[Red Ember]

Hi to all!
I tried to simulate axial compressor, but got confusing results for static pressure and temperature.
I used total pressure and total temperature at inlet and corrected massflow at exit. Here one can see my results for 4 corrected massflow values: 12.5, 13, 15 and 20 kg/s for the whole machine.
Point №17 (out) means the last stage exit, point №16 (R7) is for the cross-section between rotor wheel and stator wheel in the seventh (last) stage
As I know, the pressure should increase even in the last stator wheel domain, but it tends to decrease and just drop down for higher massflow values.
What is the reason of it? The most curious for me is the case with corrected massflow value about 34 kg/s (about 54 kg/s for non-corrected massflow), but I'm miles away from desired point yet...

Thanks in advance...

[bparrelli]

Originally Posted by Red Ember

Hi to all!
I tried to simulate axial compressor, but got confusing results for static pressure and temperature.
I used total pressure and total temperature at inlet and corrected massflow at exit. Here one can see my results for 4 corrected massflow values: 12.5, 13, 15 and 20 kg/s for the whole machine.
Point №17 (out) means the last stage exit, point №16 (R7) is for the cross-section between rotor wheel and stator wheel in the seventh (last) stage
As I know, the pressure should increase even in the last stator wheel domain, but it tends to decrease and just drop down for higher massflow values.
What is the reason of it? The most curious for me is the case with corrected massflow value about 34 kg/s (about 54 kg/s for non-corrected massflow), but I'm miles away from desired point yet...

Thanks in advance...

A few questions / things to try on your end:

1. What is the gas you are simulating? Air I assume? Also what is your equation of state and turbulence model?
2. What does the incidence angle look like at the leading edge of each blade row (especially the last stage)? Does the flow follow the blades closely or is there separation? The compressor could be in surge, which is difficult to predict with CFD.
3. What type of mass constraint do you have at the exit? There will likely be a lot of swirl after the last stage, so not having an appropriate boundary condition employed at the exit can cause unwanted physics to propagate backward. I normally use "uniform mass flux" if I know there will be swirl at my exit.
4. Have you tried running the compressor over a given compression ratio and seeing what mass flow it predicts? Just as a sanity check?

[Red Ember]

Originally Posted by bparrelli

A few questions / things to try on your end:
...........................................

About my task
I use nominal rating rpm - 12010 rev/min to get two curves: pressure ratio vs massflow and efficiency vs massflow (as on pictures I added above).
I have information about one regime only:
massflow rate about 54 kg/s (that matches corrected massflow about 13,5 kg/s), rotating 12010 rev/min, total pressure and temperature at the inlet - 99kPa and 288K, at the outlet - about 625kPa and 530K.

1. Yes, air real gas with dynamic viscosity and heat capacity depend on temperature
steady state mode, heat transfer model - total energy
turbulence model - SST, high resolution advection scheme
2. As for the surge...
My simulation yielded low massflow, compression rate and efficiency values for 12.5 kg/s corrected mass flow (see pics) and non-physical when corrected mass flow rate is bigger.
I have checked incidence angles as you advised, thanks!
As for corrected massflow 10 kg/s: it’s obvious just too little place at the inlet. I have essential backflows (due to solver log - 31.7% of the faces, 36.0% of the area) at the Inlet.
As for corrected massflow 15 and 20 kg/s: there’s no backflow at inlet, but sufficient vortexes near trailing edge.
Inlet flow direction is default (normal), I hope it’s right, cos there are only fairings before inlet guide vanes. I neglected these fairings cos it should not turn the flow somehow.
3. I add little part of channel to avoid backflows (so I have the point after outlet called "add" on my previous pictures)
4. a) At first time I tried massflow at inlet and static pressure at outlet. I failed in getting desired compression ratio about 6.25.
b) Then I tried to use low static pressure values at the outlet and to increase it gradually.
Static and total pressure values were ok, but inlet pressure reached 150 kPa instead of expected 85 (it hit the value 130 kPa from the first regime).Inlet total pressure behaved in the same way.
c) So finally I turned on total pressure at inlet and corrected massflow at outlet.

[turbo]

Use (Po, To) inlet and p exit.
Do not use mass flow inlet for compressible flow cfd.
Do not rely on the exit corrected mass flow bc, at first.

[Red Ember]

Originally Posted by turbo

Use (Po, To) inlet and p exit.
Do not use mass flow inlet for compressible flow cfd.
Do not rely on the exit corrected mass flow bc, at first.

Turbo, thank you for your answer!
I tried it before. Total pressure at inlet, static pressure at outlet. I started from 200kPa at outlet, then increased it up to 300kPa (I can't find the results, just my notes that claim that outlet parameters were nearly the same, massflow at outlet slightly decreased). Further increase yielded solver fail.

[turbo]

Then, i think something is wrong in either your geometry or operation model.

[Red Ember]

Originally Posted by turbo

Then, i think something is wrong in either your geometry or operation model.

Well, I think it's possible that geometry mistake leads to flow separation and stall.
But why mass corrected flow BC is not good? I read it works well and one can use it to get all machine speedline (instead of combine pressure BC and massflow rate BC at outlet).
May be Tref and Pref are not proper? I left it by default:
Reference Pressure = 1 [atm], Reference Temperature = 288.15 [K]
These values are close to my inlet BC (total pressure = 98.3kPa, total temperature = 288K)
What Tref and Pref values should be?

[turbo]

I think you are mis-reading its definition. What Ansys provides is EXIT corrected mass flow, not the usual inlet corrected flow. To use the BC, you should be sure of what exit Po and To would be before simulation. That is why I do not recommend.

[Red Ember]

Originally Posted by turbo

I think you are mis-reading its definition. What Ansys provides is EXIT corrected mass flow, not the usual inlet corrected flow. To use the BC, you should be sure of what exit Po and To would be before simulation. That is why I do not recommend.

It seems you've confirmed my suspicion... Well, if I propose static pressure and temperature at the outlet, will it help? Or even little mistake is not acceptable? I could get results as initialization and use just massflow at the exit?

[turbo]

You do not need static temperature to be specified at the exit. Only static pressure is required there, which is the physics in reality. Imagine you are testing the compressor now, and how you are going to modulate test flows.

[Red Ember]

Originally Posted by turbo

You do not need static temperature to be specified at the exit. Only static pressure is required there, which is the physics in reality. Imagine you are testing the compressor now, and how you are going to modulate test flows.

No, I didn't mean specified pressure at exit. I meant just to estimate static pressure and temperature approximately for each corrected massflow rate at the exit and use it as reference values. Of course there will be some mistakes. But if I get the results and use it as initial guess for each point of speedline with usual mass flow rate at the exit?

[turbo]

Still you are not with me. If you want to use the exit corrected flow BC, you need (Po, To) total at exit, and they should be normalized by the standard references of 1 atm, 288.15K. But my advice is just to use p-exit BC from the beginning.

[Red Ember]

Originally Posted by turbo

Still you are not with me. If you want to use the exit corrected flow BC, you need (Po, To) total at exit, and they should be normalized by the standard references of 1 atm, 288.15K. But my advice is just to use p-exit BC from the beginning.

I tried to use pressure at exit, but failed.
I don't understand what do you mean by normalizing. Should I do it or is it solver task?
Is it enough just to set these values (that correspond outlet values that I assume, not default ones)?
Corrected Mass Flow Rate = 10 [kg s^-1]
Reference Pressure = 3 [atm]
Reference Temperature = 400 [K]

[turbo]

Most failures in multi-staging cfd are from poor initial solution guesses at startup. You need to study the definitions of corrected flows of turbomachinery beforehand.

[Red Ember]

Originally Posted by turbo

Most failures in multi-staging cfd are from poor initial solution guesses at startup. You need to study the definitions of corrected flows of turbomachinery beforehand.

The only one time I succeeded to get results close to desirable happened with massflow at inlet and static pressure at outlet. Efficiency, compression ratio, pressure and temperature values were ok, everyting except velocity near inlet guide vanes (that was probably just because of vanes were too close to the inlet). But solution convergence was not enough - just have a look at efficiency and compression ratio. Solution continue led to parameters decrease...