3D CFD modelling
 

Hi All, i am running fluent 5.0.4 on NT. I'm solving 3d axial flow turbine problem using RNG + non-equilibrium w.f. I'm basically looking for efficiencyof the turbine at different flow rates (efficeincy is a function of tangential force, axial force, stagnation pressure drop and speed of rotor). I have a few problems ...hope you can help... [1] What pc spec do i need in order to solve a million cells model? [2] For the moment i can only solve 80000 cells models[without any grid independence] and assume that results are valid as all aerofoils are subjected to a same magnitude of numerical error[i.e. i'm making sure to keep same meshing on all blade models]. Is that acceptable? [3] At very low and very high flow rates i'm not getting any convergence. I'm suspecting that for the former, numerical round-off due to relatively low dynamic pressure is preventing conevergence. For the latter, i've noticed flow separation occuring and suspect non-equilibrium effects to be responsible for lack of conevergence. In both cases, i'm monitoring axial force,tangential force and stagnation pressure drop for steadiness and once i'm satisfied that those have stabilised, i'm assuming convergence. Is that o.k?? [4] I dopn't really understand how the turbulent model i'm using is coping with boundary layer transition [re= 0.5 million and 5 million]??????? [5] i haven't touched the realizable k-e at all. Is it worth a try??? Thanks for considering this query.

Re: 3D CFD modelling
 

A million cells would typically require more than 1 gig memory, at least if you are using the coupled solver - makes a single PC difficult to use. With the segregated solver 1 gig might be enough. Running a one-million case on a single-CPU PC will be very slow though - several days or even weeks. To run this efficiently I'd use a Linux cluster of 10 PCs or so and run it in parallel. Then you can do a run over night.

The convergence problems you are experiencing might be related to unsteady effects - have you tried to run the case unsteady? A simple fix might also be to use the standard k-epsilon model. This will over-predict turbulent energy and this might stabilize your solution, although of course it will also give you a slightly incorrect solution. But sometimes an incorrect solution is better than no solution at all :-/

I definitely think that you should try the Realizable model. It performs quite well in most turbomachinery applications. The RNG model is not as good in my experience. The only time I would consider using the RNG model is when the turbulent Reynolds numbers of the flow is very low - then the Realizable model sometimes behaves badly. This is no problem in axial turbines though.

You asked about transition. With wall-functions you will not predict any transition at all - the boundary layers will be turbulent from the leading edge. This can of course be a source of error if you think that you have a large laminar part in your specific application. There is no transition-model suitable for turbine applications in fluent as far as I know. If you need to predict suction-side transition with Fluent you will have problems. If this is important I'd use a more turbomachinery oriented code where you have ad-hoc transition models (Mayle or Abu-Ghannan&Shaw or something like that). There is not much use trying the more advanced low-Re models - although in theory they might predict by-pass transition in simple cases like flat-plates they are not capable of handling something as complex as a turbine-flow.

Re: 3D CFD modelling
 

Thank you Jonas, for your interesting comments. I will investigate the realizable model. In fluent , there's also the Spalart-Allmaras option. I found no comparative literature about it, can you please comment on its possible use for my application? Thank you very much for your kind support. ELv

Re: 3D CFD modelling
 

The Spalart-Allamaras model can be good for flows over wings etc. You could try to use it in your turbine simulation also - it might help convergence problems. However, if you have separations etc. that you want to model then it is not a good model. I'm also a bit hesitant if it is a suitable model for high-turbulence-level flows, as you have in in turbines. Comments anyone?

Re: 3D CFD modelling
 

Hi Jonas

The Spalart Almaras model is a one-equation model. For 3D flows the flow downstream of the turbine blade, will contain 3D effects, therefore the model to use is a RSM model. However if computational resources are limited, I would recommend the use of low swirl dominated RNG model coupled with the differential viscosity option.

Regards Oliver

Re: 3D CFD modelling
 

I disagree, RNG models behave badly in many turbomachinery applications and RSM models are difficult to use and not general enough for this type of applications. The only applications where I would consider using RSM is for highly swirling flows in cyclones etc. In turbomachinery flows the main importance of the turbulence model is to predict the boundary layers correctly - this is not the strong side of the RSM models in Fluent!