# Using CEL to make a 'flap' move

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

 October 11, 2010, 11:06 Using CEL to make a 'flap' move #1 New Member   James Join Date: Jul 2010 Posts: 25 Rep Power: 9 Dear all I am new to cfx, and am currently learning the tutorials etc, and have a question regarding how exactly how cel works, and how i could use functions written in the expression language. As part of my phd research, i am working on a vertical axis turbine, but the fluid is allowed to move the flaps (or blades) i.e consider it a rigid plate that is pin jointed at one end. Depending on the position of the flap the fluid will hit it, and rotate it, and this is what i need to model. (also analogous to model a door being blown by the wind- I want to know how much it would move) Many people have advised me that a cfx could do this, and I would need to write this in cel, the basically methodology iv been advised on is that the pressure on either side of the flap can be calculated and thus a resultant force. this can be then linked to a rotation on the flap. this is great but I still have a couple of questions... in terms of relating the movement would you use the relationship of centripetal force to angular velocity, ie F=m*r*Omega^2? or alternatively would you equate the kinect energy of the flap to the work done of the flap moving?? if this was the case can the function calculate the resultant force, and return the angular velocity of the flap, would cfx then automatically give the flap this angular velocity and therefore move it? or would you have to then tell it to move the calculated displacement? also does a function perform its calculation once every timestep, or for every iteration, or can you set that?? If someone could breifly explain what cfx does, and if you think the above solution strategy is valid/invalid, please feel free to comment, because as well as working out what i need to learn in cfd im a little unsure of exactly how i can calculate the magnitude of this movement. If anyone has any other suggestions or ideas of how this can be done im all ears, your help is appreciated!! Many thanks James

 October 11, 2010, 17:09 #2 Senior Member   Edmund Singer P.E. Join Date: Aug 2010 Location: Minneapolis, MN Posts: 512 Rep Power: 14 James: There are a few ways you can do this within CFX, and one major consideration is whether you are going to have mesh failure as a result of the movement. Assuming no mesh failure, you can either use the 6-DOF beta feature (make sure you don't use a user defined coordinate that is not inline with the global due to a bug in the 6DOF model), or you can use cel to move the walls (generate the mesh motion) for you. If you use the 6-DOF model (you would only need 1-DOF rotation I assume), then you can set the motion update to every coefficient loop. If you use CEL, then the motion will get updated every timestep. With the 6-DOF, you only need to specify the walls that you want to use to generate the torque for the rotation, input the flap characteristics (i.e. I and m), and the code does the rest. With CEL, you will need to query the walls and add up the torque, write the rotational equation of motion, and apply that as mesh motion on the walls. I suggest you start with something simpler, perhaps linear motion in line with a global coord.

 October 11, 2010, 18:04 #3 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,202 Rep Power: 110 If you are going to use 6DOF then have a look at the preview version of CFX V13. It has a major rejig of 6DOF and so will hopefully be better and easier to use. Also as it is in beta if you find bugs you should be able to get them fixed!

October 12, 2010, 09:31
#4
New Member

James
Join Date: Jul 2010
Posts: 25
Rep Power: 9
Hi Both, thanks for your replies

I was speaking to someone a couple of weeks ago after you (Glenn) recommended the 6-dof solver. They said that the 6 dof wouldnt work inside a rotating domain, so I wouldnt be able to use it for my problem. I have attached a jpeg of the kind of thing I am trying to model. What I have been advised to do is have a larger outer mesh that is static (to represent say the dimensions of a flume), and inside a rotating mesh. for the moving flaps I would then have a series of subdomains of dynamic mesh, to allow the movement. With this in mind do you think that the 6dof couldnt be used? and therefore would you recomend using cel to write in the flaps motion? I have just sent this question to the guys at ansys as well to get their opinion on it, and will let everyone here know their feedback, if anyone has a similar problem in the future.

if you have any other suggestions im all ears!

Thanks very much for your time

James
Attached Images
 Turbine.jpg (48.8 KB, 25 views)

 October 12, 2010, 09:48 #5 Senior Member   Edmund Singer P.E. Join Date: Aug 2010 Location: Minneapolis, MN Posts: 512 Rep Power: 14 James: Are you modeling the structure or just the flaps? Putting the structure in will complicate things quite a bit. I assume that you are turning the structure with a set (prescribed) omega? If not, this thing will just align with the flow and not much of interest will happen. If you are not using a version higher than CFX V13 P2, you might not be able to use the 6-DOF solver if you model more than one flap. Prior versions require you to use the global coordinate system as the 6-DOF reference in order for it to work correctly. This would require a translation of ICs and I into the global for each flap (since you wont be able to create an axis around each hinge point). That can get quite messy. Without the structure, you can put small cylinders around each flap, and rotate that entire cyclinder according to CEL. This can be contained within a large cylinder for the rotating structure, controlled by CEL (or constant omega which I suspect is your case). This is then contained in the large static domain. Ed

 October 12, 2010, 10:41 #6 New Member   James Join Date: Jul 2010 Posts: 25 Rep Power: 9 Hi Ed The structure doesnt need to be there in the model, as long as the flaps rotation can be restricted to 180degrees. the idea is that I shouldnt have to put an angular velocity in, the turbine is a drag type turbine, and the way the turbine works is that if you are facing into the flow, the flaps on one side will get pushed shut and spin the turbine round, as the flaps on the other side are open, so the drag is dramatically reduced. for the ease of modellng however I was intending to first model it with a fixed angular velocity, and hope to in the future develop it to rotate on its own accord. i dont have cfx 13, i am currently on a trial academic license of v12.1, although we are about to purchase the full academic package, with this i should get the update to version 13 in november when its released. do you know if v13 will allow for creating an axis around each hinge point/ make this possible at all? ""Without the structure, you can put small cylinders around each flap, and rotate that entire cyclinder according to CEL. This can be contained within a large cylinder for the rotating structure, controlled by CEL (or constant omega which I suspect is your case). This is then contained in the large static domain."" this is how i was intending to model it, but was hoping that the 6dof was going to make my life a lot easier... many thanks for your replies, its really helpful!! James

 October 12, 2010, 10:49 #7 Senior Member   Edmund Singer P.E. Join Date: Aug 2010 Location: Minneapolis, MN Posts: 512 Rep Power: 14 I would stick with CEL and dont use 6DOF. At this point 6DOF is beta, and any bugs associated with it will have to go through CFX since you will not have direct control of the implementation. Using CEL will allow you to run things a bit faster. And since it is rotation on only 1 axis, shouldnt be too hard to implement.

 October 12, 2010, 10:56 #8 New Member   James Join Date: Jul 2010 Posts: 25 Rep Power: 9 Thanks again for your help James

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Mike FLUENT 4 February 2, 2010 08:31 Munikrishna Main CFD Forum 3 November 27, 2006 14:45 Dob Main CFD Forum 0 October 10, 2006 16:45 hui FieldView 1 September 28, 2006 16:42 Bum-Seok Hyun Main CFD Forum 4 February 16, 2000 19:59

All times are GMT -4. The time now is 18:05.