[joaopffg]

Hi guys,
i'm simulating a sirocco fan in SW flow sim. and i have been having troubles with the efficiency. Below is an image of the domain (i'm currently running the program so it's just a fast print screen).
Attachment 40328

I'm using the SI system. So, the eff is equal to the flow rate times the total pressure difference between the outlet and the inlet, all divided by the power (rotational velocity [rad/s] times torque [N.m]).
I set surface goals for the outlet pressure (the inlet pressure is atm.) and the volume flow rate. The rpm is constant. And then i set a surface goal for the torque wich included all the rotor surfaces (not just the blades). I was careful to set the rpm of the revolution surfaces of the rotor to be the same as the rotating region (blades).

However the values of the efficiency are always above 1... I think it's because of the way SW is calculating the torque. I did a quick hand calculation to get the toque caused from the pressure drop in the blades and if i use this method the efficiency gets to aprox. 40% or 50%.

I would like to know if someone can explain to me how or where can i find the way that SW calculater torque and what am i doing wrong ...

The Y+ is around 60 and i'm using sliding mesh.

I can provide any other info about the simulation.

Thanks

[Ive]

Something is wrong with your attachment - clicking it gives an error.

Are the rotor surfaces other than blades inside the rotating region? If so, you do not need to specify any rotation for them separately, because the rotation is applied to all surfaces inside the rotating region.

[joaopffg]

Hi there,
sory for the error in the images, here are some fresh new ones.
dominio.jpg rotor1.png rotor2.jpg

The rotating domain only enclosures the blades (and is the same as the one in the images for the other side of the rotor). I ended up leting the program run for some more time and the torque eventualy converged to a value that made the efficiency drop to around 50%.

However i wold very much like to know how does solidworks calculate the torque. In the blade zone it probably calculates the force from the pressure difference, but in the rotating walls (walls in the midle of the rotor) i have no idea (and it may not matter, since its way smaller than the torque from the blades)

[Ive]

Glad to hear that the issue has gone. For the calculation stability and optimal convergence with the sliding boundary model, it is recommended to use the time step (in seconds) in the range 1/RPM < t < 6/RPM/N, here N is the number of blades, RPM should not be converted to RPS.
The torque is calculated as the force acting on a cell face multiplied by the radius-vector to the axis. Both the pressure and friction force components are included in the calculation of force, and at a smooth axisymmetric surface such as a wheel hub the force will be much smaller than at the blades and its input to the total torque at the wheel can be considered negligible.

[joaopffg]

Thanks for the quick reply
Abaut the torque, i had an idea of how it calculates it. I wanted to know if there is some documentation where they explay the math behind it (the formulas used). They don't mention it in the docs that come with the program.

As for the time step interval, i had no idea abaut those limits. I just chose the time so that the increment was made 2º at a time.
In your formula, 6/RPM/N, RPM is in rad? And is it (6/RPM)/N or 6/(RPM/N)??

[Ive]

Naturally, total torque acting on surface or a body is calculated as the magnitude of a vector sum of vector products of force vector and radius vector in the centroid of each cell wall face (the sum is taken over all cell wall faces belonging to the surface or body):

M = ||SUM {Fi x Ri}||

here Fi is the vector of force acting on the cell wall face, Ri is the radius-vector to the cell face centroid. There is just no other way to do it
The force vector is calculated as a sum of vectors:

Fi =Fni + Fti

here Fni is the vector of the normal component of force, Fti is the friction force vector.

RPM in the time step limits is the rotational speed (rotations per minute, RPM), not the angular velocity (rad/s). (6/RPM)/N and 6/(RPM/N) is the same.

[joaopffg]

Indeed it is the same... A guy is doing his master thesis and doesn't notice that...

Can you just tell me where you got the 1/RPM < t < 6/RPM/N, in case i have to justify using it?

Thanks for the reply

[Ive]

I have just realized that I made a mistake, it should read like this:

1/RPM > t > 6/RPM/N

so it reduces the time step for the number of blades > 6, while in my earlier post it would only apply for number of blades < 6, which makes no sense.
This recommendation is just based on the practical experience of the FloEFD support team.

You can also use the CFL condition to calculate the time step from the blade tip tangential velocity, linear size of the smallest cell inside the rotating region and aiming for the Courant number in the range 1...10. While the CFL condition is not directly applicable to implicit time stepping schemes such as the one used in the FloEFD solver, it is still a good indicator of the time step adequacy.

[joaopffg]

Thanks a lot for the help!!
Just one more thing. Is there a way to highlight the cell with the highest velocity, so i can check the Courant number on that cell?
I did a rough calculation and it gave me a Courant number of 15 on one of the cells in the impeller exit (for the 0.0002s time step i was using)

[Ive]

You can visualize the locations of the min and max of any parameter. Just create any plot (cut plot, surface plot, etc.) of that parameter and then go to Results -> Display -> Global Min/Max in the Flow Simulation menu. The red dot in the graphics area will show the location of the maximum and the blue dot will show where is the minimum (in the entire domain, not just in the active plot).
Do not worry if the Courant number reaches 15 in some cell - the solver should tolerate it.

[joaopffg]

Hi again,
i used the tool but there seams to be something wrong.
It indicates the highest velocity in a node where the velocity plot says it isn't that high. It may be because it is a node in the rotating region.
1.jpg 2.jpg

[Ive]

The max point may not lay in the plot plane.
Also, in many cases it is more convenient to visualize or calculate the velocity inside a rotating region relative to the rotating frame. It can be done by selecting the Velocity RRF parameter instead of Velocity.