[Julian121]

I have created isovolumes of the maximum momentum residuals in cfd post. The red color corresponds to the maximum momentum residuals. The blue color shows the location of elements with face angle less than 18 degress. The locations of high residuals are close to the prism layers I have created for the vanes inside the casing treatment and the left wall.
I am smiulating several configurations of casing treatments and I need to obtain pressure rise developed for each configuration. However, the pressure ratio does not converge.
I have created vector plots on two planes where the maximum residuals are and it seems that flow seperation occurs in these locations.
Is the problem of convergence mesh related or it is due to flow seperation or reattachment that take place in these locations?
Is there any way to converge the pressure rise?
I have tried transient simulations but they take too long to converge and cannot be used for many configurations.
This operating point is close to the stall point.

[Opaque]

May I ask what timestep you are using for the simulation?

Auto Timescale ? Timescale Factor?

[Julian121]

I am using physical timestep of 1/omega which is 0.003183 for my case.

I have no difficulty in obtainging converged solution near to the design point.

Originally Posted by Opaque

May I ask what timestep you are using for the simulation?

Auto Timescale ? Timescale Factor?

[Opaque]

what is the sensitivity to use 0.1/omega ?

It seems the continuity equation is having some issues, and the linear solver is working too hard (10+ work units) per iteration. Symptom the timestep is larger than it should.

[ghorrocks]

It is normal for the design point of a pump to converge nicely, but as you approach stall convergence gets much harder.

Some ideas:
* You need to make sure your numerical stability is as good as possible. Use small time steps (at least as you approach convergence), double precision numerics and improve mesh quality will all help.
* You have a small separation on the leading edge and your problem is because these separations are often unstable and probably transient.
* If you refine the mesh you will resolve the separation better, but the convergence problems will get worse.
* If you want this simulation to converge fully you probably will need to run transient. If run time is unacceptable then you need to get more computer resources.
* Do not cut corners because run time is too long. If you cripple the simulation just so it converges it will be horribly inaccurate, and then what is the point of doing it? If you are going to model these conditions then do it properly, and if the run time is unacceptable then say that this region could not be done as you don't have sufficient resources to model it properly.
* The FAQ has some further tips: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

[Julian121]

Originally Posted by Opaque

what is the sensitivity to use 0.1/omega ?

It seems the continuity equation is having some issues, and the linear solver is working too hard (10+ work units) per iteration. Symptom the timestep is larger than it should.

The outlet pressure changed a bit but still no convergence was obtained. The locations of maximum residuals changed this time.
I have defined the casing treatment domain as stationary. Is it correct? For the the interface between the casing treatment and the rotor, as Turbogrid does not allow to assign two parts to the shroud (one for the casing treatment and one counter rotating wall), I have defined an interface between the casing treatment and the whole rotor shroud. Can this cause the convergence problem?
In addition to the physical time step 0.1/omega, I tried local timescale factor 5. This time the maximum residuals decreased up to 10e-3 but again after 500 time steps no convergence was obtained. It seems local timescale is more successful in terms of reducing the maximum residuals.

[ghorrocks]

I trust you will not ignore my previous post on this thread. We have seen this question a lot on the forum so I have seen it before.

Casing = stationary, yes this is normally correct.

Inteface - I do not understand what you are saying, please post an image.

Local time scale - yes, this can assist in convergence but it should not be used in the final run to convergence - this is discussed in the FAQ I linked to. Did you read it?

[Julian121]

Originally Posted by ghorrocks

I trust you will not ignore my previous post on this thread. We have seen this question a lot on the forum so I have seen it before.

Casing = stationary, yes this is normally correct.

Inteface - I do not understand what you are saying, please post an image.

Local time scale - yes, this can assist in convergence but it should not be used in the final run to convergence - this is discussed in the FAQ I linked to. Did you read it?

Glenn, I would never ignore your comments. I always read your comments with great attention.
The reason why I was asking again, was that after following FAQ I was not able to obtain convergence.

Finally, after I used time step 0.1/omega along with SST reattachment model, I could obtain convergence close to stall! However, when the reattachment is not selected, no convergence is obtained.

Is it clear why this happens?

[Opaque]

Based on your snapshot, the MAX residuals are still high; therefore, there is a region of the flow where the equations are having difficulty to converge.

It would be good to plot the location of the MAX residual and analyze the flow and mesh quality around that area. There may still be a problem or a hint to why the SST w/o reattachment cannot converge.

SST w reattachment may be more diffusive and allow the equations to converge.

[ghorrocks]

In addition to Opaque's comments:

* I would compare the reattachment model's results, in terms of your output parameters like output torque and see if it affects things. If it has no significant effect then feel free to use it to assist in convergence. If it has an effect then you need to work out whether it is more or less realistic than the default model.
* You should also look at your results and work out if the key output parameters (I presume this is output torque) has converged to an accuracy you are happy with despite the lack of residual convergence.

[Julian121]

I ran a new simulation with a slight change to the geometry of the casing treatment. Even SST with reattachment model did not help this time. So, as you said I tried to find the locations of maximum residuals. Similarly, to my previous simulations, the locations of maximum momentum residuals and the locations of elements with face angle less than 10 degrees are separated. Red color shows the locations of maximum momentum residuals and blue color shows the locations of mesh elements less than 10 degrees.
What else should be checked to assure mesh quality is not making the convergence problem? Aspect ratio is within the accepted values.
Mach number distribution and vector plots on the planes where maximum residuals are show a circular flow motion. Can this cause the problem?
I have used double precision and 0.1/omega timestep but they cannot help either.
The parameter I am mainly interested in to find from the simulations is outlet total pressure since I need to compare the performance among several configurations. The pressure from this simulation however does not converge completely and the predicted pressure is within 101400 to 101460 Pa.

[ghorrocks]

Aspect ratio is within the accepted values.

The "accepted values" you quote are just guidelines, and some simulations have a tighter requirement and some have a looser requirement. If this device is operating near the stall point your requirement is likely to be more stringent than the guidelines so do not assume it is OK.

But when I look at your results I see the isosurface is quite blocky and your contours a little blocky too. This suggests your mesh is coarse and that means you probably have not refined the mesh adequately to get accurate results. So I would try refining the mesh. Note that as you refine the mesh your convergence difficulties will get worse.

and the predicted pressure is within 101400 to 101460 Pa.

Then that variation is tiny and other errors are going to be orders of magnitude larger than that (such as mesh density, mentioned above). If all you are getting is a 60Pa variation out of 101kPa then don't worry about it and assume it is converged. The FAQ I quoted in my first post talks about this.

[Julian121]

I have run a new set of simulations but still no convergence has been possible for three mass flow.
I was looking at the residuals of mass for my domains and I noticed that the mass residuals of the casing treatment have not reduced unlike the other domains. In the screenshot please note that RMS P-Mass in casing treatment is more than the RMS P-Mass of all domains.
Isn’t it the reason why momentum residuals do not reduce to 10e-4?
I have tried very dense mesh with and without prism layers. Although with prism layers there are some elements with bad quality due to the fillets below the vanes, a mesh without prism layers and better quality cannot still help.
The strange thing it that I have no problem in getting convergence for other mass flow such as 2.49, 2,39, 2,29, 2.15, 2.05, 1.55 and 1.43. However, the convergence cannot be obtained for 1.85, 1.75 and 1.65 kg/s.
The variation of the outlet total pressure is about 10 Pa which is small, but I do not understand why convergence issue does not happen for lower mass flow rates such as 1.55 or 1.43 which are closer to the stall point.

[ghorrocks]

Yes, the small area of high residuals is likely to be causing the lack of RMS residual convergence. You should look at the residuals in the post processor and I bet you will find a small region of high residuals, probably associated with a small separation bubble.

Why convergence for 7 different mass flows but not for 3 mass flows? Because this little separation bubble only exists for the 3 poorly converging mass flows. Some flow condition stops it happening when the mass flow is higher or lower.

If this is a separation bubble:
* Increasing mesh density will make convergence worse, not better
* Using a pure tet mesh (no inflation layers) may fix it but will mean you are not resolving the boundary layer very well. This is not a recommended approach.
* Using a larger time step might help.
* Coarsening the mesh locally in the problem ware might help
* But this is really saying that RMS residuals are not a good convergence criteria for you. Consider using convergence on your outlet parameter as a convergence criteria instead.

[Julian121]

The Locations of high residuals are concentrated toward the wall boundaries inside the casing treatment.
Yes, that’s right. The locations of high residuals are small but every time I change physical time step, the locations of high residuals change.
In my case, smaller time steps can help in terms of having smaller fluctuation in the outlet total pressure.
What is the lower limit of physical time step that can be used? Can a physical time step lower than 0.1/omega be used?
I tried local timescale factor 20 and it seemed that it was better in terms of reducing RMS residuals than the physical time step. I stopped the simulation when the residuals were close to the convergence criteria 10e-4, then I changed it to the physical time step 0.1/omega, but they increased suddenly and they did not reduce at all.

[ghorrocks]

Yes, you can use a time step smaller (or bigger) than 1/omega. 1/omega is just a guide, you can adjust it as you like from there. Don't go crazy any use 1e-10 as that will cause numerical problems but as long as you stay within a factor of 1e4 of the recommended time step you should be right.

Local time scale is good to get the residuals down but should not be used for the final run to convergence. Search the forum for the reason why.

Looking at your flow field I am surprised that you are getting a steady result on that at all. There are so many vorticies and recirculations that it appears highly unlikely that would be steady. If this is the case then a transient simulation is required.

[Julian121]

I have been working on this for a while since my supervisor insisted that getting RMS residuals down to 1e-6 is necessary even close to the stall point.
I followed the steps to identify the locations of maximum residuals as I wrote in my previous posts. One thing that was shared between the locations of maximum residuals in my results was that they were adjacent to recirculation or separation areas.
I used large physical time steps as was suggested on cfd-online but the residuals did not reduce below 1e-4. I tried different mesh, turbulence model, double precision and so on.
Then, I was reading CFX modelling guide and I found that mass relaxation may assist in convergence with oscillations in separation and reattachment regions.
I have lowered the mass relaxation gradually and now I can get the convergence up to 1e-5 easily when I use very small value such as 0.01!
However, I am concerned that using mass relaxation may affect the accuracy and using it in CFD result is acceptable at all.
Does anyone have any experience with this parameter?
Should I change it right from beginning? I found that when I use small value from start may change pressure ratio compared to when I lower it gradually from 0.7 0.6 0.5 to 0.01.

[ghorrocks]

Residuals to 1e-6 is very tight. But you might require it, you don't know if you don't check. So do a sensitivity check (compare 1e-4, 1e-5 and 1e-6) and see if you really do need this tight convergence tolerance.

Secondly, obtaining tight convergence close to the stall point is likely to be challenging. It is likely you will need a transient simulation to obtain convergence to this tight criteria.

I do not recommend you adjust the mass relaxation parameter. The default value is appropriate in almost all cases, and adjusting it to very small values can lead to misleadingly low residual values - that is low residuals but it is actually nowhere near convergence.

The recommended approach to get convergence in your case is described in the FAQ: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

[Julian121]

As the problem I am solving has several domains, should the residence time be taken as the maximum value of time over all domains?
According to the photo, should I use 0.130902 [s] as physical time step or the average over all domains should be taken?
Shall I start the run from beginning with this value?

Originally Posted by ghorrocks

Residuals to 1e-6 is very tight. But you might require it, you don't know if you don't check. So do a sensitivity check (compare 1e-4, 1e-5 and 1e-6) and see if you really do need this tight convergence tolerance.

Secondly, obtaining tight convergence close to the stall point is likely to be challenging. It is likely you will need a transient simulation to obtain convergence to this tight criteria.

I do not recommend you adjust the mass relaxation parameter. The default value is appropriate in almost all cases, and adjusting it to very small values can lead to misleadingly low residual values - that is low residuals but it is actually nowhere near convergence.

The recommended approach to get convergence in your case is described in the FAQ: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

[ghorrocks]

Start with the time step derived from the residence time over all domains. But this is just a starting point - if it is converging easily then increase it, if it is having difficulties then decrease it.