CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   deforming mesh issue : I don't get how stiffness works (http://www.cfd-online.com/Forums/cfx/80835-deforming-mesh-issue-i-dont-get-how-stiffness-works.html)

bennn October 8, 2010 04:55

deforming mesh issue : I don't get how stiffness works
 
hey everyone,

I'm trying to model 3 foils rotating around a global axis, and oscillating around their quarter-chord with an amplitude of a couple of degrees.
http://img801.imageshack.us/f/globalh.png/
http://img801.imageshack.us/i/globalh.png/

the ring is rotated using sliding mesh, and the oscillation is obtained through deforming the mesh inside the ring. the thing is I can't get the mesh to deform the way I want it to. whatever I do the solver deforms the boundary layer, especially close to the trailing edge. here's the best result I got, at maximum deformation.
http://img221.imageshack.us/f/13100241.png/
http://img821.imageshack.us/f/902c.png/

I've tried soooo many parameters. I thought the "increase stiffness near boundaries" would be the best bet, didn't work at all. then the "increase stiffness near small volume" showed "better" results, which are the pictures above. then I tried using values with an expression I'd make. I tried using (1/wall distance)^n and (1/volume of finite volume)^n with n<1 (not possible with cfx "increase near..." option) which didn't work

then I thought I would make an expression that would set the cells to maximum stiffness where I want no deformation, then minimum elsewhere (respectively 1e15 and 1e-15 says the help file). I used an arctan function to get this rounded step, together with the wall distance and then volume of finite volumes. I chose to set the step at 0.1, then 0.01, then 0.001, the deformation still occurs right at the trailing edge (you can get an idea of the scale of my simulation on the pics above). then pretty much the same with volume and same results.

all the units are good, everything is in meter so... obviously I don't understand how mesh stiffness works, beacause I was sure that with that little function and wall distance parameter it would be bullet proof, not touching any cells in the distance to the foil I'm telling him.

any help is appreciated !!!

thanks

ben

ghorrocks October 8, 2010 05:29

I have never got adjusting mesh stiffness to work for me in a real case either. I always just use a constant value and if my mesh folds I use other approaches.

Are you sure it does not work with simply a constant value (just 1.0 will do it) for mesh stiffness?

This would be one to consider doing the mesh motion in fortran. Then you can put the foils in little circular domains inside the big ring. Then you can specify rotations of the whole domain for the big ring and rotation + translation for the foils with no need for mesh smoothing. You should also be able to do this in CEL if you are brave and not require fortran.

bennn October 8, 2010 06:57

I'll try constant value right now.

I wanted to make little circular domains with sliding mesh, but cfx only allows one domain rotation in its basic interface. I guess I could do it in fortran, but a simpler way to do it would be to define a domain around the foil that moves with the foil, leaving an area around it unchanged....

anyway if anybody knows why my approach doesn't work, what happens inside cfx with mesh deformation which makes my boundary layer moves even though I defined maximum stiffness there, that would be great. I want to understand and i just can't...

thanks glen for your help

bennn October 8, 2010 07:24

nope, constant stiffness doesn't yield any good result. just the same as usual, the trailing edge moving with 1-2 cells around moving as well and further no movement.

ghorrocks October 8, 2010 07:33

Rotating domains cannot have a moving rotation axis. That's why I suggested to define the rotation+translation in a moving mesh just for the little cylinders around the foil. As you would be moving the whole mesh the smoother would probably behave itself much better. You don't need fortran for this, it can be done in CEL.

And you could do the big ring in a normal rotating frame of reference so no need for moving mesh in that bit at all.

Your approach does not work as your motion is too complicated for the smoother to handle. You might improve things with a smaller timestep but other than that I have described the only other option above.

bennn October 8, 2010 07:47

actually I'm thinking cylinder with GGI connection, the mesh inside the cylinder moving exactly like the foil. so no need for deformation anymore. the thing is it brings another GGI interface which I'm a bit afraid of as far as accuracy is concerned.

yeah I do have all the CEL needed since i had to do it for the foil itself - which has been really tedious by the way, with the final expression being really complicated.

you say the motion is too complicated, I think it's not that bad. I mean there HAS to be a way to get the cells close to the foil to not deform. I mean it doesn't require any additional algorithm, and the smoother's job would be much easier doing so than trying to deform all the tiny cells in the BL.

damn i'm thinking out loud

thanks for your help glen, I'll try and get back to the forum with results.

ben

ghorrocks October 9, 2010 05:45

Quote:

actually I'm thinking cylinder with GGI connection, the mesh inside the cylinder moving exactly like the foil. so no need for deformation anymore. the thing is it brings another GGI interface which I'm a bit afraid of as far as accuracy is concerned.
That is exactly what I was talking about. And don't be scared of GGIs. You will probably find them more accurate than the moving mesh approach anyway (noting that you will still be using moving mesh to describe your complicated motion).

bennn October 10, 2010 12:39

ok. but the thing is I really don't trust GGI that much.... on my simulation on the main GGI connection, I can see an oscillating pattern in the physical values (pressure, velocity, whatever...) at the boundary between the two fluid domains. I don't have any illustration here but I'll post as soon as I have some.

ghorrocks October 10, 2010 18:25

GGIs are very good in my experience. You might get weird stuff with coarse meshes but with a mesh fine enough to be accurate in resolving the general flow they should be fine.

michael_owen October 12, 2010 15:09

bennn,

The problem you are having is not with the mesh stiffness. It is with the mesh density. You will find it almost impossible to use mesh diffusion given your mesh. Use the cylindrical cutout method. There is nothing wrong with a GGI interface. There is no loss of accuracy at a GGI interface so long as both sides are equally and adequately resolved and well converged.


All times are GMT -4. The time now is 07:08.