Poor residual performance/convergence problems?
 

Hi all,

I'm running some Fluent simulations on a centrifugal pump I've designed. I've added some images of the pump design for completeness, as it's somewhat unconventional. For context, the impeller has a 64mm diameter and spins ~30,000 rpm, so the flow mechanics are probably somewhat complicated.

I've been running the simulations as steady state, and I am not overly happy with the residual performance. From what I've seen, residuals vary from case to case. Some sources suggest 10^-4 is loosely converged, and others suggest achieving 10^-3 can be a challenge. My residuals tend to fall just short of 10^-3, although the continuity from the attached image did not even reach 10^-2 (I'm looking to see the impacts of reducing blade number on performance, so this simulation had less blades).
I've been using monitoring points to assess convergence, as attached, and they consistently converge. I've also been looking at mass flow flux between inlet and outlet, and this simulation had 6e-6, which seems reasonable to me?

Boundary conditions are pressure inlet and mass flow outlet, both of which are appropriate for pump CFD.

As far as I am aware, the mesh quality is good. Orthogonality and skewness are more than acceptable as per metrics I found online, and 95% y+<1. Reducing mesh size seems to make convergence worse.
The simulations are run with k-w SST turbulence model using the coupled solver, with turbulence kinetic energy and specific dissipation rate relaxation factors set to 0.5, as I've read that can help convergence.

I've read that poor steady state convergence could indicate transient flow, but I am struggling with setting up and running a transient simulation.


My question is how much should I be concerned about the residual performance, and is there anything I can try to improve it?
Is it simply a case of complex flow mechanics making them poor, or am I approaching it wrong?


Thanks in advance for any replies, should you need any information please let me know.
Robbie

p.s. I've attached a CAD image and an image from an older simulation so you can see the flow mechanics in the pump, if it is any help. Flow essentially gets trapped in a vortex, and some is bled off and expanded.

I suggest you have a look at the definition of residuals in Fluent (https://www.afs.enea.it/project/nept...ug/node812.htm). In my opinion, the behaviour you get in your residuals is fine, and not particularly critical.
Because Fluent scales the continuity and momentum residuals in a particular way, I always double check the convergence with the monitors, as you correctly do as well.
My personal rule of thumb is that the energy should be below 1e-7 and the velocities 1e-4, while for the continuity I would just see if it is diverging or not. Moreover, the scaled residuals plotted by default by Fluent are averaged over all the domain, and for the continuity an average scaled residual of 0.1 tells you that your continuity has improved 10% with respect to the situation at the 5th iteration (which is also normal since you are setting the mass flow rate).
Regarding the monitors, I suggest you to enlarge the plot to see if there are fluctuations in the static pressures. If so, you should switch to unsteady solver (or at least pseudo-transient).
Two more things:
- monitor some volume-average quantities as well
- you should always try to set the static pressure at the outlet, not the mass flow rate. Hence, after the simulation is converged switch BCs to pressure-outlet and set the desired target mass flow rate. You should not see differences.

Probably you get poor residual convergence because of that separation zone I see downstream of the rotor, in that sort of pipe.

Very useful, thanks for that.


After having talked to some highly experienced CFD engineers, they agreed that as the mesh, boundary conditions, and monitor convergence is acceptable, the reason that the residuals don't decrease much is because it is likely a transient simulation. They also agreed with you in that the residual performance is not of particular concern. I will likely attempt a transient simulation.


Can I ask you to possibly expand on why I should monitor volume-average quantities, and what type of quantities these are? It seems there are many different ways to monitor values, and it is somewhat overwhelming.

From the contours you attached I can see flow separation, vortices and expansion in the outlet pipe. I do not know the Reynolds number of your operating point, but switching to unsteady simulation (e.g. URANS) might be a good next step.

For steady-state simulations, I suggest you to monitor volume-averaged turbulent kinetic energy and static pressure (i.e. average in your control volume): this is because if the flow is converged, your volume averages should be constant, without any fluctuation, because of the energy conservation in your control volume. If there are fluctuations in your monitored quantities at the boundaries, as I said this may be due to the transient nature of your flow. In this case, volume averages are still a good indication of convergence since they are less sensible to these fluctuations at the boundaries. Nonetheless, you should always monitor quantities at the boundaries as well, especially for transient flows.