CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

high rotational speed centrifugal pump

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 9, 2020, 06:41
Default high rotational speed centrifugal pump
  #1
New Member
 
Marek
Join Date: Nov 2019
Posts: 7
Rep Power: 2
marekpl is on a distinguished road
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
File Type: png 1.png (41.3 KB, 22 views)
File Type: png 2.png (72.2 KB, 22 views)
File Type: png 3.png (48.3 KB, 18 views)
File Type: png 4.png (100.9 KB, 20 views)
File Type: jpg 6.jpg (50.0 KB, 39 views)

Last edited by marekpl; January 10, 2020 at 12:28.
marekpl is offline   Reply With Quote

Old   January 19, 2020, 03:40
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,315
Rep Power: 125
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   January 24, 2020, 14:20
Default
  #3
New Member
 
Marek
Join Date: Nov 2019
Posts: 7
Rep Power: 2
marekpl is on a distinguished road
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
marekpl is offline   Reply With Quote

Old   January 28, 2020, 05:23
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,315
Rep Power: 125
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   February 6, 2020, 04:03
Default
  #5
New Member
 
Marek
Join Date: Nov 2019
Posts: 7
Rep Power: 2
marekpl is on a distinguished road
For the full rotor i set the pitch angle side 1 and side 2 to 360 degrees. Is it correct?
marekpl is offline   Reply With Quote

Old   February 6, 2020, 04:16
Default
  #6
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Posts: 1,155
Rep Power: 17
Gert-Jan is on a distinguished road
I would set 'none' for both
Gert-Jan is offline   Reply With Quote

Old   February 6, 2020, 06:45
Default
  #7
New Member
 
Marek
Join Date: Nov 2019
Posts: 7
Rep Power: 2
marekpl is on a distinguished road
The Mixing Plane interface can not be set to none. I can see only "Automatic", "Specified Pitch Angle" and "Value".
marekpl is offline   Reply With Quote

Old   February 6, 2020, 06:51
Default
  #8
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Posts: 1,155
Rep Power: 17
Gert-Jan is on a distinguished road
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
Gert-Jan is offline   Reply With Quote

Old   February 6, 2020, 06:52
Default
  #9
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Posts: 1,155
Rep Power: 17
Gert-Jan is on a distinguished road
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
Gert-Jan is offline   Reply With Quote

Old   February 6, 2020, 07:18
Default
  #10
New Member
 
Marek
Join Date: Nov 2019
Posts: 7
Rep Power: 2
marekpl is on a distinguished road
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.
marekpl is offline   Reply With Quote

Old   February 6, 2020, 07:25
Default
  #11
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Posts: 1,155
Rep Power: 17
Gert-Jan is on a distinguished road
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.
Gert-Jan is offline   Reply With Quote

Old   February 6, 2020, 07:46
Default
  #12
New Member
 
Marek
Join Date: Nov 2019
Posts: 7
Rep Power: 2
marekpl is on a distinguished road
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
marekpl is offline   Reply With Quote

Old   February 6, 2020, 07:59
Default
  #13
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Posts: 1,155
Rep Power: 17
Gert-Jan is on a distinguished road
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.
Gert-Jan is offline   Reply With Quote

Old   February 6, 2020, 11:50
Default
  #14
New Member
 
Lorenzo Bossi
Join Date: Aug 2009
Location: London
Posts: 7
Rep Power: 12
lbossi is on a distinguished road
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
lbossi is offline   Reply With Quote

Old   February 6, 2020, 12:02
Default
  #15
New Member
 
Marek
Join Date: Nov 2019
Posts: 7
Rep Power: 2
marekpl is on a distinguished road
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
File Type: png pitch angle.png (17.1 KB, 9 views)
marekpl is offline   Reply With Quote

Old   February 6, 2020, 15:59
Default
  #16
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Posts: 1,155
Rep Power: 17
Gert-Jan is on a distinguished road
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.
Gert-Jan is offline   Reply With Quote

Old   April 7, 2020, 04:16
Default
  #17
New Member
 
Ruchit Patel
Join Date: May 2018
Location: Chennai
Posts: 24
Rep Power: 4
ruchit@15847 is on a distinguished road
@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.
ruchit@15847 is offline   Reply With Quote

Old   April 7, 2020, 05:03
Default
  #18
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Posts: 1,155
Rep Power: 17
Gert-Jan is on a distinguished road
Can't comment without a picture. So please upload one.
Gert-Jan is offline   Reply With Quote

Old   April 7, 2020, 05:14
Default
  #19
New Member
 
Ruchit Patel
Join Date: May 2018
Location: Chennai
Posts: 24
Rep Power: 4
ruchit@15847 is on a distinguished road
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.
ruchit@15847 is offline   Reply With Quote

Old   April 7, 2020, 06:05
Default
  #20
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Posts: 1,155
Rep Power: 17
Gert-Jan is on a distinguished road
I mean pictures of velocity and total pressure of course.
An all in stationary frame.
Gert-Jan is offline   Reply With Quote

Reply

Tags
centrifugal pump

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Power calculation in centrifugal pump - CFD Post Hazem_9 ANSYS 1 May 11, 2017 14:22
CFX High speed wall function-ERROR Fabiio87 CFX 3 August 23, 2016 06:50
Strange high velocity in centrifugal pump simulation huangxianbei OpenFOAM Running, Solving & CFD 26 August 15, 2014 02:27
Autoblade centrifugal pump template mahdi balali NUMECA 3 February 18, 2014 08:56
how to solve the diverage of high speed centrifugal compressor, CFD code is STAR CCM layth STAR-CCM+ 3 May 21, 2012 05:48


All times are GMT -4. The time now is 02:26.