[Julian121]

Dear Glenn

Thank you very much for your wonderful explanation.

The reason why I activated heat transfer was that I needed the temperature at outlet to calculate isentropic efficiency. If I do not activate heat transfer, can I calculate enthalpy or temperature?

It is always said that compressibility effects can be neglected if flow Mach number is less than 0.3 is a simplification. So, for this reason and the reason that I was not sure if Mach number exceeds slightly more than 0.3 I chose a compressible fluid.

In CFX-Post how can I evaluate viscous heating?

So, I think I should change the physics to an incompressible fluid such as Air 25 and None as the heat transfer. Right?

Is it necessary to start a new transient simulation from the beginning?

I think I should solve a new steady case with these changes in effect which will be used as initial condition for the transient run.

[Julian121]

Following the recommendation in the post #20, I have started a new transient simulation with the following changes:

Flow is modelled as incompressible

No heat transfer is modelled

Viscous heating is not included

The number of timesteps have been increased to 70 per a passing period

The pressure ratio signal has significantly changed compared to the previous setup where flow was modelled as compressible and heat transfer and viscous heating were included.

There are significant fluctuations in pressure ratio and mass flow etc.

Is there anything wrong with this simulation?

I am using zero reference pressure due to my previous experience with compressible flow that mass flow residuals did not drop.

When flow is modelled as incompressible, should a reference pressure be set?

[ghorrocks]

If you want enthalpy of isentropic efficiency then you need to model heat transfer.

How evaluate viscous heating? A sensitivity analysis like everything else. Do a run with it on and off and see whether the difference is significant.

Please stop guessing what the time step should be. Either do a sensitivity analysis to work it out properly, or use adaptive time stepping, homing in on 3-5 coeff loops per iteration. I bet your time step size is way too big, so your results are massively inaccurate and analysing these inaccurate results is utterly pointless.

[Julian121]

Can efficiency be calculated from torque without the need to model heat transfer?

I understand that the proper timestep should be obtained from a sensitivity analysis, but what makes me worried is that why pressure ratio signals have been changed from compressible to incompressible analysis.

Please note how smooth is the pressure ratio signal with compressible analysis.

Currently, I am using SST model with very fine mesh near the boundaries.

If I use k-e or k-w models, will the transient simulation converge sooner?

[ghorrocks]

I understand that the proper timestep should be obtained from a sensitivity analysis, but what makes me worried is that why pressure ratio signals have been changed from compressible to incompressible analysis.

Let me restate my previous post: "I bet your time step size is way too big, so your results are massively inaccurate and analysing these inaccurate results is utterly pointless."

The different turbulence models you list are unlikely to make any difference on convergence rate. They are all similar.

[Julian121]

Originally Posted by ghorrocks

Let me restate my previous post: "I bet your time step size is way too big, so your results are massively inaccurate and analysing these inaccurate results is utterly pointless."

Ok, what would you do at this stage? Start a new transient simulation with smaller timestep or reduce the current timestep now and restart the simulation?

Shall I wait until a full turn is reached before changing the timestep?

The image shows the pressure ratio and the average over a period has been superimposed on it.

[ghorrocks]

Again, my previous post suggested what to do:

Either do a sensitivity analysis to work it out properly, or use adaptive time stepping, homing in on 3-5 coeff loops per iteration.

You will find the adaptive time stepping method will be much quicker and easier.

[Julian121]

Just to confirm my understanding is correct, a transient rotor stator interface is placed between rotating and stationary domains, when there exists unequal pitch ratio. Is it correct?

So, a TRS interface should not be used between two stationary components such as Inlet/IGV and Stator/Outlet?

I have been using the following TRS interfaces, but I am not sure they are the correct way of doing it:

Inlet/IGV: general

IGV/Rotor: TRS (profile transformation)

Rotor/Stator: TRS (profile transformation)

Rotor/CT: TRS (profile transformation)

Stator/Outlet: mixing plane

Please do correct me if I am wrong.

[Julian121]

Dear Glenn,

Could you please explain?

I'm confused!

[Opaque]

The "transient rotor stator" interface should be used whenever there is a relative motion between the sides of the interface.

I wonder the following:

is there is a pitch change between Inlet/IGV interface?

why a mixing plane between the Stator/Outlet interface? is there any kind of motion between either side that requires mixing?

is there relative motion between CT/Rotor? is there a pitch change here as well?

[Julian121]

Originally Posted by Opaque

is there is a pitch change between Inlet/IGV interface?

No, there is not. So, I have used a general connection.

Originally Posted by Opaque

why a mixing plane between the Stator/Outlet interface? is there any kind of motion between either side that requires mixing?

There is no motion. I made a mistake here.
Do you think it will cause convergence problems such as not getting convergence in transient simulation?

Originally Posted by Opaque

is there relative motion between CT/Rotor? is there a pitch change here as well?

Yes, the CT domain is stationary and there is pitch change between CT/Rotor.

I have not activated "Alternate Rotation Model". Does it affect the results in an axial compressor?

[ghorrocks]

Regarding Alternate Rotation Model - Recall the reference pressure removes the absolute pressure component and makes the relative pressure a smaller number which is more accurately captured by a floating point number with limited accuracy.

Likewise the alternate rotation model models some velocity components in the absolute frame rather than the rotating frame. You want to choose the default model if the flow is more-or-less rotating with the frame, you want to choose the alternate rotation model if the flow is more-or-less with the absolute frame. If you do this the velocity component magnitudes are reduced and you get better numerical accuracy.

So, for example, you would model a centifugal pump with the default model as the flow is roughly rotating with the frame rotation. But if you were modelling a wind turbine where the air pretty much just goes straight through then the alternate rotation model is better.

[Julian121]

Originally Posted by ghorrocks

Again, my previous post suggested what to do:

You will find the adaptive time stepping method will be much quicker and easier.

Following Glenn’s advice, I have started a new transient simulation with adaptive time stepping.

Now, CFX is using much smaller time steps than the transient blade row analysis.

Although the simulation is much slower, the courant number has been reduced significantly.

It has passed just 0.5 pitches so far but I think it will take many days to reach a full turn.

Is it necessary to reach a full turn to judge about the convergence?

Isn’t it better than my previous results?

[Opaque]

It depends on which frequencies are involved. If the signal happens once in a revolution (turn), there is no way the software will predict the result before a turn is modeled, agree?

Since the model is non-linear, and the software iterates to convergence, will a single turn be enough to converge with so little information about the full turn information? I will leave this one with you.

[Julian121]

Of course, no information about a full turn can be deduced from just one pitch rotation.

If I only need to predict the performance (let's say no frequency prediction is necessary at this stage), will I still need to reach many turns?

As you may know, I tried to obtain convergence with a constant time step first.

Since no repeating pattern was developed after 5 full turns, I decided to try the adaptive time stepping.

What would you do for such a case? continue the current simulation with adaptive time stepping which is much slower or continue the previous simulation which did not produce a repeating pattern after 5 full turns?

[ghorrocks]

Of course, no information about a full turn can be deduced from just one pitch rotation.

Why do you say that? If the time constant of the device is very fast that is entirely possible.

If you want a time-resolved of your device then you have to use the very fine time steps suggested by adaptive time stepping. If you use anything coarser then your results will be inaccurate.

[Julian121]

Originally Posted by ghorrocks

Why do you say that? If the time constant of the device is very fast that is entirely possible.

If you want a time-resolved of your device then you have to use the very fine time steps suggested by adaptive time stepping. If you use anything coarser then your results will be inaccurate.

Based on the mass flow signal, isn't the solution converged?

The amplitudes of the fluctuations are almost the same and the mass flow has repeating pattern.

[ghorrocks]

Yes, the last 5 or so cycles from around time step 400 hardly change, so it looks like you have reached a periodic steady state. It also says that you need about 500 time steps, which is about 9 fluctuations, to achieve it.

You are correct, from this you know about how long it will take to achieve periodic steady state.

[Julian121]

Does having very fine mesh near wall boundaries affect the time step selection by adaptive time stepping?

The mass flow changed significantly after I was thinking it was converged , but the vertical axis is still of the order of 2.396!

Given that the experimental data for this operating point shows that the mass flow should be 2.49 kg/s and the difference between them is minimal, do you think I should run it longer?

[Julian121]

Isn’t adaptive time step algorithm supposed to adjust the time step during a run?

I am not sure why CFX uses very fine time steps such as 4e-7 since the start.

It has decreased since the initial value but it has not increased at all.

Could someone please check my adaptive time step settings?