[arashn18]

Hi
I want to analyse a simple vertical wind turbine (savonius) using CFX.
The model is in a wind tunnel and I am using K-omega turbulent model (I've tried SST too) and I have defined the turbine as a new domain in Ansys desighn modeler and subtracted it from the wind tunnel. Then I defined this domain as a rotating domain in CFX.
I've tried different TSR, wind speed, rotating speed, model size, mesh size and etc but my result never get converged and doesn't reach for a steady amount of torque.

could somebody help me??
here are some picture of my analyse:
p.s. the user point 1 is torque of wind turbine.
https://ibb.co/bWL6bQ
https://ibb.co/bMJEVk
https://ibb.co/gWi3O5
https://ibb.co/njzMAk

[ghorrocks]

Something is very wrong with your simulation. Can you post some images of velocity vectors at the turbine? And some images of your mesh, and your CCL would be good.

[urosgrivc]

You dont actualy need the solid domain, do you?
are you going to do any structural or thermal coupled simulation?

Why is it transient, what is transient in this case (you only have one fluid domain am I wright?)

Is it a rotating domain or what?

Your problem seems totaly simetric in 2 directions

Where is the outlet?

You should definitly initialize this kind of problem vith a static solution.

Either i dont have enough data on what you are triing to do or a lot of things are wrong. Have you done any simpler cases before this one?

[arashn18]

vectors:
https://ibb.co/eM4ALk
https://ibb.co/hWygRQ
mesh:
https://ibb.co/bxfH0k
https://ibb.co/kSysY5
ccl:
https://ufile.io/9ndi1

[arashn18]

Originally Posted by urosgrivc

You dont actualy need the solid domain, do you?
are you going to do any structural or thermal coupled simulation?

No I don't but I used the solid domain to make the turbine as a rotating domain

Originally Posted by urosgrivc

Why is it transient, what is transient in this case (you only have one fluid domain am I wright?)

No it is steady.
yes I have one fluid domain

Originally Posted by urosgrivc

Is it a rotating domain or what?

the solid domain is rotating but the fluid domain is stationary.

Originally Posted by urosgrivc

Your problem seems totaly simetric in 2 directions

I think it is symmetric in one direction (z axis) but i didnt use the symmetric BC

Originally Posted by urosgrivc

Where is the outlet?

Damn!!!!!!!!!!!! I've defined the "out" BC as inlet!!!
What a fool I am... I am working on this project for 2 months ((
now that i correct my BC, my solution is getting converged but it has the efficiency of 30% which is not correct. the expected efficiency for this kind of wind turbine is 0.15.

Originally Posted by urosgrivc

You should definitly initialize this kind of problem vith a static solution.

how to obtain the static solution??

Originally Posted by urosgrivc

Either i dont have enough data on what you are triing to do or a lot of things are wrong. Have you done any simpler cases before this one?

no i just figured this solution out by myself. do you have any similar cases??
i have read the cfx's tuturials too but there was not any similar one.


what else do you think that is incorrect???

[ghorrocks]

You do not need the solid domain. Have a look at the rotating machinery tutorials for how to model rotating machinery. The axial rotor stator models are relevant here.

the solid domain is rotating but the fluid domain is stationary.

It does not work that way - this explains why your simulation is seriously wrong. You will need a stationary and a rotating fluid domain. No solid domains.

[urosgrivc]

Hi Arashn18

This guy had a similar problem about a year ago:
Rotating two impellers in water tank
The diference is that he had two propelers and you have one but as I remember it is a similar thing.
he also had problems vith a rotating domain part, read the post.


I thought that you were doing it transient that is why I suggested the static inicialization, but since you are doing a stationary problem that is not relevant.

[arashn18]

Thank you for ur answers... I really appreciate it

I have fixed my simulation as you told me
now i have defined 2 fluid domains:
*one is a cylinder with a turbine inside it which is rotating
*the other one is stationary cube that the cylinder is inside it.
i've defined the interface as frozen rotor and no pitch change. (I've got errors with other option of pitch change) and mesh connection of GGI.

my simulation seems much much better. now my answers got converged and it is totally mesh independent.
but i haven't got any correct torque on the blades. The torque on blades across z coordinate was negative which I think is unreasonable and its value doesn't match with experiment data.

Do you have any idea about it???

[ghorrocks]

The torque your simulation is giving is the torque at that location in rotation of the device. I suspect this device will have a very uneven torque as it rotates, so to get an average torque to compare to experimental results you are going to have to model a range of rotation angles and average across them.

[arashn18]

I have modeled the turbine in several rotation angles and all the torques that i got was negative. also the shape of the torque-angle diagram was not correct too.
the first diagram is my diagram and the second one is a experimental diagram.

there is something seriously wrong in my simulation. please help me

p.s. when i turned off the rotational domain and made it stationary, my torque value became positive!!!!!!!!!

[ghorrocks]

Please label the axes of your graphs in future. I don't want to guess what the data means.

Have you read the basic FAQ on accuracy: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

A key part of this is to have a think about your assumptions. Is the assumptions of frozen rotor appropriate? Turbulence model? Inlet condition? There are many many things to check.

[urosgrivc]

If your torque is based on the coordinate sistem that is seen in the picture abbove than I dont know where the problem is. (check if your reference coordinate sistem is in the wright spot?)
Just turn your graph upside dovn (*(-1)) isn`t it so .

And jou could inprove the outer domain by increesing the distance from the rotating domain to the outlet. (did you get any (a wall has been placed on the portion of the outlet etrors)in the solver?)

Is this turbine located in a closed shaft or out in the open in real life? If it is out in the open than I wouldnt use stationary wall as you did and this is seen from the velocity plot, I would use moving wall (vind speed) or oppening.

And do you have angular velocity for rotating domain in your simulation? if yes than it is probably incorect as the graph says static torque as I imagine this is probably ment that the turbine was not rotating while torque measurments were taken.

[arashn18]

what you are saying is completely correct. there are several problems in my simulation which i should correct and improve my results' accuracy.
thank you

[arashn18]

Hi guys

Do you know why there is a sharp velocity difference at the interface of rotating domain and stationary domain??? look at the velocity contour in attachments
it would be more difference as i increase the rotating speed

[ghorrocks]

FAQ: https://www.cfd-online.com/Wiki/Ansy...f_reference.3F

[urosgrivc]

Try ploting vectors in (velocity in stationary frame)

This velocity plot caries Omega*R velocity vith it so rotating gomain has combined values (rotating component and stationary one)

You are able to see that on your left side of rotating domain velociti increeses with radious and on the right side it gets cancled out by the onflowing fluid.