[Johan M]

Hi All,
I am simulating a high speed centrifugal pump (rpm > 20000) that consists of three domains: an impeller, a rear leakage path, and a volute. Liquid oxygen is the fluid. The impeller and leakage path blocks were modelled in the rotating reference frame, and the volute in the stationary frame seen in image 1. Due to the step down of geometry between the impeller exit, gap and volute entrance, I had to split the leakage path block into more patches, seen in image 2 and 3: the leakage path block must remain aligned with the hub surface from whats mentioned in the turbogrid tutorials. As such, I modelled the leakage path with its upper most patch aligned with the hub, and set its patch to be interfaced with the hub patch as frozen rotor denoted in red by A. I split the vertical patch of the leakage path and set it to interface with the volute using a frozen rotor interface denoted in blue by B.
I simulated a single impeller passage, with leakage path and volute using the frozen rotor method and came to reasonable results of the meanline analysis. I used a total pressure inlet and mass flow outlet.
I switched to the mixing plane interface at the formerly mentioned patches but encountered severe divergence issues. I then went through the cfd forums wiki to diagnos the issue. I have tried the following thus far:

1. Improving mesh quality
2. varying auto time scale
3. Trying a physical timescale based on 1/ω
4. Increasing the inlet total pressure boundary condition
5. Using the converged frozen rotor simulation as initial conditions for the mixing plane

The solution was converging decently until The p-mass rms residual spikes up heavily and the rms residuals are 2 orders higher than the max residuals, pointing toward possibly a local issue. I also noticed unrealistically high velocities at the interfaces (> 200 m/s) and am in the process of refining those regions.
But have had no luck so far. I would like to know if there are any suggestions of what else I can attempt? I will also make a plot of max residuals to observe where high regions are present

[ghorrocks]

If you rearrange the interfaces like this does it help things?
Image.jpg

In fact, do you need the interface between the leakage path and the rotor at all? Why not just model that as one rotating domain?

[Johan M]

Originally Posted by ghorrocks

If you rearrange the interfaces like this does it help things?
Attachment 100161

In fact, do you need the interface between the leakage path and the rotor at all? Why not just model that as one rotating domain?

Dear Ghorrocks,

Thanks for the reply. That could work, it would just require the hub to 'step down' axially. Im not sure if that is possible in turbogrid but I will look into it.

That would be ideal. I was following the Secondary flowpath Turbogrid tutorial as my reference. In there, the procedure they follow results in the secondary flow path turning into a seperate block. As such I followed the same steps for my leakage path being a seperate block.

[Johan M]

Originally Posted by ghorrocks

If you rearrange the interfaces like this does it help things?
Attachment 100161

In fact, do you need the interface between the leakage path and the rotor at all? Why not just model that as one rotating domain?

Dear Ghorrocks,

You have a point there, I forgot in CFX you can assign multiple volumes to one block.

By the way, for my original configuration, in turbogrid they will still be two seperate meshes from what Ive seen in the tutorials

I'd like to ask a follow up question in this regard. If I use the original setup but assign both the impeller and leakage path to one rotating component, is it correct to set the interface between the impeller hub and leakage path entrance (red line denoted as A) to a General Connection with None as my frame change mixing volume as both components are being solved in the rotating reference frame?

.

[ghorrocks]

If I use the original setup but assign both the impeller and leakage path to one rotating component, is it correct to set the interface between the impeller hub and leakage path entrance (red line denoted as A) to a General Connection with None as my frame change mixing volume as both components are being solved in the rotating reference frame?

Yes, that is correct.

[Johan M]

Originally Posted by ghorrocks

Yes, that is correct.

Alright I will try that out

[Johan M]

Originally Posted by ghorrocks

If you rearrange the interfaces like this does it help things?
Attachment 100161

In fact, do you need the interface between the leakage path and the rotor at all? Why not just model that as one rotating domain?

Hi Ghorrocks,

I ran a simulation with one rotating block for the rotor and leakage path. The simulation begins diverging rapidly after 35 iterations as seen by the image. The p-mass residual is the issue and spikes high, along with the mass flow at the inlet. This issue occurred when I had the two blocks as separate rotating domains with the mixing plane method, but did not occur when using the frozen rotor

[ghorrocks]

I would rerun it and save a backup file (or just stop the simulation) at 25 iterations. Load up the results file in CFD-Post and have a close look. Try to find the spot where things are going wrong. You will probably find it shows your setup has an error, or maybe a region of poor mesh or some other problem.

[Johan M]

Originally Posted by ghorrocks

I would rerun it and save a backup file (or just stop the simulation) at 25 iterations. Load up the results file in CFD-Post and have a close look. Try to find the spot where things are going wrong. You will probably find it shows your setup has an error, or maybe a region of poor mesh or some other problem.

Alright I shall do that, and likely will make contour plots of residuals to check where the max regions occur to narrow down the issue.

[ghorrocks]

Yes, that will help as well.

[Johan M]

Originally Posted by ghorrocks

Yes, that will help as well.

High residuals were shown to be in the pipe section of the domain from the contour plots. I went through a series of pipe length extensions and domain refinements to resolve this issue. For 35 iterations the mass and outlet total pressure monitors are close to the target values seen in the images. However, post 35 iterations the p mass residual spikes up and fails, confirmed by the large mass monitor increase.

Post processing just before that iteration of failure showed high velocities (> 200 m/s) at a small portion of the volute inlet cells, near the mixing plane region. Additionally, near the hub surface also showed unusually high velocities. I will refine the mesh in these regions. Besides those under refined regions being the issue, Im still uncertain as to why the simulation behaves after 35 iterations.

[Opaque]

Your initial guess seems poor, and your timescale is too much for it.

You can improve the initial guess by starting with the frozen rotor (not my cup of tea) since you already said it converges, or reduce the timescale factor by 10 and see what happens.

With 1/10 of the timescale, it may be slow converging but a first pass is to understand if it works at all, and then find out if you can optimize your calculations. Optimizing with "implicit setup errors" is nearly impossible.

[ghorrocks]

Also note that refining the mesh at a problem area is likely to make the divergence worse, not better. You will find convergence much easier with a coarser mesh - but the accuracy will reduce, of course.

The problem might be mesh quality, it might be time step size, it might be initial conditions.

You might be able to use this coarse mesh = easy convergence and poor accuracy thing to generate a better initial condition for a finer mesh simulation.

[Johan M]

Originally Posted by Opaque

Your initial guess seems poor, and your timescale is too much for it.

You can improve the initial guess by starting with the frozen rotor (not my cup of tea) since you already said it converges, or reduce the timescale factor by 10 and see what happens.

With 1/10 of the timescale, it may be slow converging but a first pass is to understand if it works at all, and then find out if you can optimize your calculations. Optimizing with "implicit setup errors" is nearly impossible.

Thanks for the suggestions. Reducing the time scale resulted in divergence earlier on seen by the image below. I will try it with the initial conditions from the frozen rotor run.

Alternatively, I was thinking of attaching the leakage path to the volute instead, and modelling it full 360 out of curiosity to see if its and interface issue.

[Johan M]

Originally Posted by ghorrocks

Also note that refining the mesh at a problem area is likely to make the divergence worse, not better. You will find convergence much easier with a coarser mesh - but the accuracy will reduce, of course.

The problem might be mesh quality, it might be time step size, it might be initial conditions.

You might be able to use this coarse mesh = easy convergence and poor accuracy thing to generate a better initial condition for a finer mesh simulation.

Is it because a coarser mesh is less likely to capture effects like wakes/vortices making convergence easier? I should have specified that I intended to refine only the cells at the volute inlet as cells at the mixing plane interafce of the impeller/leakage path were more refined compared to the volute inlet. I was thinking that the jump in cell size might have affected results

I have been using automatic initial conditions and will try something closer to whats expected. Failing which, ill likely model the leakage path mesh as part of the volute instead with a full 360 representation, and keep the impeller as a single passage

[ghorrocks]

Yes, it is partly because a coarser mesh is less likely to capture fine flow features; but mainly because the mesh adds numerical dissipation to the model which is effectively additional viscosity. This additional numerical viscosity helps stabilise the flow. But it is also a source of inaccuracy, which is why finer meshes are more accurate but harder to converge.

Yes, big jumps in mesh size are bad for mesh quality. You should avoid doing this as much as possible.

Yes, definitely try a better initial condition. But do not forget mesh quality - this is very often the cause of problems like this. If you can remesh and improve quality I guarantee it will converge better.

[Johan M]

Originally Posted by ghorrocks

Yes, it is partly because a coarser mesh is less likely to capture fine flow features; but mainly because the mesh adds numerical dissipation to the model which is effectively additional viscosity. This additional numerical viscosity helps stabilise the flow. But it is also a source of inaccuracy, which is why finer meshes are more accurate but harder to converge.

Yes, big jumps in mesh size are bad for mesh quality. You should avoid doing this as much as possible.

Yes, definitely try a better initial condition. But do not forget mesh quality - this is very often the cause of problems like this. If you can remesh and improve quality I guarantee it will converge better.

I see, thanks for the clarification.

Alright I'll have a recheck through all my meshes for quality issues