i'm now doing ventilation simulation on a room. i want to see how the heat flow up from heat source in the room. in my result the heat cannot going up, the heat just stay around the heat source. on Domain i choose Air at STP, pressure = 1,01E05 Pa, Heat transfer model = Thermal Energy, Buoyant model is 9,8 m/s2 on Gravity z comp, temp ref is 30 C. i want to know what im doing wrong?

thx before

Hi kevin I suppose you are you doing a transient simulation. what are your boundary conditions and source terms?

sacha

i have solid in the middle of a big room, the solid at 50 C temp and the room at 25 C temp, opening at roof at 25 C Temp.

now i trying to set my fluid editor in fluid domain. i think my mistake is not set the density dependency or spesific heat dependency, now i set the density depend on temperature, but i dont know about the minimum and the maximum temperature and enthalpy eqn?????

i want to ask bout the Air at STP properties form, what should i write on that form??

thx

Dear Kevin, As you said that you set g in z direction as 9.81, I suspect that you should set it as -9.81. The direction vector from the floor to the roof is in z-direction or minus z-direction?

Atit

thank you for the help, it work!

how can i know that my result is correct?? now i still not change the fluid properties, should i modified the fluid properties? (should i change the density dependency?)

Hi Kevin, are you trying to simulate a fire with that heated source? If it so, I think that your problem is that you have just conduction. Concerning the fluids and gases the heat transfer occurs mostly through convection and radiation. If that is a fire try a little exercise: set the top of that solid as an inlet for heated air. Your temperatures in the room will grow… By the way can you tell me how have you chosen the reference buoyancy temperature? I have no idea how to choose it…

To Kevin, If your working fluid is Air, I think the air in CFX in fine. I think that what you have to check if it correct or not is just your understanding how to use CFX to simulate the problem about natural convection. So pick one test case that you have the solution. For example, you can find the solution of natural convection over the flat plate from any standard heat transfer text. Then you model the condition from the text, and simulate it by CFX. If you get the same solution as the text, your understanding how to use CFX for this kind of problem is right. Therefore you can go through your problem. To Ioana, Concerning the reference buoyancy temperature, I always use the ambient temperature. From my humble experience, I found that this temperature has the effect only at some iterations from start. After some interations, no matter what is your ref. temp, it has no diferrent on your solution.

Atit P.S. Do not trust me too much. I just use CFX for solving some problems for a few months.

Hi Atit!

Thanks a lot for your answer. I try to simulate a fire into a room; well I guess I am on the good way, although I still have some difficulties: the temp at the top of the door is with 100 K less than in the experimental data. Now, I am trying to identify the causes.

Concerning the buoyancy ref temp a set it in the pre to 0…so from what you said I figure out that this cannot be the cause, right? And regarding the gravity: if the direction vector from the floor to the roof is in the +y direction, the gravity on y should be set to +9.81?

I would be grateful if you could help me with these answers, ioana

As you said you use 0 ref temp, what is the unit of the temp, C? or K? Why do you use this magnitude? By the way, because the direction of 'g' is opposite to 'Y', so the gravity in y-direction must be -9.81. I hope this help.

Atit

Hi Atit,

Thanks for you response. However at the beginning I have set the g= -9.81(y is positive from floor to the roof) but when I have look at the results: the hot air was going out trough the lower part of the room and the cold air was entering trough the upper part…so I've change the g=9.81...hmm are you sure that is with minus? And, I did a mistake when I put you last question, I was thinking to the Buoyancy Reference Density, which I have set it to 0. Do you happen to know something about this?

Have a nice day, ioana

Yes I am sure that g must be equal to -9.81. But I do not understand why do you have to use ref. density as 0, is this the sensible value? Anyway, I have some questions, 1. How do you know that you get the convergent solution? What is your convergent criteria? and what is the reason that Solver end its calculation? Is it reached the maximum iteration or the specified residual approached? If your convergent criteria is proper and Solver stopped by approaching the specified residual, I think that you have to re-consider your boundary conditions. Could you give me more information on your geometry and boundary conditions?

Atit

Hi Atit,

How are you?

First of all, yes you are right: the gravity must be set the way you said; in my case -9.81 (there is also the example from the tutorial with the cavity). So I did 2 changes in my file: 1. setting the gravity at -9.81 and 2. Changing the buoyancy ref density at 1.2 (I do not have any explanation for this, I just did it). I looked at the results and the temp looks good (although I did expect some bigger temp since the walls are adiabatic), not to mention that the hot air is going out trough the upper part of the door. (which did not happen before, with the same -9.81, but with the buoyancy density at 0.0)! However the velocity profile doesn't look good…but this is another story...

Now, a short description of my case: the simulation of the Stekcler's room: a compartment of 2.8*2.8*2.18, with an open door and a fire in the middle. In the position of the fire I considered the inlet for the methane which is entering the room trough the floor at the ambient temp, v=0.0239m/s.

I created a reacting mixture methane-air, as in the last tutorial (can combustor). The flow domain was created as well as in the tutorial (but, I've chosen the discrete radiation model, and I activated the buoyancy: y gravity=-9.81; buoyancy ref density=1.2).

For the inlet: v=0.0239, t=303.75, heat transfer=static temp, thermal radiation –local temp, component details: ch4=1.

For the opening: relative pressure=0; heat transfer-static temp-303.75, thermal radiation=local temp, component details o2=0.209.

Walls: adiabatic, emissivity=1

global initialization: oxygen –automatic with value =0.209

In my previous runs for this case I did not receive error messages, and since the residuals fall below 10-6 after 400 steps, I just stopped the simulation…

If you have any suggestion for my case I'll be very grateful… Thanks a lot for your time and contribution. Ioana

HI Ioana the Streckleer fire ha been simulated by a Dr Yehuda Sinia, who works for CFX. He presented some of his work at the user conference. His model deos not sound as complex as yours, however I'm sure you would find it useful to read. Try contacting the guys at CFX, I'm sure they will be very helpful to you ! Bob

Hi, Bob. Thanks for the tip! Have a nice day, ioana

Sorry that I reply late. I just come back from the seminar. Actually, I have no experience for the case like you. Anyway, when you said about 'Openning' as your B.C., I think that is the region that you would like the working fluid to go out, right? Can you set it to 'Outlet' and set the average static pressure to zero? I am not sure, but that might be work.

Atit

Hi,

It is rather interest to find some one working on using CFX for fire modelling. Yes, Dr. Yehuda Sinai had done quite alot of fire modelling using CFX. I got some lessons and tips from him too.

However, I am always puzzle by the BCs for "OPEN" type of boundary condition. I did quite alot of natural/forced ventilation projects, e.g. heat rejection from the a/c condensors, I always got some funny result for "pressure" type of bc. on the open faces.

Perhaps, CFX could help to address this type of problem related to "pressure" bc.

Thank you.

ALex Lee

Hi,

It is rather interest to find some one working on using CFX for fire modelling. Yes, Dr. Yehuda Sinai had done quite alot of fire modelling using CFX. I got some lessons and tips from him too.

However, I am always puzzle by the BCs for "OPEN" type of boundary condition. I did quite alot of natural/forced ventilation projects, e.g. heat rejection from the a/c condensors, I always got some funny result for "pressure" type of bc. on the open faces.

Perhaps, CFX could help to address this type of problem related to "pressure" bc.

Thank you.

ALex Lee