Modeling Car CO generation in Parking Garage

[yiyuchen]

Hi All,

I have a few questions about modeling a parking garage with CO generated by a car. Here are the questions.

1. I watched the "Park Smoke Extraction" video. In the video, resistance was used to generate the smoke. For CO, what's the right approach? Here is my thought. If I use a box to represent the car, I'll suppress the box first, then pick a vertical surface, assign scalar=1 and a velocity BC to it. Is it a right way to do it?

2. This is more general. In the "Park Smoke Extraction" video, a BC (scalar=1) was assigned to the top surface of the resistance part. But reading from below, it seems BC shouldn't be applied to the distributed resistance? 

[Jon.Wilde]

Hi,

Let me see if I can help here:

1. Yes, you could take this approach if you just want to add a known quantity of smoke to the model. Recess the outlet a little into the suppressed box too, that will help with the mesh and give you a better flow distribution
2. This is the one exception where it can work. Air will pass through naturally and then switch to scalar 1 as it exits 🙂

Does that answer your questions?

Thanks,

Jon

[matt.bemis · Accepted solution]

Hi @yiyuchen,

I recently was helping a customer with a similar application and built a demo project. Check out the share file here. Keep in mind I chose to use complicated geometry because it looks good; scaling this up a ton is not realistic. I would use solid blocks. 

Copy/Pasting some information I wrote up a while back: 

Recommended Path Forward:

A pure CO inlet represents 1,000,000 parts per million, while the area of interest is 60-100 parts per million CO. The analysis should be set up different to focus in on a smaller range. Because we are not concerned with the combustion (chemical reaction) inside the engine, the tailpipe exhaust CO concentration (mass fraction, PPM) should be calculated. This will be the upper limit of CO concentration in our CFD domain, and will be assigned a scalar of 1. By doing this we are reducing the CO concentration from “Pure CO” to “ambient air”, to “Tailpipe exhaust” to “ambient air”.

There are many online calculators/resources to find volumetric flow rate of air. Doing a quick hand calc based on a 2 L engine idling at 1000 RPM, I get a volume flow rate of 16.67 L/s. At the same time, your supporting document shows the average car emitting about 13 g/min of CO. With some conversions, it appears 1 car tailpipe exhausts 20.42075 g/s of air and 0.2166 g/s of CO. This means the exhaust CO will be 10,500 PPM. We will consider this Scalar = 1. By doing this we drop our range of potential CO concentration from 0 – 1,000,000, to 0 – 10,500. This is much more attainable, and will resolve most of the problems.

How to model car exhaust in CFD:

A couple of approaches are possible for modeling the car exhaust, and depending on the size of your domain/required accuracy, one may work better than another. It is important to remember that an idling car is not adding mass to the system; the car intake sucks air in at the front of the car and exhaust through the tailpipe at the back.

My approach: Using an internal fan with suppressed housing around it and internal boundary conditions

This is considered a “closed system” and will probably be the most accurate approach. It will also be more resource intensive. It will consider of a cylindrical tube which is assigned as an internal fan, along with a suppressed solid housing around the tube.

Outlet boundary conditions: scalar = 1, temperature

Internal fan: use material editor to assign the flow rate

Comments on material properties:

While looking at the material properties of pure air and pure CO, a few things are noted. The material properties (namely density, viscosity) are within 5% of each other. Furthermore, after realizing the highest concentrations of CO in our system will be about 10,500 PPM, it is clear the dominant material characteristics will be that of air. A new material could be defined with scalar 1 having material properties of 98.95% air 1.05% CO (mass averaged), but this seems unnecessary and an overcomplication. Furthermore, due to the hot exhaust temperatures in the domain, natural convection should be modeled. This means the material properties would have to be calculated and mapped out in CFD for a range of temperatures. Considering CFD already has this data for air, I personally would just use the default material air and set it to Variable.

Check out this cool image. Notice the custom result quantity. The isovolume represents areas that have a CO concentration of 60 PPM or higher.

Thanks,

[yiyuchen]

Hi Matt,

Thanks for this example model and the explanations. This is exactly what I needed to start with. I was going through your descriptions and the model and got a few follow up questions. They are very general and are more for my CFD knowledge as to how to set up the model. Below are a few of my questions. 

1. You recommended using a fan and assign a flow rate for the fan material. What is the difference between this approach and directly use a surface with temperature/scalar/flow rate assigned as BC? I notice by using the fan, the air will travel through the cylindrical tube from inlet to outlet, so this is more realistic as what happens in a car. Is this the reason? 

2. I can do my own search, would be possible for you to share any resources that you used to calculate L/S? I guess it's case by case so I' like to my own calc too.

Appreciate your support!

[yiyuchen]

Hello, Jon,

Thanks for the response. Matt below provided a great example. Will use that as to start with!

[matt.bemis]

Hi @yiyuchen,

Happy this helped. For the sake of completeness, I am attaching 2 PDF's that will answer your questions. 

Question #1: There is 2 different options to approaching this kind of model, and you may have heard of the terms "closed system/open system". You could solve this problem using my previously described approach with the fan, OR you could use a different approach with boundary conditions, which is a closed system. Please see the attached doc titled "Setting up bcs_fans". The important takeaway here is that if you choose to use boundary conditions instead of a fan material, it is critical you suppress (from meshing) the solid that has the BC's on it. Otherwise you have internal boundary conditions which is nonphysical and bad. Both closed and open systems work.

Question #2: I just came up with this number based on an idling car (1000 rpm, 2 L engine). I made some serious assumptions (incompressible air, constant density, etc), but it should be a good ballpark number. Check out the attached "exhaust flow rate calcs". I show how to find out the PPM based on a mass average through the system, how to modify material properties, and how to make a custom result quantity. 

Please check the docs out and let me know your thoughts. I hope it helps.

Thanks,

[yiyuchen]

Thanks, Matt. For my own model, the geometry is big, I have about 5 millions elements in the model and really want to keep it simple. So a closed system for now is probably a more suitable approach for this particular case. Will make sure suppress the parts! Thanks for the documents too!

[matt.bemis]

Hi @yiyuchen,

That sounds like a good approach. Good luck with the modeling! 

Thanks, 

[yiyuchen]

Matt, another quick one. I saw your approach 1 in the PDF, there is P=0 assigned to the bottom surface of the cylinder, can I know the modeling practice here?

[Anonymous]

The link doesn't work, can you please fix it?

[matt.bemis]

@Anonymous,

We changed cloud storage providers. New link here. It's a CFD 2018 share file.