Dear Ali

You can make some sums to check. Considering the air mass flow (from the CFD calculations), the axial variation of the absolute tangential velocity and blade speed, the same values you used to design the stage (at blade mid height, to start with) you may arrive at the power delivered by the turbine. From the power and rotational speed you will find the torque.

This calculated value must be approximately the one resulted from the CFD calculations. If not, please give-me more details about the values you used to design the turbine.

Dear Ali

   I think you can check the approximately power output from wave condition. RPM  very high, you should check tip speed ratio of the turbine as wind turbine.

hi, Ali, it seems there may be some incorrect boundary settings for the turbine blade walls, and in fluent, the rotating wall is relative stationary from the rotating coordinate system, so no need to set -2000rpm. And i also question how about your turbine configuration, and really rotating speed up to 2000rpm? 

You put the boundary condition in a wrong way, specifically as my experience you might put the velocity condition relative to other frames which is not appropriate in MRF. The reason is every rotating frame solve in the absolute boundary condition. So, I suggest to check the velocity condition at each rotatory frame and put the velocity condition in an absolute frame.

I think that flow pattern is not correct and also stagnation point is in pressure side that it is not correct. I found speed in papers and I am sure about value of that, but I am not sure about value of outlet pressure. In the papers, It is not mentioned about value of outlet pressure and just it is mentioned that outlet boundary is given as outlet pressure. This boundary condition is vague in this investigation. What should I do?

I think that outlet pressure is environment pressure eg. atmosphere pressure. Therefore, outlet gauge pressure is zero. Is it correct?

Hi Shrish Shukla ,

I didn't undearstood your statement. in this simulation, I have three boundary conditions such as, velocity inlet and pressure outlet and periodic condition.

what is your exact meaning of velocity condition?

velocity inlet is as follow:

http://0up.ir/do.php?imgf=Captureeeee.png

I am grateful that guide me more about this problem.

http://0up.ir/do.php?imgf=Captureeeee.png

hi, Ali, in the " http://i.stack.imgur.com/O62qx.jpg", i suggest you choose fluid zone and set zero velocity. Because, for rotating frame, the blade,  hub and tip walls of the rotor are all stationary relative to the rotating frame, i.e. the rotor zone here. 

H Qi-hua Zhang ,

Thanks your answer,

I will perform your suggestions. But I have some questions:

what is set up of other cases? such as casing in rotary domain, casing in stationary domain, hub in stationary domain. I set as follow:

casing in rotary domain:

relative rotational velocity of 209.43 ,in +y vector direction.

casing in stationary domain:

absolute velocity of zero,in +y vector direction.

hub in stationary domain:

absolute velocity of 209.43, in the +y vector direction.

According to your statement:

Blade and hub in rotary domain are stationary wall.

Is these set up correct?

Thanks,

hi, Ali, for any boundary wall belonging to stationary parts, the no-slip boundary is proper, because they are in the stationary frame, and for any boundary wall geometrically belonging to the stationary parts, and meanwhile adjacent to the rotor zone, setting the relative counter-rotating velocity , i.e., -209.43 is proper. 

Thanks your answer,

My English language is not good.

What is your exact meaning of " geometrically" in your statement?

what is difference between"boundary wall belonging to stationary parts" and boundary wall geometrically belonging to the stationary parts?

hi, Ali, there is not big difference, geometrically i mean this wall is physically belonging to a part, not any furthermore meaning, so if the wall is adjacent to stationary and rotor part, you will take more attentions to set its boundary condition.

Thanks your answer Qi-hua Zhang,

Therefore I set as follow:

1. blade and tip blade and hub surfaces(hub surfaces in rotary and stationary domain):

No slip wall conditions eg. stationary wall

2. casing in rotary domain:

relative to adjacent cell zone-rotational velocity 209.43 rad/s

3. casing in stationary domain:

No slip wall conditions eg. stationary wall

4. Zone rotary:

moving reference frame

relative to cell zone: fluid zone

Rotational velocity: zero

5. fluid zone adjacent rotary zone:

moving reference frame

relative to cell zone: absolute

negative rotational velocity eg. -209.43 rad/s

Are these set up good?

I studied a paper. The following sentences is mentioned in this paper as follow:

"The angular rotation of the turbine had been modelled by

applying a negative rotation to the fluid zone, with the

blade surfaces stationary. The relative rotation of the blade

and outer casing was then modelled by setting the outer

casing to have a rotation of zero relative to the fluid zone."

But here, I have two fluid zone eg. rotary zone and stationary zone after and before blade.

I don't understand above sentences in this paper!!

I am grateful that guide me more

Hi Qi-hua Zhang ,

You said the following sentence:

"hi, Ali, in the " http://i.stack.imgur.com/O62qx.jpg", i suggest you choose fluid zone and set zero velocity."

Next your sentence is right.

Now, I have question:

Is Zero velocity  for rotary domain or stationary domain??

Totally, a domain should rotate!! i think that rotary domain should be rotate.

I don't understand this your above statement.

I am grateful that guide me more.

hi, Ali, to make through this problem, you should first understand the mathematical or physical meaning of rotating reference frame and the corresponding equations there. for simplicity, assuming you are located within the turbine channel and rotating with the rotor, just as Abdul said, you will not feel the rotation, and in this situation, it is same as the stationary duct flow, so the no-slip boundary condition is proper and it is simply zero relative velocity.

Why you do not try a simpler problem to better understand the physics. I suggest that you use the approach of the paper DOI: 10.1016/j.energy.2012.07.042 . After you have these results you can start by improving you solution. Beware not have an incidence angle above stall! In this condition, the Wells turbine has a very low torque. 

http://www.sciencedirect.com/science/article/pii/S0360544212005919

Hi, Qi-hua Zhang, Thanks for allocating your time

I understand your statement and my  mentioned method in page 1 of this topic is according your statement. but exactly i don't know  that how to set about the following link:

http://i.stack.imgur.com/O62qx.jpg

In fact, i don't know set up of stationary domain exactly. 

I performed many attempts in order to set this simulation such as one is in one page of this topic. it should be solved in this mentioned method, but it is not solved!!! why??

in my calculation, torque coefficient and total pressure drop are lower than experiment, but efficiency is very high than experiment. The value of efficiency is higher than 1!!!

http://i.stack.imgur.com/TN5Fl.jpg

.............................................................................................

Today I studied a tutorial and Fluent help. I think that i should use mixing plane interface between stationary and rotary domain. Am I right?

Should i use mixing plane interface in this case?

I am grateful that guide me about this problem.

Thanks,

http://i.stack.imgur.com/O62qx.jpg

hi, Ali, yes, you should use the mixing plane in Fluent, because it is suitable for the treatment of interfaces between rotating and stationary zones. i think for "http://i.stack.imgur.com/O62qx.jpg", the tip should rotate in the counter-rotation direction of the impeller when you see from the impeller, and  you will can choose relative to the fluid zone, and rotating speed is negative relative to the rotor, i think this may help you out there.

Hi, really thanks your answer Qi-hua Zhang

I think that another its reason can be due to  steady-state analysis because this simulation is steady state.

Please see figures of page 1, large separation and incorrect flow pattern and incorrect value of efficiency can be due to this case(not creating mixing plane). Am I right?

Well, Now i should learn about mixing plane interface!! According Fluent help, I think that setup of mixing plane is difficult, particularly for applying boundary conditions of mixing plane...If it is possible, please share useful links about mixing plane interfaces.

About "http://i.stack.imgur.com/O62qx.jpg", I think that your means is Casing. Am I right? please see the following figure:

http://i.stack.imgur.com/ekV0j.jpg

casing is stationary therefore, casing(in rotary domain) should rotate negative direction relative to rotor(rotary domain) and also blade should rotate relative to rotary domain with zero rotational velocity eg. Moving wall-relative to adjacent cell zone- rotational velocity=0

I already had created two zone in rotary domain eg. rotary_tip and rotary zone

Rotary _tip zone was a region between tip and casing. Rotary  zone was a region between hub and tip!!...but now, only A rotary zone have created between hub and tip.

But still about hub and casing in stationary domain, I have not exact information.

However, thanks for your guidance.

Use just the rotating reference frame and a steady-state. Assume that the blades, the hub and the shroud are rotating walls. At inlet, impose the stagnation pressure and a velocity computed in such way that you respect the radial equilibrium $\partial p / \partial r = \rho V_t^2/R$. At exit, impose the static pressure at the hub (the radial equilibrium is used to compute the pressure along R).

Using this results, you easily compare with the data you have from present results. If was not clear ask me for details.

Moreover, using this approach you can estimate the losses arising from the tip gap and the rotating hub.

hi, Ali, i think you are not clear about how to treat the tip clearance region. so here, i give my suggestions as follows, if you are doing engineering simulations, i.e. for routine running and hope low computational cost, you can take the tip clearance region into the rotor region, so just a single rotor region including all rotor walls, and all rotor walls are all  0 speed relative to the rotor zone, and the outer annulus endwall of the rotor is relative -209 to the rotor zone, so this way is economical, simple and very efficient. hope this will guide you out there.

Hi ali

I had a similar experience

Please check the coordinate axes that rotates turbines around which