Centrifugal Pump and Turbulence Model

Michiel · January 13, 2010, 12:12

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

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

January 13, 2010, 12:12	Centrifugal Pump and Turbulence Model	#1
Michiel Member Michiel Join Date: Jul 2009 Location: The Netherlands Posts: 42 Rep Power: 17	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 15, 2010, 01:08		#4
sans 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 03:38.

January 21, 2010, 02:36	problem while simulating pump geometry	#7
yvonne 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 22, 2010, 03:27		#9
yvonne 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.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Pump Station Simulation	GUSU	CFX	6	October 14, 2009 07:40
Model of pump nonoptimal regimes get bad results	Georg	CFX	3	May 21, 2008 01:53
turbulence model	Elyor	Siemens	0	June 19, 2007 23:50
Model pump?	Neo	FLUENT	0	September 19, 2003 07:12
turbulence model for water pump	Marcio	Main CFD Forum	4	September 3, 2003 10:35

January 13, 2010, 17:32		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	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, 18:33		#3
stumpy 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 18, 2010, 03:51		#5
Michiel Member Michiel Join Date: Jul 2009 Location: The Netherlands Posts: 42 Rep Power: 17	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, 06:02		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	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, 17:38		#8
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	Can you post your output file?

January 22, 2010, 04:07		#10
Michiel Member Michiel Join Date: Jul 2009 Location: The Netherlands Posts: 42 Rep Power: 17	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, 07:18		#11
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	http://www.cfd-online.com/Wiki/Ansys...gence_criteria

January 25, 2010, 01:34		#12
yvonne 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, 04:20		#13
Michiel Member Michiel Join Date: Jul 2009 Location: The Netherlands Posts: 42 Rep Power: 17	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