Problem in Mesh Displacement at middle of Pool
 

This is a Plastic plate in middle of "Pool Wavemaker".
The density of plastic plate is tow times more than the density of water. But in Timestep of 7 "Run" is Stopped.
When I'm observing the results, the plate is beginning to revolve in a very low Time !!! ( at 0.175[s] :eek: ) and the "Mesh Displacements" is stretched at Corners in a large amount (according to fig.) until the "Run" is Stopped and represents The following Error :

ERROR #002100027 has occurred in subroutine cNWDIST. |
| Message: |
| At least one highly skewed element has been detected on a wall |
| boundary, leading to an unreliable near-wall distance calculation |
| for the turbulent wall functions. The solver will continue |
| to execute, but convergence and/or accuracy may be affected. |
| Please consider improving the mesh quality. The coordinates of |
| the element face are ( 0.2550E+00, -0.6737E+00, -0.4808E+00 ).




Some of My Configurations in CFX-Pre ;
CFX Version : 15.0
Time Steps : 0.025 [s]
My Plate Degrees Of Freedom >>> Translational Degrees Of Freedom >>> None
My Plate Degrees Of Freedom >>> Rotational Degrees Of Freedom >>> Z axis
plastic plate is Homogen and main Coordinate Frame is same Center of Mass


My Questions :
1- Why the plate is beginning to revolve in a very low Time ?? ( at 0.175[s] ??? ) :confused:
2- Why the Mesh Elements can't Support This Displacements ? :(
http://i57.tinypic.com/205sow.jpg

I don't know what you expected for the rotation of your plate... should it be sooner ?
Then try to plot the torque on your plate to understand a little bit more what happens here...

I see that you only want z rotation on your plate and your mesh is not suited for that kind of displacement. I would define a cylinder domain for your plate and mesh it with O-Grid. Then when the plate is rotating the mesh will be much more stable.

Remember : CFX can't do any remeshing during the run so if you want to model some big displacement like this you have to use tricks (like cylinder domain for the rotation).

Au contraire, mon ami! :)
It is possible to setup a remeshing script with e.g. ICEM so that it remeshes when the mesh is too distorted. However, it is quite complex to get it to work properly.

But I do agree with you that a rotating cylinder domain is best for this case.

I have heard about some remeshing scripts on this forum but since I never had the chance to try one so I can't talk about it. This kind of thing is quite amazing and I will take a look on it when I have the time (and a ICEM licence).
This kind of work always bluffs me I: creating new options like this for CFX is not an easy work.

***Thank you for your comprehensive answer Mr. "Thomas MADELEINE" :)
My TimeSteps is 0.025 (failing in Run occurs in TimeStep 16 = 0.4 [s] )
My Plate Density = 2*Density of Water (Heavier than water)
I wonder that Plate turns in 0.4 [s] :confused:. this is Very soon For rotating (Because "plate Density" is biger than "water density"
and The water is not moving still, Moreover, the Mesh displacement around Plate in fluid origin is still Blue and unmoved.)

Thank you again
I've attached for you :::

http://i59.tinypic.com/sbsbxx.png

Yes, of course

I am afraid I can't really help on why it is moving so soon...
I suggest you post your CCL (if you may) here so that we can understand what you model exactly.
Only one question: the rotation axis is in the center of your plate ? Do you model the gravity ?

For the subdomain it is something like that except that I will make the rotation axis of the cylinder the same than your rotation axis... then when the plate is rotating your whole domain can rotate without any mesh deformation.
Which software do you use for meshing ?

All Simulation CCL Attached in this Post

And also This is my ANSYS CFX 15.0 *.cfx project file and "CFX-Solver Manager" Monitor Graphs
Zip File Size : 5.22 MB
attached in "uptobox" upload Center :

Download.zip - 5.2 MB


the rotation axis is in the center of mass

do you mean "Like this" ?? :
www.youtube.com/watch?v=lBVvx3YHzNI
ANSYS CFX Toturial ==> 32.6. Simulating the Buoy with Decoupled Mesh Motion

ICEM CFD &(or) GAMBIT 2.4

On your CCL I saw that you model the gravity on the Y axis.
So I am not sure to have clearly understand what you model exactly (for me it should have be on Z), can you explain a little bit more what you are simulating here and what you expect to have please?

For the subdomain the video you linked was perfect. It is exactly what you should do to avoid any mesh deformation.

Since you use ICEM, it is really simple to do this mesh: the cylinder is O-Grid with extrusion and for the rest is is H-Grid with O-grid around the cylinder (extrusion also).

you referenced a tutorial, have you done it ?

in my Geometry, Y axis is vertical (Y=Heigh)
Please See figure 1 & 2 attached in this Post

ok . I will explain to you everything about my project.
but first, I apologize in advance that I do not speak English very well.

I'm going to Simulate a WaveMaker Tank (Piston Wave Maker Tank) and a Plate in middle of that.
My plate is allowed to rotate only in z axis (Please See figure 1 & 2 attached in this Post)
When "Reciprocating Wall" is off and we haven't any Wave, the Plate is beginning to revolve in middle of tank. :confused:

Sorry, I am not sure to have clearly understand what you mean.
I've attached Geometry model too. Please Help me what can I do in meshing ?

yes . exactly I know what to do

thank you for your explanations.

Firstly, you case : (I am not an expert with multiphase)
I don't understand why you model the gravity here: it will have no effect on water nor air (not big enough) and you forbid the Y displacement on your plate. (maybe there are thing that matters i did'nt see)

Problem is that supposing that you center is a little bit under your inertial center (or some mesh make it displaced), you will have some trouble even in calm water... you are really close to an unstable position

I also don't understand why one wall was free slip and not the others since the movement on the wall shouldn't be really big and doesn't concern you. But this is not really important, so you can leave it like this.


Secondly the meshing:
I will sadly be unable to help much I am installing ICEM now and face some difficulties... I made a (really) quick example of blocking in ICEM on paint (sorry for the quality).

You can (should) do an non conformal interface since the cylinder domain will rotate.

If you don't know what is O-Grid (we have two here), C-Grid, etc the help or the internet have some quite good example and are really helpful: it is something you can see quite often and really useful when you have some curves or boundary layout...

hope that helps a little bit

You need gravity to make the liquid stay on the bottom of the tank and the gas float to the top. So gravity is required.

Helo Mr. "ghorrocks"
Thank you for coming to this Topic
My Gravity configuration is wrong ? (Figure attached in this post)
If not wrong, then why the plate is beginning to revolve in a very low Time ?? ( at 0.4 [s] ??? ) :confused:
Mr. "ghorrocks"; Please Read My Problem in this topic (Especially First Post & Fifth Post) and tell your idea Please. I caught a big problem.
I attached all required files in this Topic
Thank you very much:)

My comment was referring to Thomas' comment:

This comment is wrong - you need gravity.

As for what is the problem this thread is talking about - Thomas has correctly identified the problem (moving mesh cannot handle the sort of motion you are doing) and the solution (put it in a rotating section of mesh connected by GGI interfaces). The convergence problem is related to the very poor mesh quality with heavily distorted meshes - in other words, a different problem caused by the same root cause.

absolutely right, sorry for my mistake.
So there are things that matter I didn't see ^^
Again, I am not formed to multiphase calculations...

Thanks you Glenn for clarifying this, I hope some days I will have some time to learned more about multiphase

hi
its related to your :
1-mesh quality , you'd better to use the hex mesh.
2- select the surface that has an interface with water, use the better sizing for that
3- specify the mesh rotating degree to the lower one
i think that your process so fast but your time step is longer than that
4- use the mesh on the boundry
good luck,M.R