[jgross]

Hi everyone,

I am using CFX to predict head and efficiency for a centrifugal pump domain, including suction, throatbush, complete impeller, volute, and discharge domains.

PumpGeometry.jpg

I would like to compare the results from steady state simulations (with frozen rotor interfaces) to the time-averaged quantities obtained from transient flow simulations as a means of validation.

I ran a pump curve study with the steady state simulation setup and found the head and efficiency prediction was sufficiently accurate (+- 10% of experimental result). However, when I run the same study (same BCs and same setup) with the transient flow simulation (total of 5 revs to make sure results were 'time-converged'), the (time-averaged for 1 rev) efficiency prediction is significantly worse, across all mass flow rates.

PumpCurveHead.png


PumpCurveEfficiency.png


PumpCurvePower.png

Although the head prediction is largely the same for both setups. The torque prediction is significantly off, as seen in the last figure for shaft power, resulting in much higher efficiency values.

Does anyone have any suggestions as to what could be causing this massive difference in performance prediction when using transient flow simulations?

My thoughts are that, considering I have used the same BCs and setup from the steady state simulation and initialized with the results from that simulation, the issue may stem from the following possibilities:

1. I am incorrectly predicting time-averaged shaft power using a moving window approach, or
2. Incorrect setup for the transient flow simulation.

I have extensively referred to the FAQs available on CFD Online for assistance, including this one and this one.

Things I have tried include:

1. Validated the results from the steady state simulation by comparing to experimental results
2. Performed a grid independence check for the steady state simulation to determine the ideal mesh density
3. Performed numerous sensitivity studies for the steady state simulation, including checks on turbulence model (used SST in the end) and physical time step
4. Tried different values of timestep for the transient simulation, with values ranging from 50 timesteps per rev to 360 timesteps per rev
5. Tried different different mesh densities during the transient simulations, including the coarse, medium and fine mesh densities from the aforementioned grid convergence study
6. Tried different values of residual for the inner loop (1e-4, 1e-5 and 1e-6)

I have attached my CCL file (saved as a TXT file so it could be uploaded) for reference. Please see Transient.txt in the attachments.

Thanks in advance!

[Opaque]

I wonder what your prediction looks like if you use the mixing plane model.

Then, you will have 3 predictions to compare and better informed to analyze the data.

I am not a proponent of the frozen rotor approximation. It had its time 10+ years ago when running transient simulations was not a trend, but with today computational resources, I will avoid it if possible.

Recall the frozen rotor approximation lets the wakes propagate too far downstream out/into a rotating component. Not physical.

[Gert-Jan]

I don't see strange things in your setup, besides that your efficiency uses omega as an expression which is not used for setting the speed of the impeller. This is a fixed value of 1000 rev/min. Can be tricky..... Are you sure everything is consistent in all calculations?

In general I trust the transient results more than the frozen stator results. Also, mostly CFX is not that far of. Given this pump of significant size, I would give it 75% efficiency or above around BEP.

So, I would like to know:
- How is it measured in the lab?
- What is included in the efficiency of the experiment?

[jgross]

Thanks for the replies guys! I will respond to each of your points below.

Opaque:

I wonder what your prediction looks like if you use the mixing plane model.

During my original sensitivity studies for the steady state simulations I tried using the mixing plane model. However, I found that the results were way off and that the frozen rotor setup seemed to give better prediction.

In retrospect, the performance prediction for mixing plane simulation was actually rather similar to what is observed in the transient results (at least at BEP), with a significant under prediction of torque leading to over prediction of efficiency.

I have not yet performed a full pump curve study with the mixing plane setup. However, I will try that and provide an update with the results from that study.

I should note that one reason I did not persue using mixing plane any further was due to this excerpt from Section 5.3.3.1.3 of the CFX-Solver Modeling Guide:

Stage analysis is not appropriate when the circumferential variation of the flow is significant relative to the component pitch (for example, a pump and volute combination at off-design conditions).

Gert-Jan:

I don't see strange things in your setup, besides that your efficiency uses omega as an expression which is not used for setting the speed of the impeller. This is a fixed value if 1000 rev/min. Can be tricky..... Are you sure everything is consistent in all calculations?

Yes, I wasn't exactly sure how to set omega from the simulation value, so I manually calculated omega in rads/s. This is consistent as 1000RPM is approx equivalent to 104.71975499999982 rad/s (the value used in my calculation).

So, I would like to know:
- How is it measured in the lab?
- What is included in the efficiency of the experiment?

These are both very valid questions.

Unfortunately, I do not have very intimate knowledge of the experimental set up as I did not run the experiment myself and have simply been given the results to use during validation.

However, I have previously discussed these results with someone who has more intimate knowledge of the experiment than myself. This person has assured me that the CFD setup largely matches the experimental setup.

One key exception to this is the inclusion of a non-rotating back plate shroud in the experimental setup. This domain has been excluded in the CFD setup for a number of reasons, which I will not go into here.

Obviously not including this domain in the CFD setup will affect the accuracy of the results, but I did not expect to see such a massive increase in efficiency. In particular, nearly 90% at BEP for a pump of this type and size seems very off to me. However, please correct me if I am wrong here.

Thanks again to both of you! I really do appreciate you taking the time to provide suggestions.

[ghorrocks]

My comments:

Are you sure your time step is small enough in the transient simulations? Your finest time step of 360 steps per rev sounds pretty coarse to me. You might need to go finer.

But my main point is you need to look at the results in detail with the post processor. Opaque made a very interesting point that the wakes can extend too far downstream in the frozen rotor approach - so I would look to see if this is affecting your results. Look for separations, wakes, back flows and any other unusual flow features and see if that explains the difference between the runs.

[jgross]

The results from the pump curve study with mixing plane interface can be found below.

PumpCurveHead.png

PumpCurveEfficiency.png

PumpCurvePower.png

At lower flow rates, the results seem reasonable, with head closely matching what was obtained in the transient simulations and efficiency & shaft power lying somewhere between the results from the frozen rotor and transient simulations.

However, at higher flow rates, the head prediction is way off. I suppose this matches what the CFX-Solver Modelling Guide suggested, as this approach does not seem appropriate for this analysis (pump and volute combo) at these off-design conditions.

In response to Ghorrocks suggestions, I have also set up a transient simulation with 720 time steps per rev. Although that is still running, the results so far seem to align closely to those obtained using 100 time steps per rev (at least at BEP). To me this suggests that the issue does not lie in the number of time steps used. However, I can attempt an even finer time step if suggested.

[jgross]

I have also had a look at the velocity flow fields to see if there are any unusual flow features that may explain the differences in the results.

The figures shown below are from simulations at BEP.

Frozen rotor

FrozenRotorFlow.jpg

Mixing plane

MixingPlaneFlow.jpg

Transient (at last time step)

TransientFlow.jpg

First thing I notice when looking at the figures is that there does indeed seem to be a large region of separation in the 'southeast' blade passage when inspecting the results from the frozen rotor simulations. Although the flow fields from the transient and mixing plane simulations both have regions of back flow, there are not nearly as pronounced as what is found in the frozen rotor case.

To me this suggests that (as Opaque said), the frozen rotor setup might give non-physical results in this case. I suppose then that the issue might be that the results are considerably affected (significantly more than I anticipated) by the exclusion of the back plate shroud, and that the results from the transient simulations (and the mixing plane simulations at low flow rates) are actually more trustworthy.

If I could, I would use the transient flow setup for my studies. Unfortunately, I am looking to use this CFD setup for a design optimization study and such computational cost would be prohibitive in this case. On the other hand, the fact that the results from the mixing plane setup are so off at off-design conditions makes using this setup not very appealing either. In particular, I worry that the CFD results would be unreliable for many designs which would negatively affect the optimization.

Given my desire for a robust yet time-effective means of evaluation, I am still leaning towards using the frozen rotor setup. However, if anyone has any advice or suggestions for me, I would definitely appreciate hearing it!

Thanks again everyone!

[Opaque]

I understand you could split the mixing plane into multiple sections.

If that is possible with your mesh setup, you could split the full interface with a section of the rotor in front of the volute/pipe section, and the rest for the remaining rotor in front of the remaining volute.

Very likely you may need to try different angles to study the sensitivity to the split angle.

Just a thought

[jgross]

Thanks again for responding Opaque.

I understand you could split the mixing plane into multiple sections.

If that is possible with your mesh setup, you could split the full interface with a section of the rotor in front of the volute/pipe section, and the rest for the remaining rotor in front of the remaining volute.

I am sorry, but I do not understand this.

Do you mean using a periodic impeller setup (like the one in the image below)?

PeriodicPump.png

[Opaque]

To create a domain interface we need to select surface meshes for side 1 and side 2.

Assuming side 1 is on the rotor side, and you have created the full rotor by replicating a base sector, I am certain you should have a list of names of the "outlet of the rotor" such as outlet 1, outlet 2, ...

Assuming side 2 is on the volute side, you may need to have the surface mesh split into "named regions" that when put together represent the 360 deg circumference. Say, they are named volute_inlet 1 and volume_inlet 2

You should be able to now create several domain interfaces:

Domain interface 1 = outlet 1 & volute inlet 1
Domain interface 2 = outlet 2+outlet 3+outlet .. & volume inlet 2

Keep in mind you rotor domain is still the full rotor. You would have split the domain interface into two or more pieces.

Hope the above is a better description now.

[jgross]

Thank you for the clarification, Opaque. I believe I understand your suggestion now.

In that case, I suppose I would need to split the volute interface such that 'volute inlet 1' interface directly corresponds to the impeller 'outlet 1' interface. From there, I would need to remesh the volute such that there is a patch-dependent surface mesh corresponding to the 'volute inlet 1' interface. Then I would run the steady state simulation with the two mixing plane interfaces representing the interface between the impeller and volute.

I can try that out for this particular case to see if that improves the performance prediction when using mixing plane interface at off-design conditions.

However, before I do that, could you explain the reasoning behind your suggestion?

My understanding is that this approach would attempt to ensure that the circumferential variation of the flow is not significant relative to the component pitch. Therefore, allowing the mixing plane interface to be applied to a pump and volute combo, even at off-design conditions.

One thing I should probably note is that I don't think this approach would be particularly feasible during my design optimization routine as the periodic impeller outlet may vary across designs. In particular, depending on the blade lean and twist, the periodic impeller outlet may be 'twisted'.

The images below show a rather extreme example of this.

Design 1:

ImpellerOutlet1.png

Design 2:

ImpellerOutlet2.png

These differences in twist (seemingly) do not matter when considering the full impeller domain, as they correspond fully to the volute inlet domain when periodic impeller domain is rotated and copied.

However, this is signicantly more tricky when creating a 'volute inlet 1' interface which corresponds directly to the impeller outlet interfaces shown above.

[Opaque]

Splitting the volute side is a workaround because if I recall a surface mesh cannot be used in two different domain interfaces.

If you could select the full volute surface mesh for both (or more) domain interfaces, the design process should be transparent to the changes in the impeller.

It is just an idea to obtain a better prediction.

An old practice with a frozen rotor approximation was to change the relative position of the impeller with respect to the volute/pipe region and study the impact on the predictions. Recall the extended wakes are an issue (as you noticed), and they do not exist because the passing impeller tends to mix them up.

[jgross]

Splitting the volute side is a workaround because if I recall a surface mesh cannot be used in two different domain interfaces.

If you could select the full volute surface mesh for both (or more) domain interfaces, the design process should be transparent to the changes in the impeller.

It is just an idea to obtain a better prediction.

Thanks for the explanation! I understand your suggestion more clearly now.

Although this approach may not be suitable for the design optimization runs, I may still try it to see if it does help improve the performance prediction for mixing plane interface setup.

An old practice with a frozen rotor approximation was to change the relative position of the impeller with respect to the volute/pipe region and study the impact on the predictions. Recall the extended wakes are an issue (as you noticed), and they do not exist because the passing impeller tends to mix them up.

Yes, I have come across a number of studies which have taken this approach. I suppose one option might be to run a few frozen rotor simulations with varied relative position and use these results to predict performance (possibly with some kind of weighted average). I believe I have seen some studies which have done that in the past.

In any case, thanks again for all of your helpful suggestions and advice!