# HVAC modelling

 Register Blogs Members List Search Today's Posts Mark Forums Read

October 25, 2011, 13:58
HVAC modelling
#1
New Member

Join Date: Oct 2011
Posts: 6
Rep Power: 7
Hi,

Excuse me for my weak English. I'm doing a HVAC simulation to discover the air speed and temeprature distribution of a small building. Then, I would like to do a transient simulation of the heating or cooling of this building, but I'm stucked at the steady part. This is going to be a part of my bsc thesis, so I'm quite newby in cfd, but I try to do my best.

I have both solid (walls) and fluid domains (air of the room). The walls are heated from the outside, and there are 3 inlets for the fresh air, and 3 outlets.

My problem is probably based on buoyancy, because without buoyancy everything is fine, the streamlines are going in the right direction, the temperatures seem correct, the heat convection is working well etc. But as I switch on buoyancy (direction of gravity is correct according to the abs. pressure), leaving everything else the same, the streamlines just make a 90deg turn after they enter to the main air domain, and they don't even find the outlet. Of course it does not converge, however because of the high timescale factors the imbalances are quite good. Also, when the buoyancy is switched on, there are problems with the outlets (wall has been placed to 1-5%).

I use SST turbulence (inc. visc. work term), incompressible fluid (air at 25) because of the low speeds (0.3 m/s @ inlet), Total energy, heat transfers are defined for the walls, and for the windows (1 of the walls is almost completely a window, but I just model this window by the heat transfer coefficient).

I upload a .doc which includes a picture of the geometry, afew other word about it, and another one with the solver specifications, and I'm curiously looking forward to your answer.

Best regards,
Istvan
Attached Files
 error_small.doc (72.5 KB, 30 views) building.doc (66.0 KB, 33 views)

Last edited by Keppi; October 25, 2011 at 14:17.

 October 25, 2011, 17:45 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,808 Rep Power: 107 Where is the air outlets?

 October 26, 2011, 00:32 #3 New Member   Join Date: Oct 2011 Posts: 6 Rep Power: 7 The 3 outlets are located on the ceiling, just as the 3 intlets. Both the inlets and outlets are really thin (inlet: 1500x18mm, outlet 1500x31mm, when the whole domain is 11m long and about 6m wide). You can see them in the building.doc, just tell me if it's clear now or not, because I can upload more picture if you want. I couldn't do that yesterday, because I don't have the program at home, so I just used some previous pictures of it.

 October 26, 2011, 07:21 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,808 Rep Power: 107 I would not use pressure averaging over your outlets, just specify a static pressure. Also you might get back flow at some outlets. This might not be a problem in this case.

October 27, 2011, 01:44
#5
New Member

Join Date: Oct 2011
Posts: 6
Rep Power: 7
I upload a picture of the result. I changed the outlet as you said, and I also changed to air ideal gas, instead of air 25deg.

So the problem is, that the incoming cool air is directed to the floor (can be seen in the .doc in my previous post), and supposed to reach it. But just after it enters, it makes a fast 90deg turn, and flows along the ceiling.

In fact, there is a slight increase of the height (the ceiling is not horizontal), and the incoming air is moving actually upwards. Like if it would be hotter than the surronding air. But the incoming air's temperature is 23deg, and the average temperature of the domain should be around 24.5 degrees, and I initialized it to 25 degrees, to see what's happening, but everything remained the same.
Attached Images
 error.JPG (70.1 KB, 48 views)

 October 27, 2011, 06:16 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,808 Rep Power: 107 These sort of flows are strongly affected by convergence. If you don't believe it then converge tighter. But it might be real - look up the Coanda effect on google or a fluid textbook.

 October 27, 2011, 06:52 #7 New Member   Join Date: Oct 2011 Posts: 6 Rep Power: 7 Thanks for you help ghorrocks! Yes, Coanda effect is possible. The thing what I still don't understand is that why does it happens only when I switch on the buoyancy? Without buoyancy the flow just goes down directly to the ground. Also, the RMS convergence is quite slow, so I only let it go until 10e-3 - 10e-4. Maybe lower RMS would increase the accuracy, but according to the documentations, 10e-3 should be enough to see the global behaviour of the flow.

 October 27, 2011, 16:47 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,808 Rep Power: 107 There is a FAQ on your convergence issue: http://www.cfd-online.com/Wiki/Ansys...gence_criteria Things like Coanda effects can mean the flow is quite wrong until tighter convergence is reached. That is why you need to do a sensitivity study. Also, it is possible the result is multi-valued - that is a fully converged solution will stick to one wall, or if the initial condition has the jet attached to another wall then that is the fully converged solution as well. Do not think that a steady state simulation has only one fully converged solution.

 December 3, 2011, 11:47 #9 New Member   Join Date: Oct 2011 Posts: 6 Rep Power: 7 Dear ghorrocks, thank you for your kind reply, and sorry for my late one. I considered the problem solved, and the cause is probably based on the cold temperature of the ceiling, which cools down the whole domain. So the incoming air's temperature is simply higher than the domain's temperature, that's why it moves upwards. Also, I would like to add humidity to the air. To do this, I added a new material with Water as ideal gas (or maybe I should use Water Vapour at 25, or else?), also Continuous fluid (or Dispersed would fit better?). In the multiphase options I switched on the Homogenous model option, since I don't want the humidity different velocity field than the dry air. Heat transfer is Total Energy, and Turbulence model is SST, as previously. I put buoyancy turbulence to production and Dissipation. The fluid buoyancy model is Density Difference. I didn't add interface transfer model, nor mass transfer. I also didn't specify radiation options on the solid walls yet (only Monte Carlo is avaliable). My question is, that do you think if these options fits well for a HVAC simulation if I would like to simulate air with humidity?

December 3, 2011, 13:07
#10
Member

Paulo
Join Date: Jun 2011
Posts: 33
Rep Power: 8
Quote:
 Originally Posted by Keppi Dear ghorrocks, thank you for your kind reply, and sorry for my late one. I considered the problem solved, and the cause is probably based on the cold temperature of the ceiling, which cools down the whole domain. So the incoming air's temperature is simply higher than the domain's temperature, that's why it moves upwards. Also, I would like to add humidity to the air. To do this, I added a new material with Water as ideal gas (or maybe I should use Water Vapour at 25, or else?), also Continuous fluid (or Dispersed would fit better?). In the multiphase options I switched on the Homogenous model option, since I don't want the humidity different velocity field than the dry air. Heat transfer is Total Energy, and Turbulence model is SST, as previously. I put buoyancy turbulence to production and Dissipation. The fluid buoyancy model is Density Difference. I didn't add interface transfer model, nor mass transfer. I also didn't specify radiation options on the solid walls yet (only Monte Carlo is avaliable). My question is, that do you think if these options fits well for a HVAC simulation if I would like to simulate air with humidity?
Couple weeks ago, i had had this question, because I was doing simulation about Evaporative cooling in HVAC. I guess to obtain Humidity you need of psicrometric chart of the place. So, i dont know if CFX consider this when you set the reference pressure of the domain.

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post xlxc34 Main CFD Forum 0 June 24, 2011 04:42 Martin Main CFD Forum 3 October 14, 2008 05:16 Carlos FLUENT 0 September 26, 2008 11:37 A Siemens 1 March 5, 2004 10:32 Harry Qiu FLUENT 0 July 1, 2001 01:40

All times are GMT -4. The time now is 20:21.