Smoke Extraction Simulation

[Anonymous]

Hi!

I am trying to simulate fire and smoke extraction in garage. At the moment I am checking is everything OK with the simulation setup by doing the steady state analysis. I encountered on few issues...

First of all pressure, temperature and scalar convergence plot was really bumpy (picture in attachment Scalar 1.jpg)...I reduced scalar to 0,9 in intelligent solution control and now scalar works perfectly (picture in attachment Scalar 0,9.jpg)...But still I have problems with temperature and pressure...Any ideas what is wrong?!

Here is the support file of simulation - https://www.wetransfer.com/downloads/f989a9e8800b0389c6eb37864683c70520150614185009/4a81ede823d8d111...

Any comments on simulation setup by the Autodesk experts?!

Furthermore, I have few questions about transient analysis which I am going to simulate after resolving the issue with temperature and pressure (hopefully 🙂 😞

1. As I sad I lowered Scalar to 0,9 in steady state simulation. Should I return it to 1,0 for transient?!

2. Initial Conditions?! On what should I put Initial conditions!? I am doing this simulation based on tutorial from wildej -

Car Park Smoke Extraction and Visibility With Best Practices Autodesk® Simulation CFD™ and from that tutorial isn't clear on what should I put initial conditions?!

3. Should I turn on the radiation?!

4. My idea is to define energy of the fire with the volumetric heat, transient boundary condition so that the energy of the fire rises with the rise of time. But when the temperature above fire reaches 68 °C the energy of fire will start to reduce because the sprinkler system will engage. Is there any way I can tell that to CFD that boundary condition starts with one equation (start of fire) and when the temperature in simulation reaches 68 °C that it switches to second equation (fire extinguishing equation)?!

5. Jet fans should start working after certain amount of time - let's say 4 minutes after the start of simulation. Is there any way I can tell that to CFD?! Or I must STOP/START simulation?! Is that way the good way because in wildeys tutorial I saw that it is not advised to stop and start the solver during a transient analysis?!

6. Time step size (0,5s) and inner iterations (3) from wildejs tutorial are good start for my simulation?! My idea is that whole simulation lasts for 8 minutes.

Hopefully someone will have patience for reading my whole post and then answering it 😄

Best regards, Branimir.

[Jon.Wilde]

Hi Branimir,

Me again 🙂

1. Yes, I would try to leave the relaxation parameters alone during a transient run

2. Initial Conditions should be on all volumes that are participating in the study - I tend to just bulk select all volumes and give them an ambient temperature

3. Try with and without radiation. We tend to find it necessary to run with it on though. As soon as we have a temperature differential higher than roughly 60-70C, the effect of radiation will start to be noticable. With a fire, I guess you are going to have some pretty high temperatures

4. You can have a temperature dependent heat load but not one that has a varying load (see the last point here).

5. The only way I can see around this would be to start and stop the analysis. It is not ideal and you will likely see a blip in the convergence but I cannot think of another way. Really we need to use boundary conditions to be able to increase and decrease the flow rate over time.

6. I would say this is a good starting point, yes. If the solve is unstable, we might need a smaller time step...

In addition, do you need to mesh all of the walls? That might save a bit of memory and time.

[Anonymous]

And do you have any comments regarding the unstable pressure and temperature in steady state solution?!

[Jon.Wilde]

Hi,

Not too sure - it might just need to run for longer.

Try extending the outlet too, we could be clipping recirculation that is trying to occur there.

[Anonymous]

OK, I will try it and get back to you. Tnx!

p.s. Any news about that natural ventilation model?!

Best regards, Branimir.

[Anonymous]

I think I found what is the problem. I am getting very strange temperature results within the boundary layer - see picture in attachment.

In your powerpoint presentation that is listed as one of potential pitfalls.

What is the best way to solve that kind of problem? Is it possible simply to enhance boundary layer only on that spot in model?! How?

Best regards, Branimir.

[Anonymous]

In newly attached pictures you can see areas with real high temperatures.

Best regards, Branimir.

[Anonymous]

I also ran a simulation without fire. Pressure boundary condition was really stable until one stage and then became really rough and unstable.

What can be the reason for unsteady pressure?! You can see picture of convergence plot in attachment.

[Jon.Wilde]

Hi Branimir,

This might be leading to divergence, caused by the high temperatures that you showed earlier.

Do try refining the mesh in these locations (to thin the boundary layer as well as improve the air mesh).

You might also like to try turning on Surface Refinement if you have not already done so.

Hope this makes a difference.

Jon

[Anonymous]

The only problem is that pressure condition becomes unstable even when I don't have the fire inside the simulation (practically it's ambient temperature in whole simulation).

As earlier sad pressure boundary condition was really stable until one stage and then became really rough and unstable (http://forums.autodesk.com/autodesk/attachments/autodesk/330/8276/1/Convergence.jpg).

What can cause that?! Is pressure plot only related to pressure boundary condition?!

Best regards, Branimir.

[Jon.Wilde]

Hi Branimir,

That curve is representative of the pressure values across every node in the model - so we need to think about where the issues might occur and investigate. My first guess would be recirculation at the inlet or outlet, can you confirm that the flow here is uni-directional?

[Anonymous]

I think yes. :S I also extended the inlet and outlet quite a lot as described on autodesk website.

It would be great if you have time to look at the setup. :S

https://www.wetransfer.com/downloads/ba58a4d621d81cf8c7c6ebd18700a50e20150623092058/8c1283ca69eebeac...

I also attached Convergence plot.jpg from the simulation.

[Anonymous]

Did you maybe check it?

[Jon.Wilde]

Hi,

I did indeed - it only just finished.

I think that what I said before is correct, you have recirculation over your inlet. This will cause solver instabilities.

Could you have a flow rate here instead and a P=0 at your outlet - and extend the outlet to try to avoid this?

[Anonymous]

I can surely extend the outlet.

But I am not sure that I can have flow rate in the inlet...In my project flow rate is at outlet and inlet is ambient...

Do you think that extending the outlet will do the trick? Or I will have to swap flow rate?!

[Jon.Wilde]

All I can really suggest is test it. At the moment, you need a longer inlet and then try it.

I would think that your flow rate in is equal to your flow rate out (phyiscs tells me this is true 🙂 ) - so does it really matter which has a flow rate?

Kind regards,

Jon

[Anonymous]

Will try couple of variants and get back to you.

Once again you are big help!

Best regards, Branimir!

p.s if you have any news regarding the natural ventilation model...

[Anonymous]

Hi wildej!

From the last week I have done a lot of test simulations...

First set of tests I have done on the model that I uploaded to you and with the pressure inlet boundary condition and volume flow rate on the outlet. Here are the parameters simulated and the results:

1. Simulation with fire and with jets; p=0 inlet boundary condition, and volume flow rate outlet boundary condition. – Pressure plot really unstable during the simulation.
2. Simulation without fire and without jets; p=0 inlet boundary condition, and volume flow rate outlet boundary condition. – Pressure plot normal/stable.
3. Simulation with fire and with jets; p=0 inlet and outlet boundary condition – Pressure plot really unstable during the simulation.
4. Simulation with fire and without jets; p=0 inlet and outlet boundary condition – Pressure plot, TED and TKE really unstable during the simulation.
5. Simulation with fire and without jets; p=0 inlet boundary condition, and volume flow rate outlet boundary condition. – Pressure plot, TED and TKE unstable during the simulation but more stable then in scenario 4.
6. Simulation without fire and with jets; p=0 inlet boundary condition, and volume flow rate outlet boundary condition. – Pressure plot really unstable during the simulation.
7. Simulation without fire and with jets; p=0 inlet and outlet boundary condition. – Pressure plot really unstable during the simulation.

After these tests I ran second set of tests where I even more extended inlet and outlet than they were. Results were more or less same as in first tests...Only difference is maybe that in scenario 4 pressure was more stable than in first sets of test.

In second set of tests I also ran one simulation (Scenario 8 in Garage – second tests.cfz) with the boundary condition setup that you suggested. Volume flow rate was defined on inlet (with scalar = 0, and ambient temperature) and pressure was defined on outlet. But the result are same, really unstable pressure.

Any idea what is wrong?! :S

I uploaded the model for first set of tests – Garage – first tests.cfz and model for second set of tests – Garage – second tests.cfz. I also uploaded Convergence plot jpegsfrom all of the scenarios from the first set of test. All of these can be downloaded here:

https://www.wetransfer.com/downloads/3bb47bae1badcbc94bfcfe1f231b35b420150630092314/a488c7

Best regards, Branimir.

[Anonymous]

Did you maybe have time to check it?

[Jon.Wilde]

Hi Branimir,

I did indeed - I also had a few issues which hindered me a little (not with your model though).

I think that this might be down to the mesh - take look at the mesh here, this is very coarse: