[Johan M]

Greetings all,

I would like to inquire whether the cfx workflow I used is correct and possibilities to over predictions of the outlet total pressure. I am simulating a high speed centrifugal pump running at 25000 rpm, delivering water at 1 kg/s. The outlet total pressure is expected to be 13.3 bar. I have been following the link as a general guideline: https://youtu.be/Ej4OhnoQvtQ?si=br_EnGXnIyPSHxEq

I have used three domains: a full inlet pipe, a periodic impeller passage and a volute shown in image 1. GGI with the mixing plane method was used at all interfaces, based on the paper: https://www.sciencedirect.com/scienc...07904X1830218X. I split the impeller mesh at the Trailing edge to represent the non-rotating vaneless diffuser region according to (minute 2:52) : https://youtu.be/nBs4Zs3rCRQ?si=2rPF2OngPHp4KwtN
The full inlet pipe and volute were meshed in Ansys meshing whereas the impeller passage was meshed in turbogrid.

In CFX Pre, I have selected a total pressure inlet of 2.5 bar, derived from the tank it's pressurized at, and a mass flow outlet. I set the vaneless diffuser patch to counter rotating in the rotating stationary frame of reference – this was done to attain a non-rotating diffuser patch in the stationary reference. I used the SST model with automatic wall treatment, double precision, and an automatic timescale of 1.
I would like to know if my setup is appropriate? Secondly I had gotten negative Cu circumferential velocities from LE to TE (the Cu = -7 to -35 at the LE/TE cut). Is this because I defined my impeller rotation opposite to the direction of positive rotation? I had a feeling as I was looking at the velocity vectors of image 2, from the cfx manual, and saw that rotation direction was opposite to the rotation in the diagram. I will attach images of my CFX Post results with velocity vectors and pressure plots as soon as I have access to the simulation pc I was using.

[Johan M]

Hi Everyone,

I have attached further images

[ghorrocks]

Your vector diagram shows the air exitting the rotor is rotating in the opposite direction to the rotor motion. Are you sure this is correct? Have you specified the rotation direction correctly?

[Johan M]

Originally Posted by ghorrocks

Your vector diagram shows the air exitting the rotor is rotating in the opposite direction to the rotor motion. Are you sure this is correct? Have you specified the rotation direction correctly?

Hi Ghorrocks,

Thanks for your reply.

My thinking as to why the vectors point in that direction is as follows based on the pump velocity vector diagram I checked from Tuzson, J. 2000. Centrifugal pump design. John Wiley & Sons:

Vectors in the stationary frame are the vectors observed by a stationary viewer. Referring to the image from Tuzson, From a stationary frame of reference, you would observe the relative velocity vectors slide onto the blade in a clockwise fashion like Vr1 if your rotor is rotating anticlockwise. Once the vectors exit the rotor, they exit the rotating frame of reference and now travel in the direction of the absolute velocity vectors: in the direction of V2. I took it from the perspective as: if im on a anticlock wise rotating merry go round and jump out of it to the non rotating floor, I would be flung anticlockwise like the exit absolute velocity vector V2

I am not 100% sure if my line of thinking was right, but I observed it to be shown with the velocity vectors from my water pump results.

Any feedback is appreciated.

[ghorrocks]

Please attach your output file, and an image showing velocity vectors (not in stn frame, just velocity so in the local reference frame).

It really looks like the impeller is rotating backwards to me.

[Johan M]

Originally Posted by ghorrocks

Please attach your output file, and an image showing velocity vectors (not in stn frame, just velocity so in the local reference frame).

It really looks like the impeller is rotating backwards to me.

Hi Ghorrocks,

I realized I had made a mistake with the info I provided: I was looking at the label above the color bar as Velocity in Stn Frame when in fact it was just Velocity vectors.

Attached are both the velocity in both frames of reference and the .out file.

I am honestly still abit confused about the direction of the vectors in the rotating frame of reference, even after reading the info on the cfd online wiki about discontinous streamlines compared to my interpretation earlier.

Additionally the .out cfx file was too large to send, I will

[ghorrocks]

If those images are of velocity then it makes a bit more sense.

If the out file is too big to post then remove the iterations from the middle of it. That should make it much smaller. Or you could just post the CCL at the top of the output file.

[Johan M]

Originally Posted by ghorrocks

If those images are of velocity then it makes a bit more sense.

If the out file is too big to post then remove the iterations from the middle of it. That should make it much smaller. Or you could just post the CCL at the top of the output file.

I have attached a zipped file containing the outfile

[ghorrocks]

At the end of convergence your max residuals are quite high yet your RMS residuals are OK. This suggests you have a small region which is problematic. You definitely should plot the residuals to the output file to locate where this problematic region is. It might be a poor quality region (then remesh with a better mesh) or in a separation zone (then consider transient).

You have the alternate rotation model on. Why is that?

You should not need 1500 iterations to converge with a steady state simulation. If you need more than 200 or 300 then something is wrong with your simulation.

Have you tried using double precision? It might converge better.

[Johan M]

Originally Posted by ghorrocks

At the end of convergence your max residuals are quite high yet your RMS residuals are OK. This suggests you have a small region which is problematic. You definitely should plot the residuals to the output file to locate where this problematic region is. It might be a poor quality region (then remesh with a better mesh) or in a separation zone (then consider transient).

You have the alternate rotation model on. Why is that?

You should not need 1500 iterations to converge with a steady state simulation. If you need more than 200 or 300 then something is wrong with your simulation.

Have you tried using double precision? It might converge better.

Hi Ghorrocks,

Thanks for the suggestions. I will plot those residuals in the next run.

I believe the alternate rotation model was automatically selected as I used the turbo set up in CFX Pre.

I see. I am fairly certain that my boundary condition choices are alright as I've used them in my Numeca Fine/Open simulations and arrived at decent results for the same scenario.

I will try it with double precision and post my results

[Johan M]

Originally Posted by ghorrocks

At the end of convergence your max residuals are quite high yet your RMS residuals are OK. This suggests you have a small region which is problematic. You definitely should plot the residuals to the output file to locate where this problematic region is. It might be a poor quality region (then remesh with a better mesh) or in a separation zone (then consider transient).

You have the alternate rotation model on. Why is that?

You should not need 1500 iterations to converge with a steady state simulation. If you need more than 200 or 300 then something is wrong with your simulation.

Have you tried using double precision? It might converge better.

Hi Ghorrocks,

Looking at the output file the impeller (R1) is the region that has the max residuals. I tried to locate these nodes in turbogrid by making a point at those locations (node 620900) but could not seem to track it even though over 929732 nodes are present.

Nevertheless, I adjusted the overall turbogrid mesh parameters to attain a better aspect ratio ratio mesh. I will post the results after the sim completes. Additionally, I reduced the residual convergence criteria to 1e-6 so maybe that is why the simulation continues past 300 iterations.

[Johan M]

Originally Posted by ghorrocks

At the end of convergence your max residuals are quite high yet your RMS residuals are OK. This suggests you have a small region which is problematic. You definitely should plot the residuals to the output file to locate where this problematic region is. It might be a poor quality region (then remesh with a better mesh) or in a separation zone (then consider transient).

You have the alternate rotation model on. Why is that?

You should not need 1500 iterations to converge with a steady state simulation. If you need more than 200 or 300 then something is wrong with your simulation.

Have you tried using double precision? It might converge better.

Hi Ghorrocks,

I still seem to be uncertain of where the issue lies. Would it be advisable to try a transient simulation, as I have already adjusted my mesh quality with no improved behavior either

[ghorrocks]

Yes, a transient solution would be the next thing to try.

[TurBoris]

Hi Johan,

I checked the out file you sent. I saw that the vaneless diffuser domain was included in R1 domain. That means it has a rotating speed. Extending a rotating part in radial direction in a centrifugal machine model would be problematic. As the radius increases, the rotational velocity increases which causes a higher velocity magnitude in absolute frame. That means, your stagnation properties in absolute frame artificially increase.

You better to split the vaneless diffuser from R1 domain and set it as stationary. Connect it to R1 with a frozen rotor or mixing plane. This way you will have a lower stagnation quantities at the exit of vaneless space domain.

Moreover, you can get more accurate results by considering the outlet distortion of the volute. The volute is not axisymmetric and creates different flow field within the blade passages (due to potential effect) . If you have a sufficient computing power run a full wheel steady analysis with frozen rotor interfaces and see the difference between sector model.

Hope these help you.