# Centrifugal Pump and Turbulence Model

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Search this Thread Display Modes
 January 13, 2010, 11:12 Centrifugal Pump and Turbulence Model #1 Member   Michiel Join Date: Jul 2009 Location: The Netherlands Posts: 42 Rep Power: 16 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) Torque_Converter and strategist34 like this.

 January 13, 2010, 16:32 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,701 Rep Power: 143 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.

 January 13, 2010, 17:33 #3 Senior Member   Join Date: Apr 2009 Posts: 531 Rep Power: 21 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.

 January 15, 2010, 00:08 #4 Member   SanS Join Date: Mar 2009 Posts: 41 Rep Power: 17 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. joshghoun likes this. Last edited by sans; January 15, 2010 at 02:38.

 January 18, 2010, 02:51 #5 Member   Michiel Join Date: Jul 2009 Location: The Netherlands Posts: 42 Rep Power: 16 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?

 January 18, 2010, 05:02 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,701 Rep Power: 143 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.

 January 21, 2010, 01:36 problem while simulating pump geometry #7 New Member   @p N Join Date: Jan 2010 Location: United States Posts: 27 Rep Power: 16 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?

 January 21, 2010, 16:38 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,701 Rep Power: 143 Can you post your output file?

 January 22, 2010, 02:27 #9 New Member   @p N Join Date: Jan 2010 Location: United States Posts: 27 Rep Power: 16 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. strategist34 likes this.

 January 22, 2010, 03:07 #10 Member   Michiel Join Date: Jul 2009 Location: The Netherlands Posts: 42 Rep Power: 16 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!!

 January 22, 2010, 06:18 #11 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,701 Rep Power: 143

 January 25, 2010, 00:34 #12 New Member   @p N Join Date: Jan 2010 Location: United States Posts: 27 Rep Power: 16 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.

 January 25, 2010, 03:20 #13 Member   Michiel Join Date: Jul 2009 Location: The Netherlands Posts: 42 Rep Power: 16 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

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post GUSU CFX 6 October 14, 2009 06:40 Georg CFX 3 May 21, 2008 00:53 Elyor Siemens 0 June 19, 2007 22:50 Neo FLUENT 0 September 19, 2003 06:12 Marcio Main CFD Forum 4 September 3, 2003 09:35

All times are GMT -4. The time now is 04:33.

 Contact Us - CFD Online - Privacy Statement - Top