CFD of HVAC/Natural ventilation

[brane1012]

Hi!

I am new user using CFD simulation software. My first task is to model the natural ventilation of hotel atrium. Because of the very warm climate the natural ventilation will be modeled in combination with FanCoil (FC) units. I have few basic questions about modeling specific items:

1. Is it possible that simulation CFD software recognizes the names of elements imported from REVIT?! For example - in Revit I have basic wall and when imported into simulation CFD it becomes CAD Surface XXX (like everything else).

2. How should I model supply/return diffusers of FanCoil unit? Let's say that supply and return diffuser of FC unit have each flow 500 m3/h. Should I define 500 m3/h only on supply diffuser and then on return diffuser define pressure p=0 or should I define flow on supply and on return diffuser?! One more thing to note - I have multiple FC units all around atrium so I have multiple supply and return diffusers.

3. How should I define floor FC units? Should I only define it as supply diffuser or there is somekind trick how to also define intake of air?

4. How should I define the entrance of fresh air used for natural ventilation? Should I define that (how?) on the surface on which I want that air to enter into the building or should I simply just delete that surface?

Best regards, Branimir!

[srhusain]

You can retain the solid wall (not suppress it) by 1) applying a thermal conductivity to same which is equal to your desired film coefficient multiplied by the wall thickness and 2) applying a temperature boundary condition on the outside of the wall.

Thus kWall = hDesired x wallThickness

Hope this helps.

[brane1012]

Yeah, I get that. That is thermodynamics.

But mostly I get a U factor from the manafacturer and in that article (which I posted in my last post) they are describing where should I define that U factor. And that's a bit confusing and I don't get it...

[srhusain]

If you have the U factor from the manufacturer, you can convert it to an equivalent thermal conductivity using the relationship I mentioned before- think of the U-factor as a film coefficient.
On a separate note, this relationship has nothing to do with thermodynamics 🙂

[Jon.Wilde]

Check out the link here too.

[Jon.Wilde]

A couple of other points - move the BC's you are applying to the top of the air extensions you have and leave them meshed. Really we need these lengths of inlet and outlet to ensure well developed flow entering and no recirculation over the exit. I am sure we covered this previously so sorry if I am repeating myself.

Ideally:

Inlet length = 5x width

Outlet length = 10x width

Your mesh is very coarse, I suggest you refine it. It is clear that the results are changing with the element boundaries and are not smooth as they should be. The floor really needs 2 elements through it's thickness to allow neat to propogate realistically.

Be aware of your convergence too. It should look smooth and all lines should be flat by the time the analysis is complete. The fact that these are so rough points to poor meshing, which should also change the results.

Also remember that these analyses are not comparable, one will have heat radiating from the floor (as it is meshed) and the other will not.

Hope this helps.

Jon

[brane1012]

Meshing I get...I will fix it, that is not a problem.

One thing that I didn't understand from your post:

Also remember that these analyses are not comparable, one will have heat radiating from the floor (as it is meshed) and the other will not.

 What is then heating the room in non meshed (suppressed floor) scenario? Isn't that suppressed floor (temperature boundary condition) also radiating?!

[Jon.Wilde]

Hi,

If you have a meshed part adjacent to the air, then the solid part would radiate according to it's own emissivity value.

If you suppress this part and assign a temperature there is no solid part to use, so CFD would use the emissivity value of air, hence the difference.

Does that make sense?

Thanks,

Jon

[brane1012]

Yeah,it makes sense. As soon as I think I am near to solution I make one step backwards 😃 then my simulation is pretty wrong...because I thought if I suppress the floor cfd would calculate radiation with my suppressed floor...but now seems I was wrong...then basically I dont have idea how to accuratelly simulate floor heating...from my hand calculations I know the total heat generation of floor and floor temperature..but I dont know how to use that in cfd 😞

[Jon.Wilde]

Well, you could use a temperature and change the emissivity of the air to that of your flooring. That would be the only wall where the air emissivity is used right? All other walls have a solid so they would not be effected 🙂

[brane1012]

Yes,that was my first idea...and in this case is ok...but in more complex situations (like when I have wall and ceiling heating) that would be problem...

Only thing that comes to my mind is that I model few masses inside revit and define complex floor. With correct dimensions,correct conductivities and everything on each part of the floor(mass)...and then I put total heat generation on part of the floor that emmites heat...

[Jon.Wilde]

Yes. So it sounds like if you apply a heat gen right now then it is not like reality - when really it should be.

We should be able to get good results with a heat load as it is essentially the same. With a better mesh you might be OK.

[brane1012]

Hm, I have done further research...

And I came to few conclusions...Feel free to comment...

First I tried with heat exchanger because floor heating basically is heat exchanger (water to air) but then I realized that it would be to complicated to simulate floor heating like this.

Then I tried defining the Radiation "fake internal BC" - on the floor top surface. Suppressed floor and ran the simulation. And it seems it works. The room temparature are now much more realistic to me. The only problem is now that I can't calculate heat flux of the floor because it is suppressed.

I attached the picture with simulation results.

Best regards.

[Jon.Wilde]

Hi,

I think you have answered your own questions regarding the heat exchanger. 

Take a look at this link about radiation though, it describes what that boundary condition is doing: Simulation CFD Heat Transfer Boundary Conditions.

Should be a pretty simple model this, provided you capture the correct inputs.

[brane1012]

Hey again!

I have done further research about how to simulate radiant heating and I have come to some conclusions...

The best help what could I find is this http://au.autodesk.com/au-online/classes-on-demand/class-catalog/2013/simulation-cfd/sm3243 (how to simulate starts at about 1h:09min).

Basically, they simulated radiant heating that they defined temperature boundary condition on the radiant heater which is in their case air (please take a look inside video). I think they made a little mistake there because emissivity factor of air is higher then other materials. So I simulated my radiant heating as radiation boundary condition with defined emissivity and temperature (also on air as described in video).

I got pretty interesting and I think realistic simulation. So please take a look https://www.wetransfer.com/downloads/b00b9929073fc4024f01d0ad5b4b532920150201144907/32cca6  What do you think about simulation?

Btw, what is the best material to simulate lights? Is glass ok?

And do you have (or do you know where can I find) any models of sitting and standing humans available for download?!

Best regards!

[Jon.Wilde]

Hi,

This looks good.

Some small pointers:

• I would refine the mesh more
• The lights have one element through their thickness - 2 is a minimum through solids where we want to try to capture a thermal gradient
• The inlets have only one element across their thickness, 4-5 should be the goal
• There are human models around but I'll have to leave it to someone else to reply, I don't have any myself

Good looking model though, pleased to see you are getting there.

Best regards,

Jon

[brane1012]

Hi again!

I have done a new simulation and I have a question about my result. As you can see in attached images I simulated air flow from a diffuser. When the air leaves the diffuser it starts to move/rotate towards the wall. Is that normal? Shouldn't it go towards the middle of the room?

Walls don't have boundary conditions so basically they are perfectly insulated.

[srhusain]

The jet proximity to the left wall will cause a recirculation which will in turn push it aside. As you move the jet toward the center, you should see this effect mitigate.

[brane1012]

So basically you are saying that mine flow is correct and realistic?!

[Jon.Wilde]

You could test this theory with a refined mesh - see if the results change at all. Makes sense to me though, there would be a recirculation on the left of the jet as it exited and this could easily nudge the flow to the right.

I would also use ADV5 here - I've seen the coanda effect work really nicely with this and you may have this trying to occur down the side wall - just a thought.