CO Generation in Car park

[Anonymous]

Hi. I need help on Car park ventilation system . Car park consist of -

1. Two Jet Fan= 1200 l/s

2. Opening (car entry/ exist)= 9 ppm CO concentration is assumed at all-natural ventilation. 

4.CO Generation =0.0846 g/s

5. Mechanical exhaust= 5600 l/s

objective :- To find CO concentration and to find optimal location of jet fans .

I have created the model in Revit . It is assumed that CO source are located in Driveways . This is what i have done . 

Material,

scalar mixing of Air  & CO

Density of Air :-  1.225 kg/m3

Density of CO :- 1.14 kg/m³

Two Jet fan with flow 1.2 m³/s and 1200 rpm

Boundary condition,

At co vent :- Mass flow rate =0.0846 g/s , scalar  transient 

At Mechanical exhaust :-  Volume flow rate = 5600 l/s, scalar  transient 

At Jet fans :-  Volume flow rate = 1200 l/s, scalar  transient 

At ramp / Natural air inlet = pressure 0 , temperature=26 °C , scalar = 0.000009

Solution,

Transient for time = 1 hrs 

Diffusion coefficient of CO in air = 0.662 cm2/s 

Problems :- 

 CO concentration does not change with time and i am not getting proper results. I cannot justify  use of jet fans from my result . I ran it for 1 hr and my CO concentration decreased to 2 ppm at end which is not possible so there is something wrong with my boundary conditions . I am new to Autodesk CFD i have used Ansys Previously and my results are completely different . I have attached  CFZ file please review the file and let me know fixes i need to make.  

[Jon.Wilde]

Thanks for posting, I have taken a look and can see a lot of things that need to change:

1. Suppress the solid parts unless you need to see heat transfer through them
2. You cannot assign any internal Boundary Conditions (BCs) and all of yours are
   1. Move the inlet and outlet to the outermost surfaces
   2. All the internal inlets need to be assigned to parts that are suppressed from the mesh
      1. I would also suggest you recess them into these parts a little bit to better reflect reality or they will simply diffuse
3. The jet fans cannot be modelled like this. I would suggest you have a cuboid with the fan assigned (to move the flow) within the casing. It needs to have a uniform cross section
4. Remove the scalar from your outlet, I would suggest you do not know this value and this is over constraining the model
5. It would also be far better to have cuboid extensions (5x length vs width) on the inlet and outlet with the BCs at the end, not so close to the internal air volume
6. Your air material - is CO or temp the overriding factor? It might be that temperature is, you need to decide and define the material with one or the other
7. All inlets need a temperature assigned, some are missing this right now
8. I would get this running steady state (ss) first, there are a lot of things to fix before jumping into transient
   1. Even when you do, I would run flow first as SS, set initial temperature and scalar conditions to all volumes and run the thermal as transient with the flow locked - much faster! It would mean you are not accounting for gravity of course
9. If you run it all as transient, you will need a far smaller time step 1s or less I would guess
10. Within physics you need heat transfer and gravity on
11. I didn't get to the meshing yet :)
    1. I am confident that you need a finer mesh than the default, especially where the air makes a jet or you have complex flow

Hope that helps to give you a good start.

Did you see the webinar we ran on this?

Thanks,

Jon

[Anonymous]

Thank you for your response. I tried to simulate as per you suggestion but result was not satisfactory . I should also add i am new to this software so i might have missed something .I have few problem 

1. I am trying to simulate CO concentration in car park . Temperature is to show room temperature and temperature of co when it is exhausted from car so that it reflects more natural condition. 

2. I  watched you webinar and read few your previous post on tunnel ventilation still i could not solve my issue on jet fans. so i decided to run the simulation without using jet fans . Instead of increasing my CO concentration decreased which is funny . 

3. I have also added scalar of 0.02 in my co- source because it is assumed exhaust from car 

without using catalytic converter has 30000-20000 ppm CO concentration.

4. sorry I did not get your point number 2 , 

1. "I would also suggest you recess them into these parts a little bit to better reflect reality or they will simply diffuse"

I have attached CFZ file and a screenshot of error i am getting for jet fan .please review the file and please help me . 

[Jon.Wilde]

This looks a lot better, nice work 🙂

A few small issues remain.

Well, this is a big one but easily fixed. I think you might have the air volume rather than the ceiling suppressed, at least that is what I am seeing here.

Your jet fans are also close to working, you just need a cuboid sitting in here with a flow rate assigned to it (zero rpm):

I would still extend the inlets and outlets so they are about 5x longer than their width (or height, whichever is larger).

That ought to leave you with a nicely running model I think!

[Anonymous]

Thank you for your prompt reply. Here are few changes i made according to your suggestion . 

1. I was able to apply jet fan material according to your suggestion . Do the material itself is a boundary condition for Jet fans ? 

2. I have applied co-air mixture instead of suppressed ceiling . 

3. I have not extended the inlets and outlets yet . Can i extend them in CFD itself or i should go back to Revit to change the geometry . 

Problems i am still facing :-

1. CO concentration is above 500 ppm which is undesirable  . It have simulation results using Ansys which is bellow  60 ppm .

2. I cannot still verify my jet fans are working or not . I your webinar Flow from Jet fans are clearly visible but i cannot see it in my model . 

3. I case of Scalar , I have set 0 for pure air & 1 for CO . 9 PPM CO means 0.000009 scalar & 20000 PPM means 0.02 scalar ? I just want to cross-verify .

4. Can we use some thing like CO sensor . Suppose i am interested in CO concentration at particular CO sensor at certain period of time . IS this possible using Autodesk CFD ? 

I have attached CFZ file and a screenshot of Simulation result . please review the file and help me. 

[Jon.Wilde]

1. I was able to apply jet fan material according to your suggestion . Do the material itself is a boundary condition for Jet fans ?  You need to go back to Revit and model a cuboid shape within rectangle indicated above, make it as thick as the central portion of the case too. You definitely cannot assign a fan material to the casing, this should just be whatever material you use in reality. It would not have a BC assigned but a fan material.

2. I have applied co-air mixture instead of suppressed ceiling . 

The ceiling is concrete or something and not air I would presume? Assign everything as it is in reality. You can also just suppress it from the mesh as I do not think you need to include it in the calculation

3. I have not extended the inlets and outlets yet . Can i extend them in CFD itself or i should go back to Revit to change the geometry .  Yes, please do this in Revit (might as well recess those internal outlets while you are there too 😉 )

Problems i am still facing :-

1. CO concentration is above 500 ppm which is undesirable  . It have simulation results using Ansys which is bellow  60 ppm . Sure, this is because the setup is incorrect, let's question the results once we know it is running well 🙂 I would also suggest comparing to test and not another software, which might also have errors, although I see the point

2. I cannot still verify my jet fans are working or not . I your webinar Flow from Jet fans are clearly visible but i cannot see it in my model . As above 🙂

3. I case of Scalar , I have set 0 for pure air & 1 for CO . 9 PPM CO means 0.000009 scalar & 20000 PPM means 0.02 scalar ? I just want to cross-verify .  I think yes, check out this article: PPM

4. Can we use some thing like CO sensor . Suppose i am interested in CO concentration at particular CO sensor at certain period of time . IS this possible using Autodesk CFD ? I do not think we can, others might correct me here?

Are you now confident that your air material should very its density by scalar and not by temperature?

Hope that helps

Jon

[Anonymous]

Thank you Jon. You have been great help. I have updated model as per your help. 

1. I have extended inlet and outlet 5X length and recess them . 

2. I have assigned Fan material as you suggested . I think fan is  working now (correct me if i am wrong )

3. I have refined mesh size. 

Query 

Are you now confident that your air material should very its density by scalar and not by temperature?

 Yes, i think so . Density depends on temperature so is not it the same since both are interrelated? Also how do i define CO concentration as per Temperature? 

Result,

Still result are not good. Correct me if  is the setup is incorrect . I have attached CFZ file and Screen shot of result . Please review the file and help me.