SimScale CAE Forum

Axial Flow Compressor Sim -Max iterations exceeded error


#1

Hey,

So what I want to calculate is the pressure ratio across the stator to the inlet guide vane. I keep getting max number of iterations exceeded error. I am assuming this has got to something with my boundary conditions. I have defined a max flow inlet and a pressure outlet at 1atm along with a initial pressure of 1 atm. I want to study the static pressure rise across the compressors. I would appreciate if someone could have a look at my set up and let me know if anything is wrong.

https://www.simscale.com/projects/jwick/axialcompress/

Thanks and regards,

John


#2

Hey @jwick,
i saw in the mesh log, that you have 15 illegal faces, may you can simplify more your geometry ?
It is my first idea, maybe it has nothing to do with the error.
I also try it out.

Best regards
Kai


#3

Hi @jwick, how is this going? the latest compressible run that you cancelled looked ok?

Best,
Darren


#4

Hey @1318980,

Yea. It seemed to run ok but it was taking really too long. But I guess thats the way with compressible flows. Have a question, should I use the absolute velocity of the incoming flow to calculate my mach no or the relative velocity of the blades to define whether to run a compressible or incompressible analysis. My incompressible sim ran just fine. I am more interested in the pressure rise across the stage and since my incoming flow velocity is 20 - 30 m/s the mach no is relatively low.

Best,

John


#5

Hi @jwick unfortunatelly yes they take a considerable amount of time to run and not much can be done to speed it up. The most compression will likelly be at the blade tips, so this will need to be the calulation to make, so normal velocity = radius * rad/s and if mach number is higher than some amount then consider it compressible. The catch is usually we say mach number 0.3 is compressible, however, some times the local machnumber may be more, for examble if the blade is spinning with a normal tip mach number of 0.1, as flow passes round the aerofoil it may accelerate higher going around the balde closer to 0.3 or above. So it might be that you run an incompressible and find that actually it should be compressible.

Best,
Darren


#6

Hi @jwick,

Also just noticed this:


The MRF is too close to the rotor and therefore poor mesh quality occures at the trailing edges.

I would recomend moving the MRF closer to the rear stator:


So this doesnt happen.

Best,
Darren


#7

Hi @1318980,

Yes. Just noticed that. I ll make the changes and see how it goes. Thanks again.

Cheers


#8

@1318980,

I also wanted to ask when I look at my pressure contours. A high pressure is generated at the inlet zone and keeps dropping across the cross section. I know this is because i defined a zero value pressure outlet.and in actuality the pressure should increase from the inlet to the outlet. How should I define my boundary conditions ? Should I just use a random non zero value at the outlet to counter this ?


#9

Hi @jwick, for compressible cases, using 0Pa at the outlet is not physical and you should use a value that is realistic to the conditions, normally, this is set to atmospheric at sea level if you need an arbitary realistic value. If incompressible, then the value actually doesn’t matter, leave it at 0Pa and the pressure values are just gauged against 0Pa, you could add whatever pressure you like to return it to absolute pressure post-process.

Is that what you mean? or do you mean the pressure values at the inlet are unphysical?

Best,
Darren