Greenhouse effect by infra red radiation

[david.moreira]

Hello friends

urgently I need your help by Favot, for my thesis architecture
I am using CFD simulations to test different designs of greenhouses and the effect on ventilation (ACH (Air Changes per Hour)), temperature and humidity.

the attached model represents the current design of the greenhouses of my case study, I will use from baseline .. my aim is to test the 2 most critical, high summer temperatures (40 ° C) cases, and high levels of humidity in winter (100%), as the case summer I placed 29 ° C as a condition of temperature in the mass of outside air (variable), the air inside the greenhouse I have left with a condition of film coefficent 40 ° C and 20W. the rasultado has given me pretty well, but I would like to achieve simulate 40 ° inside the greenhouse not by a coefficent film, otherwise than by radiation and the greenhouse effect due to the materiality of outside the greenhouse. That's possible??(Ie, product exit block infrared radiation inside the greenhouse)

I think that would bring realism to my study, because although in the present case, this well start with 40 ° C .. the variation of my design could vary that condition, you understand?

in other words, I'm trying to build a single CFD model that can be used to analisar different geometries (with Design Study Builder) where the imputs are only the following:

-geometry
-materiality
-wind speed
-direction of the wind
-temperature land
volume-temperature outside air
-geolocalizacion
-date
model-guidance
-humidity produced by plants

and as ouputs:

-temperature inside the greenhouse
Ach (Air Changes per Hour)
-humidity

Note: currently have the temperature inside the greenhouse as an input and not an ouput

Thank you very much in advance

[Jon.Wilde]

Hi,

You would need to share a CFZ (support file) for us to open it and see what you are doing 🙂

It sounds like you need a double sided material right? So it allows radiation in but less out? I am not sure if we can do this or not, maybe with a surface material on the side of the glass though.

Do avoid using any internal boundary conditions, they are only to be used on the boundary of the model 🙂

Thanks,

Jon

[david.moreira]

thank you very much for the prompt response Jhon

I am against time and need urgent help

I attached the model format CFZ

best regards

[Jon.Wilde]

Hi,

I can see a few things to comment on here, bullet pointed for expediency 🙂

1. Remove the outlet temperature, it will be different to 29C
2. Remove the temp from the side walls and the top also
3. Right now, it looks like your greenhouse is made of air? Does it need a glass material?
4. Resistances - you have a 0.5 FAR in one direction and 100% open in the others, is that correct?
5. Remove the film coefficient that is internal to the model, boundary conditions can only go on boundaries 🙂
6. Use a film coeff rather than a temperature underneath the ground unless you are 100% sure about it - this temp would act like an infinite heat sink to maintain 20C
7. Use Advection Scheme 5
8. Get this running well with steady state before using transient
9. When you run transiently, all volumes will need an initial condition to get their temperature defined
10. Your mesh is too coarse, but that might be the last thing to think about. Ideally you need 2 elements through the thickness of any part and at least 5 through any fluid gap

Hope that helps!

Jon

[david.moreira]

Again, thank you very much for the speed.

since you posted, I worked on changes sujeridos for you and performing simulations

I have done all points, exept point 3 and 10

point 3 and had tried before but had failed to successfully
point 10 did not understand (I do not speak much English, I'm from Chile and use google translate)

the results are what I was looking around, I am analyzing the geometry is the atual greenhouses in my case study and conosco the temperature value for the dates you have selected in the settings of the sun (summer in Chile at 13:00 = 40 ° C inside the greenhouse, with 29 ° C outside temperature)

I doubt even with settings below the surface of the earth, I used a film coefficient of 20 ° C and 10W, but not if it's okay, I attached screenshots of the following results

-previous settings (attached)

-down surface temperature 20 steady state

-down surface temperature 20 transient (attached)

-down surface C film 20C 10W transient (attached)

-down surface C film 20C 10W steady state (attached)

-CFD model Setting suggested (attached)

which do you think is the best configuration for the bottom surface of the earth?

other question I have is; it is possible to obtain the ACH (Air Changes per Hour) Mass flow rate or volume of air inside the greenhouse, for the ACH as a result

Thank you very much in advance

best regards

[Jon.Wilde]

No problem 🙂

For meshing, check out our help: CFD Meshing - you need more mesh - the results should look smooth and not jagged.

I made this video also, but it is in English: Meshing in CFD (The pdf of the presentation is here, you might be able to translate this 😉 )

What you have looks loads better, great work!

I would lower the underground film coefficient to 5W but it should be pretty OK.

For air changes - go to Solve -> Result Quantities and enable LMA, this will give you the local age of air, which is very similar.

Also, leave Intelligent Solution Control (ISC) on for steady state runs (Solve -> Solution Controls). It can be off for transient.

Thanks,

Jon

[david.moreira]

Hi Jhon

again thank you very much for the help

I have done a simulation with AML, but selecting air volume inside the greenhouse with result-part does not throw me the result of the LMA, only the volume and temperature, I'm doing good or I see the LMA result elsewhere?

Thank you
Best Regards

[Jon.Wilde]

You would need to use a cut-plane/ISO surface 🙂

[david.moreira]

Hi Jhon

You've really helped me a lot with my thesis, thank you been attained to realize my study time I have left, although I still have one thing to solve, and this does not bother you more.

I have my file configured for CFD analysis and I intend to use a sequence of commands loop type script (python) to analyze many geometries (geometries as 1000) that have generated using the software Rhinoceros 5.0 format * .. and what .sat I ara my script is to open my sample file, update the geometry and save results, again and again.

The problem I have is that (I miss the process manually) to update the BC geometry remain, but I change materials,
I have tried using rules to solve the problem but it is not me, CFD does not recognize my geometrias bombres, does not recognize the materiality, when I select Rule manager-> apply now, nothing happens. you suggest me to upgrade geometry without changing the values ​​of materiality?

again thank you very much
Best Regards