Compressor working as decompressor...
 

Hello,
I am modelling compressor, and in contours I see that it works as decompressor:
http://i.imgur.com/cQUDM.png
I have also local overpressure located at top of screen- why?
What to do with this case as on screen: http://i.imgur.com/azUUj.png ?

It seems that your solution has diverged.

Please check your turbulence model, discretization scheme, under-relaxation factors and boundary conditions.

Specifically, it looks as if your y-velocity is diverging, causing all others to fail. I would suggest:

a) Make a better initial guess for the y-velocity
b) Make the under-relaxation factor for momentum smaller.

Please let us know what URF's you're using.

You might also let us know if there are any text-based errors appearing on the screen; for instance, do you get a "temperature limited to XXXX kelvin" error?

ComputerGuy

So do you suggest to make for example 50m/s at y-velocity to make compressor working easier?
URFs are default: Courant number 5, (sometimes solver makes it lower, to for example 0.05)
Modified Turbulent Viscosity 0.8,
Turbulent viscosity 1,
Solid 1.
Sometimes I receive messages about limiting temperature. I made many different simulations and I am not able for now to say when is this.
I use as BC to inlet and outlet Modified Turbulent Viscosity 0.001.
Gauge, Initial pressure=0 atm at inlet, operating pressure 1 atm, at outlet gauge pressure=1atm.
Thank you in advance.

First question: are you modeling solid formation in the compressor?? It seems as such with your URFs. If you are: solids in fluent are treated as large momentum-sinks, and thus it's not surprising that you have convergence errors. I would take smaller time steps for sure, and potentially do some grid refinement.

Next, think about doing 2 things:
1) Make your y-velocity initial guess more reasonable. I don't know if 50 m/s is good for your system, but if it is, then use that. The better the guess you can give fluent to start with, the better the solver will be able to converge.
2) If you're getting temperature errors combined with divergence, think about setting the limits on your solve a little bit tighter. For example, they're probably default which (I think) are: min: 1 kelvin, max: 5000 kelvin. Generally, this isn't a big issue, but for hard-to-converge cases, you can set the limits to be more realistic, especially if you have temperature-dependent material properties or phenomena (solidification).

Think about what a reasonable minimum should be...perhaps 250 K? Think about what a max should be...Perhaps 600K in a compressor? I don't know, but it's not likely 5000 K.

Play with those two things, and potentially relax momentum a bit (make its factor smaller) and let us know.

ComputerGuy

You can specify mass flow inlet as the boundary condition for the inlet face.

I am not modelling solid formation, I have only walls as boundary conditions.
Smaller time steps at Steady Solver? Is it possible?
My y-velocity was computed from inlet, when I made BC for inlet: Gauge pressure: 0atm, Initial pressure -0.1atm. I am planning to change to zeros when solution converges and make futher calculations. Is it good idea?
I regulated temperature limits to 250K<T<600K. I limited pressure to 5atm max too, because sometimes I got 20-100atm.
What do you think about Modified Turbulent Viscosity=0.001?
Where can I relax momentum?

I don't want to make mass flow inlet as BC due to check when solution is converged- when continuity equation is fulfilled.

Tom,

I was confused, as you have a Solid under relaxation factor listed. I thought this must have been for phase change.

Time steps in a steady-state solver are not possible.

I'll have to think about this a bit more -- I don't really understand how you've set up this problem at all. Generally, especially in steady-state modeling, you initialize the solution "close to" the end solution. That is, you want to initialize pressures, velocities, temperatures, etc. within the domain to be what you'd expect them to be. I don't think initializing them, then re-initializing as you're stating, is a good idea in your case.

I hope you figure out the problem, because until I look at your case, unfortunately I don't think I can help further. If you need more help, it will be useful to list all of the following:

Boundary conditions for fluid inlet and outlet...Pressures, turbulence levels.
Fluids used: are they isothermal properties or do they vary with temperature?
Compressor blade direction -- is it rotating in the proper way, or is it reversed?
Initialization conditions: what pressures, temperatures, and velocities are you using?

Good luck.
ComputerGuy

I sometimes get areas of local hiperpressures. Like on this picture: http://i.imgur.com/vITQN.png Why is this?
Solver Steady, density based.
I use Energy equation, Spalart-Allmaras model with default ratios.
Air is ideal gas.
Rotational speed 100000rpm.
At inlet: Gauge pressure: 0atm, Initial pressure: -0.1atm, Modified Turbulent Viscosity=0.001
Operating pressure: 1atm.
At outlet: Gauge pressure: 1atm. Backflow Turbulent Viscosity Ratio 5.
Velocity calculated at Initialization from inlet by pressure is 45m/s.
Formulation Implicit.
Flux Type Roe-FDS.
Solution method is Gradient: Green-Gauss Cell Based.
Flow: Second Order Upwind.
Modified Turbulent Viscosity: First Order Upwind.
Very often I get diverged solution after about 40-60 iterations. Mass flows aren't going in proper way. (at outlet is constant for all iterations, at inlet is smaller during iterations.)
Rotations are in proper way.

Actually I try to help the compressor to make flow in correct way- I made outlet initial pressure at 0.1atm, what do you think about this?

Problem solved with limiting temperature and pressures and changing pressure models (cell based, green gauss based etc.).