|
Rotating a sphere
Hello
I'm trying to apply spinning on a sphere in the air, but I don't know how to do it, I've done two models one in 2D and another in 3D, someone told me it is with the dynamic mesh, but I really don't know how to do it, can someone help? |
Another easier way is using MRF model (Multiple Reference Frame Model). You basically need to define an axisymmetric volume, such as a cylindrical volume to enclosure the sphere.
When you set up the model, you need to define this volume as a MRF zone, giving it an origins and axis vector of rotating. Also, you need to specify the wall of your sphere as a rotating one. This is pretty much of it. Quote:
|
I've done the geometry and mesh in Ansys Workbench, do you apply that MRF model in Fluent? I'm trying to find that option in fluent but I can't find it, in the cell zone conditions there is a option in edit that says motion type, but that one doesn't appear,could you please help me
best regards Quote:
|
I would really appreciate if someone could supply me with a udf model of a rotating sphere
|
you don't have to use a UDF to define the MRF zone.
I don't have a Fluent in hand, so the description may not be accurate. If you are using Fluent6 (i guess not), go to boundary conditions, choose the volume you want to set as a MRF zone. There's a drop box when you set the volume, select the option 'multiple rotating frame', also set the origin of the axis, vector of the axis, and the angular speed. Also, remember to set the sphere wall as a moving wall. Go to boundary conditions, set the wall, select 'moving wall', 'rotating', 'absolute speed', etc. If you are using Fluent 12 (I never used a workbench, but I assume it has Fluent 12 with it), go find you volume in 'cell zones', not in 'boundary conditions'. Do the same thing above. When all conditions are set, just initialize it, and plot a velocity contour on walls to double-check if your setting was right. Quote:
|
Tnhx for the help, the Ansys I'm working is 12.1 and I just have one more question, it's regarding the geometry, I have done 2 diferent types:
First solution: I've done a cylinder defined as fluid with a hollow sphere in it on workbench, and in Fluent I can only define the moving wall in the boundary conditions for the hollow sphere, in the cell zone conditions I only have a fluid zone, my question here is do I use MRF zone on the fluid? Second solution: I've done a cylinder defined as fluid with a frozen sphere in it defined as solid, in Fluent at the cell zone conditions I can define MRF zone on the sphere, but at the boundaty conditions there is one named ball (defined as wall) that when I edit I can't change to moving wall, and when I do the analyses it doesn't recognize the solid as one passes through it I would like to know which solution is the best, and how I can correct the problem in either of the chosen on? best regards |
If you only want to study how the air response to the spinning shpere, I'd suggest to go the first way.
Yes, set the fluid zone as 'moving reference frame'. Go to 'Cell Zone Conditions', click the volume you want to set as MRF, click 'Edit', Set 'Motion Type' as 'Moving Reference Frame', set correct 'Rotation-Axis Origin' and 'Rotaion-Axis Direction'. Initilization. You should be good to go. I'd suggest you quickly go through a FLUENT MRF manual. If it's not available for you, check this, http://jullio.pe.kr/fluent6.1/help/html/ug/node370.htm Also, it will be good if you can check the offical MRF tutorial. Good Luck. Quote:
|
Why not just have a stationary sphere, then set boundary conditions as (rotational) moving wall?
|
I agree, LOL.
MRF probably is not the best model to use here. Quote:
|
Quote:
Quote:
|
What is a Magnus coefficient?
|
Quote:
|
I might misunderstand but isn't it just another word for lift?
Remind, you can actually specify in which sideways direction you want to calculate the lift coefficient. It can be in any direction you want (although it should be perpendicular to the incoming flow). |
Hello
I've done the analysis on the sphere with one option on stationary wall and another with rotation and the results of cl and cd are really close to one each other, I think it's not working... |
Hi, gave it a try in 2D. For my settings I found:
0 rad/s -> cl = -5e-5, cd = 2.7 5 rad/s -> cl = -7, cd = 3.9 Here's a picture of the stream functions: http://img168.imageshack.us/img168/8250/spinc.jpg Does your simulation work for 2D? If you're doing 3D, are the orientations of the axis of rotation and the cl vector correct? |
In 2D, I defined the k-e standard model and defined a inlet velocity of 10 m/s, what was yours? after the iteration my values were:
0 rad/s -> cl = 2.41e-2, cd = 8.9e-1 5 rad/s -> cl = 2.17e-2, cd = 8.9e-1 the cd values were the same, I think something is wrong, I edited the ball (wall) in boundary conditions and put (in wall motion) moving wall with rotational and speed 5 rad/s, I left the rotation-axis origin x-0 y-0, does this influence something? best regards Quote:
|
That is really strange ...
I've copied some of my settings. I am calculating in 2D (but not axisymmetric). My sphere radius is 1 m. My domain is a bit small of course, but it's just a quick start. Some settings: fluid: regular air velocity inlet: 1 m/s outflow boundary sphere: moving wall, rotational, origin x=0 y=0, speed = 5 rad/s, no slip standard k-epsilon, standard wall function for 1st upwind: wall y+ = 50 +/- 10 cd = 3.9 cl = -7 for 2nd upwind: wall y+ = 49 +/- 9 cd = 1.9 cl = -10 It's a first rough attempt, but I can definitily see some lift being generated. I hope this helps |
By the way I'm not sure about the reference area. I think I put it at 1 m, but probably it should be 2m??
|
My radius was 34,5 cm, I have a question where do you apply this:
for 1st upwind: wall y+ = 50 +/- 10 cd = 3.9 cl = -7 for 2nd upwind: wall y+ = 49 +/- 9 cd = 1.9 cl = -10 I got my cl and cd from the last values on iteration window, I applied Second order upwind to momentum, turbulent kinetic energy and turbulent dissipation rate in the spacial discretization Quote:
|
2 Attachment(s)
This how my mesh looks like:
|
4 Attachment(s)
this is what I did, I'll give you some more images on the results
|
4 Attachment(s)
This is the velocity (vector, pathline and contour) and the pressure contour with the inlet velocity=1 and the moving wall=5 rad/s
|
Sorry that was a bit unclear. That part is the results. Where you can set 1st or 2nd upwind under solution.
Anyway, with a rotating wall you should be getting some lift here, one way or the other. You don't by any chance have a 'specified shear' wall? That could explain your results. |
Hi, when I looked at your results again, I saw they actually show a slight asymmetry. This is good news, as it indicates that your moving wall boundary condition is actually at work (assuming you're calculating steady).
I'm not sure about your version of Fluent, but in the Monitor->Forces dialogue, you might want to check that the cl is in the correct direction (probably the y-direction). This might be the answer, since the flow seems unsymmetric but still you don't get any lift. Another thing you might try is to speed up the rotation to, say, 50 rad/s and see what happens? I'm interested what is going on so please let me know if this works, Jack |
5 Attachment(s)
I've checked the axes as shown in the picture and changed it to Y, the force was already 1 in Y, as for the rotation I changed it to 137 rad/s and left the inlet as 1 m/s, cl=-5,75e-3 and cd=2,96e-2, I also put other pics of results
Quote:
|
Hi, it seems your in business now. There is definitely an effect in the velocity and pressure plots, and you are getting lift. The lift might seem a bit small, but it could be ok for this case. As a last check of the mechanism you could reverse the rotation and see if the lift is inverted.
Your residuals are 0.001. May I suggest you lower them to 1e-6? This will lead to nicer convergence of the cd and cl. There should be enough experimental data on rotating cylinders to check your simulation. Good luck! |
I'm just having problems with defining the velocity, in a real situation do you have any ideia about the velocity and angular velocity I should define on the ball? I've tried searching for real values but all I can find is articles with wind tunnels...
Quote:
|
There is some data in:
Sarah Barber, Matt Carre, Soccer Ball Aerodynamics which is a chapter of the book: Martin Peters, Computational Fluid Dynamics for Sport Simulation, Springer-Verlag (2009) |
In this case, when I input rotation to the ball, it's the cl coefficient that's equal to the cs coefficient that's equal to the cm magnus coefficient, right?
Quote:
|
I tried contacting the both of them, only Matt Carre responded, he told me it's very difficult to simulate the airflow around a sphere in CFD and that he wasn't an expert on CFD, I think Sarah Barber is the one that did the simulation part, but she didn't respond, I'm trying now to do the 3D part, my only problem is with the velocity and angular velocity, I know that to have the spin I have to put the angular velocity much higher than the inlet velocity, but I really don't think that the angular velocity of a football in flight can reach 500 rad/s (which is the higher value I had to put for it to show the magnus effect) and that's the main problem I'm having
Quote:
|
Hi, here I have a plot that gives experimental values for a soccer ball. The spin parameter (R omega / u) ranges 0.00 to 0.20. The magnus coefficient is almost linear and coincidentally appears to be roughly as large as the spin parameter, it ranges from 0.00 to 0.22. These are rough values and I haven't really read this chapter so I'm not into the details.
See if this information can get you going. If you want I can send you a copy of the plot tomorrow, I'll have to look for a digital version. Good luck |
where Re=2.1e5
|
Ok I'd really appreciate if you could send me those results, by the way what were the values you used to obtain the spin parameter and magnus coefficient?
Quote:
Quote:
|
Hi, as far as I understand these are experimental values for a scale model soccer ball, from a book I have here. The spin parameter is defined:
radius X angular_velocity / flow_velocity The magnus coefficient is taken from the lift force, measured in the experiment. I will upload the plot tomorrow. I'm afraid it has a reference to yet another reference. So I hope you can find the original data ... |
So the spin parameter was calculated, right? it wasn't input in fluent?tnhx for the help, I'll be awaiting the plot tomorow
Quote:
|
Hi,
There is a lot of information on: http://www.grc.nasa.gov/WWW/K-12/airplane/beach.html Here they have a ideal lift for both the cylinder and the sphere. It's all in lb/ft etc. so beware of the conversion. This might perhaps be a first verification for (low Re?) results. Then, the next step might be some validation. Here, you might also start with low Re (so you could have a Laminar model??). Then there is some very nice experimental data in: B. Oesterlé and T. Bui Dinh, Experiments on the lift of a spinning sphere in a range of intermediate Reynolds numbers, Experiments in Fluids, 1998 For example they have the following plot (gamma is the spin parameter, read article or abstract for definitions): http://img442.imageshack.us/img442/4327/spina.jpg So if you would like you could try to reproduce this plot, by changing Re and spin parameter. For the soccer ball model I'm afraid I don't have a digital image of the plot. Anyway, it accumulates to the following: Re = 2.1e5 spin_parameter = 0.00 - 0.20 cl = 1.1 * spin_parameter (roughly) However this is for a soccer ball which is not really a sphere... Hope this helps, good luck! |
Right now my main difficulties are in the fluent part, where I now see that according to the spin parameter where the range is 0-0,20:
Sp=r*ang_vel/flow_vel If I input a velocity flow of 30 m/s on the inlet for example, what value do I consider on the rotation angular velocity speed of the ball?(I did a conversion by doing v=w.r where w=v/r but I don't think that's right), or can I input a value of Sp in fluent? Quote:
|
ang_vel = flow_vel * Sp / radius
|
I obtained an angular velocity of 17,4 rad/s, considering sp=0,2 and v=30m/s, if I input these velocities on fluent I won't obtain lift, when I input a velocity higher than the angular velocity I can't obtain lift, I tried inputing for example w=500 rad/s and v=12m/s, then I obtained lift but it was just testing
QUOTE=jack1980;257507]ang_vel = flow_vel * Sp / radius[/QUOTE] |
Have you set the direction of the spin vector and lift vector perpendicular?
|
| All times are GMT -4. The time now is 21:13. |