wind turbine
 

Hello everybody!

I'm working on a three blade horizontal axis wind turbine of 29m of radius. I have a 120º sector cylinder of 5R of raidus, 5R upstream and 15R downstream.
My mesh is a 4 mill cells hexa mesh with rather good quality.

The target is to measure the torque generated for 15m/s and 10rpm. To achieve this I'm increasing the windspeed from 5m/s to 10m/s and 15m/s, with 1rpm, 2rpm and 3rpm of angular speed.

I'm using single precision (I've also tested double seeing no differences), SIMPLE, least squares for gradients, 2nd order for pressure and 2nd order for momentum. Residuals started at 1e-7, then I've reduced them to 1e-5 and 1e-4 to speed up convergence.

I've first tried the steady laminar case, but with no success. For 5m/s I got reversed flow at pressure outlet, and for 10 and 15m/s I got very low torque coefficient, almost 10 times lower than the experimental data.
At least flow vectors seemed to be correct.

Then I've tried the transient laminar case. I've used 1st order time scheme to use the adpative timestepping: 1e-7 to 1e-3 s.
Torque coefficient looks better but reverse flow appears and vectors looks the opposite way they should be! I've even doubted if the sens of rotation is okay and have tried the opposite. Results are the same.

How can I avoid the reverse flow at pressure outlet?
This can be due to not large enough domain, but I've checked literature and mine is pretty okay...
It can also be due to bad boundary conditions, but I'm using the usual: velocity inelt, periodic, symmetry and pressure outlet.

Can anybody tell me how reverse flow can be avoid?
And if it is the main cause of such a poor predicition?
Is my rotating reference frame okay? or it should be the opposite? See pictures.

Any comment or suggestion is highly appreciated.

Thanks a lot!

How could it be laminar?

reversed flow in farfield and in few cells should not be the problem. Try some turbulence model as you have to decide it based on your reynolds number and keeping in view dia of your wind turbine and relative velocity, I don't think flow is laminar.

I know it's not a laminar flow, but I wanted to test this case as a upper limit of torque prediction as I had read.

I've run the case with k-omega SST model (inlet default values). No change in the solution. Reversed flow appears in the same amount and torque coefficient es still very low.
When I check the flow patern it's complety wrong. Absolute velocity vectors go the opposite way and relative vectors too! (see pictures) What's more, turbulent viscosity ratio limited to 1e5 is starting in a few cells!

Why is the flow going the opposite way? Is the rotating reference frame right as I exposed in the first post http://www.cfd-online.com/Forums/flu...tml#post421762
Or is it due to the reversed flow?

I'm stuck! Please help! Thanks

Looks like you have wrong boundary conditions and flow angles.

How did you determine them?

You know in wind turbine incoming flow is higher angle (towards 90) and relative flow is less than stall angle. Whereas in your case I see relative velocity at right angle to turbine? and free stream velocity is coming from trailing edge to leading edge !!! Absolute velocity should remain same Why this is so?

R you running your case at very low RPM? This is also because of weired flow angles (but still it should not make freestream air coming from rear side). If so the don't nt expect solution and convergence at such off design condition and massive separation is expected and you are trying to get solution in stall regime.

Moreover with laminar flow your flow gets more worsen as laminar flow has more tendency for separation.

PS: are you sure solution is fully converged?

Well, I upload a picture of the wanted flow angles that I guess helps to understand the case. Inlet velocity is 5m/s for this case with an angular velocity of 1.034 rad/s.
Incident velocity is okay, but relative due to rotating ref frame is the opposite. I've also tried the other sense of rotation but it looks the same.

I guess flow coming from trailing to lead edge is due to reversed flow disturbing all the flow. Or maybe for bad rotation of the reference frame. That's exactly what I want to solve.

well we need to find out the root cause of this behavior. I suspect the wrong case set up at some point. Where it is I dont know!!!

Yes, there must be some set up error. :(

Relative flow should be parallel to incident flow coming from inlet as it is rotating with the ref frame.
So absolute one, observed from outside the rotating ref frame, should look like the real flow.

Right?

You should be able to obtain a steady solution with some turbulence model. When you chose a turbulence model, re-initialize the flow from the inlet b.c. You may want to change the symmetric b.c. to velocity inlet b.c. at first. The reversed flow may appear at the outlet for first tens or hundreds steps but will disappear thereafter. Make sure that the origin and axis for your rotation frame is set right. Never use laminar flow model unless you are a hundred percent sure what you are doing. Do not turn on the unsteady solver because it is unnecessary here. You may need to reduce the URF or use the coupled solver with a smaller Courant number with your final inlet velocity and rpm but you do not have to increase them gradually.

One basic question: Do you have twist and camber in blade?

To inlet b.c.? Would that be realistic? and when should I change that back to symmetry?
Should I try non shear stress wall b.c.? Would that help to avoid the reversed flow at outlet?

I'm sure about the center of rotation, I moved the mesh to make it the (0,0,0). I'm not pretty sure about the rotating axis: (0,0,-1) or (0,0,1). I want the turbine to rotate clockwise. I've tried several options:
1) Rotating reference frame clockwise, relative flow should be anti-clockwise? (see last post picture)
2) Rotating reference frame anti-clockwise
3) Rotating mesh clockwise

In all cases there's reversed flow in the same amount (23k cells in outlet) and vectors for absolute flow goes the opposite way!
Which setup should I use? Rotating reference frame in the same sense as the turbine? Opposite to it? Which difference is there with rotating mesh?

Thats's what I thought about the steady solution. This flow doesn't seem to be very time-dependent for an optimun angle of attack.

No need to increase rpm-windspeed gradually? That's what I read at fluent user guide.

Yes, the blade is twisted but its center line is stragith from hub to the tip.

Thanks!

Use right hand rule to determine + or - z .

Also be careful in giving tangential flow angle. Sign is important.

For Axial flow direction I am trying to digg my memory but cannot recall :mad:... Look into fluent help :o

I am applying the right hand rule, what I don't know is how the relative flow-frame movement is.

What do you mean by tangential flow angle? The angle of attack? It is determined by the axial flow speed (inlet) and the angular velocity.

I don't get your point here.

Ok. Let me explain:


1. Wrap you figures in the rotation direction. You thumb will give you - or + sign. If it is pointing towards positive z then it is +1 if it is in -ve z then you have -1.

2. Lets say you rotation axis is -Z and now if you incoming air is going towards +z direction then you will give the -ve component of angle in axial direction. If it is totally axial flow then you will have the -axial component (i.e. -cos0 = -1).

If incoming flow is at some angle then you will have to specify the tangential component as well. Again if it is in the direction of rotation then it is +ve otherwise -ve.

While specifying the boundary conditions you don't need to consider the relative flow velocity and angle. It is taken care by solver. But if it is different than the expected direction and magnitude then your boundary conditions must be wrong.

Hi, Bollonga, could you please post the result of the TUI command
/report/summay yes "report.sum"
so that we could put the discussion on a more firm basis.

I've tried using wall bc with zero shear stress instead of symmetry condition and reversed flow has disappeared, at least for the laminar case U15m/s-30rpm. Residuals cannot reach 1e-5 (see picture 1).
Torque coefficient is still low CT=0.008, and it oscillates too much, from 0 to 0.015 (see picture 2).
Relative flow looks the right way (see picture 3).

I'm trying now the k-omega SST case, I'll share my results.

You have the report in the zip file.

How you define the coefficient of torque? did you make a custom field function?

Did you get the point about setting the axis of rotation and flow direction?

Why you want to have the 1e-05 as convergence criteria? it is too tight convergence criteria in Fluent

No, I'm measuring moment coefficient of every wall surface for center (0,0,0) and axis (0,0,-1)

Yes, without reversed flow the rotation seems to be the right way.

I don't know, I just wanted to get it very converged. Which will be an appropiate value?

Torque coefficient = torque you get from CFD / Maximum torque (V4 = 0)

Maximum (theoretical) torque is = 0.5 * density * Area * V1^2

Reverse flow should not the your rotation axis criteria. :rolleyes:

Very converged : I think 1e-03 or 1e-04 is good convergence. You can compare them to find out the convergence error. You should also monitor some other value of your interest such as power coefficient or torque coefficient.

I know, I was talking about moment coefficient = torque I get from CFD

I know it's independent, but when I checked the resulting flow it was going the opposite way and I think it's due to reversed flow in the outlet that modiefies all the flow pattern.

I'll check that once I have good results. Thanks.

You realize that your rotor speed is around 30 rpm, do you?

Yes, I do. Is it too much? I've been reading that this is the rotor speed for some comercial wind turbines.

I've run the k-omega SST case with 1% inlet turbulence and 0.05m as length scale. Now the moment coefficient is negative! I'm measuring moment along (0,0,1) while rotating reference frame is about (0,0,-1).
The issue is that the laminar case results in a positive coefficient for the same axis definition!

Which is the correct coefficient sign? Is it acounting for the work the fluid is doing on the blade (so it should be positive with my setup) or is it the for the blade working on the flow?

Watching the coefficient history it appears to oscillate over a wide range.

Flow looks the right direction, but I see some separation and I guess it shouldn't be any.

I attach pictures of residuals, moment coefficient history, relative velocity vectors, static pressure contours and pathlines.

is magnitude ok?

Which magnitude? Everything is full scale.

I've reduced the angle of attack from 12º to 10º by reducing wind speed, Cm has improved but there's still some oscillations around its value (picture 1). I've also compared it for TI=1% and TI=5%. The first being logically a little bit higher.

There still some separation (pictures 2, 3 and 4), is it supposed not to have any? Reynolds number is pretty high at this section (Re=6 e6) so even for a 10º angle of attack I guess dettachment is possible.

Also, I'm not pretty sure about which is the optimun angular speed for a given windspeed if I can also choose the blade alignment.

To avoid the reverse flow at pressure outlet, you should use Alternate Rotation Model in the Domain setting.
The attachment picture shows the streamline without/with alternate rotation model.
http://www.cfd-online.com/Forums/att...1&d=1384939471

What is the difference between both models?