[Achilleas]

Hello all,


I am modeling an axial-flow turbine, known as Wells turbine, using CFX as a solver. It is composed of a rotor with untwisted airfoil blades of symmetrical cross section radially set at 90 degrees stagger angle. I have 4 blades but if we'll take into account the axisymmetric geometry of the turbine, it is not necessary to mesh the whole geometry of the turbine but only one quarter of an overall domain. Periodical boundary conditions are imposed on the neighboring surfaces of the turbine. My model consists of three domains. "Inlet" and "Outlet" domains are stationary while "Rotor" domain is rotating with some angular velocity (i.e. 2000, 3000, 4000 rpm). All of them are fluid domains with air at 25 oC as the fluid. I am using "k-omega SST" as turbulence model setting advanced turbulence controls such as curvature correction and production limiter. Reference pressure is 1 atm. At the inlet I input a normal speed and at the outlet I have Static Pressure with relative pressure at 0 atm. I am quite confident that the generated mesh has a valid quality. The elements amount to approximately 11 millions with the smallest size at the rotor domain. Frozen rotor interfaces connect the domains. No-slip boundary conditions are imposed on the domain walls. In the middle part of the domain, I have used either numerical cells which are rotating with the blades of the turbine with constant angular speed or numerical cells which are stationary. The analysis type is "Steady state". I should say that I have completed series of simulations in which I was changing the angular velocity. In every different angular velocity I was studying the behavior of the turbine in different inlet velocities, in order to be able to compare the results with those which will arise in the long term by a transient analysis. The solution has converged at all cases.

The problem that I encounter regard the value of torque mainly at high inlet velocities. The highest inlet velocity that I am studying is 17.5 m/s. In those high velocities the airflow becomes detached from the blade. However, the value of torque which has came of the funtion “torque_z()@Whole_Blade”, is greater than values where flow seperation doesn't occur and I was expecting that I would have the peak in a diagram Torque-φ. Is my statement logical? What I am doing wrong at this case? I thought that the k-omega SST turbulence model wasn't suitable for higher inlet velocities. In fact, SST model is applicable for low Reynold numbers. So, it is the most correct choice for my case. However, I have checked a lot of available turbulence models. Also, I have checked an even more dence mence. The problem still remains.

mesh.jpg

setup.jpg

Thank you in advance for your assistance,
Achilleas

[ghorrocks]

Have you looked at the flow field to see why the torque is still increasing? Obviously CFX is missing something it the torque is meant to drop off.

SST has not restriction on high speeds. It works fine. In fact I think you will find as the flow heads into the gross separation regime the choice of turbulence model makes no difference as turbulence does not contribute to the torque on the blade.

[Achilleas]

Thanks for your reply,

I agree that CFX does not calculate something. More specific, I believe that the torque function does not take into consideration the mass flow force.

What do you believe about that?

As you can see in the pictures below, the backflow (with inlet velocity equal to 17.5 m/s) cover almost the whole surface of the blade. So, the torque should be negligible. It is obvious that I have stall conditions.

Do you know how I can fix it?

Backflow.PNG

Backflow-2.jpg

Achilleas

[ghorrocks]

What is the mass flow force? Torque integrates the wall shear and pressure over the surface. No other forces act on the body.

Just because it has stalled does not mean you will get no torque. It is deflecting the flow quite a bit so that will generate a torque.

Have you read the FAQ on accuracy: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

[Achilleas]

You are right about torque integration.

I said negligible not that I will get no torque.

Yes, I have read the FAQ on accuracy.

[ghorrocks]

Can you show the torque versus flow rate curve you are getting, and what you expect it to be?

[Achilleas]

All of my simulations have the same form, concerning the diagram of torque-flow rate.

I think that I can detect the stall point by a decrease in the turbine torque.

I expect a decrease of torque after a point, not a continuous increase according to flow rate.

Torque-Flow rate.PNG

[ghorrocks]

Why do you expect a decrease of torque after the stall point? And a second question, is the graph you showed at a fixed rpm?

Dynamic pressure = 0.5*rho*v^2, so as the velocity increases the pressure applied will increase too. So the pressures applied to the rotor will increase as the flow rate increases. So you would expect the torque to increase as the flow rate increases.

[Achilleas]

Yes, the graph that I showed you is at a fixed rpm.

Do you claim that if we have a very high value of velocity as an input we will get a very high amount of energy?

If I understood correct, I disagree with you.

As much as you increase the velocity and concequently the incidence angle, the minimum pressure is decreased at the suction side, while the corresponding minimum pressure is increased at the pressure side. As a result of this, the pressure gradient at the suction side is increased and at the pressure side is decreased. This affects the growth of boundary layer, mainly at the suction side. So, the functional behavior of the blade is altered significantly with increasing of incidence angle. Thus, as much as you increase the velocity, you will get a higher pressure drop, indeed, but after a critical point the losses because of boundary layer are increasing and the capability of switching work between the blade and fluid is decreased. When we have a massive detachment the blade exists stall and it stops operating as a mechanism that create force and trasport energy.

That's why I expect the drop of torque after the stall point.

[aja1345]

Originally Posted by Achilleas

Yes, the graph that I showed you is at a fixed rpm.

Do you claim that if we have a very high value of velocity as an input we will get a very high amount of energy?

If I understood correct, I disagree with you.

As much as you increase the velocity and concequently the incidence angle, the minimum pressure is decreased at the suction side, while the corresponding minimum pressure is increased at the pressure side. As a result of this, the pressure gradient at the suction side is increased and at the pressure side is decreased. This affects the growth of boundary layer, mainly at the suction side. So, the functional behavior of the blade is altered significantly with increasing of incidence angle. Thus, as much as you increase the velocity, you will get a higher pressure drop, indeed, but after a critical point the losses because of boundary layer are increasing and the capability of switching work between the blade and fluid is decreased. When we have a massive detachment the blade exists stall and it stops operating as a mechanism that create force and trasport energy.

That's why I expect the drop of torque after the stall point.

Hi Achilleas,

I think that your means is maximum pressure at the pressure side in the following sentences. Am i right?

"the minimum pressure is decreased at the suction side, while the corresponding minimum pressure is increased at the pressure side."

In fact, corresponding pressure is maximum pressure at the pressure side.

Please see the following figure about wells turbine:



About high pressure drop that you are saying, How did you reach to this conclusion? In fact, you are saying that when pressure drop increases, torque decreases. Am i right? About this case, explain more please.

But i agree with you that you said: torque decreases because of massive separation flow in stall point.

Thanks.

Best.

Aja

[ghorrocks]

Well, let me put it another way: The CFD results do not match your expectations. So is the CFD wrong or your expectations? I cannot count the times my expectations have been wrong in scenarios like this.

So I would approach this with an open mind.

Check the CFD results - why is the CFD showing the torque increasing when it beyond the stall point? Is that reason realistic? If not then what physics have you missed which stops it occurring?

And check your expectations too - get some experimental results or look in the literature. Do they show the torque dropping as you expect? As good as your reasoning is I would be looking for independent confirmation of this expectation.

[Achilleas]

aja1345: Τhe pressure at the pressure side is increasing according to velocity by any means you look it. I said higher pressure drop as much as you increase the velocity. It is a result from the others that I said.
I said that torque decreases after a critical point because of increasing losses due to the boundary layer.
Reread my post please and notice your graphs to see what I mean.

ghorrocks:

I see your point of interest. Firstly, I have to say again thanks for your help.

In the literature, speaking for the same problem, some of the authors show the torque dropping and some others show the torque increasing after the same point but, the latter note that the RANS models fail to model turbine performance under complex stall conditions. I am trying to understand how this difference between the authors exists and how the first managed to fix it.

The next step is to get some experimental results.

[ghorrocks]

At the big angles of attack this thing runs at any turbulence model should be OK. So your comment that turbulence model choice makes a big difference seems strange to me. That is what I would expect anyway, and I have already said what I think about expectations

[Oscar J]

Hello all, im developing an efficiency study for this same axial turbine. So far i have performed some simulations using a structured mesh of around 2 millions elements (1 million for the rotor section with O-grid topology around the naca wing) and Spalart-Allmaras as turbulence model. When i reach high inlet velocities, around the 17.5 m/s mentioned by Mr. Achilleas, the torque continues to increase, when many authors claim to get a decreasing behavior due to stall phenomenon. At first sight, the main differences i can notice with Mr Achilleas simulation is the solver im using, which is Fluent (sorry, i know the thread is related to cfx, but this was the only related to my issue) the elements count (11M vs 2M) and the velocity vectors (im not getting that big recirculation zone in suction side). I would like to know if you figured out the issue with the torque behavior at high inlet velocities. I was thinking that the mesh density in rotor section could be the issue, but after knowing the resolution of Mr Achilleas mesh, im not sure about it now. I have other questions aswell, like how to implement the C-grid topology and satisfy (with quarter O-grids?) the periodic condition on rotor-section meridional faces. I will be very grateful for any reply/suggestions on the subject. Thanks in advanced.

[ghorrocks]

It is not possible to diagnose the problem without a detailed look at your setup. In the meantime, have you read the general FAQ on accuracy: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

[Achilleas]

Hi Oscar,

It's been a long time since I dealt with this study. I did not manage to solve this "problem" and I followed the idea of some authors who stop at the first drop of the torque, specifying in this way the stall point. However, I am really interested in this and how we can eventually achieve the expected results.

Firstly, could you please upload a picture of your domain? You use same boundary conditions with me? Furthermore, let me know:

1) more about your numerical set-up. You use a pressure or density based solver? Please share the reference values of density, pressure, temperature, viscosity and Reynolds number. How you define your fluid properties? I would also like to know how you calculate the fluxes and which reconstruction scheme you choose.

2) Did you check your mesh? Is it of high quality? One cell is enough to create problems. Are you able to see any runtime divergence ?

3) Spalart-Allmaras models needs a y+ approx to 1. Did you use such a resolution of the boundary layer? Did you estimate the thickness of the boundary layer in order to create a proper number of inflations?

Notes:

1) In my personal opinion Spalart-Allmaras turbulence model is more suitable for external flows. Did you try SST k-ω with your mesh?

2) Concerning the grid, the largest number of cells is not always good. After a point we introduce error in the solution. The 11 millions grid could be wrong.

Kind regards,

Achilleas

[Oscar J]

Hello again, Ghorrocks and Achilleas. First of all, im extremely thankful for the quick response you provided to me, also, i want to apologize for my late reply. After reading your replies, i was trying a few general changes on my study, in order to elaborate an appropriate response for you.

To both Ghorrocks & Achilleas:

- Im attaching pictures of my domain and my structured mesh (O-grid topology). Additionally, i will attach an image of a differente mesh (C-grid topology) i've been working on for further tries. The latter is based on the work of Torresi et al., which im trying to follow closely.

My domain represents only one blade (0.125m chord length (c)) passage and is divided in 3 cell zones***: Inlet (2c length, static zone), rotor (0.48c, rotating at 2000 rpm) and outlet (7c, static). I have also considered a turbine tip gap in my model (0.01c). My boundary conditions are:

* vel-inlet (1% turb. intensity, 0.00125m turb. length scale).
* press-oulet (0 Pa gauge pressure, radial equilibrium).
* periodic boundaries (meridional faces).
* no slip condition for all surfaces (hub, blade, casing).
* rotor zone rotates at fixed rpm value; vel-inlet varies in order to match certain flow coefficient/angle of attack for comparison/validation purposes.
* rotor hub and blade surfaces rotate with the rotor cell zone (that is, with 0 relative velocity to the latter).
* casing surface at rotor zone rotates with same angular velocity but opposite sense relative to rotor zone rotation.

1) I have used pressure based, steady state solver with absolute velocity formulation. For my reference values, i have set density, temp and viscosity from default air properties (1.225 kg/m3, etc.), length is 0.125m (c), area 0.0125m2 (blade has 0.1m spanwise), velocity 62.83 m/s (at rotor tip) and Re based on length (c) and velocity just mentioned.

In addition to solver settings, i have used Simplec for p-v coupling. For spatial discretization, i ran a first set of iterations using 1st order upwind and the final set with 2nd order upwind. I checked convergence based on CD, CL and mass flow rate balance between inlet and oulet surfaces, with a convergence criteria of 0.01%.

2) 3) The structured O-grid topology mesh used so far has around 2.1 million elements, y+<1 and what i consider a decent quality (Icem metrics):
- Quality 0.58 min., 0.96 avg.
- Orthogonal quality 0.45 min., 0.96 avg.
- Skew 0.40 min., 0.96 avg.
- AR (fluent): 5542 max., 202 avg. (<3000 at blade surface)

Regarding BL thickness, using Blassius solution (only thing that came to my mind to assess BL thickness) for a flat plate, i estimated it and i can say that the grid has at least 22 layers inside the calculated BL thickness. Cell growth rate is <= 1.2 from blade surface and in all domain in general.

Notes:

1) I tried with Spalart-Allmaras firstly because the low computational cost relative to other 2-eq models and secondly because is the model used by Torresi, et al., showing very good quantitatively and qualitatively agreement with experiments.

Few days ago, i ran a SST k-w simulation (using Spalart-Allmaras previous results as initialization. Correct approach?) and i ended up with very similar results, more critically, similar torque behavior (higher torque with higher inlet vel., even after the stall point predicted in experiments). I can say, however, that my results agreed quite well with experimental and other numerical results under normal operating conditions (that is, before stall conditions).

2) I will try with the other mesh mentioned above (see pictures), which is based on a C-grid topology around blade, which has very similar features as the one used by Torresi et al. alongside the Spalart-Allmaras model.

Additional notes:

***Since the beginning of this study, i have been a bit confused about whether or not to divide the domain in 3 different cell zones (as i actually did), one of which is rotating relative to the other static ones (inlet and outlet), so, is those divisions necessary for my specific steady state study? should i use just one rotating cell zone for the whole domain (with appropriate static and moving walls)?
***After some high inlet velocity value, Achilleas gets a big recirculation zone in blade's suction side. My model replicate that flow feature but in a way smaller scale (see pictures). In the case that i have a correct cell zone config., could my rotor zone's length (0.48c) be affecting the flow behavior downstream blade? may i ask how did you set your cell zones/domain?
***In the same way as you, i have read other authors (e.g. Shaaban, S. (2016)) say that RANS models fails to predict flow under stall conditions, so i wonder how Torresi et al. have achieved results that agreed with reality, even after stall, using S-A, K- and K- SST models...

I hope that all the info wrote so far can explain the approach taken to develop my study. I would like to know about any mistake you can find in the above exposed and also i would like to know from Achilleas's configuration and any additional suggestions from Ghorrocks as well.

I will be waiting for any reply from you, thanks in advance.

Oscar Jauregui.

[Oscar J]

Additional picture

[ghorrocks]

As you are using Fluent, not CFX I can only give general advice.

First of all the general FAQ I previously quoted on accuracy is important. I would not have quoted it otherwise. If you have not done a sensitivity check on your mesh size, convergence and time step size (if transient) then you are just guessing.

Once that is complete you need to consider the key physics. The biggest issue I see here is the Spalart-Allmaras turbulence model. While you say other authors have had good results with SA, this may have been due to luck rather than its inherent qualities. In fact stall prediction is a challenging topic for any turbulence model. I recommend trying a more sophisticated model such as SST, but you may have to advance to DES and SAS family of models to correctly predict this.

[Achilleas]

I can not understand a lot from this picture but, as I see, you may have problems with the aspect ratio if you use a y+=1. Furthermore, the skewness of the cells in the leading edge may be problematic. If you also comment about your numerical set-up it would be easier to discuss some things.