Simulate propelling force from water over a passive turbine
 

Hello all,

I am starting with Ansys and CFD analysis, so sorry for any obvious question. I have this project of a turbine inside a pipe. The water run through this pipe and rotates the blades of a passive turbine, which is attached to an free axis. I would like to calculate the axial rotation force created by this contact (water+blades).
Every tutorial I found is about the blades actively rotating and propelling the water. I want the inverse situation. Attached is a simplified model.

Initially my doubt is only if it is possible to do, which way I should start looking for and how complex it will be. As I said, I am starting in this field and don't know exactly the limitations.
Thank you very much for the time.

Best regards.

This model is quite simple.

You guess a rotation speed for the rotor and do a rotating frames of reference model using the fixed speed. This will give you an output torque. You then adjust the rotation speed and re-run it until you get close to zero net torque, and then you have the steady state rotation speed of the device.

Do not make the mistake of trying to run this as a rigid body and allow it to find its own steady state speed. This is MUCH harder and MUCH longer than the approach I described.

Also, another newbie mistake is to model the rotor as a solid. You do not need this, just model it a cavity in the fluid mesh (like the tutorials do).

Thank you very much ghorrocks. That was exactly what I was looking for, a brief idea about where to start researching. I guess I understood your suggestion. I will try to do the MRF and check the results :)

Since I am doing this master research, I also want to learn the maximum as I can about CFD. Do you think is worth to learn later how to model it as a rigid body and let find it own SS speed? I mean as a curiosity? Or this is too complex and useless?

Again, thank you indeed.
Regards.

I recommend you do as wide a range of simulations as you can. So feel free to do it as a rigid body simulation. You will find out exactly why it is more difficult than it looks :).

Would it be posible to write an expression that would look at the old walue of torque monitor point and than step by step go tovards 0 walue.

Something like OMEGA = oldOMEGA * (if old torque < 0 ,0.8, 1.2)

So it would step the angular velocity walue (this is just an idea I havent tried it though)
Would this work?

Try it and find out :)

The issue is whether it is numerically stable. Almost always it is not, so the simulation diverges. You need to add some damping to get it to converge and that is difficult in CEL.

This problem seemed interesting to me, so I went and tried it out myself. I will put on some updates if I manage to make it automatically find its angular velocity based on mass flow, that is the goal of course and it will be a challenge for me.

Image of problem setup and results

https://drive.google.com/open?id=0Bw...lh6OGhsQ3dZMk0

be careful for the cilindrical walls of the rotating domain which are not rotating.
ps. I know i could hawe curved the turbine blades in a more apropriate direction, but I think its ok for 10min vorth of time that vent into the design.

Guys, I can't even express how helpful you are being :) Thanks.

Urosgrivc, your simulation seems really good and it is exactly what I was looking for. Did you use MRF method? I will use CFX to try, but I am a little bit lost on how to create the rotating frame.
Is it possible to share your file with me?

Thanks again.
Regards,

Yes i have used MRF method.
The simulation works wery nicely now.
of course I can share files :)

This is the link to archive files (17.2 ansys):

https://drive.google.com/open?id=0Bw...Gg5d2RUVXRURHc

Files will be avaliable only for few weeks as I use gdrive for other stuf asveal and this takes 1/2 Gb of space.

Play around with it :)
I dont know if there are any limits around mesh size for student version, if there are, make mesh a bit coarser.
Mesh has inflation layers almost on all surfaces and is quite fine even in areas it wouldnt have to be, I didnt take enough time for meshing.
There is some extra describtion in the note->(green arov in workbench on top of the cfx column)
There is an input (omega) and output (Nm) parameter included so you can change angular velocity from the workbench.

have fun ;)

That sounds perfect. Because of people like you, the world is better hehe :)
I don't think the version will be a problem, I am using 18.0 student version. At least I will be able to look the setup and learn the configs.
So glad!!

Thanks!

Dear Urosgrivc, again, don't even know how to thank you.
I already downloaded the files. I am at work right now, but will look deeper on it tonight. These are really valuable files for me :)
If I have any doubt, I will let you know.

Thank you very much!!

Dear urosgrivc,

I tried to recreate your simulation, following exactly the same steps as you did. Finally I got a result, but I think I didn't understand exactly how to find the Torque generated in the axis. Also, I didn't know how to insert the Output parameter.

As I understand, we set the initial condition to 10 rad s^-1 in the Turbine, and a mass flow rate of 10 kg s^-1 on the inlet... Ok, now I got a result, but what now? Sorry for the beginner questions, as I said, I am starting on CFX.

Attached is a velocity plot of my results, if you want I can send you any other files.

ps: unfortunately, the student version has a limit of 500.000 elements. In any case, I already learnt a lot from your model.
Thank you indeed!!

Your model looks quite nice.

Torque is monitored by an expresion -> torque_axis@location
-axis is eiher x,y,z depends on your coordinate sistem
-location is a 2d surface like turbine surfaces (where you want tomeasure the torque) in my simulation I also added the torque of the shaft.

-Output parameter is there just to help you find the corect angular velocity quicker and more easily as you dont need to open pre or post to change the angular velocity (there is another way so you can change it during solve) or to look at the results.(you ll have to change this parameter till torque is 0 this is your angular velocity at a given mass flow) do this for fev mass flows and you will get yourself a (mass flow/omega graph)
You set the output parameter in cfx post so you do need to run few iterations than open post and under Expressions tab right click on the torque expression and click use as WB output parameter.

-For convergence there is a monitor point so while the solver is solwing you can see a graph of torque when this stops changing the simulation has converged.

I hope that your outlet is not too close to the turbine as this will effect results, If you would put the outlet further away and got diferent results than this is not ok.