- **FLUENT**
(*https://www.cfd-online.com/Forums/fluent/*)

- - **Fan Modelling: turbulence model
**
(*https://www.cfd-online.com/Forums/fluent/45907-fan-modelling-turbulence-model.html*)

Fan Modelling: turbulence model
Hi, am modelling a radial fan, (axial inlet, radial outlet) with these characteristics: 1500 rpm outer radius 0.13m Re periphery~1.3x10^5 The domain includes passages through narrow gaps, and I need to model heat transfer. I set boundary conditions at inlet Ptot=0 and at outlet pstat=0. I used k-epsilon realizable with Enhanced wall treatment. y+ value is around 2. I have been getting mass flow rate around 30% less tahn experimental one. Questions:
Do you think the turblence model have a strong influence on the mass flow rate in this case? Shall I leave the k-epsilon and go for a low-Re such as k-omega maybe SST? Thank you all Jo |

Re: Fan Modelling: turbulence model
Hy Jo,
The turbulence model is an important issue only if the fan is operating far from the normal (optimal) operating conditions, especially at low mass-flow rates. In such conditions, B-L separations on the blades, flow recirculations inside blade passage and other related phenomena whose prediction accuracy is highly dependant on the turbulence modeling, could strongly influence the results. But, in the case of radial fans, there is another aspect that must be considered (and I bet that this the problem in your case too). Usually, these fans are designed with an evolute type diffuser. This means that the gap between blade tip and fan casing in the radial direction is highly variable. In these conditions, the SRF or MRF models are NOT applicable (the error will be more than significant, directly proportional to the variability of the radial tip gap)!!! For an accurate simulation, you MUST use Sliding Mesh model. That means: - you must use different rotor and stator fluid zones and non-conformal interfaces between; - you must use the unsteady solver (but for a faster statistically converged solution, you must use a steady solution as starting point); - you must use approx. 200-250 time steps/complete rotation (divide this number by the number of blades (n) and round it up, then multiply the result with n to obtain the final value), with 5-10 iterations/time step; - you must run the simulation for at least 2.5-3 complete rotations (use mass flow at outlet as convergence monitor), and record the mean final value of the mass flow after reaching statistically steady flow. As a turbulence model, I would recommend you the SST-kw model, but for good results you don't need to use a y+=1 mesh, a wall function mesh will do just fine (not to mention that it will shorten your computational time!). All the best, Razvan |

Re: Fan Modelling: turbulence model
Razvan... It sounds like you have considerable experience with such analysis scenarios. Your reply was very insighful. Thank you! Question: you recommended using a SST-kw model along with a "wall function" mesh. I was of the impression that SST-kw always needed a good Y+~1 mesh for accurate heat transfer...but I may be wrong. Can you provide any insights into this from your experiences?
Thank you! |

Re: Fan Modelling: turbulence model
Hi Glenn,
I actually kind of overlooked the heat transfer aspect and concentrated on the flow. If this is not well resolved, there is no reason to go any further, don't you agree? Talking about accurate heat transfer with two-equations RANS turbulence models is like talking about reaching 200MPH with a 50HP car. You will never get it! All these models overestimate heat transfer coeff. by 25-100%. SST-kw included. And that is true for high quality meshes, with y+<1. For wall function meshes, the things are even worse. The minimum model to use when good heat transfer calculations are intended is v2f, but meshes have to be about twice as dense as for the two-eq models, and y+<1. The REAL heat transfer calculations must use LES, with a lot denser meshes and overwhelming computational effort. If I were making such a simulation, I wouldn't include any heat transfer to the fan's walls, and consider, in a first approx., the temperature of the fluid at inlet as the temperature of the fan's components. That can't be too far from the reality for a convection-cooled fan. There are two facts that support this: - the temperature variation from the inlet to the outlet due to the compression is only a few degrees for this kind of fan; - the velocity of the fluid inside the fan is way higher than the velocity of the cooling air outside (e.g. the heat transfer from the working fluid to the fan's components is orders of magnitude faster than from the components to the exterior), which translates into wall temperatures at equilibrium much closer to the hot internal fluid than to the cool outside air. Of course, this is true for an ordinary industrial fan, but Jo's fan could be working in different conditions. Razvan |

Re: Fan Modelling: turbulence model
Hello Razvan, Hello Glenn, Thank you all for your help and contribution. I would like to ask few questions again. It's not completely clear why for k-omega SST Fluent suggests to use a y+~1 mesh and Razvan says there is no need. Ok for heat transfer is not accurate anyway, but what about velocity field: Razvan do you think we have a hope to get at least that right with a y+~1 mesh? Question 2: Razvan you say that two equat. RANS models usually overestimate heat transfer coefficient by 25-100%. Is it something coming from your experience from comparing simulation results with experimental data / exact solution? Is there some literature (papers/textbooks) which I can read and find out about that? Question 3. Razvan you say: The minimum model to use when good heat transfer calculations are intended is v2f. What do you mean with v2f? Finally I would like to apologies because I called my model a fan which is actually not and I mislead you. I called it a fan to simplify. It's an electric engine of which I am studying the cooling. The geometry design is probably far from an ideal aerodynamic one. The stator which carries the coils is cooled by the air blown in by the rotor discs. I could send a snapshot of model if it helps to clarify. Due to the specific problem, I can't neglect the heat transfer.
Thank you for your appreciated suggestions Jo |

All times are GMT -4. The time now is 07:40. |