Centrifugal Pump and Turbulence Model
I'm analysing a centrifugal pump in off design situation. The pump runs on relative high speed. The goal is to predict the performance curve, and in a later stadium I like to analys the erosion pattern. The erosion patern is strongly depenent on the local fluid velocitys, which is dependent on the actual turbulence.
I have tried 3 turbulence models in CFX 11. See below for the description of the analysis. Wich of the turbulence models I used are good enough for acurately predicting actual turbulence in a wall bounde flow like a centrifugal pump? And, what is the effect of adding a cavitation models to this simulation? Do I have to use other turbulence models when running a cavitation study? Model The model represents a centrifugal pump with an inlet pipe, impeller and casing. The impeller has 4 blades. The eye diameter is 750 mm and outer impeller diameter is 2250 mm. The impeller blades are 2D curved with an involute curve. The inlet pipe opening and casing outlet opening are 700 mm diameter. Mesh Mesh is of the unstructured type with inflation layers on all walls of 0.08 m thick. Inflation layers are not applied to model inlet, model outlet and domain interface areas (or should i apply inflation also to this areas??). Due to curved edges and surfaces in the impeller, the inflation layer is in some regions a lot thinner. Number of Nodes: 178234 Number of Elements: 645712 Domains The model includes 3 domains; Inlet pipe, impeller and casing. Impeller is defined as rotating with a rotational velocity of 311 rpm. Other domains are stationary. Heat transfer option is set to none. Domain interfaces From inlet pipe to impeller there is an planar circular domain interface defined as general connection with a frozen rotor frame change model. From impeller to casing there is a cylindrical domain interface with same settings as mentioned above. Boundary conditions Inlet pressure 1 bar. Outlet mass flow rate 3500 kg/s. All other surfaces are defined as wall with no slip. Also tried to define the casing walls as free slip, but this gave unstable analysis. Turbulence models The calculation is performed with 3 different turbulence models;
Results The Reynolds Omega Stress and K  Omega models give simular results. The K  Epsilon model gives a little bit higer local velocity's and higher ratio of average pressure and minimum pressure. (Results are observed in a 2D mid plane) 
If you are looking at multiphase stuff like this the choice of turbulence model often becomes of secondary importance as the multiphase physics dominates over turbulence behaviour. So my first suggestion would be to use ke from your list  but I note you have not looked at the SST model and that would be my default choice.
I would only go to RSM models if turbulence anisotropy is a big effect. If you have cavitation AND particles you are going to have a hard time to get this to converge. So only use RSM if you really can justify it. 
178k nodes sounds pretty coarse for 4 blades + casing + inlet pipe. The first thing I would recommend is a mesh dependency study before you worry about the differences due to turbulence models.

Hi, if you have some tested numbers your job of validation would be a lot easier. Stick to the SST or ke turbulence models. Inflation on the walls are very crucial. With less number of layers the flow might look very good but in reality it could be completely the opposite. Perform a mesh sensitivity study as others have mentioned.

Ok, thanks for the help!! So for centrifugal pump better stick to SST turbulence model and concentrate on the mesh and multiphase physics.
I have modeled a new volute, the old geometry had some difficult surfaces to mesh. With the new volute the mesh looks much better. About the inflation layers. What is the best way to determine the thickness? When talking about a pipe, should the thickness be 0.05 times the radius or more like 0.2 times the radius? 
Read the documentation on meshing for a general guide to meshing. For specific information you can't beat a sensitivity study  try a range of options and determine for yourself the best one.

problem while simulating pump geometry
Hi! i have successfully simulated 2 d geometry of a centrifugal pump, but now, when im tryin out 3d im facing problems. After the iterations start, i get "turbulent viscosity error" what could be the reason?? is my mesh too coarse in some areas?? If so, why isnt adaption helping me solve the problem?

Can you post your output file?

Thanx a lot for the quick reply Glen!
However I resolved the problem yesterday. My geometry consists if rotating a regenerative impeller inside the pump casing. While making the geometry I inadvertently subtracted the impeller volume from the bulk; where as i should have split the two volumes and then deleted the impeller volume. 
Well, I have been working on some different mesh settings. With mesh rifining to a total nodes of +/ 450K the difference in result after 100 iterations drops down to 1.52%.
Only the convergence history looks the same over all runs and it isn't verry satisfying. RMSP mass flats out at 70 iterations on a valeu of 5e005 and should be OK according to the manual. Umom, Vmom and Wmon stay above 1e003 which should be <5e004. Is it usefull to run this calculation untill it reach the convergence goals, or should I change the set up the accelerate convergence? In relation to the turbulence models, I will stick to SST and focus on the more important issues. Thanks for your help so far!! 

Im not able to upload a file as it is more than 97 kb. Im getting turbulent viscosity error in the same. kindly suggest other means of uploading this file.

Hi Yvonne,
If you have a gmail account you can use google docs to upload files up to 250MB. I have never used it, but i have just uploaded a test file: https://docs.google.com/leaf?id=0B2e...ZTAxMTM4&hl=nl 
All times are GMT 4. The time now is 06:49. 