Energy balance with CFDesign
I am having a serious problem with some heat transfer studies:
I am currently trying to investigate different types of fins for heat transfer, the thing is that I can seem to get realistic results no matter what I do.
why not realistic: I have effectively choked the boundary layer between the fins so badly that when you examine the theory on fins , I have effectively made my fins obsolete --> hence would naturally expect to see that although my surface area is greater my Q[w] would be lesser - and what I am actually getting from the analysis is the opposite ?!?
I have tried all the following solutions:
1. switching to low Reynolds K-e scheme - to attempt capturing the "choke"
2. enhancing the layer number to 5 - to better represent the boundary layer
3. added refinement regions
anyone has any idea?
P.s. my BC are identical to the ones used in the online help site:
1. To define an opening (usually the top surface), assign Static Gage Pressure = 0.
2. assign a temperature constraint to the opening, specify a Film coefficient = 2 W/m2K and Reference Temperature = ambient temperature.
3. Leave the bottom surface unspecified to simulate an insulated surface. The exception is if the bottom surface has a constant temperature or if heat is entering or leaving through the surface. Specify a temperature, a heat flux, or a film coefficient, respectively.
4. a Total heat generation boundary condition to components that dissipate heat.
Hello yoav.. Have you chatted with the support team about this? Hard to picture what you are trying to do without seeing the model
I'm also writing to make you know of the useful discovery my wife's daughter enjoyed browsing your webblog. She even learned a wide variety of pieces, with the inclusion of what it's like to have an incredible coaching nature to let the rest effortlessly know specific impossible subject areas. You truly exceeded readers' desires. Many thanks for producing those good, dependable, educational and even fun tips on that topic.
thanks for your reply, however, this is exactly what i am trying to avoid - a private solution to my simple heat sink fins problem.
what i want is to hear from someone who has managed to model a proper heat sink with fins for natural convection - why?
try emulating the following problem, and you will see why:
1. create any basic design of rectangular fin array using any CAD program you see fit, and use normative analytic models for achieving optimal distance between the fins - such as the Bar-Cohen-Rohsenow model (see piture i attach)
2. set up the fin array in a natural convection "bucket" configuration and follow all the "best practice" rules as offered the user guide and online help web site.
2. run an analysis on a model with proper fin spacing
3. now run a model with a denser array.
what you would expect is, that due to "choke" effects --> the resulting heat dissipation in the overtly choked model to be lesser --> hence less Q[watt] dissipated from the array -->
BUT, what you will find is--> that no matter what you do, including the options i offered above (in my original post)--> you will get an unrealistic calculation that:
even if you model a ridiculously dense array - which are obviously ineffective and ridiculously "choked" -the more fins you put the more Q[watt] you will dissipate - which is obviously wrong the the presented "choked" case.
(of course i use the wall calculator in the results tab to get the total Q[watt])
P.s. to avoid erroneous results from edges when using the wall calculator - i have created the most simple geometric fins as possible
follow these guidelines and you will see the problem :)
i have it!!!
well after some research and some iterations i have managed to find the solution to my problem.
the problem: failure to model the "choke" phenomenon in too thinly spaced fins in a heat sink.
the source of the problem: if one would have read the original post he would see that the BC i have used on the fin array was either:
1. Constant T BC on the fin array
2. constant Q BC on the fin array
the reason was: i wanted to model and measure the amount of Q dissipated from my fin array.
background: the "choked flow" phenomena is a fluid dynamics phenomenon that occurs when due to lack of spacing--> two opposing boundary layer interact with each other and interfere with each others flow pattern, hence causing an increase in shear forces and thus reducing the flow velocity vector entering the Region --> the result is a slower flow and hence an increase in temperature at "choked regions" --> effectively reducing the effectively of the heat sink fin array.
what was wrong with my model: by creating a boundary condition (remember BC are forced on the solution throughout the iterations) i forced the solution to maintain constant temp on the array--> hence forced the fluid to flow homogeneously between the fins regardless.
the same problem would have raised should i have forced a BC the dictates Total heat generation Q on the fin array volume itself- for the same reasons
(by forcing a measured amount of heat uniformly on a volume whose surface i want to model --> i force - though less strictly then with the constant T BC - a dT and V to accommodate the uniform dQ from the surface .
the solution: add an external heat source volume on the entire "floor" of the heat sink fin array (thick enough not to impose on the mesh size) , set all its "wetted" faces to have h=0 at t=ambient (the only non-wetted face is the solid-solid interface with the fin array) - hence making sure no heat is dissipated from it other then through the fin array, assign the same material to it as with the fin array.
--> this way the "floor" of the fin array is modeled to have a constant homogeneous heat source, while the fin array is free to develop T gradients and second order flow phenomena such as with "choked" flows.
|All times are GMT -4. The time now is 03:04.|