CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Rotating a sphere

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   April 16, 2010, 06:12
Default Rotating a sphere
  #1
New Member
 
Rick
Join Date: Mar 2010
Posts: 27
Rep Power: 7
RiKR0K is on a distinguished road
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?

Last edited by RiKR0K; April 16, 2010 at 08:33.
RiKR0K is offline   Reply With Quote

Old   April 16, 2010, 11:26
Default
  #2
New Member
 
Ling
Join Date: Jun 2009
Posts: 25
Rep Power: 8
nstar is on a distinguished road
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:
Originally Posted by RiKR0K View Post
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?
nstar is offline   Reply With Quote

Old   April 16, 2010, 14:29
Default
  #3
New Member
 
Rick
Join Date: Mar 2010
Posts: 27
Rep Power: 7
RiKR0K is on a distinguished road
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:
Originally Posted by nstar View Post
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.
RiKR0K is offline   Reply With Quote

Old   April 27, 2010, 11:38
Default
  #4
New Member
 
Rick
Join Date: Mar 2010
Posts: 27
Rep Power: 7
RiKR0K is on a distinguished road
I would really appreciate if someone could supply me with a udf model of a rotating sphere
RiKR0K is offline   Reply With Quote

Old   April 27, 2010, 22:57
Default
  #5
New Member
 
Ling
Join Date: Jun 2009
Posts: 25
Rep Power: 8
nstar is on a distinguished road
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:
Originally Posted by RiKR0K View Post
I would really appreciate if someone could supply me with a udf model of a rotating sphere
nstar is offline   Reply With Quote

Old   April 28, 2010, 06:37
Default
  #6
New Member
 
Rick
Join Date: Mar 2010
Posts: 27
Rep Power: 7
RiKR0K is on a distinguished road
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
RiKR0K is offline   Reply With Quote

Old   April 28, 2010, 10:47
Default
  #7
New Member
 
Ling
Join Date: Jun 2009
Posts: 25
Rep Power: 8
nstar is on a distinguished road
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:
Originally Posted by RiKR0K View Post
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
nstar is offline   Reply With Quote

Old   April 28, 2010, 11:15
Default
  #8
Senior Member
 
Jouke de Baar
Join Date: Oct 2009
Posts: 125
Rep Power: 8
jack1980 is on a distinguished road
Why not just have a stationary sphere, then set boundary conditions as (rotational) moving wall?
jack1980 is offline   Reply With Quote

Old   April 28, 2010, 11:17
Default
  #9
New Member
 
Ling
Join Date: Jun 2009
Posts: 25
Rep Power: 8
nstar is on a distinguished road
I agree, LOL.
MRF probably is not the best model to use here.

Quote:
Originally Posted by jack1980 View Post
Why not just have a stationary sphere, then set boundary conditions as (rotational) moving wall?
nstar is offline   Reply With Quote

Old   April 28, 2010, 11:46
Default
  #10
New Member
 
Rick
Join Date: Mar 2010
Posts: 27
Rep Power: 7
RiKR0K is on a distinguished road
Quote:
Originally Posted by nstar View Post
I agree, LOL.
MRF probably is not the best model to use here.
Quote:
Originally Posted by jack1980 View Post
Why not just have a stationary sphere, then set boundary conditions as (rotational) moving wall?
I left the cell zone conditions of the fluid as stationary and at the boundary conditions I changed the hollow sphere to moving wall and added rotation, I just have another question, in the monitors section I can plot the cl (lift coefficient) and cd (drag coefficient), how can I plot the cs (spinning coefficient or magnus coefficient)?
RiKR0K is offline   Reply With Quote

Old   April 28, 2010, 12:05
Default
  #11
Senior Member
 
Jouke de Baar
Join Date: Oct 2009
Posts: 125
Rep Power: 8
jack1980 is on a distinguished road
What is a Magnus coefficient?
jack1980 is offline   Reply With Quote

Old   April 28, 2010, 12:12
Default
  #12
New Member
 
Rick
Join Date: Mar 2010
Posts: 27
Rep Power: 7
RiKR0K is on a distinguished road
Quote:
Originally Posted by jack1980 View Post
What is a Magnus coefficient?
It's the effect of the spin you shoot a ball elsewhere the center, it's also called the sideways coefficient
RiKR0K is offline   Reply With Quote

Old   April 28, 2010, 12:23
Default
  #13
Senior Member
 
Jouke de Baar
Join Date: Oct 2009
Posts: 125
Rep Power: 8
jack1980 is on a distinguished road
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).
jack1980 is offline   Reply With Quote

Old   April 29, 2010, 13:59
Default
  #14
New Member
 
Rick
Join Date: Mar 2010
Posts: 27
Rep Power: 7
RiKR0K is on a distinguished road
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...
RiKR0K is offline   Reply With Quote

Old   April 29, 2010, 16:09
Default
  #15
Senior Member
 
Jouke de Baar
Join Date: Oct 2009
Posts: 125
Rep Power: 8
jack1980 is on a distinguished road
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:



Does your simulation work for 2D?

If you're doing 3D, are the orientations of the axis of rotation and the cl vector correct?
jack1980 is offline   Reply With Quote

Old   April 30, 2010, 05:51
Default
  #16
New Member
 
Rick
Join Date: Mar 2010
Posts: 27
Rep Power: 7
RiKR0K is on a distinguished road
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:
Originally Posted by jack1980 View Post
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:



Does your simulation work for 2D?

If you're doing 3D, are the orientations of the axis of rotation and the cl vector correct?

Last edited by RiKR0K; April 30, 2010 at 06:43.
RiKR0K is offline   Reply With Quote

Old   April 30, 2010, 07:44
Default
  #17
Senior Member
 
Jouke de Baar
Join Date: Oct 2009
Posts: 125
Rep Power: 8
jack1980 is on a distinguished road
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
jack1980 is offline   Reply With Quote

Old   April 30, 2010, 07:47
Default
  #18
Senior Member
 
Jouke de Baar
Join Date: Oct 2009
Posts: 125
Rep Power: 8
jack1980 is on a distinguished road
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??
jack1980 is offline   Reply With Quote

Old   April 30, 2010, 08:00
Default
  #19
New Member
 
Rick
Join Date: Mar 2010
Posts: 27
Rep Power: 7
RiKR0K is on a distinguished road
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:
Originally Posted by jack1980 View Post
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
RiKR0K is offline   Reply With Quote

Old   April 30, 2010, 08:34
Default
  #20
New Member
 
Rick
Join Date: Mar 2010
Posts: 27
Rep Power: 7
RiKR0K is on a distinguished road
This how my mesh looks like:
Attached Images
File Type: jpg mesh.jpg (69.7 KB, 46 views)
File Type: jpg meshzoom.jpg (36.4 KB, 39 views)
RiKR0K is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
rotating sphere boundary conditions franzisko OpenFOAM 3 October 5, 2009 07:08
Flow over rotating sphere csmistry CFX 3 August 11, 2009 19:07
udf for rotating sphere lisa FLUENT 0 March 25, 2006 15:58
help in udf regarding a rotating sphere rakesh FLUENT 0 March 23, 2006 13:11
meshing F1 front wing Steve FLUENT 0 April 17, 2003 12:37


All times are GMT -4. The time now is 10:44.