
[Sponsors] 
July 15, 2008, 09:09 
Open boundary condition

#1 
Guest
Posts: n/a

Hi i am dealing with a problem having conjugate heat transfer solid domain, which was placed in atmosphere.....so that it gets cooled naturally through free air
So what would be the best suitable boundary conditions..hence it would come under Natural Convection plz suggest the realistic BC's Secondly my doubt was what would be best suited to define as input heat source  whether heat flux or heat generation value  plz kindly suggest thanks in advance 

July 15, 2008, 22:38 
Re: Open boundary condition

#2 
Guest
Posts: n/a

Hi,
If you are doing a CHT simulation you do not specify boundary conditions on the solid. The heat transfer is worked out internally to the simulation. You do need to specify boundary conditions around the air domain. That should be made to suit what you are trying to model. As for the heat source  again match what you are trying to model. You can also specify an initial temperature with no heat source so you get the natural cooling rate. Glenn Horrocks 

July 16, 2008, 01:07 
Re: Open boundary condition

#3 
Guest
Posts: n/a

Hi Glenn! thanks for the response....
But i would like to give you a litter clear picture regarding my problem to have a suggestion ....for BC's I was having a heat source with supplied power in Watts.But to define in problem as energy of heat source which would work better ie 1)Heat flux defnition on interface region of solid and air or 2)defining heat generation value in sub domain. or i need to know it does make any difference of defining heat source? Secondly coming to BC's of air domain... i had an experimental results for the model tested in open atmosphere with the same power supplied for the solid domainie by Natural Cooling So i need to know what BC's will best suit that realistic situation . .. plz help.....i will be greatfull for the response Thanks in advance 

July 16, 2008, 01:59 
Re: Open boundary condition

#4 
Guest
Posts: n/a

Hi,
Heat flux on surface or body  depends what the heat flux is. If it is heated by electrical resistance then a reasonable approach is usually to make it throughout the body. If it is being heated externally by something like a radiative heat source then a boundary heat source is more appropriate. You still have not described what you are modelling. How hot it it? How big? The surrounding atmosphere  any air currents? How enclosed? Is radiation significant? Glenn Horrocks 

July 16, 2008, 02:56 
Re: Open boundary condition

#5 
Guest
Posts: n/a

Hi Actually my problems comes like cooling of heatsink.
i had experimental value of temperature after getting cooled in open atmosphere of heatsink . ie the heat sink was placed in some room with no external air currents..hoping of still air movement ,...and considering fluid will move due to Buoyancy,,,and it was not placed in any enclosure...so as in open air..and ambient conditions only So for this case can i consider OPENING bounary conditions for all the six faces of air domain Thanks in advance Nav 

July 16, 2008, 12:50 
Re: Open boundary condition

#6 
Guest
Posts: n/a

choose h = 20 [W m^2 K^1] and Tinfinite (Outside Temperature) = 300 [K] as your boundary condition(enviromment conditions) or:
oundary Type = WALL Location = SIDE_WALL,WALL_2 BOUNDARY CONDITIONS: HEAT TRANSFER: Heat Transfer Coefficient = 20 [W m^2 K^1] Option = Heat Transfer Coefficient Outside Temperature = 29.5 [C] I use heat flux [W m^2], but it depends on your study. 

July 17, 2008, 01:55 
Re: Open boundary condition

#7 
Guest
Posts: n/a

Hi,
You still have not explained what you are doing. How big is it? How is it being heated? You can put opening boundaries on the exterior faces but these are likely to lead to convergence problems. Make sure you put the boundaries far enough away to not affect things. Glenn Horrocks 

July 17, 2008, 03:13 
Re: Open boundary condition

#8 
Guest
Posts: n/a

Hi Rogerio
you had suggested me to define heat transfer coefficient. But in my problem I had certain heat source that has to be supplied, So can i define Heat generation (Wm^3)value in sub domain region and leave blank for source coefficient..??or could i go for defining heat flux ie (Wm^2) and leave the flux coeffient without defining? i mean leaving those coefficient empty does effect the situation? and get heat transfer coefficient plotted in post processor as 'Wall heat transfer coefficient' as part of the results.. ?? Plz respond could i go in that way..? Thanks in advance 

July 17, 2008, 07:46 
Re: Open boundary condition

#9 
Guest
Posts: n/a

I do not know what you are intending to simulate, but i would choose:
h = 20 [W m^2 K^1] and Tinfinite (Outside Temperature) = 300 [K] as your boundary condition (enviromment conditions) at walls and I will use heat flux [W m^2] applied at a 2D region specified as your another boundary condition. 

July 17, 2008, 07:48 
Re: Open boundary condition

#10 
Guest
Posts: n/a

I havenīt did it: "...So can i define Heat generation (Wm^3)value in sub domain region..."


July 17, 2008, 08:50 
Re: Open boundary condition

#11 
Guest
Posts: n/a

hi
i am dealing with electronic components cooling problem. I am trying to cool a heatsink which would be supplied with a power of 40W(that could be considered as continuous supply ) Just i was trying to develop case study for a solid of conjugate heat transfer which was placed in open atmosphere ,that might be some room .Considering the heat sink would be attached to some pcb board and hanged in the middle of the room and supplied with that power. I was doing this to consider simple case of cooling electronic component ,Next i would like to extent the study for the sink placed in some enclosure(ie realistic case as if cooling some electronic components in enclosure.i would look for the difference of temperatures placed inside and outside of enclosure. So hop i explained the problem.. So now plz suggest if OPENING BC would work for the airmedium... ,by applying pressure as BC's,and ambient temperature thanks in advance 

July 17, 2008, 08:55 
Re: Open boundary condition

#12 
Guest
Posts: n/a

Hi
i defined my problem in one of my post above ,plz look at that.. I am intending to plot temperature and heat transfer coefficient as my part of my results.Can't i do that by defining heat source? thanks in advance 

July 17, 2008, 09:00 
Re: Open boundary condition

#13 
Guest
Posts: n/a

Hi yes you could also define heat source as heat generation(Wm^3) value during the case of conjugate heat transfer by creating subdomain.
you could get more clear information on this from tutorial 14 Conjugate heat transfer in a heating coil in ansys 11 cfx version HElP . 

July 17, 2008, 21:51 
Re: Open boundary condition

#14 
Guest
Posts: n/a

Hi,
Yes, now I have some idea of what you are trying to do. For the heat input, you can either use a heat source on the boundary of the heat sink domain or put another solid domain for the heat source and use a volumetri heat source there. Yes, openings will work but as I said they can sometimes be diffiult to converge. Glenn Horrocks 

July 17, 2008, 21:54 
Re: Open boundary condition

#15 
Guest
Posts: n/a

Hi,
Rogerio is not on the right track. You do not define a HTC, the simulation works it out based on the local flow field and the turbulence model you use. Just use an interface between the solid domain (heatsink) and the air domain and CFX will calculate the HTC. Glenn Horrocks 

July 18, 2008, 02:04 
Re: Open boundary condition

#16 
Guest
Posts: n/a

Hi Glenn thanks for the response. i had done the simulation by defining heat source,and BC's of airmedium as 'OPENING' .i got the solution converged at 1e4.
But the problem was regarding heat transfer coefficient. I am feeling to have atleast basic equation Q=h*A *del(T)to be proved. I am getting Temperature after cooling and got plot of those result,but regarding 'h'when i plotted "Wall heat transfer coefficcient" in POST processor the value was very much less when compared to required 'h' to suite the equation. So could you help me in plotting 'h'(heat transfer coefficient) .If any variable is required to define specially or any variable existing to plot in post processor? Thanks in advance 

July 22, 2008, 09:10 
Re: Open boundary condition

#17 
Guest
Posts: n/a

Iīm studying a problem like uīre studying. Iīm using heat flux [W m^2] īcause i have experimental data of heat flux q"[W m^2] and placed on a 2D region. My heat flux represents a 2.12 [W], in a specified time. The heat flux varies on the time.
Donīt forget to make the interface domain, because, the fluid will penetrate on solid as youīre plotting the velocities. By the way, do you have any turbulence model? In openning boundaries, what is your boundary condition? If you wanna see my geometry, please add me at MSN: rogeriobrito2007@hotmail.com or Skype: rogeriofbrito. 

July 23, 2008, 02:33 
Re: Open boundary condition

#18 
Guest
Posts: n/a

Hi
Yes i need to plot heat transfer coefficient in postprocessor,which variable i should use for it?or any user defined variable required ?if so help me in defining the expression for the variable.. thanks in advance 

July 23, 2008, 23:02 
Re: Open boundary condition

#19 
Guest
Posts: n/a

Hi,
The heat transfer coefficient is in the results by default in a CHT simulation. Keep in mind the reference temperature for the HTC, it is either calculated locally by default or you can set it to a value which is more useful for comparisons to published data. Glenn 

July 25, 2008, 01:12 
Re: Open boundary condition

#20 
Guest
Posts: n/a

Hi Glenn Thanks for the response...
i got relative value of heat transfer coefficient plotted,by defining 'tbulk for htc' in expert parameters. I said earlier regarding my problem of taking "OPENING" as BC.So i did with that case and got the solution converged.General Q=h*A*(delT) has also satisfied.. So can i go ahead taking this simulation..? Thanks in advance.. Regards Nav 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
How exactly the "pressure outlet" bdry condition compute properties on the boundary?  yating9901  FLUENT  3  June 28, 2010 12:26 
Problem installing on Ubuntu 9.10 > 'Cannot open : No such file or directory'  mfiandor  OpenFOAM Installation  2  January 25, 2010 10:50 
RPM in Wind Turbine  Pankaj  CFX  9  November 23, 2009 05:05 
OpenFOAM with IBM AIX  matthias  OpenFOAM Installation  20  March 25, 2008 03:36 
Slip boundary condition what is inside  normunds  OpenFOAM Running, Solving & CFD  2  June 4, 2007 06:45 