Negative power and torque(Axial Turbine analysis)
 

Dear all,
I have modeled an axial turbine in CFX. I used the macro calculator to get the torque and power and it gives me negative torque and power! What does it mean?
If a negative torque is just mentioning the direction of rotation so why should I get a negative power(since P=T.Omega)?
Thanks

It means you have not hit the steady state operating condition.

For instance, if you run a turbine at too high a rotational velocity you will get negative net torque - this means the rotor is running too fast and will decelerate. If you run it too slow it will generate positive torque and accelerate. The steady state operating point is where the net torque is zero.

What is the value of total pressure (stationary reference frame) at inlet and outlet? What type of boundary conditions you are applying at inlet and outlet.

Thank you both.
The rotor speed is -1000 rpm, the input BC is a mass flow of 250 kg/s and the output BC is static pressure of 1 atm.
The results are attached.

1. cant you apply the total pressure at inlet?
2. Why efficiency is more than 100%, it seems that either rotation direction is wrong (working as compressor) or solution is not converged.
3. Did you model the NGV before the rotor, if no how you are specifying the velocity components in axial and tangential dirction along with correct sign. (obviously r component is zero).

did you specify the correct rotation axis in macro calcular panel?

1.Unfortunately not.
2.I know that, the rotation direction is correct but the interesting point is that even changing it will not lead into a positive magnitude.
3.I have specified mass flow rate at inlet in turbo mode.

Yes

Your mesh looks very coarse. Have you read this FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

Especially the bit about mesh resolution?

@ghorrocks: I decreased the mesh size to 0.003 but no lock... it is still negative.
and the solver manager shows this for every step in the out file.
+--------------------------------------------------------------------+
| ****** Notice ****** |
| A wall has been placed at portion(s) of an OUTLET |
| boundary condition (at 40.1% of the faces, 43.3% of the area) |
| to prevent fluid from flowing into the domain. |
| The boundary condition name is: R1 Outlet. |
| The fluid name is: Water. |
| If this situation persists, consider switching |
| to an Opening type boundary condition instead. |
+--------------------------------------------------------------------+
The solver reaches an rms value of 1e-4 at about 50 steps.

1. decrease static pressure at oultet
2. From the Picture of your geomtry, why geomtry converged to single line on hub side, is this a design feature.

1.Static pressure is zero.
2. That is where hub ends.

can you please attach the ccl file?

Here it is.

Look a bit deeper. Graph the torque versus mesh size. Is it trending in the right direction? Is it all over the place? This can tell you if you are close or not.

You outlet is showing lots of back flow and the suggests your outlet is too close to the blades. You will need to extend your domain further downstream.

And please show some images of the flow field - steamlines would be nice.

I guess you are making some common/basic mistake in setting-up the problem in CFX. Are you clear that the rpm are -1000 or 1000. Could you please show some pics of CFX pre with axis visible.
What about reference pressure, is it also equal to 0?

by default in CFX pre if you give negetive speed(- sign) then rotor rotates anticlockwise.
find the enthalpy drop ,for turbine the enthalpy will reduce it from inlet to outlet.

not necessary, it depends on the geometry and also whether it is turbine or compressor. Just take an example of twin spool turbofan engine.

First of all, thank you all.
Decreasing the mesh size did not influence the torque.
Extending the domain at downstream increased the backflow area to 90 percent.
Omega equals -1000rpm and as I said even changing it to 1000 did not influence the negative torque.

Sounds extremely unlikely. What meshes did you check?

Then you need to go further downstream.

it seems that the blade is not following the flow or vice versa. Did you use the reference equal to zero or 101325?
On pressure contour plot, scale shows the pressure from 3e+06 to -1e+07, looks strange?

Well things are getting stranger...In the Passages and Alignment section the Passages per Mesh, Passages to Model and Passages per 360 change automatically to 27,27 and 108!
Every time I change them to 1,1 and 4 but as soon as I close CFX-Pre and reopen it they are changed. I am modelling a quarter of a 4 blade turbine so why CFX is changing these parameters?

should not happen, could you please past the snapshot of cfx pre witht the stated problem

Here it is.

make the passage per mesh equal to 1

I did this more than 10 times but as soon as I close CFX-Pre it changes again

it is not possible !!!!

Dear one,

I also get this type of problem in Cfx-post.

While i initialize the stator and rotor in Turbo mode.
By default the number of passage in 360 degree is 12 i got, if i change it to 52 in stator and 58 in rotor, but the report generate for turbine shows the mass flow rate as per 12 passage rather than 58 passage for moving bled outlet

NET TORQUE - Fluent
 

Hi,
I'm simulating a Wind Turbine but I don't know the Cp vs lambda curve. I read your post about the net torque procedure. In fluent (ANSYS CFD) I can know the momentum Z (rotation axes) for every blade. This momentum is always positive at different angular velocity:
wind speed = 6 m/s,
angular velocity 10-50-100-150 rad/s
Mz= 0.23 - 4.18 - 6.17 - 6.73 Nm
Is this the net torque?
regards

can i ask if compressor torque negative, which means that is rotor run too fast too?

You have to be careful about your definition of positive and negative. But assuming your comment means that a compressor is producing a negative torque (ie a torque in the direction of rotation), that means the compressor is running too slowly and will speed up. So the steady state speed of this compressor is faster than you have modelled.