Community
CFD Forum
Welcome to Autodesk’s CFD Forums. Share your knowledge, ask questions, and explore popular CFD topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Smoke ventilation from parking lots

20 REPLIES 20
Reply
Message 1 of 21
sahar.rubin
2129 Views, 20 Replies

Smoke ventilation from parking lots

Hi!

I have a problem with setting transient solver for the expansion of fire in a parking lot.

I reviewed I think any smoke tutorial and guidelines you have and still have some questions:

1. How do I set the transient solver correct and how can I know how much time passes?

For this example lets assume I need to see what happens in 10 minutes after the "car" catches fire.

 

2. What is the correct wattage needed for the boundary condition of the "car" volume?
Assuming the "car" is a cubic volume as shown at the file attached, who catches fire.

 

3. Whatever you can add to smoke ventilation and visualization

 

4. Can you please check the other inputs and give your opinion on the design.

The details for the design (for others also 🙂 ) :

 

General details:
2000 m^2 parking lot, avrage. Height 3.2m, total volume: 6400 m^3.

For 8 air changes needed -> 2 outlet of 15000 cfm each, one free vent inlet.

 

Materials:

Ducts, Volume = Air (variable)

"Car" = Resistance (Fire):

     Through Flow K = 0.85

     Normal Direction 1 K = 0.85

     Normal Direction 2 K = 0.85

     Conductivity = 200 W/m*k

     (all constant)

   Flow direction of Fire material picked towards up (Z vector)

Jet Fan Case = Metal (Suppressed)

Jet Fan "Fan" = Custom Internal Fan ("Typhoon"), by sizes and preferences as manufactured:
     Flow = 2.7 m3/s

     Rotational Speed = 0 RPM

     Slip Factor = 1

     (all constant)

   Flow direction towards the front of the jetfan (x and y vectors depend on location in the parking lot)

 

Boundary Conditions:

"Car" =

     (Volume) Total heat generation 5000 W

        Steady state

        Temp dependent - Disabled (What does it mean???)

     (Surface) Scalar 1, Steady state.

 

Ducts outlets:

     (Surface) Volume Flow rate 15000 ft3/min each.

     Steady state.

     direction - towards the outside of the volume.

 

Free Inlet:

     Scalar = 0.

     Pressure = 1.01325e+06 dyne/cm2 (As Environment)

     Temperature = 30 Celsius

 

Initial Conditions:
Air Volume = Scalar 0

 

Mesh Size

Auto with adjustments in the fans and ducts (0.6 with uniform and spread)

 

Solver:

Control:

Main = need your help 🙂
Result Quantities =

    Scalar = on

    Smoke Visibility = On; Parameters:

        Extinction Coefficient = 37000 ft2/lb

        Sign Visibility Constant = 3

        Combustion Particulate Yield: 0.008.

Physics:


Flow = on

     Incompressible.

Heat Transfer = on

Auto forced convection = off

Gravity Direction = 0,0,-1 (-Z here)

Radiation = off

Advanced:

     General Scalar:

            Diffusion coefficient: 0.12 cm2/s.

 

 

Sorry for the long question, I just thought others would appreciate it , I looked in many furors and no one really solve this problem...

Thank you SOOOO MUCHH!!!!!!

 

Sahar Rubin,

Mechanical Engineer.

 

20 REPLIES 20
Message 2 of 21
Jon.Wilde
in reply to: sahar.rubin

Hi Sahar,

 

It sounds like you are just about there to be honest.

 

You do need a gap beneath the fire, for the air to flow from the room, up into the resistance and out of the top. Your resistance is about the right size, just have it open to the air beneath rather than closed off - does that make sense?

I would just leave the inlets as P=0, this is gauge pressure so just standard atmospheric conditions.

 

To answer your questions:

 

1) I would start with 0.5s and see if that is stable. With scalars we recommend just 1 inner iteration. If this is not stable, you might require a smaller step.

Set the stop time to 600 (seconds are the default unit)

Set the number of iterations to run to -1 (this means it is ignored)

Intelligent Solution Control is off, which is good (this ensures we run to 10 mins and do not stop at a false convergence)

 

2) This is hard to say, a number of kW most likely. Do you not have any sort of design requirements here? 5000W is a good start.

 

3) Use Planes and ISO surfaces to investigate scalars. 0 will be clean air and 1 will be 100% smoke. The numbers inbetween will be a mix of the two

 

4) I would add a uniform mesh to the fans - we need 5 elements from inlet to outlet (of the fan material). Then you will also need mesh regions to capture the jet - did you see my pdf?

 

Have you had training with CFD? Your setups are very good 🙂

I hope that helps.

 

Kind regards,

Jon

Message 3 of 21
sahar.rubin
in reply to: Jon.Wilde

Hi Jon!

Thanks for the quick reply!!!

I did put a gap beneath the fire, as you mentioned in another conversation I saw here 🙂

about 0 gage, if I put the 0 gage for the inlet, wouldn't it change the inlet to outlet? What I mean is, if I put the inlet to 0 gage and I want to keep suction of 30000 cfm from the room wouldn't it harm my calculation?
As I mentioned, I have 2 outlet (extraction from fans by ducts) of 15000 cfm each and one free inlet (means the the air comes naturally through the simulated duct/hole in the ceiling - I do this to simulate air infiltration while smoke extraction is needed, if you have a different approach I would love to hear it 🙂 )

 

about the solver:

     would start with 0.5s (time step size?) and see if that is stable. With scalars we recommend just 1 inner iteration. If this is not stable, you might require a smaller step. 

     Set the stop time to 600 (seconds are the default unit)

     Set the number of iterations to run to -1 (this means it is ignored) (time steps to run?)

     Intelligent Solution Control is off, which is good (this ensures we run to 10 mins and do not stop at a false convergence)

     what about Save intervals? How do I use it and what is it basically?

 

I've seen you PDF and it really helped! 

what do you mean by: "we need 5 elements from inlet to outlet (of the fan material)"?

 

never had any training, just reading a lot from furors, asking question (to be precise, asking you questions 🙂 ), and trying tutorials and reading material in Autodesk's wikihelp, 
I've been using the software for only 2 weeks now!

anyways, thanks for the compliment 🙂 and moreof, thanks for reply so fast and helping so much, you are the best!


Sahar

Message 4 of 21
Jon.Wilde
in reply to: sahar.rubin

Hi Sahur,

 

No problem, it is a pleasure to help. You are learning very fast with no training, I am impressed!

 

The inlet pressure should not actually matter, as the dP will be the same regardless. But sure, leave it as it is, no problem at all.

I can see where you are coming from and I think you are correct, it will certainly help wih interpreting the results and may well be very helpful in creating a positive pressure.

 

Time Step Size: 0.5s yes. We may well need to reduce this if you face any divergence, time to test it and see.

The -1 is for the Timesteps To Run yes. This means that we do not need to think about how many timesteps we will run as we tweak the timestep size to improve the stability of the analysis. It will just always run to 10 mins.

Save intervals: These are used if you wish to backtrack at any point and look at the results at a point between zero and ten minutes. We recommend saving no more than about 40-50 steps in one analysis (just incase the file becomes too large to open, rare but it can happen). So you could set this to save every 30 seconds, and you would then have 20 results over the course of the analysis that you could animate. Something like this.

 

Regarding the fan material - this is a before and after of what the mesh should look like. I selected the volume, gave it a uniform mesh and refined it to the level we need. From the inlet face to the outlet face we now have 5 elements (not that it really helps here but you can right click the part and select preview to see the mesh on the surface). You will likely also need the refined mesh regions to capture the jet. As these are a little tricky to manipulate in CFD, you could always draw them in CAD. They would still have an air (variable) material assigned to them but you would also be able to select them for additional mesh refinement.

 

Mesh on a fan.png

 

Regarding the fire, I would remove the solid part here so that the air can enter around the edges beneath the fire. The solid around the edge of the fire can stay though, that often helps. Does that make sense?

 

Gap Here.png

 

Please let me know if I have not answered all of your quesions, I think I have 🙂

 

Best regards,

Jon

Message 5 of 21
sahar.rubin
in reply to: Jon.Wilde

thanks again!

 

only one last thing:

"Car" =

     (Volume) Total heat generation 5000 W

        Steady state

        Temp dependent - Disabled (What does it mean???)

     (Surface) Scalar 1, Steady state.

 

and in the boundary conditions everytime i put it on steady state, and i don't really know how will it change if i'll adjust it to transient?

 

i'm running a simulation now, i'll upload the result to help others and for your review 🙂

 

Thank for everything!

 

Sahar

Message 6 of 21
Jon.Wilde
in reply to: sahar.rubin

Hi Sahar,

 

That just means that we can have heat loads (or heat losses) which switch on and off depending on the temperature at a particular location. Here, the lead load will remain at a constant 5kW whether you run steady state or transient.

We only use transient BC's if we wish them to change over time.

 

Kind regards,

Jon 

Message 7 of 21
sahar.rubin
in reply to: sahar.rubin

Hi again.

 

ok, after a lot of time calculating, i stopped it after 147 iterations (which means about 1 minute) and the results aren't what i thought would be,

 

1. the temperature hardly changed, which isn't likely to happen when fire bursts.

2. in conticuation with 2, hardly any smoke, and something funny happend, look at the inlet, there's some smoke gathering there, Why???

3. the velocity magnitude looks different than in the steady state mode, it looks round rather than long in steady state solver..

what am i doing wrong???

Message 8 of 21
sahar.rubin
in reply to: sahar.rubin

just some more attachments 🙂

 

thanks!!!

Message 9 of 21
Jon.Wilde
in reply to: sahar.rubin

Hi Sahur,

 

This is likely down to meshing/timesteps. Do you have the CFZ to hand?

 

I do have a few support cases to run through first but will be onto this as soon as I can be.

 

Thanks,

Jon

Message 10 of 21
sahar.rubin
in reply to: Jon.Wilde

The .CFZ is attached here,

whenever you can it'll be amazing

 

thanks for everything Jon!

 

Sahar

Message 11 of 21
Jon.Wilde
in reply to: sahar.rubin

Hi Sahur,

 

Is this the same CFZ as last time or did it not save correctly? 

There are a few things I was expecting to see that I cannot:

 

A gap under the fire - this needs to be connected to the main air domain. We could just make that solid block air in the meantime as that would be closer to what we need but it would be better to change the CAD.

Fan mesh refinement (you can use groups here to speed this up and assign them all at once)

Air jet regions.

 

Kind regards,

Jon

Message 12 of 21
sahar.rubin
in reply to: Jon.Wilde

it's the same .CFZ because there is a gap under the fire, and in my other computer i did the adjustments and arrange the mesh as you said, 

the results are after the changes.

 

so, what's wrong ?
why doesn't the space heat??? (now the other computer continues and after 250 iterations the max temp. is 32.071)

Message 13 of 21
Jon.Wilde
in reply to: sahar.rubin

Hi Sahur,

 

There do need to be some changes made, I can do some of this but some needs to be done in CAD.

 

1. The underside of the fire must be connected to the main air volume - so that the clean/semi-clean air can enter, flow upwards through the 'fire' and exit out as 100% smoke. Trim off the bottom section of that solid part you have here to allow for this.

 

Airflow.png

 

2. Add some refinement regions for the fans - I recommend doing this in CAD, although as your fans are in-line with the x and y axes you could use meshing regions

 

Example Mesh Region.png

 

 

3. Another point I noticed is that we should also assign an Initial Temperature to the air volumes.

 

Does that all make sense? I am not sure if I am making myself clear.

 

Kind regards,

Jon

 

 

Message 14 of 21
sahar.rubin
in reply to: Jon.Wilde

Hi again 🙂

ok, i did everything you said and "surprisingly" it worked great!

the fire burns, and the smoke commensing, some problems though:

 

1. I can't ventilate the smoke ! i extract 60000 cfm for 16 air changes and i can't really understand the results, (2 attached)

 

2. how can i know how much wattage to assign for the fire? 5000W doesn't really affect the volume and 4MW is really too much, now i tried 0.5MW but it's just a speculation...

another thing, i know fire changes during time, don't i need to make the total heat generation transient?

 

3. it it correct to assume that scalar is smoke (thats why inlet gets 0 and fire gets 1), if so, why isn't there a similarity between smoke visibility and scalar?

4. how can i see the results as is in the guidelines

 

thanks for everything! Smiley Very Happy

 

Sahar

Message 15 of 21
Jon.Wilde
in reply to: sahar.rubin

Hi Sahur,

 

I just ran this for 20 iterations (timestep 0.5 - I think 1s is too large, 0.5 is pushing it). I did spot one other point which I am not sure I mentioned. The fan mesh refinement also needs to be applied to the fire - at least 5 elements from bottom to top (inlet to outlet).

 

To answer your questions

 

1. I can't ventilate the smoke ! i extract 60000 cfm for 16 air changes and i can't really understand the results, (2 attached)

You have a constant smoke production, should this be the case?

Have you checked that the flow is behaving as you expect? Use global vectors to check inlets and outlets and vectors on cut-planes to help visualise it

 

Global Vectors.png

cut-plane Vectors.png

 

Looking at a vertical cut - we may need more mesh - there is still not additional volume to capture the jet from the fans.

Try a 0.7 refinement to the air and see if the results change - ideally they will not as we already had enough mesh.

 

Jet fan mesh.png

 

2. how can i know how much wattage to assign for the fire? 5000W doesn't really affect the volume and 4MW is really too much, now i tried 0.5MW but it's just a speculation...

another thing, i know fire changes during time, don't i need to make the total heat generation transient?

There are so many different specifications here that it is hard to comment. I have seen a wide range of heat loads assigned... Do you have any sort of specification to meet that might provide some guidance?

 

3. it it correct to assume that scalar is smoke (thats why inlet gets 0 and fire gets 1), if so, why isn't there a similarity between smoke visibility and scalar?

Scalar 1 is smoke. Scalar 0 is air. The diffusion coeff tells CFD how well they mix.

There shoud be a rough similarity between the two but they are not the same values  - please see the attached

4. how can i see the results as is in the guidelines

Use an ISO surface - I believe a few were used here. Clearly, they only show a single value for scalar so you may need a few to cover the full spectrum.

 

Quick example (you can right click on the legend to tweak colours):

ISO.png

Message 16 of 21
sahar.rubin
in reply to: Jon.Wilde

Thanks for the fast reply (Once again 🙂 )

 

- I changed it to timestamp 0.5 and the 5 elements to the fire as you said.

 

1. The case supposed to simulate a car catching fire, something like:

 1.JPG

 

the smoke coming out of the car is pretty constant, it can be an assumption.

The flow is behaving exactly as I expected.

Still, why doesn't the smoke visibility clears near the exhausts???

 

2. Don't have any guidelines for the wattage, it changes as I said.. I thought you could recommend on something from your experience.

 

3. OK

 

4. So I use the ISO surface for scalar (and just paint it - from black to white ?

 

Thanks again! 

I'm summarizing all of our comments to a document, when it'll finally be as we want and have all the conclusions I'll upload it so everyone can learn and you won't need to deal with people like me Smiley Very Happy

 

Sahar

 

 

Message 17 of 21
sahar.rubin
in reply to: sahar.rubin

The enlarged picture:

 

1.JPG

Message 18 of 21
Jon.Wilde
in reply to: sahar.rubin

You can assign a transient load to the fire, no problem. The only tripping point CFD seems to have is a transient scalar value, that needs to stay at 1.

 

I will check with my colleagues on this one, right now you have 162C so can certainly use a higher power output.

Have you tried assigning the first curve you have shown?

 

As for the outlet, I need to run it out a little. I would have thought the smoke would only fully clear once the fire had stopped but at least you can control it's path of evacuation?

 

Kind regards,

Jon

 

 

Message 19 of 21
sahar.rubin
in reply to: Jon.Wilde

i can set the fire evacuation route and that's ok, but i need to extract the smoke to enable people to escape and make the air breathable,

 

now i tried to do the same without fans and extraction, the temp was raised but there was less smoke to deal with, it just clears out for me that the extraction or smoke doesn't work, can you try it also and see the differences?

 

how did you make this beautiful ISO plane? could you send pics of the preferences? or write them down?

 

thanks !!!

Message 20 of 21
Jon.Wilde
in reply to: sahar.rubin

Regarding the ISO surface, I only did 3 things:

 

  1. Add an ISO surface
  2. Change the quantity to Scalar (I think I had Colour By as velocity)
  3. Go to Edit and drag the slider to the desired value

You can then right click on the Scalar and Velocity legends and change the scale/colours.

 

As an additional and important note:

 

You also still need to add mesh refinement regions for the jets.

 

Kind regards,

Jon

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report