topic Car park ventilation and CO extract model in CFD Forum

Car park ventilation and CO extract model

rpadovani — Mon, 02 Feb 2015 20:30:34 GMT

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

Re: Car park ventilation and CO extract model

Anonymous — Tue, 03 Feb 2015 10:58:40 GMT

Hi,

Could you share the .cfz file?

Best Regards,

Re: Car park ventilation and CO extract model

rpadovani — Tue, 03 Feb 2015 11:11:00 GMT

Hi,

cfz file uploaded in the dropbox link below

CFD car park

Re: Car park ventilation and CO extract model

rpadovani — Tue, 03 Feb 2015 21:50:20 GMT

Can anyone help me with this model please?

Re: Car park ventilation and CO extract model

Anonymous — Wed, 04 Feb 2015 18:26:02 GMT

Hi Roberto,

Assign boundary conditions Pa=0 to all exits where the air leaves from car park area. Also extend the boundary conditions like the picture below

Your CO mass flow rate depends on time then you need to assign transient boundary conditions with piecewise linear time curve. In steady state condition you can assign the direction of flow but in transient analysis your CO mass flow rate must be negative values.

You can manipulate with mesh region but you should do it in your cad model.

Actually i don't know the answer of this question. I'm sure Jon will help you a lot.

Best Regards,

Re: Car park ventilation and CO extract model

rpadovani — Wed, 04 Feb 2015 22:08:59 GMT

Thanks Berkan_vent

I have some questions on your comments below

1) I will definetely extend the boundary conditions wherever required as you mentioned. But is this necessary when the openings are assigned with a volume flow rate? Please note this is a mechanically ventilated car park with fresh air openings. The openings you marked below are mechanically ventilated and with a set supply and exhaust flow rate. My understanding is that we need to extend the areas around the boundary conditions assigned with P=0. If you look at my model, the car park entry and exit doors on the left hand side do have an extension. The only area I would have to change and extend geometry is the outlet ramp to the car park to the floor above, which is on the right hand side of the model placed on the top surface.

Also you mentioned that I should assign P=0 to all exits. I have only assigned P=0 to the fresh air inlets and outlet (ramp to the level above). All the mechanically ventilated exits have a volumetric flow rate applied and no pressure because otherwise the boundary conditions would be over constrained.

2) OK I will assign a negative value with a piecewise linear function. But I would think a steady state boundary condition would apply a constant value from time =0s in a transient analysis. Is that the case or I should never use steady state boundary conditions in a transient analysis?

3) Noted will create the region in CAD

4) Jon please help me with this question . It is crucial for my analysis, I need to understand how the scalar value relates to PPM. I am almost 100% sure PPM is not scalar divided by 1e+06, otherwise I would be getting concentration levels of more than 1000 PPM in my current model when realistically should be around 50PPM.

Thanks again for your help.

Regards

Roberto

Re: Car park ventilation and CO extract model

rpadovani — Thu, 12 Feb 2015 14:47:21 GMT

Hello all,

I made changes to the geometry of the car park model as suggested above and simulation had very good convergence.

I still however have issues with the scalar value. I assigned scalar value 1 to surfaces with mass flow rates equivalent to the carbon monoxide emissions and 0 to all other fresh air intake surfaces.

The scalar value of the air domain however rapidly increases during the transient simulation to levels above 1000ppm or scalar value of 0.001. Even during the first 60s when the mass flow rate assigned to the CO is zero, the scalar value around the boundary condition increases. Please note that I assigned scalar value of 0 for air domain initial condition.

Is this the correct method of simulating diffusion of carbon monoxide by applying a mass flow rate to a floor surface opening with scalar value of 1?

John Wilde can you please shed some light here?

Link for latest model is attached. Thanks

Regards

https://www.dropbox.com/s/0oie0gxvvhd2o2j/Corso%20Carpark%20Final%20Setup_110215%20v6_support.cfz?dl=0

Re: Car park ventilation and CO extract model

Jon.Wilde — Thu, 12 Feb 2015 15:52:38 GMT

Hi,

Sure I can comment. Thanks for helping so far Berkan, nice to see 🙂

You can just use steady state values on the BC's if the values are constant. With the scalar values this might even be the cause. Unless variables are changing over time, just use steady state.

The pressure on what I guess might be an inlet should just be on the top surface and should there be a scalar value here?

Do you need to turn gravity on? It seems like this might be a little more realistic with it as you have air density changing with scalar.

Mesh your fans well - we need a uniform mesh on them with 4-5 elements from inlet to outlet.

The same goes for the lower inlets - the central portion of these might only have 1-2 elements across the width, which is likely to be too little.

Hope this helps.

Jon

Re: Car park ventilation and CO extract model

rpadovani — Fri, 13 Feb 2015 15:35:24 GMT

Thanks Jon

I made all those changes and the air velocities and vectors are all looking good in terms of expected air flows from inlets and also jet fan thrust.

I am still however getting high CO ppm results and they keep getting higher and higher as the simulation progresses. The exhaust rate designed for the car park was based on the local regulation that allows a 51PPM average increase over an hour and there are some assumptions on the CO emissions per car over 2 min.

The problem I think is that the convergence takes a very long time almost 700 iterations but I setup CO boundary condition as constant. Therefore by the time the air flows are stabilised in the calculations the CO concentration is already too high. Do I need to set the CO boundary condition as piecewise linear and turn it on after a certain number of cycles like 700?

I run a time step of 0.5s and inner iteration of 1. How did you setup the solver in the smoke analysis example? Did you allow for some convergence time before turning on the fire?

My revised file is attached.

Thanks

https://www.dropbox.com/s/jsln6kbh9eoocuf/Corso%20Carpark%20Final%20Setup_130215%20v7_support.cfz?dl=0

Re: Car park ventilation and CO extract model

rpadovani — Mon, 16 Feb 2015 12:48:38 GMT

Jon

I have now run this model for 1700 timesteps but, as I mentioned in the previous post, the scalar values are excessively high. The order of magnitude just doesnt make sense based on the small mass flow rate setup in the floor boundary conditions.

I also have another question. There are several inlets in this carpark, which I mistakenly left out of the model, which are metallic louvers and therefore have some resistance for the fresh air intake. In this case it would be incorrect to assume Pressure of 0Pa. What is the correct methodology? Shall I assume some static pressure, how do I estimate this value? Or shall I use a different boundary condition?

Thanks

Roberto

Re: Car park ventilation and CO extract model

Jon.Wilde — Mon, 16 Feb 2015 13:20:53 GMT

Hi,

I've had a chance to look at this model and have a few comments that I hope will help.

Is the P=0 on the top an inlet or outlet? Might need a Scalar and temp here?

Yes, you should model all inlets, again with P=0, scalar and temp. You could look to model a resistance to help capture the louvre, would it make much difference given the low flow rate? Could just try without initially.

Are you confident with the 0.28 cm^2/s diffiusion coeff? This seems quite high to me and would certainly effect the results, allowing the Scalar 1 to spread faster. I would have thought it would be lower, although I cannot find a value at the moment, I appreciate this is not so useful. Anyone else?

Hopefully this helps.

Kind regards,

Jon

Re: Car park ventilation and CO extract model

rpadovani — Mon, 16 Feb 2015 14:07:01 GMT

Hi John

The P=0 on the top surface is supposed to be an outlet , that is to represent the opening to the open carpark on the floor above. I tried to simplify the geometry and did not draw the ramp up to the 1st floor.

Look at the results of velocity vectors at 1700 timesteps, there is air going out and coming in almost similar to a vortex. Refer to image below. How do I know if this is indeed an inlet or outlet when there are several exhaust grilles in the proximity of this opening?

I thought about adding resistance material in the louvered inlets but as you mentioned it would be another unknown variable to impact results. I will try initially without resistance as you mentioned.

I have to be honest that I google searched Carbon Monoxide diffusion coefficient in air and found 0.208cm^2/s but was not a known source like ASHRAE or CIBSE. I would appreciate if anyone in the forum could let me know if this is a reasonable value.

As I mentioned in my previous post , do I need to introduce the CO mass flow rate later in the transient simulation after all air velocities converge at about 1000 timesteps?

Another observation is that even after refining the mesh of the fan element and the region in front of the jet fans, I am getting nowhere near the velocities/thrust claimed by the manufacturer ( min 5m/s for almost 20 meters forward of the jet fans) as shown in the image below. Thanks again . Regards

Re: Car park ventilation and CO extract model

Jon.Wilde — Tue, 17 Feb 2015 09:02:19 GMT

Hi,

Ideally we would only have any boundary condition as either an inlet or outlet. Typically we extend these outlets until flow is only travelling in one direction - if you use the bulk calculator, which way is the flow mainly travelling? I think first I would think about extending this volume upwards.

Saying that, maybe in reality it is both an inlet and outlet and flow does indeed pass through it in both directions?

You could try running with a Scalar=0 and Film coeff of 5W/m2K at ambient temp and see if this allows the incoming flow to be reset to the correct values and also allows air to escape sensibly.

What does your mesh look like on a cut plane through your fan and the air ahead of it?

Regarding when to add the CO - I would try to match reality as closely as possible. So if it is not added until the flow is established, we should probably take this approach.

Kind regards,

Jon

Re: Car park ventilation and CO extract model

rpadovani — Thu, 19 Feb 2015 13:41:28 GMT

Jon

According to my hand calculations of the bulk airflow movement in the space, the large top opening surface is an outlet. However some air will escape back into the air domain because there are mechanical exhaust grilles just below the ramp opening to the floor above.

I also added the 3 louvre areas that were missing in the previous model and it looks like from the run so far that it gave a pressure relief and a more balanced air flow pattern between the top and bottom half of the car park.

I extended the mesh region ahead of the jet fan to 10m as shown on the image below

I also added a linear piecewise function for the CO inlet so it only goes from scalar 0 to 1 after 1000 timesteps.Mass flow rate also goes from 0 to minimumm flow rate after 1000 timesteps. So far so good but I have to wait for 1000 timesteps to verify CO air dispersion.As I mentioned all of my previous results had a very very large average scalar number.

Last question, is there any way to simplify the mesh since I have 18 million cells that is taking me an average of 700 timesteps per day (24hrs) to run? I need to complete 1 hour or 3600s.

Thanks

Roberto

Re: Car park ventilation and CO extract model

Jon.Wilde — Fri, 20 Feb 2015 10:38:22 GMT

Hi,

This looks better. It is OK to have a little recirculation at the outlet - so long as you have sensible conditions like pressure and a film coefficient there.

I would suggest that the mesh outside of the region looks pretty coarse - perhaps a manual mesh might be far more useful here? I would try it out. I am sure this would help cut down on the number of elements too.

Kind regards,

Jon

Re: Car park ventilation and CO extract model

rpadovani — Sun, 22 Feb 2015 23:13:14 GMT

Hi Jon

I added the film coefficient to the large top opening (outlet) as you suggested and also introduced scalar value of 1 for CO after 1000 timesteps. I understand we have to follow the actual operation of the ventilation system, but my question was more in regards to the time to converge simulation versus the actual time to develop the airflows in real time operation . I mean in real life the jet fans and extract fans wouldnt take 10 minutes to fully develop airflows to nominal velocities.

The mesh is not ideal as you mentioned . I agree´with you that a manual mesh would give a smoother transition from a detailed area with fine mesh to a coarser mesh area. The problem here is that is going to take me a considerable amount of time to remesh with the risk of having the same issue with the high scalar value at the end. In addition I would think this manual mesh would result in a larger number of elements even though the mesh is more optmised?

Anyway, I did run this model for 1660 timesteps over the last 3 days. The first 1000 timesteps without the boundary condition of CO with scalar value 1 were looking very good with the exception of some recirculation in some of the inlets and the outlets. The air velocities after the jet fans were looking much better, closer to the manufacturer specs. Then after introducing the CO scalar 1 at 1000 timesteps, the average scalar value in the air mixture domain went ballistic to values at 600 and -10000. At 1600 timesteps the scalar value was above e+06, clearly diverging. If I run the simuation with the CO boundary condition as constant scalar 1, the problem doesnt occur ( well I didnt run constant scalar 1 past 500 timesteps to verify if it is the recirculation that is causing the problem).

My solver parameters were:

timestep: 0.5s

inner iterations:1

gravity on

advection 5

Is there anything else I can do apart from doing a manual mesh ? I am almost convinced Autodesk CFD cant handle problems with diffusion of very small concentration of CO in air. The results always start at average scalar value of 10e-02 (when I run constant scalar). This is equivalent to 10,000PPM. I have a total mass flow rate of 4,245g of CO per hour for the whole area of the car park or approximately 1L/s of CO volumetric flow rate. Considering the total volume of the car park is approximately 10,000,000 L, an average scalar value of 0.01 would equal 100,000 L. As you can see the order of magnitutude of the scalar results does not make sense.

Is there any documented case study for CO extraction? I can see that 99% of the cases discussed here and in the youtube channel are about smoke ventilation where the scalar value are much higher than the CO concetration case.

Is there anything I can do in the solver parameters to fix the scalar problems?

Is there a better way of setting up the boundary condition for the CO mass flow rate so that the CO velocities are not high and CO velocities are not vertical in the Z direction? I need to increase the area of the CO boundary condition away from the main airflow domain, is that possible? What else can I do?

I am sending a copy of the latest model file in the dropbox link below. I am also pasting images of the recirculation of air in 3 of the top inlets and the 2 outlets and an image of the jet fan air velocities. The recirculation of the inlets occur in a low pressure zone of the car park at the top left. There are 4 new inlets I added in this top left region to represent the louvers ( which I havent added any resistance) and low velocity air is actually escaping the inlet rather than entering.Do I need to delete scalar and temperature boundary condition in theese inlets where results show air exiting?

Thanks

Roberto

https://www.dropbox.com/s/y7etzhdtx63pq9l/Corso%20Carpark%20Final%20Setup_200215_support.cfz?dl=0

Re: Car park ventilation and CO extract model

Jon.Wilde — Mon, 23 Feb 2015 10:15:50 GMT

HI,

Let me see if I can help here. It might be better to number your points, there seem to be a lot, I willl try to answer everything.

Firstly, a lower diffusion coeff is often easier to run, so I think we could rule that out as the problem
I am looking at your model right now. We do need to be sure that anywhere flow can enter has a Scalar value assigned. There are a few openings without - if they are not 100% outlets, then I would add this. A film coeff also. As I said before though, ideally we want zero recirculation over a boundary, this might be the main issue
I am not too clear on the design spec you need to work within here. But could you run this in two stages? First a Steady State analysis to get the flow moving with just steady state flow conditions and see what happens. Does the flow enter and exit where you expect it to and do you have the right boundary conditions assigned? Then we could use re-initialise the Initial Conditions and run a transient study from the last iteration. As the densities are so similar, you could even lock the flow (by unckecking the 'flow' box) and running a thermal only analysis. Might that work for you? It would certainly be faster
I would try 3 inner iterations (as per the guide) and see what the convergence looks like. Are we flat lining for each of the three or is CFD unable to converge on the timestep before moving 0.5s to the next?

I think that covers everything?

Best regards,

Jon

Re: Car park ventilation and CO extract model

rpadovani — Mon, 23 Feb 2015 12:17:01 GMT

Thanks Jon

I will apply those changes and see if it works.

One last item from my previous post:

5. Do I need to change direction of mass flow rate applied for CO boundary condition? Would the boundary condition on the floor be affected by the airflow in the main domain? I am running a test shoe box model with one inlet and one outlet but boundary conditions for CO mass flow rate on the side walls and results so far are more within the order of magnitude that I expect in terms of CO concentration. What do you think? What if I have a volume connecting all the existing CO boundary condition surfaces and apply only one boundary condition horizontally on this bigger volume so scalar 1 mixes with scalar 0 away from main air domain, almost like an underfloor air distribution system?

In regards to your comments on item 3, shall I run steady state with scalar 0 boundary conditions only and introduce scalar 1 CO for transient analysis afterwards?

The regulatory code for ventilation of car parks in Australia basically stipulates that a max 51ppm rise over a 9ppm intial condition is allowed over an hour at exit peak time with 50% of the car park full . There is a methodology to calculate the total CO mass in this peak hour based on driving distances and number of parking spaces.

Thanks and will let you know if the below changes fixes the model

Regards

Roberto

Re: Car park ventilation and CO extract model

Jon.Wilde — Mon, 23 Feb 2015 12:59:28 GMT

Hi,

How you have this setup so far should be OK with regards to Scalar 1 I think. Especically if you establish a flow field first.

Run the Steady State without scalar on, then you don't need to worry about changing the model at all. You can leave all the boundary conditions as they are but just change them to steady state.

Kind regards,

Jon

Re: Car park ventilation and CO extract model

rpadovani — Fri, 27 Feb 2015 14:03:24 GMT

Jon

I run the steady state over 868 cycles and converged nicely with velocities and turbulent energy and dissipation almost constant towards the end. The recirculation was reduced significanlty with the film coefficient. I also added resistance in the openings with louvers with 66% free area in the outward direction. and mesh was refined further from last model.

I then checked all boundary conditions and added the scalar 1 to the floor boundary condition surfaces.

The simulation is running at 120 timesteps now and the scalar values are already unrealistically too high.

As I was reviewing the model again, I noticed I set the CO scalar 1 mass flow rate to 0g/h during the steady state simulation. This would completely disregard the mass flow rate of scalar 1 during the transient simulation since "flow" is unchecked.In this case scalar 1 will enter the air domain with a very high velocity which explains the high scalar values.

Questions:

1) Can I rerun my steady state with the mass flow rate for scalar 1 turned on (but CO set to scalar 0) and resuming from last iteration 868? Would the model converge again with this additional boundary condition in steady state?

2) I am running inner iterations for transient to 3 but with a timestep of 0.5s the simulation for a whole 3600s will take almost 2 wks to complete. Would it be reasonable to use 1s timestep?

Thanks

Regards

ROberto