CFD of a Centrifugal Compressor
Hello, thanks for the screens.
Now the situation is more clear. Please let me know how many blades you have in the compressor.
The convergence plot looks like you have applied too low steps between the blade's exchange position.
More or less the condition inside the fluid depends on the blade position and they are repeatable, so in a fully "convergence" flow if you have 12 blades after every 30 degrees of rotation we should get the same value in every place. Our goal is connected to dividing that 30 degrees by the number of steps to properly catch the change which appears during the path. In the case upper if you apply 3 degrees per time step the blade replacement will be simulated in 10 iterations.
In that case, I could propose to run:
- Run the simulation for 200 iterations and set the time step to blade equal to 1( that will allow you more or less compute the initial condition in a relatively quick time with the frozen rotor)
- Continue the simulation and apply the time step value to have 10-20 time steps per blade replacement
- Run the simulation for 5 rotations of the rotor.
After that, you will also need to compute the average value on the inlet and outlet to get proper results, in the solve go to the save intervals and save the summary every 1 iteration.
If you get stable results we could start fighting with the most powerful software called MS Excel to get average values on the inlet/outlet.
Best regards,
Karol
To be honest I rather expected different results.
Pressure should look in the last steps more like that.
Please let me know if you apply uniform mesh in the rotating region and refine the mesh near the blades. You could also attach the simulation, I will look into the settings.
The temperature is in constant because software by default does not compute the thermal gas expansion. So the pressure does not have an influence on the density and temperature. the compressible flow also does not have that possibility, so we could try to do it with the subsonic flow but I am not able to guarantee that we will get the proper results.
BR
Karol
Ok, I tested a few additional mesh settings and calculation settings. In this post, I will also make a quick summary to defend my proposition of the of solution.
To properly solve the compressor simulation we need to have the possibility to catch the thermal gas expansion to determine the density difference between the inlet and outlet. Autodesk CFD is able to catch it only in subsonic simulation.
From the second side, we need to use a rotating region with a small degree time step to catch changing position of a blade and frequency of the compression(that pressure plot a few posts above). The field at the end of the simulation should have a repeatable value and should depend on the position of the blade.
When I try to solve the simulation with moving blades and subsonic flow, every time I get extremely high velocity neat the wall layer which later in a few iterations filled the entire domain and software crashes. Reducing the wall layer size, increasing the amount of it, decreasing the time step, and changing boundary conditions do not solve the issue.
With that, we could try to solve the simulation in the approach which I proposed at the beginning with a steps solution with a quasi-steady-state at the beginning and later decreasing the time step and compressible flow, but that will not change the density of the fluid properly or just compute the quasi-steady state solution with the subsonic flow.
I personally think that the second option is better. Even if we do not have to catch the change in time, we cover the physics behind the process correctly.
So long story short, stop the simulation on the first step( number of blades 1) and run the simulation for 600 iterations.
The results should look like that.
Probably we will be not able to get something better.
BR
Karol
