[Julian121]

I am solving a problem with two boundary conditions:

First setup:
Reference pressure: 0
Inlet total pressure: 100135 Pa
Inlet total temperature: 288.5 K
Outlet mass flow: 0.05 kg/s

Second setup:
Reference pressure: 100000 Pa
Inlet total pressure: 135 Pa
Inlet total temperature: 288.5 K
Outlet mass flow: 0.05 kg/s

For the first case that I set the reference pressure to zero, mass residuals decrease below 1e-6 (image1), whereas when I set the reference pressure to 100000 Pa the mass residuals hardly reach 1e-5.
Why does this happen?
Shouldn’t they produce the same convergence plots?

[ghorrocks]

The mass residuals are not important when the momentum residuals have not achieved 1E-4 yet. It is the worst equation which is important. I regard both simulations as poorly converged and would not consider one better than the other.

The second setup has the reference pressure set properly and will normally converge better because of it. Of course there are always exceptions, but they are unusual.

[Julian121]

Does this type of oscillation of mass flow and pressure ratio show a transient behavior?

[Opaque]

When you observed convergence dependence on the reference pressure,
were you running in single or double precision?

[Julian121]

Originally Posted by Opaque

When you observed convergence dependence on the reference pressure,
were you running in single or double precision?

I was running in single precision.

[Opaque]

Try double precision, there should not be that much difference between reference pressure > 0, and the double precision run with either value of reference pressure.

[ghorrocks]

Some simulations are sensitive to reference pressure, even when running double precision. Double precision just gives you more margin from numerical precision problems, it does not eliminate them.

Having said that, this question appears to be a routine single phase, incompressible simulation. In that case Opaque's comment is probably correct

[Julian121]

It seems that running double precision does not change convergence dependence on the reference pressure for my case.

Surprisingly, the imbalances of the zero reference pressure is of the order of 0.0001, whereas the 100000 pa setup has the imbalances of the order of 0.01!

I have stopped the transient simulation after four full turns since no steady in mean (periodic pattern) was developed. That setup was using 100,000 Pa as the reference pressure.

Do you think using zero reference pressure will change transient simulation solution?

[Gert-Jan]

In my opinion, CFX is just trying to tell you that it cannot find a fully stable solution. Probably there are instabilities resulting in a fluctuating solution. You can try reducing of increasing the timestep. But it is likely that this is what it is.
Alternatively run a transient case and determine an average solution and determine the standard deviation as well to determine where the fluctuations originate.

[Julian121]

According to the experimental data, there should be a stable solution for this mass flow. I don’t know how I can justify it if no stable solution is found this time.

My new transient run based on the zero reference pressure, instead of 100000 pa, is in progress now but I am not certain that a periodic pattern is developed this time.

For the passing period selection, I have selected rotor domain as the domain for time steps calculation. In the time transformation method for a transient rotor-stator tutorial the passing period is based on the stator rather than rotor. Is it correct? Shouldn’t it be based on the rotor?

To assess the convergence of the transient simulation, I have defined a statistical monitor which computes arithmetic average of the pressure ratio and other expressions. Should the averaging be done over completed interval or running interval? Am I doing it right?

Originally Posted by Gert-Jan

In my opinion, CFX is just trying to tell you that it cannot find a fully stable solution.

Can it be a sign of stall/surge?

[Julian121]

For a TRS simulation with profile transformation when there exist several domains, should the passing period be calculated as the longest passing period of all the domains?

I have used just the rotor domain to calculate the passing period but I am not sure this is the correct way.

[Opaque]

The selection of the period will allow an easy calculation of the timestep by the software. It also allows that after an integer number of timesteps the start of the next period is recovered.

The accuracy of the solution (discrete values obtained from the algebraic equations) is a function of the timestep size (and spatial mesh), but not of what period was selected to control the simulation.

Have you been able to simulate a simplified version of your model? Say only two components: stator/IGV and a rotor with no cavities or add-ons?

[Julian121]

Originally Posted by Opaque

The selection of the period will allow an easy calculation of the timestep by the software. It also allows that after an integer number of timesteps the start of the next period is recovered.

The accuracy of the solution (discrete values obtained from the algebraic equations) is a function of the timestep size (and spatial mesh), but not of what period was selected to control the simulation.

Have you been able to simulate a simplified version of your model? Say only two components: stator/IGV and a rotor with no cavities or add-ons?

For a simplified model including IGV/Rotor/Stator I can obtain a steady state solution easily and the residuals reduce very smoothly up to 1e-5.

After I add the CT (cavity), the problem arises.

I have checked the CT mesh many times but no steady solution is possible.

As you know I have been trying to run a transient simulation but no periodic pattern has been devloped so far.

Shall I run a transient simulation for the simplified model?

[Opaque]

Great.. You got a working baseline model.

Can you estimate the mass flow coming through the cavity into the other component (rotor?)? If you can, I would not add the cavity yet, but set an inlet boundary condition with such mass flow and the proper incoming direction.

You can now study this enhanced model and see if it works/converge without issues. This will separate if the problem is the cavity itself, or the new flow injection causing the problems.

[Julian121]

I was going to use the injected mass flow from the cavity to the rotor as the inlet boundary condition like you said, but I found out that the mass flow rate is of the order of 1e-5!

I measured it on the both sides of the interface but it is almost the same.

The streamlines show that the flow goes inside the cavity, but it is not clear why it is very low.

I checked the other operating points and they had almost the same mass flow.

The mass flow I am using at the outlet is 1.5/37 kg/s (37 is the number of stator blades).

[ghorrocks]

You are calculating the mass flow over the whole interface. There is flow going in and flow going out and it cancels out to give almost zero - hence your 1e-5 mass flow number. This number is useful in working out the imbalances in your flow (ie accuracy), but it is not what Opaque suggested. massflowAbs might be more useful.

You are going to get a separation off the front edge of this cavity and that is likely to be transient. This is going to cause convergence difficulties. So it does not surprise me that this feature makes convergence harder.

[Julian121]

I used a higher viscous fluid (100 times air viscosity) and the difficulties with convergence disappeared in the cavity!

Does it not show that the problem is not the cavity itself, but rather transient flow prevents obtaining a steady state solution?

OK as it seems that flow separation inside the cavity has transient behaviour, I used larger physical time scale and coarse mesh inside the cavity but they did not help.

I have tested 0.1/omega to 100/omega. Should I use larger than that?

I have tested mesh of the order of 200000 to 500000 nodes. Is it coarse enough?

If the reason I am not getting converged solution is transient flow behaviour, why I cannot obtain a converged solution with transient simulation?

[ghorrocks]

I used a higher viscous fluid (100 times air viscosity) and the difficulties with convergence disappeared in the cavity!

Yes, that is as expected. High viscosity equals low Reynolds number which means more stable and more likely to be steady state flows. This is basic fluid mechanics.

For tips on convergence see the FAQ: https://www.cfd-online.com/Wiki/Ansy...gence_criteria

If you say you have tried everything then you have to accept the final paragraph on the FAQ - your simulation is transient and the only way forwards is a transient simulation.

If you are not getting convergence with a transient flow then your time step is too large. Make it smaller. Even better, use adaptive time stepping to find the time step for you, homing in on 3-5 coeff loops per iteration. Make sure the first iteration size and minimum time step is low enough you never hit it.

Is your mesh fine enough? Do a mesh sensitivity study and work it out.

[Julian121]

I forgot to tell you that the compressor I am modelling is a subsonic compressor and Mach number is 0.3 at the tip at most.

While flow should be incompressible, I am using a variable density fluid (air ideal gas as material in CFX).

In addition, I am modelling heat transfer with total energy and viscous heating included.

Aren’t they the reasons why the transient simulation is not getting converged?

I have tested a constant density fluid such as Air 25 in steady state, but it did not help in convergence.

[ghorrocks]

Make sure you understand the key non-dimensional numbers and what they mean.

Reynolds number is the ratio of the inertial forces to viscous forces. In other words how much dissipation compared to the flow speed. This is the parameter which shows how stable/unstable it is.

Mach number is the speed of the flow over the speed of sound. It determines how significant compressible effects are, and whether compressible flow features like shock waves are present.

Incompressible flow or compressible flow does not matter for Reynolds number. Likewise heat transfer, total energy and viscous heating. None of them are the fundamental parameter for flow stability, Reynolds number is.

Why do you have compressible flow activated if the flow is not that fast?

Why do you have a heat transfer model running? Do you need the temperature for something or is it just because you are using a compressible fluid?

Why do you have viscous heating activated? It appears highly unlikely this is significant, so don't waste computer power in calculating it.

It is unusual (but not impossible) for compressible flows to converge better than incompressible flows. Normal practice is to use the simplest simulation which includes all the physics you need, so I would suggest you use an incompressible fluid, no heat transfer (unless you need the thermal field) and no viscous heating. Your simulation will be significantly faster like this and possibly more stable. I realise this contradicts advice from other posts.