Convergence curves.

Thanks for any answer,
Attesz

Why do you say you are well converged? Residuals of 1e-4 is loose convergence in many cases. You may need to converge tighter. Have you looked at http://www.cfd-online.com/Wiki/Ansys...gence_criteria

The GGI error you showed may just be a CFD-Post rendering error. It is possible the solver is correct but CFD-Post is not showing it correctly. Not sure, but keep an open mind.

Hi all,

I've checked the yplus values, and since there are different velocities in the compressor's flow field, it's not to easy to generate a good mesh.

Because on the blades, the velocity is about 300m/s, I need to set the first boundary layer on that wall to 0.00001 mm, but by using 1.2 expansion factor, I get a huge difference between the last boundary layer and the first tetra (the well known meshing problem). On the inlet, I've more lower velocities, and the resolving of the boundary layer there may not so important, i think.

So, I want to use different yplus in my model:
yplus under 2 on the critical walls where separations develops,
and "bigger" cells on the other walls by using wall function and yplus over 30.

Is it a good way? Can it cause errors?

Thank you!

Attesz

Thanks for your answer. You are right, it's not converged well. I've set the physical timescal 100times higher, but has no significant effect. I attempt, that I should check the mesh..

And the Post rendering error is can be right, because there isn't any "error" in the pressure and density contours, only in tempreature. It's interesting.

Thanks for your answers again!

Attila

To fix this add additional prism layers until the transition is good. This results in large grids - but that's CFD for you.

Yes, that is the way to go.

Thanks Glenn!

Otherwise, how can the size difference between the last boundary layer cell and the first tetra affect the results? Can it cause a bigger numerical error than the wrong modelled near-wall physics, for example yplus between 2and 20?

Attila

The accuracy of the numerical discretisation is reduced, and numerical instability increases.

That is problem dependent. You will have to find out for yourself on your simulation.

Thank you.

In my compressor simulation there is a huge separation started from the leading edge. I think, it's unreal at PR1. First, i attempted it caused by the mesh quality, but I've resolved the mesh and the boundary condition at the starting point, without any result.

Now, I've read in the documentation, that the two equation turb. models can overpredict the turbulence energy, so Production Limiters needs to be used. Maybe this is the problem in my simulation (in help they write about the increased tubulence energy at the stagnation point, and in my case it's exactly the same), but there is two Production Limiter: Clip Factor and Kato Launder. Which is prefferred in my work? Can is cause numerical error where the turbulence kinetic energy calculated correctly?

Thanks for any advice!

Attesz

I would not fiddle those factors unless you know exactly what they mean. The constants in the turbulence models are set by people a lot smarter than me so I don't like to change them.

Almost always the problem is elsewhere. Either a numerical accuracy problem, or that the turbulence model is inappropriate for modelling what you propose and no amount of fiddling with constants will fix it.

Thanks. With this prod.limiters, I don't change any constants in the model! The quantities will be calculated by the original form of the turbulence model, but they give wrong results in stagnation points. This is described clearly in documentations. The production limiter works only in the stagnation point, where wrong results can be generated, but elsewhere not. Anyway, I've started a simulation with this, I will share the results.

Best regards,
Attesz

OK, I will be interested in the results.

Hellow,

very interesting thread in here!!! I made similar steady-state simulations of a centrifugal compressor with vaneless diffusor and volute. It´s a turbocharger-compressor with 100 000 RPM and backswept blades. I simulated the 360°-case and used the frozen-rotor-model and the sst-model as well. For me it was possible to catch the characteristic jet-wake-model. For backswept blades the wake-area at impeller exit should appear in the suction-shroud-corner. The wake-area moved in a correct way when i changed some geometrical parameters. I compared it to literature (dissertation Lohmberg 2000). So it moves to the hub when the rake (lean angle at impeller exit) becomes positiv. You can see it in the pictures. I do not understand the idea of using a physical timescale that is bigger than fluid timescale. In the CFX-help i only find the recommendation delta t=0.1/omega....1/omega (omega=angular velocity) for steady state rotor-stator-problems. That leads to very small timescale for my problem (10^-5 ... 10^-4). I thought you can use large timescales when you have a full-steady-state-problem, but thats not the case for a compressor, even in operating point. However I used delta t=0.01s :) and i still got acceptable results. I also got an overestimation of total pressure ratio of about 0.5 in the surge-region and an overestimation of total efficieny of about 5 percentage points, but i think thats still ok, because i got some Ansys-simulations here and they were not better with a much finer grid. It´s due to massflow-dependent losses in in- and outlet that cannot be reflected in the simulation...

Greetz from Susann

Hi Susann,

can you post some information about your mesh in impeller and in boundary layer?

Thank for your post!

Attila

Hello Attila,

nice to meet you again :)
My grid is relatively coarse. I have a tetraeder-grid with 5 prism layers.

Max size of tetraeder:
Hub, Shroud = 2 mm
Blades = 1 mm
Leading Edge =0.5 mm
Trailing Edge =0.25 mm
Tip =0.125 mm
RSI in/out =1/0.5 mm

The 5 prism layers have the following characteristics:

first prism height =0.00893 mm
height ratio =1.2 mm
end prism height =0.016 mm
total height =0.0625 mm

With this mesh i get y+-values between 1-10 on the impellerblades. Values y+<2 are very rare so that "Low-Reynolds"-Method should be used only on small parts of the impellerwalls. But I had to use a coarse mesh because of computing time. Did you find something about the problem of different separation regions and strenghts between stationary and transient results? Because i have the same problem now...separation and backflow is much stronger in the stationary Frozen-Rotor-result. I got some pics for you here from Blade-to-Blade-view (0.9 blade height). The first pic shows the Frozen Rotor- and the second pic shows the Transient result. Transient result is made of the arithmetic averaged data (transient statistics) of the last revolution of the impeller blades after 27 rotations. The Jet-Wake-pattern changed too when i made the transient simulation.

Greeeeets from Susann

I assume you use SST. These values are not correct. Did you get accurate results compared with measurements (i don't remember)?
I think, yplus above 20 and 10 cells in boundary layer will not slow down your simulation significantly. But you will get accurately results, for example in separations. Otherwise, why do you think that stronger separations are wrong? TRS simulation is propably more accurate than steady.

I'm using now 20 cells in boundary layer to get yplus above 1. My model is 120deg periodic, and so i get 8million element :)

I've a large separation started from the splitter blade, and I think its not real. I've tried a lot of modifications, but no result (higher grid density, tuning SST with production limiters). Thats why I asked for your settings.

If you have any suggestion, please let me know. I'm working on it one a year without results, and i begin to get bored :o

Best Regards,
Attesz

Hey Attila,

why do you think theese y+-values are not correct? Thats what CFX shows me in POST...:confused:...the characteristic compared to measurements and Ansys-results looked pretty good too. My transient simulation showed less separation than the steady state solution. Thats what makes me confused as I thought transient simulation should capture more of these phenomena.
Your separation spreading from the splitter blade is it on pressure o suction side of the blade? Looks like pressure side? Thats weird! Why do you know that its wrong and not physically correct?

I mean, that yplus should be above 20 when you use only 5 cells (but 10 cells is preferable), to get accurate wall function results.

My separation starts near the leading edge of the splitter blade, and grows on its suction side. The problem is not with this separation (or wake region). It causes lower operation performances, for example in my simulation I reach the surge under the measured operational point. In the pictures You can see the results used Pressure Ratio 1. When I increase the PR, the separation grows, and closes the outlet area of the impeller. I think, thats why I reach the surge earlier.

I will post some other results soon.

Best Regards,
Attila

In steady state the separations will be "averaged". But we know, its always a transient simulation. When you get less separation with transient, I think, its correct, but maybe people who are smarter than me can you explain it better...

Hellow Attila,

i think the y+-values calculated in CFX do not only depend on number and height of prism layers but also velocities in impeller and thickness of boundary layer. So i don`t know how you got the value of y+>20 with 5 prism layers?

And I think it´s totally normal if you reach surge much earlier than experimental measurements, because there is a difference between numerical surge and real surge...especially with our steady state simulations! How much is the difference between simulation and experiment?

le susn

Often operational point and surge point are very close so that I think that numerical surge point can be reached before operational point in some cases. :)