# high rotational speed centrifugal pump

 Register Blogs Members List Search Today's Posts Mark Forums Read

January 9, 2020, 06:41
high rotational speed centrifugal pump
#1
New Member

Marek
Join Date: Nov 2019
Posts: 7
Rep Power: 2
Hello everyone,

I am simulating the flow in centrifugal water pump. This is quite a special case because the pump has a very low specific speed of 12, a high speed of 30,000 rpm and very low flow rate. For the purposes of the simulation, I prepared the structural rotor mesh in Turbogrid and the unstructured volute grid (maximum skewness is 0.712). The grids have 283320 and 1205389 elements, respectively. The geometry consists of a static inlet part (to avoid effect of boundary conditions), impeller, volute, and pipe (to avoid backflow). The boundary conditions are total pressure inlet and mass flow outlet. The turbulence model is SST, and high resolution shemes. I also used the mixing plane and rotor segment approach to save computing power.
However, my results are unsatisfactory, high RMS residuals, on the order of 10 ^ -3, and a head rise 36% higher than the design one. I think that the hydraulic efficiency is also too high. I tried to reduce the timescale factor from 3 * 10 ^ -5 (auto) to 5 * 10 ^ -7 but this does not improve convergence and even causes divergence. I think that the key issue in this case is the very high rotational speed pump, because at lower speeds (15,000 rpm) the RMS residuals go below 10 ^ -4.
Do you have any advice or suggestions on what I can do wrong? Whether mixing-plane approach is appropriate in this case. Should a special approach be used for a pump with such a high rotational speed?

I also have a question related to transient simulation. Should the Couranat number always be less than 1 in the entire computational area to get reliable results?
Attached Images
 1.png (41.3 KB, 22 views) 2.png (72.2 KB, 22 views) 3.png (48.3 KB, 18 views) 4.png (100.9 KB, 20 views) 6.jpg (50.0 KB, 39 views)

Last edited by marekpl; January 10, 2020 at 12:28.

 January 19, 2020, 03:40 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 16,315 Rep Power: 125 Some FAQs: Non-convergence - https://www.cfd-online.com/Wiki/Ansy...gence_criteria Accuracy - https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F Courant Number < 1? No. CFX is an implicit solver and can handle Courant Numbers > 1. But this simulation is a steady state one anyway, so Courant Number is not relevant. Courant Numbers calculated on psuedo-time steps from steady state simulations are not meaningful. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

January 24, 2020, 14:20
#3
New Member

Marek
Join Date: Nov 2019
Posts: 7
Rep Power: 2
Thanks Glenn, I've already tried the things listed in the FAQ. I changed my strategy and tried similar simulation for a larger pump with flow rate of 125 l / s and a speed of 1770 rpm. I used the full-rotor model and mixing-plane interface. I set Pitch angle to 360 degrees. RMS residuals conveged nicely below 1e-5.
Then I tried to do the same simulation for the pump described above. As soon as I start the simulation, after a few iterations I receive
Quote:
 A wall has been placed at portion (s) of an INLET
and then
Quote:
 ERROR #004100018 has occurred in subroutine FINMES. | | Message: | | Fatal overflow in linear solver.
and the simulation diverged. I've already tried
- run simulations with initial conditions obtained using the FROZEN-ROTOR interface
- reduce timescale
- extend the inlet pipe
- run simulation on the first order shemes
When using the FROZEN-ROTOR interface, this error is not occur.
Do these solver settings make sense? What can cause a divergence?

Last edited by marekpl; January 24, 2020 at 14:21. Reason: quote error

 January 28, 2020, 05:23 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 16,315 Rep Power: 125 Stop your mixing plane model before it crashes (or at least save a backup file) and have a look at it in the post processor. That might give you some clues as to what is going wrong. Try using the frozen rotor simulation as an initial condition for the mixing plane model. Make sure the pitch ratios are correct. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

 February 6, 2020, 04:03 #5 New Member   Marek Join Date: Nov 2019 Posts: 7 Rep Power: 2 For the full rotor i set the pitch angle side 1 and side 2 to 360 degrees. Is it correct?

 February 6, 2020, 04:16 #6 Senior Member   Gert-Jan Join Date: Oct 2012 Posts: 1,155 Rep Power: 17 I would set 'none' for both

 February 6, 2020, 06:45 #7 New Member   Marek Join Date: Nov 2019 Posts: 7 Rep Power: 2 The Mixing Plane interface can not be set to none. I can see only "Automatic", "Specified Pitch Angle" and "Value".

 February 6, 2020, 06:51 #8 Senior Member   Gert-Jan Join Date: Oct 2012 Posts: 1,155 Rep Power: 17 DOMAIN INTERFACE: Default Fluid Fluid Interface Boundary List1 = Default Fluid Fluid Interface Side 1 Boundary List2 = Default Fluid Fluid Interface Side 2 Interface Type = Fluid Fluid INTERFACE MODELS: Option = General Connection FRAME CHANGE: Option = Transient Rotor Stator END MASS AND MOMENTUM: Option = Conservative Interface Flux MOMENTUM INTERFACE MODEL: Option = None END END PITCH CHANGE: Option = None END END MESH CONNECTION: Option = GGI END END

 February 6, 2020, 06:52 #9 Senior Member   Gert-Jan Join Date: Oct 2012 Posts: 1,155 Rep Power: 17 Or for steady state (Frozen Rotor): DOMAIN INTERFACE: Default Fluid Fluid Interface Boundary List1 = Default Fluid Fluid Interface Side 1 Boundary List2 = Default Fluid Fluid Interface Side 2 Interface Type = Fluid Fluid INTERFACE MODELS: Option = General Connection FRAME CHANGE: Option = Frozen Rotor END MASS AND MOMENTUM: Option = Conservative Interface Flux MOMENTUM INTERFACE MODEL: Option = None END END PITCH CHANGE: Option = None END END MESH CONNECTION: Option = GGI END END

 February 6, 2020, 07:18 #10 New Member   Marek Join Date: Nov 2019 Posts: 7 Rep Power: 2 Ok, so for Frozen Rotor and Transient Rotor Stator, "none" is the right setting. And what settings should I choose for the Mixing Plane interface and full rotor.

 February 6, 2020, 07:25 #11 Senior Member   Gert-Jan Join Date: Oct 2012 Posts: 1,155 Rep Power: 17 This is the setup for a full rotor. Over 360°. That is what I do all the time. So, maybe I don't understand. Otherwise: share a picture how your setup looks like. Last edited by Gert-Jan; February 6, 2020 at 10:22.

 February 6, 2020, 07:46 #12 New Member   Marek Join Date: Nov 2019 Posts: 7 Rep Power: 2 My settings below: DOMAIN INTERFACE: S1 to R1 Boundary List1 = S1 to R1 Side 1 Boundary List2 = S1 to R1 Side 2 Filter Domain List1 = S1 Filter Domain List2 = R1 Interface Region List1 = Inlet 2 Interface Region List2 = Passage OUTFLOW,Passage OUTFLOW 2,Passage OUTFLOW 3,Passage OUTFLOW 4,Passage OUTFLOW 5,Passage OUTFLOW 6 Interface Type = Fluid Fluid INTERFACE MODELS: Option = General Connection FRAME CHANGE: Option = Stage DOWNSTREAM VELOCITY CONSTRAINT: Frame Type = Rotating Option = Constant Total Pressure END END PITCH CHANGE: Option = Specified Pitch Angles Pitch Angle Side1 = 360 [degree] Pitch Angle Side2 = 360 [degree] END END MESH CONNECTION: Option = GGI END END

 February 6, 2020, 07:59 #13 Senior Member   Gert-Jan Join Date: Oct 2012 Posts: 1,155 Rep Power: 17 I asked for a screenshot of your geometry. Nevertheless, if you have full 360 of the pump as shown in your first query, you don't need "stage". Last edited by Gert-Jan; February 6, 2020 at 10:22.

 February 6, 2020, 11:50 #14 New Member   Lorenzo Bossi Join Date: Aug 2009 Location: London Posts: 7 Rep Power: 12 Marek, what re the pump specifications? I see specific speed of 12 but in which units? Aside from RPM, can you also provide head, volume flow rate? First you should check the model is right, I see the volute has very small area and I don;t see any vaneless diffuser, these may be an issue. Try running with the inlet + impeller + straight outlet, so you avoid the effects of the volute and see if that converges __________________ Lorenzo

February 6, 2020, 12:02
#15
New Member

Marek
Join Date: Nov 2019
Posts: 7
Rep Power: 2
I send a screenshot in the attachment.
I wanted to perform simulations with the mixing plane interface because as I understood from this source https://www.cfdsupport.com/TCFD-manual/node113.html, it allows averaging the values over the entire circumference of the outlet from the rotor. It seems to me that this would avoid the need to perform several simulations for different positions of the rotor relative to the volute. Do you think this is correct?
Attached Images
 pitch angle.png (17.1 KB, 9 views)

 February 6, 2020, 15:59 #16 Senior Member   Gert-Jan Join Date: Oct 2012 Posts: 1,155 Rep Power: 17 The link refers to OpenFOAM. I don't understand what you want to do with it. I always take the full 3D geometry of my pump (both impeller and volute over 360°). Then using transient analyses and averaging over time, I get the data I want. For this, I never use the 'stage'-option. According to my knowlegde, stage is only required if you use part of the impeller and part of the volute. So, if you also want to do a full 360° calculation (that is why we started this discussion), you don't need 'stage'. But to be honest, I still don't know what you want to do since you don't share a screenshot of your geometry, so I can't help.

 April 7, 2020, 04:16 #17 New Member   Ruchit Patel Join Date: May 2018 Location: Chennai Posts: 24 Rep Power: 4 @marekpl Did u solve your problem? @Gert-Jan I am facing the similar kind of problem. I am running steady simulation of rocket LOX turbopump with Inducer+Impeller+Volute design for 40000 RPM and 4.89 kg/s mass flow in CFX. BC : Inlet - Total Pressure in Stationary Frame with 2.4 bar Outlet - mass flow rate I am using full 360 degree geometry of Inducer, Impeller and Volute. There are three domain - Pipe (stationary), Inducer+Impeller(Rotating) and Volute (Stationary). I am using Frozen Rotor as interface between Pipe and Inducer & Impeller and Volute. But I am getting lower total pressure (in stationary Frame) at Volute outlet than Pipe Inlet. Total Pressure is increasing till interface between Impeller and Volute and after that it is reducing. The difference in mass flow rate between inlet and outlet is coming 0.02 kg/s. Please help me. I don't know what's wrong going on whether it is high RPM or high mass flow or wrong setup of simulation.

 April 7, 2020, 05:03 #18 Senior Member   Gert-Jan Join Date: Oct 2012 Posts: 1,155 Rep Power: 17 Can't comment without a picture. So please upload one.

 April 7, 2020, 05:14 #19 New Member   Ruchit Patel Join Date: May 2018 Location: Chennai Posts: 24 Rep Power: 4 Please Find the attached domain Pics. Initially I was getting the warning of Reversed flow at both Inlet and Outlet. Then I increased the Inlet and outlet section. But Still I am getting warning at Inlet. Last edited by ruchit@15847; April 7, 2020 at 06:54.

 April 7, 2020, 06:05 #20 Senior Member   Gert-Jan Join Date: Oct 2012 Posts: 1,155 Rep Power: 17 I mean pictures of velocity and total pressure of course. An all in stationary frame.

 Tags centrifugal pump