[Shobhit11]

Im doing steady state 3D simulation of a centrifugal pump using impeller geometry generated using BladeGen with data given by Vista CPD for some particular operating conditions. The volute geometry was also based off Vista CPD data. CFX was used to setup the simulation. Assuming that the setup(boundary conditions, interface def, solver settings etc) was correctly done, is the following streamline plot correct for starting points at the rotor inlet?

Screenshot 2024-04-01 110124.png

Why are continuous streamlines starting from the rotor inlet and reaching the stator outlet not observed?

PS. Convergence was not reached, around 200 iterations were performed.

[ghorrocks]

The reason is related to this FAQ: https://www.cfd-online.com/Wiki/Ansy...f_reference.3F

The streamlines are not doing what you probably think as the rotor is in a rotating frame of reference and the volute is in a stationary frame of reference. So the streamlines are being calculated across two frames of reference.

[zacko]

Looking at the streamlines near the leading edge, they do also look way off. Is the mass flow correctly entered?

Also, tell us more about your setup. Can you post your .OUT file for reference?

[zacko]

Moreover, the outlet domain of your impeller seems to run inside (or even outside??) the volute channel, that looks odd to me.

[Shobhit11]

At the rotor inlet, static pressure of 1 atm was specified and mass flow rate of 0.05 kg/s per component was specified at the stator outlet. However as pointed out, the stator and the rotor did not meet at a single surface(pic for reference).

Screenshot 2024-04-01 180929.png

Neither does the streamline plot of velocity in stn frame appears to be correct.

Screenshot 2024-04-01 182727.png

It was puzzling considering that both of them were generated using the same Vista CPD data. I could not find how to generate the .OUT file but the file below does contain the setup info.

setup.ccl.txt

It has been some time since I've been stuck on this so any help is highly appreciated.

[zacko]

The .out File will be created after the solver (successfully) stopped. It will be inside the directory of your result file.

The outlet domain of the impeller should not be used. If you disable it (just not include it in the rotor domain setup)., do the interface of the volute and the outlet of the impeller meet? What interface did you specify between impeller and volute?

Did you consider pitch angles at the interface?

[Shobhit11]

The outlet domain for the rotor was already disabled while TurboGrid component was used for meshing but it didn't make much of a difference to be honest. The rotor outlet was anyways protruding into the stator part.
As regards the rotor-stator interface condition, the following setup was used:
Screenshot 2024-04-02 002919.png

I considered the pitch change to be automatic assuming the solver would take care of the same but the solver shows the following message:

In Analysis 'Flow Analysis 1' - Domain Interface 'S1 to R1': Pitch Change option 'Automatic' is not valid if side 1 or 2 of the interface has a 360 degree or greater pitch angle, zero radius, mesh faces normal and parallel to the rotation axis, or mesh faces at the hub curve (low radial or axial position) which are thin in the radial or axial direction.

Also, the zipped .OUT file is attached herewith.

CFX_001 - Copy.out.zip

[zacko]

Thanks for the Out File.
Here are some comments:

1) You have a mass flow rate of 0.05 kg/s per channel. You run with water, that would result in a Flow rate of 1.06 m^3/h (assuming 6 vanes for the impeller).
Is that really correct? The volute and the impeller do not look like small specific speed size - is that correct? What Head do you expect?

2) Why do you specify an OPENING at the rotor inlet? Do specify a total pressure boundary condition at the inlet instead.

3) The pitch angles seem to be calculated correct (60 ° / 360 °). But, since CFX throws the error, enter the pitch angles by your own in CFX Pre and run again.

4) Increase your max iterations. I highly doubt the run will converge within 400 iterations.

5) RMS value of 1e-4 is too loose. You should maybe consider changing to 1e-5 or 1e-6 for RMS.

[ghorrocks]

The simulation looks either under converged (ie: inaccurate) or massively off design conditions. I would check convergence, and if that is OK then look at the operating point and I suspect you will find it will run better at a different speed/flow/pressure point.

[Shobhit11]

Many thanks for your quick reply.

I had to make the rotor inlet as opening due the solver sort of blocking the inlet (it says that a wall has been placed at a portion of the inlet and suggested to switch to an opening type boundary condition instead) when static pressure boundary condition of 1 atm had been applied at the inlet. The simulation ended erroneously in about 100 iterations.

.OUT file: output1.zip

When I used opening boundary condition at inlet with relative pressure of 1 atm and mass flow rate of 4 kgs^-1 per component it did run for around 800 iterations although the velocity residuals had become kind of periodic and I doubt further running would result in <1e-5 accuracy.
Also, I did specify the respective pitch angles at the interface.

.OUT file: output.zip

In the post processing when I plotted the streamlines starting from the rotor inlet, I did get a much better plot but the flow doesn't reach the outlet seemingly, it kind of recirculates.

Screenshot 2024-04-02 162707.png

[zacko]

What is the design flow rate of that pump?

You are talking about 0.05 kg/s per component and then about 4 kg/s. This is a HUGE difference. Your pump does not operate in its preferred operating region it seems, which might also be the reason why you have already recirculation at the inlet.

[Shobhit11]

As per the operating conditions given in the Vista CPD module, the given values of flow coefficient, power and head coefficient implied that the mass flow rate at the design point was about 5.5 kg/s.

When I did the simulation with outlet mass flow rate of 5.8 kg/s, I did get the following streamline plot (for 25 seed points at the rotor inlet):

Screenshot 2024-04-03 151452.png

It has much lesser recirculation, so it is close to the design point I suppose. Can you please verify the same?

[ghorrocks]

It sure looks to be running better. I would keep going higher flow rate.

[zacko]

It looks much better now. The streamlines on the pressure and suction side of vane still look a bit off for me...

[Shobhit11]

Maybe the streamlines are a bit odd in the impeller suction and pressure side because it the variable 'Velocity' that I'm plotting and not 'Velocity in Stn Frame'. However when the second variable is used, the following plot shows up:

Screenshot 2024-04-03 194115.png

Any explanation for this?

By the way thanks for your time. This all was part of a project and I had to somehow present the results convincingly.

[zacko]

"Velocity" here, represents the velocity in the rotating frame. Which is - looking at the velocity triangle - the relative velocity. The variable "Velocity in St Frame" represents the Velocity in the stationary frame, thus the absolute velocity in the velocity triangle.
Looking at the streamlines in an impeller, which is rotating, the variable "Velocity" is correct. The streamlines should (ideally) follow the blade. But yours not look like that. In my opinion the outlet domain should not be there. (see red marked area in the screenshot down below). It is running inside the volute.

[Shobhit11]

Okay, I understand. Seemingly the geometry wasn't properly constructed.

[zacko]

Originally Posted by Shobhit11

Okay, I understand. Seemingly the geometry wasn't properly constructed.

Maybe.

Idk if you have time or are willing to further investigate that case. In case you want:
When you define your R1 domain (impeller) in Pre do not include the geometry that includes "OUTBLOCK" only use "INBLOCK" and "PASSAGE".
Then, define the interface new and run the simulation again.
Would be interesting, to see the result then.