# CHT

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 March 26, 2008, 06:17 CHT #1 skarp Guest   Posts: n/a Hi I am using CHT to simulate heat transfer of convection and conduction. Consider a L shaped pipe. Considered flow as fluid domain and wall(8mm thick)considered as solid domain in steady state. Flow boundary condition is In -opening-static pressure entrain- pressure 1.36 bar and temperature 800C Out -opening-static pressure entrain- pressure 0.35 bar and temperature areaAve(T)@REGION:Out Solid domain Cast iron-pure substance,CHT and particle solid. Heat transfer-Thermal energy for both,Turbulence k-eplison Inferface-conservative interface flux and wall-adiabatic After solving Imbalance are less than 0.05% convergence up to 1e-4 for heat transfer,turb,momentum In cfx post The heat transfer to the wall is 797C. The heat loss from flow to wall is only 3C which is not acceptable. Kindly tell me what is wrong in my simulation

 March 26, 2008, 09:14 Re: CHT #2 andy2O Guest   Posts: n/a Adiabatic = perfectly insulated. So it seems from your description (if I've understood it correctly) that the outer wall of the pipe is perfectly insulated. So the heat cannot escape from the outer surface of the pipe wall. Therefore the pipe will be close to thermal equilibrium with the fluid. Therefore heat fluxes in the pipe wall are small - probably just a small heat flux along the length of the pipe. Therefore little heat is being transferred from the fluid to the pipe. Therefore temperature differences between the fluid and the pipe wall will be small. If you want to study heat loss from your pipe then you need to choose the outer boundary condition on the pipe to carefully model your actual scenario. Probably you need a heat transfer coefficient boundary condition, derived from an empirical correlation or from a separate CFD study. Adiabatic boundary conditions are unlikely to be a good choice. Regards, andy NB: Heat transfer / heat loss is usually measured in terms of energy loss per unit time i.e. Watts (W), or frequently Watts per unit area (e.g. W/m^2). It is not measured as a temperature in C... so make sure you're looking at the right data.

 March 26, 2008, 10:46 Re: CHT #3 skarp Guest   Posts: n/a Thanks andy I know only the surrounding temperature of air near the pipe outer wall. It is 170C.Can I give pipe outer wall temperature as 170C or I have simulate a convection of air near the pipe wall I have completed a simulation by giving pipe outer wall temperature as 170C and run at steady state. I have observed the temperature distribution on the outer wall of pipe is 170C. The temperature from inside to outside is 800C-170C drop. In real condition , whatever may be the case, whether the temperature of the object outer is equally to air temperature surrounded by it.

 March 26, 2008, 13:45 Re: CHT #4 andy2O Guest   Posts: n/a "Can I give pipe outer wall temperature as 170C... ?" Probably not. If the thermal resistance of the boundary layer is important in your model, then this is not a suitable boundary condition. The boundary layer thermal resistance usually is important for un-insulated metal boundaries with natural convection. So, you need to work out if it is important for you, and how you can model it: 1) Look in an engineering heat transfer text book / reference book such as "Heat Transfer" by Holman to find empirical correlations for heat loss by convection from cylidrical bodies and pipes. Use these to estimate the heat transfer coefficient at the outer surface of the pipe. You can use the correlations from the book to to assess how important the boundary layer thermal resistance is (*). You can also use this heat transfer coefficient in the CFD model boundary condition. Don't forget that radiation heat losses will probably be very significant too at these temperatures. So radiation heat losses will need modelling, either by hand calculations or in a CFD model. Also, don't forget about any forced external flows from cooling fans, etc blowing onto the pipe. [(*) You should know a typical heat flux from at the pipe wall from your other calculations - you can use that data together with the heat transfer coefficient to perform a simple hand calculation to predict the temperature drop across the boundary layer surrounding the pipe and decide whether it is significant in your results.] 2) You can include the outside air in your simulation. However to resolve heat flow accurately to predict the heat transfer coefficient you need low values of y+, etc in you simulation and you will need to model a large domain, so this will not be a trivial task. It is up to your engineering judgement to decide which of these is methods is appropriate for your particular task: Option 1 is quick and easy - you should probably try that first as it can be done quickly and will act as a check on any CFD you do. Option 2 may be necessary - it may be more accurate if you do it correctly. Certainly you should assess the impact of thermal radiation too, whatever else you do. You will have to make the decision based on your aims, time / budget, data, etc... Hopefully other people will provide other suggestions too. Regards, andy

 March 27, 2008, 21:43 Re: CHT #5 Rogerio Fernandes Brito Guest   Posts: n/a how about choosing this? As boundary conditions, u can put that all the faces of the tube are submitted to a constant convection heat transfer coefficient (h = 25 W/mēK). The temperature of external enviromment could be this one: Tinfinite = 298 K

 March 28, 2008, 01:19 Re: CHT #6 skarp Guest   Posts: n/a Dear andy Can u kindly provide me the detail how to get the heat transfer co-efficient for the pipe outer wall through cfd. the pipe material is Cast Iron.

 March 28, 2008, 04:25 Re: CHT #7 andy2O Guest   Posts: n/a Where on Earth have you got those numbers from? - Why 298K when skarp has already said surrounding air is at 170 C = 443 K? - What correlation are you using to get h=25 W/m^2/K? Without evidence to back them up these numbers are *completely* meaningless. Any customer / professor / reviewer would (and should) simply throw the report of this study away if these numbers are used without supporting evidence to show they are valid.

 March 28, 2008, 09:27 Re: CHT #8 andy2O Guest   Posts: n/a "Can u kindly provide me the detail how to get the heat transfer co-efficient for the pipe outer wall through cfd" Skarp, I am sorry, but I don't have time to describe this in detail now. Here are some brief comments, but please take other peoples advice if possible - as I have not got time to describe the steps properly now: Basically you need to either: a) set up one big model, including the inside and outside of the pipe and simulate everything (external air, pipe and fluid in pipe) using a low-Reynolds number turbulence model such as SST with y+ values of about 1 on each surface. In this method you do not need to impose a heat transfer coefficient on the pipe wall, as that is just an interface in your model not an external boundary. or: b) set up a model of the air outside of the pipe only, with prescribed temperatures on the pipe outer wall using a low-Reynolds number turbulence model such as SST with y+ values of about 1 on the pipe's outer surface. Depending on your geometry, you may be able to use a 2D simulation for this and just study a cross section through the pipe. Then extract heat transfer coefficients for the pipe surface from this model using CFX Post. Then impose these heat transfer coefficients on the model of the pipe and recompute the temperatures. You will probably need to update the temperatures in the pipe model and repeat the external simulation to recompute the heat transfer coefficient a few times until it the two models become consistent. In both cases, note that natural convection from a pipe may be time-dependent (the plume may oscillate in position), so converging the CFD may require a transient simulation. It is hard to say before you try it. Both methods have advantages and disadvantages - you will have to make a judgement about which is best for your study. Both methods require more work to account for thermal radiation, which may be important. Have you tried looking up heat transfer correlations in text books such as "Heat Transfer" by Holman? Have you found out if thermal radiation will be important in your model? I think these are the most important tasks before starting more CFD. Good luck. Sorry I cannot provide more detail here. Regards, Andy

 March 29, 2008, 04:17 Re: CHT #9 skarp Guest   Posts: n/a Thanks andy. I have got new idea from u.I will implement it and tell u within a week. Hats off for valuable info. regards skarp

 April 11, 2008, 12:29 Re: CHT #10 skarp Guest   Posts: n/a Hi andy 1.Is there any need to create a subdomain to defined the source as given in heating coil example? 2.If i model a pipe with BC inlet(opening condition) and outlet(opening).The pipe is placed inside a big box in which box has inlet and outlet(opening). pipe - water flow box - Air flow CHT simulation The flow of air in the box is towards the entry of pipe inlet (opening condition). In this case whether air enter into water under specified condition. If the pipe has in and out opening condition and air flow on the Box

 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 stawrogin OpenFOAM 0 May 17, 2011 15:42 PCFD CFX 4 July 12, 2010 13:49 sandeep_tu CFX 1 May 12, 2009 18:54 michelle CFX 1 April 21, 2008 04:06 Parthipan CFX 7 September 4, 2007 05:29

All times are GMT -4. The time now is 19:41.

 Contact Us - CFD Online - Privacy Statement - Top