Hello.

Using CFX 11.0 x64 with workbench (Intermediate skills). I need to model a plate, which oscillates around it's tip +-20 degrees from it's starting position at a frequency of around 40Hz. I have also some static bodies in this simulation. I seen a topic on this forum, about creating some meshes for different body positions prior the solving process for loading them during the analysis. The question is how exactly is this done? Also, how can I calculate the time step for this case and what turbulence model should I use?

Thank you in advance for help.

Check out the CFX tutorials. I think Tut 20 talks about Junction Box routines to load in different meshes during a run. There is an oscillating plate tutorial as well, I think it's number 21. I would imagine that unless the plate touches another surface you could probably get away with just using a moving mesh and not reading in different mesh files.

Hi,

I think the oscillating plate tutorial is coming in V12, at the moment it is a beta version. Unless you are using V12 beta you will have to wait until it is released.

There are two main approaches to doing this: 1) If the plate simply rotates you may be able to put the plate in a rotating frame of reference and connect to the main flow with a GGI. This is a very good approach if applicable. 2) Model the motion with a deforming mesh. This can be done either by a) specifying the location of the boundary nodes and allowing the solver to work out the position of the internal nodes (this can lead to mesh folding or negative volume elements if the motion is excessive) or b) generate the meshes beforehand and read the new meshes as the simulation progresses.

Regards, Glenn Horrocks

Sorry for hijacking the thread, but how is it possible to

"b) generate the meshes beforehand and read the new meshes as the simulation progresses. "

I know that it's possible to read new mesh files with junction box routines (as in tutorial 20, p 343), but I'm more interested in the mesh creation itself. The manual says that:

1) The coordinates of the first mesh in the sequence must be identical to the initial solver-internal mesh coordinates. This ensures that a node map between the user and initial solver-internal mesh coordinates can be generated.

2) The topology (i.e., connectivity) of all meshes in the sequence does not change. This ensures that the map between the user and solver-internal mesh coordinate can be re-used.

How can such meshes be generated, where the topology is the same?

Regards, Johannes

Thank you, I'll look through the 20th tutorial.

This device works like a fish tale. It should generate thrust force. The centre of rotation of the plate is at it's tip, while the other end oscillates up and down +-15 degrees and it is somewhat like 20mm away from the static body surface. I used about 0.0005 for face spacing in that area (the chord of the plate is 0.3m). I have gone through the Oscillating plate tutorial, but it seems to me that I won't be able to get through with simply deforming mesh.

Hi,

If the only motion is a rotation then I would try a rotating frame of reference. Will that work?

Glenn Horrocks

Do you mean like this: http://img49.imageshack.us/my.php?image=43765510eg8.jpg

I mean placing the plate in the rotating region and assigning it a CEL expression?

Hi,

Yes, that is the idea. Define the rotating region's speed as a CEL expression which is either pre-defined or a function of forces on the plate or whatever.

Glenn Horrocks

Trouble again: CEL shows an error when I'm trying to assign a motion to the rotating region, using sin() function with "t" argument (I want the sinus to use time, so I can make the plate oscillate). It's about dimensions, that the expression resolves to seconds, while dimensionless value expected.

Hi,

Something like sin(t/1[s]) should do it. This makes it unitless.

Glenn Horrocks

Everything works. Everything helped me a lot. Don't know how to thank you