Airflow Simulation

[Anonymous]

Hello fellow CFD-modelers,

My task is to model the airflow in a 2-room appartment under various thermal and humidity conditions. As a result I must locate weak spots where condensate should appear.

I am having problems in setting the correct boundaries, I read the tutorials but somehow I can't make it going.

so the question is:

what boundaries should I set, to solve following:

outside : -25 Celsius, Humidity 75%

inside: 20 Celsius, Humidity 50%

for the airflow from outside i set up temperature and humidity at the inlets. but i can t figure out how to set the initial room temperature and humidity.

Thanks a lot!!!

Alex

[Jon.Wilde]

How about a different approach, just using the dew point temp to investigate where you will have condensation rather than worrying about humidity?

Avoid internal boundary conditions if you have any assigned. Move the air with Internal Fans.

You would need to run a transient analysis and use Initial Conditions on all volumes (temp and humidity).

Hope that helps,

Jon

[Anonymous]

Hello Jon,

Thanks a lot for taking time to answer my question.

The air is evacuated by two ventilators to the exterior. Assigned here two volume flow rates.

Inlets i set to pressure 0, temperature and humidity. The air is practically sucked in.

I could not work with moist air material, used air instead.

Will try your solution and get back to you.

Thanks,

Alex

[Jon.Wilde]

This sounds sensible 🙂

[Anonymous]

Sadly, I can not get any results.

I really need some help with this. I modeled two outlets (volume flow rate) and two inlets (pressure=0, temp= -15 Celsius, humidity= 0.85).

I set initial conditions to temp= 20 C and humidity = 0.5 to every single volume.

Somehow I get a humidity of 0.2 inside after simulating transient for 2 hours in real life. As I have no experience with this software other than the tutorials, I am sure I am making some mistakes setting the simulation up.

Thanks!

[Jon.Wilde]

Are you running flow only as steady state and then heat transfer only as transient? I think this might be sensible.

What air material are you using and what time step size and inner iterations?

[Anonymous]

Hello Jon,

I used transient for all steps, with a time step of 60 seconds. I am using moist air as material.

Thanks for replying,
Alex

[Jon.Wilde]

Try converging flow first then running without flow on as transient (it will just use the same flow result for the rest of the study), should be loads faster.

A 60s time step is huge if you don't do what I suggested above. Very difficult for CFD to converge on a point 60s into the future and then jump forwards again. Maybe a 0.5s time step could work like this.

Using the two step approach you can probably get away with 10s or 20s as a time step with 3 inner iterations (guestimate)

[Anonymous]

Hello,

I did as you suggested. Sepparate analisys showed good results for flow and heat transfer. However, I still get 0% Humidity inside. What are the proper simuation settings for a scenario:

Mix inside air (with initial temperature and humidity) with air sucked from outside (with different temperature and humidity)

Thanks a lot

[Jon.Wilde]

I can't see any P=0's as openings, I suspect that is your issue 🙂

Do not use 'unknown' conditions for this type of analysis (they are for compressible models usually).

Hopefully that helps!

Jon

[Anonymous]

This was my last try, I hoped it would work but it didn't. P=0 didn't help that much either. It seems that the humidity of 0.5 is somehow not initialized. 😞

Thanks,

Alex

[Jon.Wilde]

A few points:

1. Your mesh is very coarse, the results are not at all smooth
2. Refine your inlets and outlets to ensure 3-4 elements through the thickness of an air volume (absolute minimum)
3. Try a smaller time step, 10s is large to calculate air flow - use 0.5s as recommended before
4. Humidity works fine for me (CFD 2016 SP2)
5. Turn off the result quantities you don't need 🙂

Humidity (with a coarse air mesh still):

[Anonymous]

I will be back with updates. What value does the blue color has in your simulation?

Mine brings it up to 0.03 or such near to zero values.

That is why I think I am doing wrong. it s almost physically impossible to dry out the air completely in a few minutes :((

Thanks,

Alex

[Jon.Wilde]

Hi Alex,

With a mesh this coarse, that is exactly what I would expect - CFD is trying to produce a nice gradient but there are not enough elements for it to do so. Try adding a mesh refinement region - I think this will smooth out the transition to something a lot more realsitic.

Thanks,

Jon

[Anonymous]

Jon,

What is the best way to refine the mesh? I am a bit overwhelmed.

Thanks,

Alex

[Jon.Wilde]

In this instance, probably a meshing region.

Did you already run through our online tutorials?

There is a nice webinar on Meshing here too.

[Anonymous]

Hello,

Thanks for linking me the tutorials. I managed to set up 4 elements in the fluid. However I got 7.5 mil elements now. Is it possible to use autodesk cloud simulation as a student? I think my laptop is about to collapse even though it has a reasonable configuration 😄

Thanks.

[Jon.Wilde]

I would think that 4-5m should be enough here - how about a manual mesh?

The cloud is only availble if you have credits unfortunately, so I think your only option right now (for free at least) is to run locally.

[Anonymous]

Hello Jon,

I did some refining on the mesh as you said, and I was lucky to be able to validate the result because the real life model has sensors allover, so thanks!

The next bug in my model that I bumped into would be the fact that I should limit the air that is sucked in.

I have to ventilators that push the air out and two inlets, where at the time i set p=0 and humidity and temp. However i need to limit the airflow volume to 30 m3/h because that is the capacity of the built in piece.

Is this setting somehow doable?

Thanks a lot,

Alex

[Jon.Wilde]

Hi Alex,

You are very welcome 🙂

Do you know what flow rates you will get from each outlet? Could you change these so that you had 30 m3/hr total?