Pressure ratio calculation in a transient run
 

I am doing a transient simulation of a compressor to evaluate the pressure ratio.
How should pressure ratio be calculated in a transient run?
For example, I am running for 5 passing periods and each one has 100 time steps.
Should it be calculated as the arithmetic average of pressure ratio in each of 100 time steps or it should be evaluated at the end of each passing periods?

Evaluating the pressure ration at the end of a passing period will only give you the instantaneous pressure ratio, which I am not sure what use it has.

However, you can compute a running average using the same number of timesteps per passing period if the time average (based on such period) if of interest to you. By doing a running average, there is no influence on when the period starts/finish, and the value should steadily converge to a single number as the simulation progresses.

I have two more questions:

First: is the running pressure ratio different than the actual pressure ratio?
Should the running pressure ratio ultimately reach the actual pressure ratio developed by the compressor?

Second: I have written an expression (massFlowAve(Total Pressure)@Outlet / massFlowAve(Total Pressure)@Inlet) which computes the pressure ratio in a steady run. Does this give me the true running pressure ratio in a transient run or I should use “Trn Stats”?

I can only suggest how to evaluate a given calculation, i.e. how to realize a formula using ANSYS CFX expression language. However, I cannot advise on the meaning or significance of what you are trying to evaluate since that it is up to you.

The software will evaluate what it is told to do.

Here is a list of questions that may help you

What are you trying to achieve with such a calculation?

What is the physical interpretation of the pressure ratio? or where does the formula come from?

If you were in the laboratory with the machine, can you measure the pressure ratio directly or indirectly?

Many of those quantities are meant for steady state interpretations; therefore, for unsteady calculations, they must be revisited based on significance, or ability to measure in the laboratory (directly or indirectly).

Hope the above helps you

When transient simulation is initialized by a partially converged steady state result file of another operating point, which one of the initialization options should be used?
Does the continue history from need to be checked?

Not sure what the options are right now, but Continue History From basically just adds the time steps of your new simulation to the ones you already had. So if your first run went to 1000 steps, the new run will start with 1001. I'm not sure if this is actually valid when using steady state as initialization because time and timestep are not available in this content.



You won't need Continue History From.

I can choose between automatic or cached solution data or current solution data or initial conditions. Which one should be used? Does it matter at all?

I think I got what you meant by running average pressure ratio. Please correct me if I am wrong.

I set transient statistics in CFX-Pre, which compute arithmetic average of total pressure, pressure etc over passing period.

Then, if I want to monitor the running average pressure ratio during a run, I use the following expression:

massFlowAve(Total Pressure.Trnavg)@Outlet / massFlowAve(Total Pressure)@Inlet

Here, I did not use transient average pressure at inlet since it has already been defined as boundary condition.

After the convergence, the pressure ratio should not be changed. Right?

Not exactly.

The time average of Total Pressure/Pressure should reach a steady value if the solution converges. However, the mass flow used in the massFlow(..) function is the mass flow at a given time instance; therefore, the quantity still has instantaneous contributions.

What pressure ratio are you interested in?

1 - Time average pressure ratio between inlet and outlet?

Time average of massFlowAve(Total Pressure)@Outlet /
Time average of massFlowAve(Total Pressure)@Inlet

2 - The pressure ration between the time average pressure at inlet and outlet?

massFlowAve(Time average of Total Pressure)@Outlet /
massFlowAve(Time average of Total Pressure)@Inlet

I have used "Time average of" as an operation on a variable. The formulations above are different and only (1) can become steady in a transient periodic. Of course, the time average window must match the period of interest.

Hope the above helps,

All I need is to evaluate pressure ratio for different configurations of a compressor and casing treatment and then draw a performance map.

I have experimental pressure ratios in the form of total pressure at outlet / total pressure at inlet and static pressure at outlet / total pressure at inlet for those configurations.

What formulation would you think is suitable?

I would think the first formulation is more suitable to the experimental data.

I still have doubts about the meaning of a formulation such as massFlowAve(Total Pressure.Trnavg)@Outlet.

Does this give time averaged total pressure at outlet at the end of passing period?!

Total Pressure.Trnavg

is the time average of Total Pressure within the averaging specified window.

What is your time averaging window? and how did you specify it?

Are you running Transient analysis mode, or Transient Blade Row analysis mode? Are you using a transient blade row pitch transformation model of some kind?

I am using transient blade row with profile transformation since I am simulating a segment of full annulus.

The time averaging window is assumed as the passing period of the rotor.

I specified it in output frequency as equal to the passing period of the rotor.

Am I doing the averaging correctly over the time interval required to complete 1 pitch?

“Trn stats” does not ask for time averaging window, but I assume that it uses the time interval I specify in “Trn Results”.

Shouldn’t Total Pressure.Trnavg calculate time average of total pressure over the time interval specified in “Trn Results”?

If massFlow(..) function is the mass flow at a given time instance, how can I compute pressure at a given boundary?

Is the following formulation correct?

Time average of Pressure.Trnavg@Outlet

As far as I know, the solver can compute a monitor point via expression, say

Expression Value = massFlowAve(whatever you want)@Locator 1/
massFlowAve(else)@Locator 2

You can activate the Monitor Statistics functionality, and use the averaging you need.

Similarly, you can monitor such expression in ANSYS CFX SolverManager, and create additional statistics (right click on the monitor plots and see options)

Thank you Opaque. I managed to calculate the average of pressure ratio over a passing period by setting a derived variable.

I have run the simulation for about 400 time steps (20 passing period). Each time step has 5 coefficient loops.

After 400 time steps, no periodic pattern is seen in the pressure ratio and other parameters. Does it indicate that the setup has a problem or I must run more iterations?

I have kept the IGV/Rotor and the Rotor/Stator interfaces as mixing-plane and have changed the Casing Treatment/Rotor interface to transient rotor-stator. It is not clear for me whether I should change them to TRS or not. Could you please explain?

Using mixing plane, you will never get the transient interaction between the IGV and the rotor.

If you do not get a periodic solution, your setup is not complete yet.

Be aware that for transient your reduced setup must account for the pitch change between the different rows in the machine unless you are running with the appropriate number of passages per row.

I have changed those two interfaces to the TRS as well.

This time I am using 10 time steps per a passing period.

After about 7 passing periods, although the pressure ratio changed a little bit, there is no periodic pattern.

I have noticed some information about “Non-overlap area” is reported in CFX-Solver.

Shall I continue this run or there is a problem with the setup?

The CT-Rotor domain interface non-overlap on side 2 seems large.

Is the computed pitch on either side correct? Perhaps post the CCL for this specific domain interface?

The other two domain interfaces seem to be set up correctly.

Yes, the pitch ratio is correct. I am modelling 1 rotor blade out of 38 and 3 CT vanes out of 120.

Should I rotate one of these domains to reduce the non-overlap area? They do not match.

Maybe this is the reason why I was unable to reach convergence in steady solutions.

You are specifying the pitch angles on both sides of every rotor-stator interface, correct? Therefore, I assume you had problems with those interfaces and you are forcing the pitch, correct?

If you run with Pitch Angle/Option = Automatic only for the CT to Rotor interface, what kind of result are you getting? Same non-overlap issue?

Or more radical approach (assuming the machine can work w/o the CT component) is to remove the CT from the model, and run with a wall on that part of the rotor domain. Does the model behave sensibly?