CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Centrifugal Pump and Turbulence Model (http://www.cfd-online.com/Forums/cfx/71739-centrifugal-pump-turbulence-model.html)

 Michiel January 13, 2010 12:12

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;
• K – Epsilon with scalable wall function.
• Reynolds Omega Stress with automatic wall function.
• K – Omega with automatic wall function.

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)

 ghorrocks January 13, 2010 17:32

If you are looking at multi-phase stuff like this the choice of turbulence model often becomes of secondary importance as the multi-phase physics dominates over turbulence behaviour. So my first suggestion would be to use k-e 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.

 stumpy January 13, 2010 18:33

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.

 sans January 15, 2010 01:08

Hi, if you have some tested numbers your job of validation would be a lot easier. Stick to the SST or k-e 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.

 Michiel January 18, 2010 03:51

Ok, thanks for the help!! So for centrifugal pump better stick to SST turbulence model and concentrate on the mesh and multi-phase 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?

 ghorrocks January 18, 2010 06:02

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.

 yvonne January 21, 2010 02:36

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?

 ghorrocks January 21, 2010 17:38

Can you post your output file?

 yvonne January 22, 2010 03:27

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.

 Michiel January 22, 2010 04:07

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 1.5-2%.
Only the convergence history looks the same over all runs and it isn't verry satisfying. RMS-P mass flats out at 70 iterations on a valeu of 5e-005 and should be OK according to the manual. U-mom, V-mom and W-mon stay above 1e-003 which should be <5e-004. 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!!

 ghorrocks January 22, 2010 07:18

http://www.cfd-online.com/Wiki/Ansys...gence_criteria

 yvonne January 25, 2010 01:34

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.

 Michiel January 25, 2010 04:20

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 17:16.