[highorder_cfd]

Hi
I am modelling a liquid ring pump (see https://www.youtube.com/watch?v=HCz47991g38).

I am using a homogeneous free surface model with surface tension active, no buoyancy and I am running the simulation as full transient rotor/stator (the first idea was to run a steady state MRF, but after few runs failing and a discussion with a couple of ANSYS technical support guys it came up that it is better to go straight to full transient for this kind of applications as they do not converge as steady state).

I have init the domain volume fraction with a water ring anulus, the tetha component of the velocity field with omega*radius and the pressure with 0.5*omega^2*radius^2*density.

I am using segregated volume fraction (the coupled diverges) and each time step is around 3 degrees)

After a couple of cycles run in transient the water ring start to settle and the simulation makes a bit of sense.

However I have still a problem: in the first few cycles part of the water mass flow rate is carried out outside of the domain by the air, so eventually the water ring inside the pump is thinner then how it should be (lower blades tips are not wetted surfaces) and the values of suctions pressure I get at the inlet are rubbish. (I have even tried to consider a water inlet to compensate this water, but no luck)

The idea would be to run the first 2 or 3 cycles replacing inlet and outlet with walls, to settle the fluid and prevent water coming out (stage 1), and later switch the walls to the proper boundary condition (phase 2). I have tried this but convergence is rubbish and the water mixed with air with no free surface after few cycles.

The second idea would be to use a degassing boundary condition at the outlet, but in this case I could not use the free surface model, I should switch air to dispersed phase and increase the complexity of the model/assuming diameter of bubble etc (FYI at the moment on 14 cores takes around 15 hours to run one cycle....)

Any idea on how to converge this case? Any help would be much appreciated.

Cheers

[ghorrocks]

Am I correct in saying the problem is in setting up the liquid ring at the correct thickness? Are you specifying an initial condition with the ring at the correct thickness and rotating correctly? You should be able to specify it such that it starts in an approximately stable condition.

[highorder_cfd]

Hi Glen, thanks for your reply. Someway yes.
Actually in terms of initial condition I did the best it is possible to do, at least based on my knowledge. As said I have initialised the volume fraction as an anulus with thickness as in the experimental conditions, theta component of the velocity omega*r and pressure 0.5*density*omega^2*r^2. However this is still a kind of approximation of how the inital condition should be. Indeed usually in this kind of pumps the blades rotation axis is eccentric with respect to cylindrical chamber axis. Using the initial condition I have prescribed (with respect to the chamber axis), I saw it takes a couple of cycles to have the flow field settled properly (I think this is mainly due to pressure and velocity distribution approximation). This is why I would like the pump to perform a couple of cycles without loosing water.

Any suggestion will be much appreciated.

Thanks

Originally Posted by ghorrocks

Am I correct in saying the problem is in setting up the liquid ring at the correct thickness? Are you specifying an initial condition with the ring at the correct thickness and rotating correctly? You should be able to specify it such that it starts in an approximately stable condition.

[ghorrocks]

segregated volume fraction (the coupled diverges)

That is a sign that your simulation has numerical instability. When tightly coupled it won't converge, so a looser coupling allows enough slack that it can at least try to converge. You will want to be using coupled VF I suspect.

each time step is around 3 degrees

Your problem is quite likely to simply be too large a time step. Have you done a time step sensitivity study to find what size time step you really need? Where did 3 degrees come from?

[highorder_cfd]

Hi Glenn

I have used a time step of about 3 degrees as I found some suggestion on a research paper for this kind of applications. Actually I have also tried with 2 degrees and 5 degrees (and 10 coefficient loops) and noticed that with more than 3 degrees convergence problems might arise.

However I think your thoughts might be someway right, indeed from the runs I did I can tell you there were convergence issue for around the first 200 time steps (and after that momentum and mass fraction started to converge properly). My understanding is that once the flow starts to be periodic, 3 degrees are fine, but in the startup phase this is not sufficient to get a converged solution in the time steps.

With a time step of 2 degrees I am now trying to increase the number of linear iterations to 20 to see if this can help. I will tell you later if this has worked (this is running right now).
By the way, if I want to improve the solution of each time step in the initial phase of the simulation, apart from further degreasing the time step and increasing the number of coefficient loops, do you think that underelaxation would help? (having a time step of around 1 degree seems too small??). Indeed I have noticed that in the coefficient loops some of the linear systems are failing F.

Thanks

Originally Posted by ghorrocks

That is a sign that your simulation has numerical instability. When tightly coupled it won't converge, so a looser coupling allows enough slack that it can at least try to converge. You will want to be using coupled VF I suspect.



Your problem is quite likely to simply be too large a time step. Have you done a time step sensitivity study to find what size time step you really need? Where did 3 degrees come from?

[ghorrocks]

I am now trying to increase the number of linear iterations to 20

? Do you mean coefficient loops? These are not linear iterations, that is done in the linear solver and very rarely needs changes. The coefficient loops frequently need changing and they are where the non-linear coefficients are updated for the linear solver.

Your comments make me very suspicious that the problem is indeed too large a time step. I recommend you use adaptive time stepping, homing in on 3-5 coeff loops per iteration. Make sure the lower and upper limits on time step are wide enough that it will not hit them.

Also: You have a surface tension model activated. Are you sure that is required? Surface tension models are very expensive numerically (make the required time step much smaller) so unless surface tension effects are actually required I would not model it.

[highorder_cfd]

Yes, I meant coefficient loops (not linear iterations)

Originally Posted by ghorrocks

? Do you mean coefficient loops? These are not linear iterations, that is done in the linear solver and very rarely needs changes. The coefficient loops frequently need changing and they are where the non-linear coefficients are updated for the linear solver.

I am not a big fan of the adaptive time step but I will give it a try, thanks.

I believed it was reasonable to include surface tension (this has been modelled in some research papers I found. However I will try to run without to see if this helps.

I will investigate these points and let you know.
Thanks for your suggestions, I appreciate your support.

Originally Posted by ghorrocks

Your comments make me very suspicious that the problem is indeed too large a time step. I recommend you use adaptive time stepping, homing in on 3-5 coeff loops per iteration. Make sure the lower and upper limits on time step are wide enough that it will not hit them.

Also: You have a surface tension model activated. Are you sure that is required? Surface tension models are very expensive numerically (make the required time step much smaller) so unless surface tension effects are actually required I would not model it.

[ghorrocks]

Yes, adaptive time stepping can create problems. But it is a way of finding the time step size your simulation requires quickly. So you can use it to find the necessary time step size, then you rerun the simulation using fixed time stepping with the time step size the adaptive technique determined.

Or you can find it yourself with a sensitivity study. Both will work fine.

[highorder_cfd]

Glenn, just a doubt. I am not considering any phase change and thermal effect. Do you think is still worth to model a water inlet to compensate the water carried out by the air (in the physical model)? I am just thinking if under my conditions I should expect or not a water volume fraction at the outlet in the numerical model (or if this is just a numerical issue).

[ghorrocks]

I have no experience with this device so cannot say for sure, but I would expect that this machine would create some splashing, droplets and foam; especially if it is operating off the design condition. Capturing these effects will be difficult.

I would certainly start with a simple splash-free model and get that working reliably and accurately before you consider anything like that.

[highorder_cfd]

Glenn, I did some tests and tried with various time steps.
The time period is 0.04s and I have even tried with time steps in the order of 10^-5 and 10^-6s. With very small delta t the simulation fails in the first time steps and coefficient loops (the linear solver fails F). I have even tried to under relax the linear solver solution with factors of 0.9/0.8 but no luck.
With larger time steps, in the order of 10^-4 (a couple of degrees of rotations), the simulation proceed (just some coeffient loop fails but eventually the time steps are solved). However I still have water coming out from the outlet and positive pressure at the inlet (I would expect negative one, as I am running vacuum pump).
Any idea?

Originally Posted by ghorrocks

Yes, adaptive time stepping can create problems. But it is a way of finding the time step size your simulation requires quickly. So you can use it to find the necessary time step size, then you rerun the simulation using fixed time stepping with the time step size the adaptive technique determined.

Or you can find it yourself with a sensitivity study. Both will work fine.

[ghorrocks]

If the solver fails with small time steps it suggests your simulation is numerically unstable. This means it is having a hard time converging and this can lead to all sorts of problems (like what you describe).

So I would look at why your simulation is so unstable. These FAQ give some general comments: http://www.cfd-online.com/Wiki/Ansys...gence_criteria and http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

Please post an image of your mesh, especially any regions of poor quality mesh. Also post your output file.

[highorder_cfd]

Hi Glenn, this is an industrial project, so unfortunately I cannot post any figures here.
However I think I have managed to complete a first run and now the things look converging better with a 2 deg time step and 20 coeff loops per deltaT. The problem was due to the outlet, which because of back flow was partially switched to a wall. Actually I did not change it before, as in this kind of pump, the cylinder outlet duct has a kind of valve preventing the back flow (thus the CFX Outlet was simulating it properly), however by switching to an Opening now after one cycle I get the free surface behaving correctly and a constant water mass flow rate coming out from the outlet (this mass flow rate is more or less how much I expected). After 4 cycles the free surface looks good and simulation pointing in the right direction. The mesh needs to be refined but this is a decent starting point now.

However I still have a major issue. At the inlet I would expect negative pressure (below the atmospheric pressure), as this is a vacuum pump, whereas the pressure I get from the analysis is positive (the modulus is similar to the experimental value I have for the suction pressure).
As boundary conditions I have specified air mass flow rate at the inlet and Opening Pressure at the outlet equal to the atmospheric (therefore for fluid coming out, static pressure = 0 Pa). Is there anything I am missing here with the boundary conditions?
The other possibility would be to specify the (Total) suction pressure at the inlet (that I have from pump tests) and static at the outlet (0 Pa), but I am not sure how the convergence will be with this. And however I would expect simulation giving good results even with mfr at the inlet. Is there something silly I am doing?

[ghorrocks]

So it looks like the outlet boundary was the source of significant numerical instability. But you still need to do a time step sensitivity study to check your time step size is OK. It affects accuracy and simulation stability.

If you are getting positive pressure at the inlet it could be that you are putting too high a flow rate into the thing. Try a lower flow rate. It will have an operating curve of inlet pressure versus flow rate, so you need to model enough points on the operating curve that you can define the curve before you know how the device behaves.