[Johan M]

Hi everyone,
Ive been attempting to simulate cavitation in a cryogenic centrifugal pump. I was using the steady state, cavitation disabled, converged solution as my initial conditions. My boundary conditions were a total pressure inlet and a mass flow outlet. My domain consists of an inlet pipe, periodic sector of an impeller and a volute.
I used the Raleigh Plesset cavitation model. The cavitation condensation and evaporation coefficients were attained from : https://www.mdpi.com/1996-1073/15/14/4943. I modified the vapor pressure to that of LOx at 100K using REFPROP. The remaining parameters (mean diameter, max density ratio, cavitation rate under relaxation etc) were kept as their defaults.

My monitor results showed periodic fluctuations as seen in the attached image (left half are discharge pressure and right side are inlet mass flow). Vectors plots of the domains (the inlet pipe, impeller and volute) showed normal behaviour (no inlet recirculation/ unusual deadzones). The issue lies in the inlet pipe mass flow rate being significantly higher (over 5%) than the discharge flow rate.
Ive tried reducing the automatic timescale factor helped “smooth” out these fluctuations but ultimately did not result in convergence. From looking at past forums, I believe the next step is to attempt a transient simulation, but I’d like to know if there are any other alternatives I can try before investing that computational time.

Any advice is appreciated

[ghorrocks]

This FAQ explains your options: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

First make sure your mesh quality is as good as you can get it. Mesh quality will make a big difference to convergence in this case - and do not believe the "ok" shown at the top of the output file for mesh quality for a multi phase model, these cases require a higher level of mesh quality than single phase models.

But you are likely to be correct - in my experience cavitation models usually require transient simulations to obtain convergence. If you look at the results you have got so far you will probably find the cavitating region is irregularly shaped. This is a sign that there is no steady state solution for this case.

[Johan M]

Originally Posted by ghorrocks

This FAQ explains your options: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

First make sure your mesh quality is as good as you can get it. Mesh quality will make a big difference to convergence in this case - and do not believe the "ok" shown at the top of the output file for mesh quality for a multi phase model, these cases require a higher level of mesh quality than single phase models.

But you are likely to be correct - in my experience cavitation models usually require transient simulations to obtain convergence. If you look at the results you have got so far you will probably find the cavitating region is irregularly shaped. This is a sign that there is no steady state solution for this case.

Thanks for advice. I will try to improve the mesh further before going the transient route. Additionally, I've made the inlet pipe length equal to 2.5*impeller diameter originally - ill increase this lenght in my non-cavitation, steady state simulations and see if I can improve the convergence ( my discharge pressure monitor was shown to be "noisey" by my collegues and I have opted to improve its convergence further before enabling cavitation)

[Johan M]

Originally Posted by aqibfaz

So, is it solved? We're also facing almost same issue since last night.

Hi there,

Unfortunately not yet. Currently implementing Mr. Ghorrocks advice. I will update this post once I get more results.

What adjustments have you done thus far to your cavitation simulation to improve convergence?

[Opaque]

A little piece of advice, not the solution to your current problems.

Ansys CFX can write the residuals as a solution variable in the results/backup files. Once the residuals are settled, either to a flat value or within an reasonable oscillating range, you can isolate which region of the flow is refusing to converge.

If the region is within the area of interest for the simulation, more work is required. If the region is far away, hidden in an unimportant corner or cavity, it is up to you to decide if more work is worth doing.

[Johan M]

Originally Posted by Opaque

A little piece of advice, not the solution to your current problems.

Ansys CFX can write the residuals as a solution variable in the results/backup files. Once the residuals are settled, either to a flat value or within an reasonable oscillating range, you can isolate which region of the flow is refusing to converge.

If the region is within the area of interest for the simulation, more work is required. If the region is far away, hidden in an unimportant corner or cavity, it is up to you to decide if more work is worth doing.

Hi Opaque, thanks I will try to find and isolate this region with this method

[Johan M]

Originally Posted by ghorrocks

This FAQ explains your options: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

First make sure your mesh quality is as good as you can get it. Mesh quality will make a big difference to convergence in this case - and do not believe the "ok" shown at the top of the output file for mesh quality for a multi phase model, these cases require a higher level of mesh quality than single phase models.

But you are likely to be correct - in my experience cavitation models usually require transient simulations to obtain convergence. If you look at the results you have got so far you will probably find the cavitating region is irregularly shaped. This is a sign that there is no steady state solution for this case.

Hi everyone,

After a few weeks of failed attempts, I'd like to provide an update:

steadystate simulations with cavitation enabled resulted in massive flow imbalances being present.

After mesh improvements, adjustments of cavitation model parameters I decided to switch to a transient simulation with cavitation enabled. My transient simulation parameters are below:

timestep: selected such that it results in one degree of motion per timestep
Totaltime: selected so that the impeller moves 30 degrees
Min coefficient loops: 3
Max coefficient loops: 10
Convergence criteria: 1e-5

However I am still getting huge inlet recirculation, even after 30 degrees of rotation. Initially I got recirculation values of 62% of the faces/ 53% area. I had high aspect rations (over 10 000 due to a small first layer height [2e-7m]) and low orthogonality (below 0.01). I improved the mesh abit AR (6000~) and the number of orthogonality cells < 0.01 reduced. This mesh resulted in I recirculation values of 4% of the faces/ 3% area. The inlet mass flow monitors for the before and after quality improvement is attached

Still, my mass flow rate imbalance is high (over twice the percent of nominal). In my steady state sims, a long, low-pressure region below the vapor existed at the inlet pipe. We suspect it might be the backflow through the leading edge that is contributing to this phenomena. To this end my collegue modified the geometry at the inlet shoulder and it omitted the vapor region. I then ran a transient cavitation sim on this geometry but was still met with the former errors, rulling out the inlet vapor region as the possible reason for the imbalance.

Currently, I am running out of options as to what I should attempt next. I could keep trying to improve the mesh as had a direct influence on the recirculation. Additionally, Im also running a water equivalent version of the pump and will update my post on those results.

I was advised to try a cavitation sim with properites of the cryogenic fluid at a lower temperature and vapor pressure

[ghorrocks]

Definitely keep trying to improve the mesh. Aspect ratios of 6000 are not good for cavitation models so try to improve that.

Also, smaller time step might help. And definitely stay with a transient model.

Finally, your maximum residuals are really high. Output your residuals to the output file and have a look at where in the model these high residuals occur - they will tell you the section of the model which is having troubles converging. You can then focus your mesh quality improvements on this region.

[Johan M]

Originally Posted by ghorrocks

Definitely keep trying to improve the mesh. Aspect ratios of 6000 are not good for cavitation models so try to improve that.

Also, smaller time step might help. And definitely stay with a transient model.

Finally, your maximum residuals are really high. Output your residuals to the output file and have a look at where in the model these high residuals occur - they will tell you the section of the model which is having troubles converging. You can then focus your mesh quality improvements on this region.

Thanks, I will try those options. On the aspect ratio, is there a maximum target aspect ratio you would recommend I don't exceed for these kinds of cavitation simulations? Besides the default 1000 maximum recommended in the user guides?

[ghorrocks]

The 1000 in the manual is for single phase flows. You have a very numerically unstable multiphase flow, so your recommendation will be more strict than that. It is hard to estimate what it is as it varies for each case. For instance in some surface tension modelling I did a few years back I found that to get the Laplacian pressure correct (within about 5%) I needed to keep the aspect ratio under 1.2. So some multiphase models are extremely sensitive to mesh quality. The cavitation model is unlikely to be that sensitive, but I guarantee it will run better and converge easier if you significantly improve the mesh.

[Johan M]

Originally Posted by ghorrocks

The 1000 in the manual is for single phase flows. You have a very numerically unstable multiphase flow, so your recommendation will be more strict than that. It is hard to estimate what it is as it varies for each case. For instance in some surface tension modelling I did a few years back I found that to get the Laplacian pressure correct (within about 5%) I needed to keep the aspect ratio under 1.2. So some multiphase models are extremely sensitive to mesh quality. The cavitation model is unlikely to be that sensitive, but I guarantee it will run better and converge easier if you significantly improve the mesh.

Thanks. Currently my cryogenic transient cavitation sim is still experiencing recirculation/ vapor forming in the inlet pipe region. While troubleshooting that scenario, I am running a water analog version of that pump configuration that is transient and has the cavitation model enabled (all the transient settings are retained).

After 360 degrees of rotation, my inlet mass flow rate is roughly coming close to my nominal 7.4 kg/s flow rate. I would like to know if it is correct to expect sort of a fluctuation in my monitors of mass flowrate/ discharge pressure that lines up with my vane pass frequency? Currently I have not quite yet observed these patterns in my monitors (I have 7 blades)>

Kind regards,
Johan

[ghorrocks]

Whether you see the vane passing frequency in your output depends on what type of stage transformation model you are using, how you are modeling it, what you are modelling and many other factors.

But in general, yes, you would expect to see the blade passing frequency in the mass flow. I suspect your case has not run long enough to settle down to a periodic steady state yet, so I think more simulation time is required.