[marekpl]

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?

[ghorrocks]

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.

[marekpl]

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

A wall has been placed at portion (s) of an INLET

and then

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?

[ghorrocks]

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.

[marekpl]

For the full rotor i set the pitch angle side 1 and side 2 to 360 degrees. Is it correct?

[Gert-Jan]

I would set 'none' for both

[marekpl]

The Mixing Plane interface can not be set to none. I can see only "Automatic", "Specified Pitch Angle" and "Value".

[Gert-Jan]

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]

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

[marekpl]

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.

[Gert-Jan]

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.

[marekpl]

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

[Gert-Jan]

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".

[lbossi]

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

[marekpl]

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?

[Gert-Jan]

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.

[ruchit@15847]

@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.

[Gert-Jan]

Can't comment without a picture. So please upload one.

[ruchit@15847]

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.

[Gert-Jan]

I mean pictures of velocity and total pressure of course.
An all in stationary frame.