I would like to study the flow of air in a rotating turbine. The goal is to create an air flow from the bottom by rotating the turbine at 15.000 rad/s.
I am using Floworks 2009 for the first time for this project.
So, before working on the real turbine model I made several tests on a very simple form of the turbine in order to choose the best way to simulate it,
since there are different ways to add a rotation on a model.
I made some tutorials to put the turbine in rotation in order to see how the air flows, but from all the tests I had very different views of the flow
So far, I could see that there are 6 different ways of modelisation:
Using a Global Rotation, a Rotating Region or Moving Walls with an Internal or an External analysis.
So, I would like to know which one is the best solution to observe the aspiration of my turbine.
Here are the screens I made for each method, with some explanations about my choices (all the examples following were made with a -20 rad/s rotating speed):
1) Global Rotating - External
There is only the turbine in its computational domain (the lid is disabled: I used it to have a reference for flow trajectories).
2) Global Rotating - Internal
There are the turbine and a lid (with atmospheric pressure boundary condition).
3) Moving Wall - External:
I selected all the walls of the turbine and I made them rotating with Real Wall Boundary Condition.
4) Moving Wall - Internal:
I selected all the walls of the turbine and I made them rotating with Real Wall Boundary Condition again. The lid is set with atmospheric pressure boundary condition.
5) Rotating Region - External:
There are the turbine and its rotating region which cover all the turbine.
6) Rotating Region - Internal:
There are the turbine and its rotating region which cover all the turbine. Both of them are surrended by a lid with atmospheric pressure boundary condition.
As you can see there are many differences among the results, depending of the method used. Which one would you think is the best to simulate our case,
considering that the rotating speed is around 15.000 rad/s ?
Thank you for replying.
I am new in Gambit and I want to create a geometry of a stirred tank: I have the geometry of the tank, and the blades.
How can created?:mad:
@anamariaM: I think you are in the wrong forum, this is not a Gambit user forum.
@Naith: There are only two ways of doing such an analysis. Global and Local. The rotating wall is a boundary condition (BC) for surfaces. this BC only applies to surfaces and will give them the corresponding velocity profile for the surface of a rotating surface. The same goes to the stator surface. It simply says the velocity profile towards the surface goes to 0 m/s if the surface happens to be in the rotating region.
Ok here a little closer to your tests:
1) This works if you have no large assembly around your turbine that cannot be applied stator wall to. Imagine a wind turbine without the beam on which it is mounted.
2) This is the same as 1) but for internal cases. Imagine a flow metering system in a pipe. simply everything is rotating and you'll define the pipe walls as stator since they are not rotating in reality
3) As mentioned not applicable for turbines of any case. This would apply to a zylinder or ball that is rotating and therefore driving the flow but not for anything that has extremeties such as blades or ribs.
4) same as 3)
5) This case you can apply to a wind turbine with beam where the rotating region is not covering the beam. with that the influence of the beam can be considered.
6) the same as 5) just for internal cases.
In general the difference between local and global is I think clear and it is especially used depeding on the whole geometry. As long as everything (except the turbine or fan, or rotor in general) is rotational symmetric such as cylinders or spheres it works perfectly and you can apply stator walls to these rotational symmetric walls that are stators. As soon as you have several rotors that either not on the same axis or counter rotating you will have to use local rotation.
If you look closer on the results of 6) and 2) you'll see they are very similar and I would say the slight difference is due to the interpolation on the rotating region interface and probably the mesh.
Also 1) and 5) do look very similar. In general you should use a larger domain for external calculations since the computational domains walls can have an influence on the results if they are too close.
Also a better way to define a rotating region is shown in the attached image of one of your results. Use the rotating region as marked in red and apply for surfaces that are rotational symmetric the moving wall BC to reduce the computational needs that the rotatinal region causes. Always condsider to use a minimum of 3 cells between rotor walls and the rotating region walls and from rotating region walls to stator wals. with that you will also understand why I suggest changing the rotational region inside the rotor and use the moving wall BC on the rest of the surfaces. You'll save minimum 3 cells in 360° which will also benefit in calculation time.
For the question if local or global either decide from what I mentioned above or I would have to see your model to give you a better suggestion.
I hope this was useful.
Thanks a lot for you reply, it is really useful. Concerning my model, I will use a Global rotation in an external analysis, which seems to be the best way, according to your message (since I don't have any stationary part), and to the tests I made on the real assembly.
By the way, I've got another question : after simulating with these parameters, most of the flow trajectories seem ok, except that they are going through the blades, as you can see on the images attached. I don't think it's because of the mesh, since I'm using a customized one, very accurate.
So I'm wondering : is that only a "visual" representation, due to the fact we are studying in a rotating coordinate system (making the flow leaving the turbine in a rotating trajectory), or is it a bug of any kind ? And if it's the first case, is there a way to prevent it ?
Thanks again for replying.
Thank you very much for help:)
this is not a bug. Since we work in a rotating reference frame (RRF) and nothing is actually "moving" from the geometry side, the flow trajectories are shown as if the turbine is moving so fast you just see a blur. If you would now bring particles into the flow, you would also see the same flow as the trajectories show you. It's just that the geometry is not moving but the flow would look like this. So as you said, it's the first point you mentioned. You can switch the settings of the trajectories from relative to rotating frame to change how they are seen, so from which reference frame.
In any case the real trajectories look like this. You can reduce the effect by using an animation where you let the turbine rotate too with the capabilities of SolidWorks to move the geometry and use the trajectories as arrows and maybe pulse them if the whole thing is for nice pictures and animation but in reality it is important to consider the flow as it is and that's what is shown to you.
Does that help?
Yes, thank you, once again it helps a lot.
I've got another question:
I would like to simulate an aspiration device which sucks the air above the turbine. In fact it's like a vacuum.
I know that the pressure drop is around 5pa to create this aspiration so i would like to create a pressure drop between the top and the bottom of a plate.
I don't understand the difference among static pressure and total pressure so I don't know what is the best way to do it?
Thanks for help.
The difference between static and total pressure is the pressure due to velocity or stagnation pressure. Basically total pressure Pt contains the static pressure Ps, potential pressure Ph (due to the difference in hight) and stagnation pressure q:
Environment pressure is not really the pressure of the environement (1atm) it destinguishes the static pressure if the flow leaves the volume trough the opening or total pressure if it enters the volume. so the value you enter here is either static or total pressure depending on the direction of the flow.
Does this help?
It finally worked with the pressure drop method. Sorry for the late replying, the project I was working on has now ended, your replies were really helpful all along, thanks for help.
i am using shipflow to model an amphibious tank.
i have made the model in SHIPFLOW design,
i made a reference plane and then i tried to generate a section group.
the section group is not being created.
it is giving the following error.
'INFO section calculation failure [boundary coincidence]' :confused:
someone please help me in this matter.
thank u very much:)
I was having the same problem (like Naith), and I read all u had replied. It was really handy, thanks.
but I have a question:
when we are talking about turbine, then the rotating shaft speed is an output. so we can not put an amount as an input. Indeed I have a case in which I have to determine amount of power generated by the turbine knowing that inlet pressure and its temperature. How can I say to (solidworks) that my turbine blades are "rotating regions" while I dunno its speed (beacuase it asks me)?
Thanks a lot.
Yes, you would want a fluid driven motion in a turbine case for a fan you have a motion driven fluid flow. FlowSimulation/FloEFD is not directly capable of letting the fluid drive the turbine. How ever ther is a workaround for something like that. You can use a parameterstudy for that. Basically you define a parameter that can be altered by the software between two values, in your case the RPM for example between 500 and 20,000 RPM (the value you are looking for has to be in this range) and then define a goal dependency for example an equation that has to fit be fullfilled. For example a maximum torque of your generator or something like that. Now when you start the parameterstudy the software does iterate to the value for which the goal you set has the best fit.
As an simple example:
Imagine a valve with a ball or plate sitting on a spring and depending on the force on the ball or plate the it is moving until it found its equilibrium. In that case the value you want to change is the distance of the ball to simulate the spring movement. The dependency is the spring equation with the spring constant. FlowSimulation/FloEFD now calculates the first simulation with for example 2mm spring deflection and then the maximum with 15mm deflection. Vor 2mm it would be 5N fluid and 2N spring force corresponding to the spring equation and for 15mm 40N fluid and 80N spring force. In the 2mm case the fluid is stronger so the spring would move further back in the 15mm case the fluid is to weak so the spring would move further to the front so the value must be bewtween the minimum and maximum vlaue and is now trying to itereate to this position with a maximum iteration number and a defined goal accuracy since it is hard to hit the exact value you would define a little margin.
I hope this helps,
Contra rotating rotor simulation using mixing plane method
I am trying to simulate flow around Contra rotating rotor using mixing plane method. I have some doubt in defining boundary condition on rotor blade.
I defined Front rotor and Second rotor as Stationary wall.
Front rotor is rotating in Counter clock wise direction (according to Right hand thumb rule). So i define the fluid in the Front rotor region as Moving reference frame which rotates about X- axis (1 0 0) at -1800 rpm (negative sign for Counter clockwise direction), Relative to Cell zone:- absolute.
The second rotor rotates in opposite to that of Firs rotor about X-axis (1 0 0) at 1800 rpm (Positive sign for clockwise direction). relative to cell zone: Opposite to front rotor Fluid
When I check the Relative velocity vector, The Direction of the relative vector for the front rotor is along Counter Clockwise direction which is wrong ( it should be in clock wise direction because of the fact that the blade rotates in counter clock wise direction) but the relative velocity vector for the second rotor looks perfect.
Please can someone help me to define the proper boundary condition.
thanks in advance for your information,
First, do not define the rotor surfaces as stator as they are rotors not stators.
Second, if you modeled the rotating region and apply a rotation region boundary condition to it, you should while the boundary condition window is open an arrow showing the direction for your right hand rule, just to make sure that is correct. If you cannot see it, try to hide the geometry as it might cover the arrow.
Let me know if that works.
Other than that it depends when you look on the results. It can happen that the flow is fowing in the wrong direction at some point in the beginning but should be right towards the end of the convergence process. Sometimes you really have to let it calculate for a while to let the flow adjust.
Hi Boris Marovic,
"do not define the rotor surfaces as stator as they are rotors not stators"
Do you mean that I need to set rotor surface as a moving wall.
I thought that, For a rotating reference frame, FLUENT assumes by default that walls rotate with the grid, and hence are moving with respect to the stationary (absolute) reference frame. Since the rotor is rotating, I defined rotor as a stationary wall. But I am not sure whether it is correct or not.
Could you please correct me.
Ok, since you mentioned Fluent, you might be in the wrong forum. This part is for FloEFD, FloWorks (now Flow Simulation) & FloTHERM, not Fluent.
Discontinuity at rotating region boundary
I'm new to CFD analysis and I was wondering if the velocity discontinuity found at the rotating region boundary is expected. Is it due to the mesh. In the image attached by Boris_M, we see abrupt colore change between the rotating region and the free fluid.
The image was originally not from me, I just marked the red box to show a better rotating region. I have no idea how coars the mesh is and it can come from the mesh. Usually there is also a boundary condition interface that can cause some diffusion in the interface between rotating and non rotating region.
|All times are GMT -4. The time now is 05:09.|