CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Moving mesh (http://www.cfd-online.com/Forums/cfx/93893-moving-mesh.html)

 ankit.rokr October 29, 2011 16:53

Moving mesh

Hi,

I am simulating a flapping wing in static fluid. I have seen tutorial 22.Since i am considering my wing to be a rigid boundary i wanted to know how can i incorporate oscillatory motion about one end point of wing for user defined mesh deformation.

 ghorrocks October 30, 2011 05:28

In user defined mesh deformation you can specify whatever mesh motion you like, so you then specify oscillatory motion.

 ankit.rokr October 30, 2011 09:59

1 Attachment(s)
I have attached image of my simulation geometry. I am using 2D extruded mesh. The elliptical hole represents wing and i have applied no slip wall boundary condition on it. The remaining portion is fluid. I wanted to oscillate the wing about one of ellipse's extreme point. I wanted to know how can i put specified displacement of mesh in Boundary details of wing(i.e elliptical wall boundary) in order to simulate oscillating motion.

 ghorrocks October 30, 2011 16:59

This is a straightforward application of moving mesh. Have you done the moving mesh tutorial examples?

 ankit.rokr October 31, 2011 05:57

Yes i have seen an example of moving mesh in tutorial 22 of cfx. In fact i am able to move this elliptical wall linearly in one direction(i.e. vertically downward or upward) in a similar way to tutorial 22. But now i have to rotate it around its one end. I wanted to know what are the expressions or command i need to give in order to rotate it.

 ghorrocks October 31, 2011 06:52

Then you just need to specify an oscillatory motion expression. This might help you get started: http://en.wikipedia.org/wiki/Rotation_matrix

 Far October 31, 2011 06:55

Glenn you are very much helpful to forum

 Doginal November 1, 2011 12:19

I found this thread very useful for helping come up with my equations of motion http://www.cfd-online.com/Forums/cfx...g-domains.html

Also the tutorial posted here: http://www.cfd-online.com/Forums/cfx...h-meshing.html shows some good expressions for applying rotation on a moving mesh

Hope this helps

DM

 ankit.rokr November 3, 2011 15:00

Thanks Doginal for this help.I understood what are the expressions and settings i need to use. I had tried with both the methods given in the above specified links. But each time it shows error in the first iteration and terminate the solution.Let me describe my problem once again. I am using 2D extruded mesh in square domain with elliptical hole. The elliptical hole represents wing and i have applied no slip wall boundary condition on it. The domain represents fluid. I wanted to oscillate the wing about one of ellipse's extreme point. Any ideas/ help is greatly appreciated, and if you need more information about the problem just let me know.

Thanks
Ankit

 Doginal November 3, 2011 17:09

Have you looked into using a rotating domain instead of a moving mesh. Basically, create an inner circular domain within the square domain. Put the shape that you are trying to oscillate so that the center of rotation is in the center of the circular domain then specify a rotation for the circular domain. It is very easy to set up, probably a lot easier than moving mesh.

You should be able to create a moving mesh that will do this but the rotating domain may be easier.

Edit: also if your getting an error, what is the error

 ghorrocks November 3, 2011 17:48

I agree with Doginal - if the motion is only rotary then this is better done as a rotating frame of reference. It is more accurate, does not have negative volume element problems and will run much faster.

 ankit.rokr November 4, 2011 08:33

Actually in my simulation i wanted to see the effect of flapping wing in a static fluid medium. So instead of rotating the the whole domain i just wanted to oscillate the wall(i.e. elliptical whole in square fluid domain) which physically represents wing in 2D. Can you suggest me some way to solve this problem? Any help would be highly appreciated.

 Doginal November 4, 2011 15:10

Sorry now i'm confused. Are you oscillating in a rotating motion or translating back and forth.

If you use a rotating domain, you do not rotate the whole domain. Instead you create an inner domain and rotate that. You still have a static fluid medium. This really is the easiest way to deal with rotation about any point. When using mesh deformation, simulation can take way longer and i have found require more memory (probably not an issue with a 2D simulation). If this looks like what you want but are unsure how to do it just post up, its simple to explain.

If you still want to use a moving mesh, please post the errors thats occurring and/or your CEL functions. Its hard to determine whats going wrong with out that information. From my personal experience its usually the result of me defining my functions wrong however it could be issue like timestep, BC being defined wrong (make sure outsides set as stationary mesh and sides set as unspecified mesh) or many other things

edit: http://www.cfd-online.com/Forums/cfx...g-domains.html look at the picture in the first post and look at case 2. That is what we mean to set up the problem except just rotate the domain there will be no translation. Also to change the point on the ellipse you wish to rotate about you just set the center of rotation to the center of the inner domain.

 ankit.rokr November 5, 2011 07:52

1 Attachment(s)
Hi,
I have attached domain geometry having two domains as per your suggestion. I have to oscillate elliptical hole about circular domain center at a given user defined angular velocity(transient problem with initial velocity of fluid domain being zero) in the static fluid setting to check the resulting velocity and pressure distribution.Since i have not done any rotating domain problem previously, could you please specify the domain settings and boundary conditions to simulate this problem. Tell me if i need to add something extra in this geometry for this simulation.

 Doginal November 5, 2011 18:00

The set up of the domain and boundary conditions would be the same as if you where doing a moving mesh.

The only difference is at the interface you specify an interface. I would give the help files a quick read for interfaces just so you understand what the options mean and what you are doing.

For this case I would use a
Interface model - general connection
Frame Change/mixing model - transient rotor stator
Pitch change - Automatic or None (should be the same result but with automatic it will give you a warning i believe)
Mesh connection - GGI

Once again i suggest reading the help files to get an understanding of the options. Also a couple things to be watch for, make sure the interface is significantly away from the ellipse so that it doesn't interfere with the results, also I have found that changing the mesh sizing at the interface can help reduce any errors from flow moving across it. (just make sure its not overly course). If your just using a static fluid and the interface is sufficiently away from the ellipse that should not be a problem anyways.

Also another thing to note that confused me at first with this type of problem is when your looking at the results in post. there is a difference between velocity and velocity in stationary frame. The a contour plot of "Velocity" will show the velocity relative to the motion of the mesh which will make things look weird. You probably want to use "velocity in stationary frame"

Hope this helps

DM

 ankit.rokr November 6, 2011 15:05

1 Attachment(s)
Hi,
I used interface between square and circular domain in the manner you suggested last time. Then i specified outer domain(square excluding circle) as stationary frame and inner domain(circular domain with elliptical hole) as rotating frame. In the geometry center of circle is center of oscillation for ellipse(specified as wall). Since i wanted a static fluid medium i specified the angular velocity of rotating frame(i.e. ellipse) as zero rad/s and elliptical wall as 1 rad/s(for an instance). After doing this it does not even start the solution and a message saying"Workbench was busy so the Start command could not be executed" appears.But when i specify the same angular velocity to circular domain and elliptical wall boundary it gives solves. But physically the domain surrounding the wing should not be rotating.When i checked the resulting velocity distribution, it does not show vortex formation around the wing tip which was expected. Velocity in Stn frame does not show any distribution.
Please correct me where i am going wrong.

kind regards
Ankit

 Doginal November 6, 2011 16:30

The full inner domain should be rotating. remember its the mesh rotating not the fluid within the domain.

Since i wanted a static fluid medium i specified the angular velocity of rotating frame(i.e. ellipse) as zero rad/s and elliptical wall as 1 rad/s(for an instance).

I'm not sure what you mean by this. You should not be setting different velocities. Do you have specified mesh deformation still on? if so it should be off.

To specify the rotation. You need to make sure the inner domain is its own domain. Then set the domain motion to rotating. The set the angular velocity to what ever function defines your rotation.

 ankit.rokr November 7, 2011 14:26

Thanks Doginal for all the help in my simulation. Now i have pretty good idea about the simulation.I have one more doubt about rotating domain. If i am specifying 1 rad/s angular velocity for inner domain, what angular velocity of elliptical boundary wall should be specified in wall boundary condition(Wall velocity->Angular velocity->Magnitude), in order to simulate a condition in which wall is rotating at 1 rad/s (w.r.t. absolute frame of reference) in static fluid medium? I am confused between 1 rad/s or 0 rad/s.

 All times are GMT -4. The time now is 18:17.