Car park ventilation and CO extract model

[rpadovani]

Hi CFD Community.

I need some urgent help with a scalar mixing and carbon monoxide extract analysis.CFD dropbox link

I am working on a car park ventilation analysis to assess Carbon monoxide levels in accordance with the local Australian regulation. I watched the video on youtube that details the CFD setup for smoke analysis which is somwhat similar to CO extract analysis so I followed the steps according to the tutorial.

I am however facing some problems and have queries on the results I am obtaining in the current model.

I created the geometry in REVIT and added caps for all the openings which includes the car park entry and exit gates, ramp to the level above, mechanical ventilation supply and exhaust grilles. I also created the detailed geometry for the jet fans following the guidelines of the youtube tutorial for smoke analysis. I then supressed all solid elements except for the jet fan element ( jet fan casing was also supressed). I intially allowed for 0.2kW heat flux from the vehicles ( 111 cars in total) but after getting some strange results in the that surface with temperatures up 120oC, I decided to turn off the heat transfer and run ventilation only. The CO emitted by each car is 50g per hour according to the calcs done following the local regulatory code ( I initially assigned to small surfaces on the floor but afterwards changed to a side surface of the car suppressed surface) . I then assigned scalar value of 0 to fresh and mechanically supplied air and scalar 1 for the Carbon Monoxide inlets. Pressure 0 for the car park open inlets and outlet to the level above.

The local code stipulates that the CO rise must be limited to 51PPM within 1 hr ( 60ppm max within 1 hour, assuming a starting point of 9PPM). Therefore the simulation must be transient for 3600s which quite a lot in terms of computational time but my machine could complete this within 3 days.

Anyway I found the following problems that I cant find a solution anywhere in the Autodesk community forums and I hope you can help me.

1) After running the simulation for some 500 timesteps the air velocity from the exit gate opening short circuit the entry gate opening creating air flow pattern in a loop that grow indefinetely up to 1200m/s and above. In the first 200 timesteps the air flow patterns look reasonable. Is there any anything wrong with the geometry of the car park openings with Pa assigned to 0? I was thinking of stopping the simulation at 200 timesteps and checking the air velocities in the carpark entry and exit door surfaces, then assigning these values manually as boundary conditions and deleting the pressure boundary condition. What is the best approach here?

2) Do I need to assign constant value transient boundary conditions for a transient analysis? All of the boundary conditions are constant. I tried to assign a step curve for the CO mass flow rate so to start after a delta T but the arrow always point to the surface in the transient boundary value. With a steady state boundary condition I can choose to reverse the direction of the flow. I decided to leave all values as steady state boundary conditions.

3) As part of the guideines for the jet fan analysis I refined the mesh in the fan solid object with 5 elements accross the width, refined the exit flow surface and spread changes. I then tried to add a local refined region in fornt of the jet fan exit flow but the solver rejected stating that I created a mesh that is more refined than a suppressed element. Without the refined region the jet fan velocities are quite lower than the manufacturers data. Could you please help me with this error? How can I create this region. What is an appropriate size for the region 10m x 2m x 2m?

4) This is the most intriguing question for me. My current set of results running steady state or transient shows a very high scalar value for the amount of CO supplied to the air domain. The CO rate is only 50g/hour for a huge air domain but the CO concentration rapidly rise above 1000PPM even closer to the mechanically ventilated supply air grilles. There are several questions in the forums but I have to repeat the same question. IS the PPM concentration simply the scalar value divided by 1,000,000 or there is something else in the algorithm of the scalar value of the air mixture?

I am sending the model in the attached dropbox link. I will be very appreciated if you could get back to me with some light in the above questions.

Kind Regards

Roberto Padovani

CFD model car park 

[rpadovani]

Hi Jon

I followed all your recommendations but also changed the geometry of the CO intake away from the main air flow volume. The steady state analysis of flow only converged very well, recirculation of air in the outlets were reduced significantly. I then added scalar 1 to the CO boundary condition. However the scalar results are still too high.

The order of magnitude is 1000x higher than what should be. The transient simulation already run 880 timesteps and after an initial steep rise of the scalar value , it stabilised now at an average of 0.0408 which is roughly 40000ppm. The result as I mentioned is almost 1000 higher of what it should be considering the total CO intake in the car park is 4,245g/hour. In the first timestep of the transient simulation , the average scalar value went straight from 0 to 0.015595 which would be almost impossible for such a high volume of the air of the car park.

I also run a simple shoe box model with one inlet and one outlet and side wall intake for the carbon monoxide. The average result of the scalar value in the air mixture was also too high. That indicates the problem is not specifically related to the complexity of the model or mesh.

1) Do you have any other suggestion to fix this issue with the scalar results?

2) Do I need to enter the CO boundary condition in the form of air velocity or volumetric flow rate as opposed to mass flow rate?

3) Or this is just a limitation with the scalar calculation mixing a very small volume of one fluid into a very high volume of another fluid?  

I am sharing the latest version of my model on the link below, and also showing a screen print of the results and convergence graph.

https://www.dropbox.com/s/u68oe7x237lyx1j/Corso%20Carpark%20Final%20Setup_020315_support.cfz?dl=0

[Jon.Wilde]

Hi,

1. What is your ppm at the inlet? We were talking about this here and it would follow that if you are equating scalar to ppm, your Scalar 1 would be 980392 ppm, is that right?
2. Any flow rate should be fine here
3. There is nothing that I am aware of at all

Kind regards,

Jon

[rpadovani]

Hi Jon

PPM at inlets would certainly be 980,292 ppm but the volume of CO per second is very small. if the average scalar value of 0.04 is applicable to the whole air volume then it would equate to 400Kg of CO in just 10 minutes. The total intake for the car park as set in the boundary conditions is 4245 g/hour. So even disregarding the air exhausted in the 10 min of the simulation, the scalar value shows a result impossible to achieve since there is not enough scalar 1 mass flow rate to fill up 400Kg of scalar 1 in this period of time.

Below is an image of the scalar result at the inlet

[Jon.Wilde]

Hi Roberto,

I see what you mean. Have you tested this on a smaller model at all? I feel sure it should work but guess we ought to test it properly at this stage to be sure.

Kind regards,

Jon

[rpadovani · Accepted solution]

Hi Jon

I found a solution for the problem. As I said in previous posts the problem was the fact the order of magnitude of the air velocities near the CO boundary condition was too high even moving the surface outward by 800mm. The mesh was never going to be fine enough to properly capture this high transition in air velocity from the boundary surface. The high air velocities within those cells drove the scalar value to unrealistic values.

To overcome this problem I artificially increased the flow rate of the CO boundary condition and propotionally reduced the scalar value. This is acceptable since the combustion gases are a mixture of many substances including CO and mainly CO2. The approximate CO scalar value of the combustion gases is 0.02. To make the air velocity in this boundary condition even higher I increased my original CO mass flow rate 500 times and reduced scalar value of CO to 0.002. It is also important to note that temperature out of the tailpipe is very high and CO would have a much lower density and therefore higher CO concentration would be closer to the ceiling. Another point is that the air velocity of the combustion gases out of the pipe would be much higher than what I had initially in my model because the pipe diameter is very small compared to my large CO boundary conditions.

Please refer to final set of results below. It is just unfortunate my cloud simulation did not download to my computer all the saving intervals, so I cant create an animation video. The Cloud simulation got stuck after finishing at 100% so I decided to stop simulation at my computer and interval saves never worked. I think the final results file size of 37GB didnt help..

Thanks again for the help in the trouble shooting.

Regards

Roberto. 

[Jon.Wilde]

Hi Roberto,

This is both great to hear and great to understand!

I would be wary of saving too many time intervals when running on the cloud, just because of the huge amounts of data to download. It can work but I tend to save 20-30 steps as a maximum.

Thank you for sharing this 🙂

Jon

[Anonymous]

Hello Roberto

please can share again your last model

https://www.dropbox.com/s/u68oe7x237lyx1j/Corso%20Carpark%20Final%20Setup_020315_support.cfz?dl=0

link is broken

thanks.

[rpadovani]

https://www.dropbox.com/s/vhwpcda813gb0k7/Corso%20Carpark%20Final%20Setup_020315_support.cfz?dl=0

[Anonymous]

Thank you very much Roberto, for someone starting as me, this is a lot.

[Jon.Wilde]

If you are just starting out, you need to see this also 😉

Smoke Extraction Webinar.

(Don't forget to leave Roberto some Kudos 🙂 )

Thanks,

Jon

[Anonymous]

Hi,

Could you share the .cfz file? 

Best Regards,

slot online

[Jon.Wilde]

...and please kick off a new thread if you wish to have a discussion about it 🙂

[rpadovani]

Hi, I actually shared a cfz file before. As Jon Wilde suggested can you please open a new thread with specific questions regarding your project?

[Anonymous]

Dear All,

I am in the process of trying to model a carpark similar to this, but just much larger. I am playing with the file that has been provided, and upon solving the model, when in results page I cannot generate a birds-eye showing the scalar concerntrations, I can only see any of the distribution if I am looking from the bottom of the fluid, i have only the fluid turned on, and only the scalar variable set to few, without any vectors applied like the example image showed, I was wondering if someone could give me more guidance on how to get these scalars to show properly from top to bottom, as it feels like the top of the volume is blocking the view of the results. 

Thank you, attached is an image of what I am seeing from above (should be showing at least the red scalars of the CO leaving each car in the model, instead its just showing air.

[Jon.Wilde]

Try two things:

1. Show Scalars on an ISO surface to be sure that you do have results of value in there - change the ISO value to close to 0 to experiment
2. Change the scale of the Legend with a right click to see if this is the cause. My guess is that the 1 value is way more dominant than the 0 one

Hope that helps,

Jon

[Anonymous]

Cheers John, have been changing the scale and using planes in order to check if the scalar variable is diffusing. I will most likely upload a model I have put together as I am not sure if the in-flow flow rates are making their way into the model/ feels like the scalar is diffusing only into the solid itself, not the actual space.

[peter2ramy]

Hi Roberto,

I have similar issue with the CO concentration level. I live in Australia , do you have a phone number, would be much easier to discuss on the phone if you have some time

Thanks

Kind Regards,

Peter

[rpadovani]

Hi Peter 

You can call me on 0414427250 this Friday to discuss your query. Regards

[MEPG.BIM1]

Can you share cfz file? thanks