

In your reading, consider Eq. (2.11) of the tech guide, the full momentum balance.  The usual way to think about tunnel or pipe flows is the mechanical energy balance at steady state.  In such as case, the only terms that remain in the momentum balance are the \grad{H} and \div{\tau} terms---the pressure drop is balanced by the stress on the walls of the tunnel.  But you can see that in an unsteady, variable density situation, there are many other terms at play that can balance the equation.  And my theory is that it is the du/dt term that is giving us the most trouble in this analysis.  I've added output for this to the development code, but have not had time to play with it.

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/a69fd05c-76f0-459a-9142-e4c667a6d160%40googlegroups.com.

[Matteo Pachera]

I looked at the equation in the tech guide, if I'm not mistaken the source of my problem is the first term (du/dt) which is increasing the value of H. This is also the reason why I can have the same longitudinal velocity even if the H profiles are different. Is there any way to reduce these strong fluctuations (du/dt), obviously apart increasing the size of the mesh?

[Randy McDermott]

I don't have an answer yet.  But I don't think we are specifying the problem correctly.  You keep coming back to "reducing fluctuations", which implicitly has the limit U=constant, which means we should be able to specify it.  Increase it or decrease the volume flow until you get the pressure you like.  I think this is the only way to keep the fluctuations under control if the fire is so large that it is creating wild pressure fluctuations.

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/6f3fc3c2-601b-432d-8b31-4f82dc2fafea%40googlegroups.com.

[Matteo Pachera]

I know that could be a solution, but the result of my simulation is the longitudinal flow which I don't know at the beginning of the simulation, while I know the pressure conditions at the portals. If I would try your approach of imposing the longitudinal velocity I will have to run several simulations in order to converge to the final result where the pressure at the portals correspond to my boundary conditions, and I think this could be too time consuming. However, thanks for you patience and help, now I think I'm better understanding the problem.

[Randy McDermott]

My suggestion is to use a bisection method with every increasing grid resolution.  You should be able to approximate the volume flows at coarse resolution, which should run fast.  Given the uncertainty involved in specifying the pressure as a boundary condition, I think this is the best engineering approach.

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/c49a1b74-6b2a-4d56-85c8-e355eeade675%40googlegroups.com.

[Matteo Pachera]

Dear Randy

I am trying to follow your approach, so I simulated my tunnel using different grids and different fires with a velocity boundary condition at the inlet. I looked at the pressure at the inlet of the tunnel to compare the results obtained with different spatial resolutions, but they show some discrepancies. 

The pressure in all cases has a good trend, however I think there are still some problems induced by the large velocity fluctuations in the fire region.

I attach some pictures with the results: Pressure at the inlet portal, pressure along the tunnel for different fire powers and grid's resolution.

Thanks, 

Matteo

[Randy McDermott]

Matteo,

There will always be fluctuations in all the fields near the fire source in an LES.  Once you have fluctuations, and turbulent conditions locally, you have to consider all the terms in the momentum balance.  I don't think you are going to come up with a simple analysis (I could be wrong).  But I don't think this means there are "still some problems" near the fire.  When you dig into the code term by term the equation is balanced by construction.

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/42d9523d-c0f6-46d7-97d2-99404e6e501d%40googlegroups.com.

[Matteo Pachera]

I know that there are some fluctuations and I understand that I can't expect a steady state solution coming out of a LES simulation. The problem I'm facing is that I don't know which grid resolution I should use for my calculations. When I simulated the tunnel using pressure at the inlet and at the outlet I found that the 0.25 m and 0.125 m grids where fine enough to be mesh independent, by comparing the longitudinal velocity. With the inlet velocity imposed, I compared the pressure at the inlet to evaluate the influence of the mesh resolution, but I see that the results are not mesh independent anymore. 

I know that from the balance of the forces this is the result of the simulation, but I expect that refining my grid I should have some results that are not dependent from the spatial resolution. Maybe my grid is still too coarse and I should refine it further, but I thought that 0.125 m was already sufficient for a tunnel. 

[Randy McDermott]

Tunnels are not well understood from a computational point of view (as you are experiencing).  Resolution of the fire plume may not be sufficient for resolution of the boundary layer controlling pressure losses in the tunnel.

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/b55c0779-83c3-4e33-976c-c6b8d51656a3%40googlegroups.com.

[Matteo Pachera]

So do you suggest to use finer meshes and see if the results converge to an asymptotic result? I will try to run, maybe a smaller domains, with a finer grid and I will report the results as soon they are ready.

[Randy McDermott]

Typically, LES of channel flows use a stretched grid.  These are not always practical, but may be required for tunnels.  We don't have good tunnel validation, so it is hard for me to give guidance.

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/5e7630ed-21ba-44c2-be48-1b4f953daeb8%40googlegroups.com.

[Matteo Pachera]

Dear Randy,

I just finished a couple of test calculations with different meshes applied to a really simple 2d case, input_tunnel.fds. The tunnel has a longitudinal velocity of 3 m/s imposed at the inlet portal and the HRRPUA is 2.5 MW. 

I used just one mesh to avoid possible issues due to multiple mesh interfaces. I ran the same case with 5 different grids resolutions with square elements: 0.5 m, 0.25 m, 0.125 m, 0.0625 and 0.03125 m. I couldn't use a finer mesh because the computational power of my computer was not sufficient. 

I monitored the temperature and the pressure along the tunnel and I report here some results averaged in time when the flow conditions become steady. 

The temperature in figure temperature_tunnel shows a good agreement between the different meshes and the contours as well show a similar temperature field.

The pressure distribution along the tunnel is presented in pressure_tunnel and it shows that the pressure is strongly affected by the grid's resolution. I also plotted the pressure at the inlet portal as function of the grid's size, pressure_mesh, but it doesn't seem to reach any asymptotic value. 

The pressure profiles look fine, but the pressure at the inlet changes a lot when I use different mesh resolutions. Do you think that the mesh is still to poor for this kind of problem?

Thanks

Matteo

[Randy McDermott]

Matteo,

Thanks.  This is an interesting study.

Notice that in this configuration, as you increase the grid resolution you are changing the stratification at the outlet.  By the final (highest) resolution it looks like you may even have a back flow into the domain.  The 1D theory would assume a perfectly mixed plug flow through the domain.

Couple things to try.  First, specify the velocity at the outlet and pull the flow in.  Next, put DEVC for MEAN pressure on inlet and outlet--you are interested in DP.  Last, make sure you plot the HRR and insure you are completely burning the fuel.  In fact, for this study, it would be cleaner to simply specify an INIT line with HRRPUV (match total HRR of burner).

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/bea0e532-9025-4944-9180-dbe46af32fb8%40googlegroups.com.

[Matteo Pachera]

Dear Randy,

Regarding the boundary conditions are you thinking about a pressure inlet condition with a velocity outlet or a pressure inlet condition with a mass flow outlet? I would prefer the second one because then I can easily estimate the velocity at the inlet, but I don't have much of experience with this BC in FDS.

I will try to set the HRRPUV in the model and compare it with my current results. 

Regarding the devices, I already filled the tunnel with them but I deleted them from the file I posted.

Last curiosity about FDS: if I have a 2D calculation does the thickness of the domain in the y direction affect the results? I was wondering if the aspect ratio in that direction might influence the numerical results.

Thanks for your help,

Regards,

Matteo

[Randy McDermott]

Mass flow outlet is fine.  The key is to get all the flow elements headed in the same direction.

DY in 2D should not matter.  If it does, submit an issue.  Thanks.

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/6d401405-c7e3-4759-88f2-cc6419d9f8e5%40googlegroups.com.

[Matteo Pachera]

I ran the new simulations imposing the HRRPUV and the mass flow at the outlet equal to 5 kg/s/m^2. I attach the complete input file including the devices that I used to produce the outputs of the simulations, input_tunnel.fds. The PRESSURE, the TEMPERATURE and the SUBGRID KINETIC ENERGY are calculated along the whole length of the tunnel. I used a spatial resolution similar to the previous case 1.0 m 0.5 m 0.25 m 0.125 m and 0.0625 m.

I calculated the average temperature (temp.png), pressure (pres_devc.png) and subgrid kinetic energy (sub_grid_kinetic_energy.png) using the devices and averaging the flow between 150 s and 300 s after reaching steady state conditions, (pres_time.png). The results have a better agreement among them also for the pressure, just mesh 5 shows a pressure trend different from the other simulations. 

I also plotted the pressure obtained from the slice file, pres_slice.png. This is exported with the fds2ascii tool in the same time interval and later I averaged the results along the height of the tunnel. 

The distributions of pressure obtained with the two methods are similar but I expected them to be the same. What could be the reason of this difference?

Dear Randy,

Dear Randy

To view this discussion on the web visit <a href="https://groups.google.com/d/msgid/fds-smv/c49a1b74-6b

[dr_jfloyd]

DEVC outputs are data at cell centers and are averaged over DT_DEVC.

SLCF outputs are the cell center data interpolated to cell corners (unless CELL_CENTERED=.TRUE. is defined) and are instantaneous values.

[Matteo Pachera]

Thanks for your quick answer, so if I use the same DT_DEVC and the same DT_SLCF with a CELL_CENTERED=.TRUE option enable should I get the same results?

[fde]

No, because DEVC is averaged over DT_DEVC time, whereas SLCF will show momentary value. CELL_CENTERED only is different from default by not averaging with surrounding corners. 

[Randy McDermott]

You can try adding TIME_AVERAGED=F on the DEVC line to get instantaneous values.

--
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/a16ba546-b700-4ffd-8ade-103636bbf4e3%40googlegroups.com.

[Matteo Pachera]

I tried also to set TIME_AVERAGED=F on the DEVC lines but the results are still different ,pressure.png, I reran my simulation with the coarse mesh using the CELL_CENTERED=.TRUE. option enabled.

The results obtained with the DEVC have a similar time history, the one not averaged has higher fluctuations, but they oscillate around the same value, pressure_time.png.

I noticed that in the slice file even if I used the option CELL_CENTERED=.TRUE. my values are stored on the nodes of the cells while I expected to have them at the center, can it be the reason of the difference?

On Thursday, 7 December 2017 13:35:50 UTC+1, Randy McDermott wrote:

You can try adding TIME_AVERAGED=F on the DEVC line to get instantaneous values.

On Thu, Dec 7, 2017 at 3:36 AM, fde <yilmaz....@gmail.com> wrote:

No, because DEVC is averaged over DT_DEVC time, whereas SLCF will show momentary value. CELL_CENTERED only is different from default by not averaging with surrounding corners. 

On Thursday, December 7, 2017 at 7:43:51 AM UTC+1, Matteo Pachera wrote:

Thanks for your quick answer, so if I use the same DT_DEVC and the same DT_SLCF with a CELL_CENTERED=.TRUE option enable should I get the same results?

On Wednesday, 6 December 2017 17:38:32 UTC+1, dr_jfloyd wrote:

DEVC outputs are data at cell centers and are averaged over DT_DEVC.

SLCF outputs are the cell center data interpolated to cell corners (unless CELL_CENTERED=.TRUE. is defined) and are instantaneous values.

On Wednesday, December 6, 2017 at 11:11:12 AM UTC-5, Matteo Pachera wrote:

I ran the new simulations imposing the HRRPUV and the mass flow at the outlet equal to 5 kg/s/m^2. I attach the complete input file including the devices that I used to produce the outputs of the simulations, input_tunnel.fds. The PRESSURE, the TEMPERATURE and the SUBGRID KINETIC ENERGY are calculated along the whole length of the tunnel. I used a spatial resolution similar to the previous case 1.0 m 0.5 m 0.25 m 0.125 m and 0.0625 m.

I calculated the average temperature (temp.png), pressure (pres_devc.png) and subgrid kinetic energy (sub_grid_kinetic_energy.png) using the devices and averaging the flow between 150 s and 300 s after reaching steady state conditions, (pres_time.png). The results have a better agreement among them also for the pressure, just mesh 5 shows a pressure trend different from the other simulations. 

I also plotted the pressure obtained from the slice file, pres_slice.png. This is exported with the fds2ascii tool in the same time interval and later I averaged the results along the height of the tunnel. 

The distributions of pressure obtained with the two methods are similar but I expected them to be the same. What could be the reason of this difference?

--
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.

[Randy McDermott]

I am not sure how (or if) fds2ascii knows what to do with CELL_CENTERED data.  I could imagine you are not exactly getting the pressure from the same plane in both cases.  I would trust the DEVC.  I usually use Simo's slread.m script in Utilities/Matlab/scripts to process SLCF.

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/72344e94-49d3-4a58-8bfd-678b8b1b2f9a%40googlegroups.com.

[Matteo Pachera]

Dear Randy,

I have been working for a while on the simulation of a simple tunnel with the HRRPUV approach and I found some interesting results in terms of pressure distribution. I simulated a simple case with 4 different meshes (1.0 m, 0.5 m, 0.25 m and 0.125 m) and I compared the results. 

The results obtained with the first 3 meshes are similar in terms of pressure, velocity and temperature distribution, however, the results obtained with the finest grid are quite different from the others. I saw in the validation repository that in case of simulations with a fine grid the flux limiter is CHARM so I tried one simulation with this option enabled, but there was only a minor improvement. 

Considering my problem I would like to ask if is there any limitation to the grid's size when fine grids are used? My D* is about 4.6 so the ratio D*/dx for the different grids is 4.6, 9.2, 18.4 and 36.8 and the last mesh is out of the range that is usually suggested for the FDS calculations, 4-16.

I attach to the post the input file that I used and some graphs of the temperature, velocity and pressure along the tunnel. 

[Randy McDermott]

In the high res case, are you getting correct HRR?  Can you try this test without HVAC and see if you see the same results?

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/31642c95-5c30-40ac-8992-fd616f1166e1%40googlegroups.com.

[Matteo Pachera]

Yes I have the same HRR of 50 MW, see the picture, I can try to run the case using other BC. 

I chose the HVAC just to have the same inflow and outflow conditions for every scenario.

[ingraban]

Dear FDS users and supporters

This is a very informative thread when it comes to pressure calculations for tunnel fires. Similar to Matteo, we are currently trying to get a plausbile pressure distribution along a road tunnel with fire. 

First, we had to abandon the idea of multiple meshes as the default FFT solver did not lead to credible results. So we follow the recommendations in the extended section 9.3 of the night-time user handbook, switching to LES and the GLMAT solver. Then, we also stopped modelling a fire, but used a volumetric heat source instead - although our ultimate goal is to model the fire. 

"gittertest01" shows a grid variation for a volumetric heat source of 30MW with an inlet condition of 2.5 m/s flow velocity and an open outlet. Although backlayering is predicted reasonably well (the variation can be attributed to small differences in the HRR), the pressure profile is not grid independent. 

"gittertest03" shows a grid variation for the same case. Only the boundary conditions have been changed, applying the HVAC boundary conditions as Matteo did. As you can see, the pressure profile looks more sensible and appears to be more or less grid independent. 

We thought, we found a solution. 

But "gittertest04" shows the same configuration. Only, the volumetric heat source has been replaced by a pool fire. Apparently, the pool fire induces pressure fluctuations. The pressure fluctuations increase with grid resolution. The time average of the pressure distribution is affected significantly. The flow velocities and smoke propagation do look ok, although with higher resolution in "gittertest04", the pressure fluctuations (here shown for x=0 for dx=25cm) even affect the heat release rate.

For you reference, I include the FDS file "TestFire", which is the pool fire case from "gittertest04" for a 50cm grid resolution. 

We tried the remedies against instabilities that are proposed in the user manual section 9.3. Do you have another idea?

[Randy McDermott]

Thanks for your observations.  I agree that adding a heat source to the tunnel is the next logical step in complexity.  I will play with your case to see if I can improve grid effects.

Note, however, that if you using GLMAT, then multiple meshes should be fine (the way I read your comments, it sounds like you abandoned FFT *and* multi-mesh; if you use one mesh FFT is the same as GLMAT).  If not, please submit an issue.

--

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/7823cf39-754c-4491-84be-f20febe448b5%40googlegroups.com.

[ingraban]

By "multiple meshes" I meant meshes with varying grid resolutions. And that appears to be impossible with GLMAT. 

I ran a few tests with GLMAT and FFT. For the tunnel with a heat source, the results match. For the pool fire cases, I get different time-average pressure profiles (both not plausible). Probably this is due to the pressure oscillations, which might introduce an element of random? Or the two solvers do handle the oscillations differently. 

 

[Randy McDermott]

OK, correct, GLMAT needs uniform resolution at the moment.   I am reproducing your results with the thermal plume.  I need to do more work, but so far things are pointing to the need for considerably high resolution to converge the pressure drop across the plume and the wall stress down stream of the plume.  I will let you know when I have more definitive results.

To view this discussion on the web visit https://groups.google.com/d/msgid/fds-smv/dcc49ca6-6f06-4c57-99cb-95873d5bc341%40googlegroups.com.

[fde]

I am trying to understand the calculations and measurements. I see that plots show the static pressure but QUANTITY='PRESSURE' is not static pressure as discussed before. Is that correct?

[Randy McDermott]

QUANTITY='PRESSURE' is static gauge pressure.

To view this discussion on the web visit https://groups.google.com/d/msgid/fds-smv/32aae492-c665-41a9-8264-5c1d49d70cf0%40googlegroups.com.

[fde]

I remember in few threads  that perturbation pressure is also included to the QUANTITY='Pressure', therefore it is not completely static pressure. Was it about some other subject?

https://groups.google.com/d/msg/fds-smv/x3HBp6QILEY/AQIBFClXBwAJ

[Randy McDermott]

The perturbation (or hydrodynamic) pressure is part of the static pressure.  Simply, it is p in the Navier-Stokes equations.

To view this discussion on the web visit https://groups.google.com/d/msgid/fds-smv/d663d0ee-0642-4718-aaee-de7269d43183%40googlegroups.com.

[ingraban]

I ran another series of simulations with the volume source HRRPUV. This time, I varied the heat release rate. And I changed the shape of the heat source, putting it in a 1m high layer on the ground. I tried to model some plume behaviour. The pressure profiles resemble the pool fire cases and the oscillations are back, although less pronounced as in the pool fire case. 

 

[fde]

This is not directly relevant to the thread but as a validation point of view, is there any study regarding pressure rise in tunnel fires? I could only found an equation of pressure difference due to buoyancy; dP=(1-T_e/T_m)*rho*g*dH in Tunnel Fire Dynamics book. 

My idea is that the calculation of pressure difference between Tatm and on the surface of escape door in the tunnel or on the ceiling (for example ventilation dampers). Could you give any lead so I can look into further?

[ingraban]

The is a number of articles on the throttling effect (pressure drop in a horizontal tunnel caused by the fire). Most of these papers are based on CFD calculations (FDS and others) and the results are scattered all over the place. There is little experimental evidence. And having these difficulties achieving a credible pressure profile along the tunnel makes me doubt at least some of these published CFD studies.

[Randy McDermott]

I am still working on the problem.  I hate to start this kind of lore... but there seems to be a marked difference in the results when setting CONSTANT_SPECIFIC_HEAT_RATIO=T on MISC (using constant specific heats).  See if this helps your cases as well.  I do not yet understand why using temperature-dependent specific heats leads to different results.  But when I use CP(T) the pressure oscillates more, and these oscillations seem to be very sensitive to changes in DX and DT.

Can you point to a few of the papers you reference regarding the acceleration of the tunnel flow past the plume?  Thanks.

--

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/5368c080-60bf-4b35-8bf0-e0e304b17f43%40googlegroups.com.

[matteo.p...@gmail.com]

Hi Randy,

I found these two papers about the topic: "Interaction Between Duct Fires and Ventilation Flow: An Experimental Study" (https://doi.org/10.1080/00102207908946897) and "Dutrieue, R., and E. Jacques. "Pressure loss caused by fire in a tunnel." BHR Group, AVVT 12 (2006).". 

In the Dutch guideline "Aanbevelingen Ventilatie van Verkeerstunnels" there is also an equation for the estimation of the pressure losses due to the fire but I can't find the reference paper.

I also think there are other research works about pressure losses in ducts when flows of different densities mix together that are not strictly related to fire in tunnels.

Thanks again for putting your time in this work. 

[ingraban]

Hi Randy

Thank you for putting in some time on this. I tried to re-run one of the previous cases, just adding 

&MISC CONSTANT_SPECIFIC_HEAT_RATIO=.TRUE. /

, but got an error message 

The addition of 

&WIND STRATIFICATION=.FALSE. /

&COMB SUPPRESSION=.FALSE. /

did not help. The same error message appeared.

[Randy McDermott]

Your case should run.  Is it possible you ran out of memory?  I reduced your x cell count to 525 with STRATIFICATION=F and SUPPRESSION=F (good idea) and without GLMAT (no need if single mesh) and the case ran (I am on my home laptop, which is an old mac, I'll try again later on our cluster).  GLMAT will take a lot of memory, so you only want to use it with MPI and small (64^3 or less) cell counts.

--
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/720e6959-a8a4-406e-b7b0-d211db3ae834%40googlegroups.com.

[ingraban]

It does not look like a memory problem. Before the error message appears, there is less than 20% memory use. And shouldn't the case with Cp(T) use the same or even less memory? I tried a different computer, but got the same error message. Switching GLMAT off doesn't help either. 

It is a Win10 Pro intel i7-8700 CPU with 16GB. 

[Randy McDermott]

Ingraban,

As I said before, your case should run.  There is a bug in 6.7.0 that has been fixed in the current development version of the code.

Using 6.7.0 release, I got this to run,

&MISC RESTART   =.false.

      SURF_DEFAULT='Wand'

      GVEC      = 0.,0.,-9.81

      NEAR_WALL_TURBULENCE_MODEL='WALE'

      CONSTANT_SPECIFIC_HEAT_RATIO=T

      STRATIFICATION=F

      SUPPRESSION=F

      CFL_VELOCITY_NORM=1

      FLUX_LIMITER='CHARM'

      /

Give this a try and let me know.  As I mentioned before, if you use a single mesh, just use FFT solver (take out PRES line).  If you use multi-mesh, then add GLMAT back.

On Mon, Dec 10, 2018 at 10:50 AM Salah Benkorichi <benkori...@gmail.com> wrote:

Check section 7.2 & Table 7.1

You're using LES mode and default is set to FALSE.

Select  SVLES mode and set

CONSTANT_SPECIFIC_HEAT_RATIO=.TRUE.   

now it runs. 

Randy can provide further detailed explanation.

On Mon, 10 Dec 2018 at 15:40, Salah Benkorichi <benkori...@gmail.com> wrote:

I didn't look in details to your case, but the error seems to be coming from the CONSTANT_SPECIFIC_HEAT_RATIO=.TRUE. 

comment it and the case runs fine.

To view this discussion on the web visit https://groups.google.com/d/msgid/fds-smv/8d358b5a-a0eb-442d-ba8f-385174683f53%40googlegroups.com.

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

--

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/CABK0Y1%3DS8b_Eg3G6nGyKopOtjJhUYX55YgXRYhiwukDd%3DEVWjg%40mail.gmail.com.

[ingraban]

Thanks a lot. The error appears to come from the combination of LES and CONSTANT_SPECIFIC_HEAT_RATIO=T. The case can be started with SVLES and VLES, though.
I'll be back with the results. 

[ingraban]

Here I've got two simulations of a 24 m2 pool fire defined as HRRPUA giving 30MW total HRR. Grid size is 33cm. HVAC boundary conditions. 

• cp const:
  CONSTANT_SPECIFIC_HEAT_RATIO=T
  SIMULATION_MODE = 'VLES'
  NEAR_WALL_TURBULENCE_MODEL= 'WALE'
  STRATIFICATION      = F
  SUPPRESSION         = F
  etc.
• cp(T):
  SIMULATION_MODE = 'LES'
  NEAR_WALL_TURBULENCE_MODEL= 'WALE'
  SOLVER                     = 'GLMAT'
  etc.

The first graph shows the 60s average mean pressure along the tunnel for both simulations. The second graph shows static pressure for x = 0m as 1s-average over time.

In the simulation, cp(T) gives less oscillations, but both pressure profiles are not plausible. 

Still, the only way I found a credible pressure profile was modelling the fire as large volumetric heat source imposing minimum oscillations (plume movement). But this is not the purpose of our study...

[Randy McDermott]

Let's move this to the issue tracker.  I created a new issue here

https://github.com/firemodels/fds/issues/7040

--

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/890bcc39-1286-4107-afa8-ab4df14562b2%40googlegroups.com.