CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ANSYS Meshing] Dynamic Mesh with Inflation Layer (http://www.cfd-online.com/Forums/ansys-meshing/107157-dynamic-mesh-inflation-layer.html)

 grayback87 September 19, 2012 03:33

Dynamic Mesh with Inflation Layer

1 Attachment(s)
Hello I'm a final year student of civil engineering degree. I'm doing a CFD simulation of the Vortex-Induced-Vibration on a circular cylinder.
I made an UDF and I made some simulations with dynamic mesh, but i have one question:

Is it possible to make a dynamic mesh with inflation layer (orthogonal mesh)?

I think it's only possible with TRI-mesh ( I read it on Fluent user's manual) but I read some papers of sciencedirect, in which the author used orthogonal mesh to do some dynamic simulations.

(I used Juan B.V. Wanderley a,, Gisele H.B. Souza b, Sergio H. Sphaier a, Carlos Levi 2008 paper. www.sciencedirect.com)

 grayback87 September 19, 2012 03:38

1 Attachment(s)
Sorry I try to upload another picture. And I have to do it on the reply.

This picture is from the same paper.

"In addition, the generated grid is locally
orthogonal to the body surface to facilitate the implementation of
the boundary condition on the body. In order to concentrate grid
points at the wake region behind the cylinder and body surface, an
exponential stretching is used in both circumferential (x) and
radial (Z) directions. In each time step, the entire grid is
regenerated after the body displacement, so that the external
boundary is kept fixed"
this is a part of the text in which the author explains the grid.

I need some help please :D.

I know how to make tri-mesh dynamic mesh, but not orthogonal. (i think its better and more accurate in order to get the best results).

Thanks.

 grayback87 September 21, 2012 03:19

Please I need some information. If this is impossible to do I need to know , because it's important not spending more time in this thing.

Thanks

 cfd seeker September 21, 2012 03:21

By Inflation you mean boundary layer mesh or you mean structured mesh?

 grayback87 September 21, 2012 03:24

Inflation its the name that ansys meshing uses to do the Boundary Layer mesh ( I think that Boundary Layer its the name Gambit give to it).
Yes I mean some kind of structured mesh in order to do the mesh more fine in the boundary to capture better all the effects.

I'm only capable to run a mesh with tri-elements in the region that moves with the cylinder.

 Far September 21, 2012 04:46

Quote:
 Originally Posted by grayback87 (Post 382483) Hello I'm a final year student of civil engineering degree. I'm doing a CFD simulation of the Vortex-Induced-Vibration on a circular cylinder. I made an UDF and I made some simulations with dynamic mesh, but i have one question: Is it possible to make a dynamic mesh with inflation layer (orthogonal mesh)? I think it's only possible with TRI-mesh ( I read it on Fluent user's manual) but I read some papers of sciencedirect, in which the author used orthogonal mesh to do some dynamic simulations. (I used Juan B.V. Wanderley a,, Gisele H.B. Souza b, Sergio H. Sphaier a, Carlos Levi 2008 paper. www.sciencedirect.com)
Is it one way or two way simulation? if one way then you can go with structured meshing in the inner zone and unstructured meshing in the outer zone. And again structured meshing in the outer most zone.

 grayback87 September 21, 2012 04:54

Its only one way simulation ( inlet boundary to pressure outlet) ( the wind go from left to right)

I divided the mesh in 3 zones, Inlet zone (structured) moving zone (unstructured) and outlet zone (structured again).

It's what you have asked me?

 cfd seeker September 21, 2012 08:19

Quote:
 Originally Posted by grayback87 (Post 382917) Inflation its the name that ansys meshing uses to do the Boundary Layer mesh ( I think that Boundary Layer its the name Gambit give to it). Yes I mean some kind of structured mesh in order to do the mesh more fine in the boundary to capture better all the effects. I'm only capable to run a mesh with tri-elements in the region that moves with the cylinder.
Sorry I was in hurry at that time....As the picture shows you are using fully structured mesh all around the cylinder both in viscous and in-viscid part of the mesh so why to worry about the boundary layer mesh? From your first two posts I think you need guidance regarding structured and unstructured meshes while using dynamic mesh.

Quote:
 I think it's only possible with TRI-mesh ( I read it on Fluent user's manual) but I read some papers of sciencedirect, in which the author used orthogonal mesh to do some dynamic simulations.
Fluent use three methods to update the mesh at the next time step in dynamic mesh(I assume you are using fluent)
1. Smoothing
2. Layering
3. Remeshing

"Smoothing" works for both structured(which you are naming as "orthogonal") and unstructured meshes but it is generally recommended for unstructured meshes, "Layering" purely works for structured meshes while "Remeshing" method works only for unstructured meshes

 grayback87 September 21, 2012 08:30

Thank you for the response. I didn't know smoothing method was capable to make dynamic mesh with orthogonal-elements. I will make a new mesh and I will try.

P.S.

The pictures isn't from my work, there are from the Paper i used to compare my results.

I used a combined mesh, with orthogonal mesh in the zone which doesn't move and tri-mesh where the cylinder is able to move.

I will upload pictures from my mesh later.

 cfd seeker September 21, 2012 08:35

Quote:
 Originally Posted by grayback87 (Post 382484) Sorry I try to upload another picture. And I have to do it on the reply. This picture is from the same paper. "In addition, the generated grid is locally orthogonal to the body surface to facilitate the implementation of the boundary condition on the body. In order to concentrate grid points at the wake region behind the cylinder and body surface, an exponential stretching is used in both circumferential (x) and radial (Z) directions. In each time step, the entire grid is regenerated after the body displacement, so that the external boundary is kept fixed" this is a part of the text in which the author explains the grid. I need some help please :D. I know how to make tri-mesh dynamic mesh, but not orthogonal. (i think its better and more accurate in order to get the best results). Thanks.
Quote:
 I know how to make tri-mesh dynamic mesh, but not orthogonal. (i think its better and more accurate in order to get the best results).
If you are using fully structured mesh around the cylinder go to "Dynamic Mesh" tab toggle on "Layering" and use can also toggle on "Smoothing"(optional) and do remember Spring Based Smoothing" is by default switched off for non triangular/non tetrahedral cells so type on the main screen...../define/models/dynamic-mesh-controls/smoothing-parameter> spring-based smoothing for all cell types [no] yes....to switch it on for quad/hexa cells
If you are using structured(orthogonal/hexa) mesh in the boundary layer and unstructured mesh in the outer part then you have to define two "Fluid Zones" in the mesh i.e one for the boundary layer and one for the outer layer....for structured(orthogonal/hexa) boundary layer mesh toggle on layering and for outer unstructured mesh toggle on smoothing and remeshing

 cfd seeker September 21, 2012 08:41

Quote:
 I used a combined mesh, with orthogonal mesh in the zone which doesn't move and tri-mesh where the cylinder is able to move
So you mean boundary layer mesh will not deform with the rotation of the cylinder and you want it to move with the cylinder? isn't it?

 grayback87 September 21, 2012 08:51

Quote:
 Originally Posted by cfd seeker (Post 382960) So you mean boundary layer mesh will not deform with the rotation of the cylinder and you want it to move with the cylinder? isn't it?
Yes i mean a boundary layer mesh which will not deform with the MOVE in vertical mode(transversal to the fluid) (the other moves are constrained), I
dont need the cylinder rotate or move in longitudinal .

The vortex induced vibration in vertical mode its something like this

 cfd seeker September 21, 2012 08:56

Quote:
 Originally Posted by grayback87 (Post 382963) Yes i mean a boundary layer mesh which will not deform with the MOVE in vertical mode(transversal to the fluid) (the other moves are constrained), I dont need the cylinder rotate or move in longitudinal . The vortex induced vibration in vertical mode its something like this http://www.youtube.com/watch?v=aOfqdQs66jA
Ok so in this case you will not toggle on "Layering" for the boundary layer mesh because it is not deforming with the movement of cylinder, so this portion of the mesh does not require any mesh update

 grayback87 September 21, 2012 08:58

thank you thank you thank you :D

I'll try and i will show you the results... (maybe in 2 weeks)

Thank you again!

 fluentworkshop September 24, 2012 07:30

Help

Hi grayback87
I can correct it for you.
I suggest doing that with Gambit software.because you must have two separate zone.

 cfd seeker September 29, 2012 01:06

 grayback87 September 29, 2012 12:59

Hi, finally i did it ! It moves without problem.
But Now I'm doing some benchmarks, I mean, I'm comparing with the literature, Cd vs Re in stationary and other things.

I used Remeshing and it works very fine

 fluentworkshop September 29, 2012 15:39

Hi
I suggest that you try to use Layering Method. (with another Mesh)
Layering method is very rapid and Remeshing method is slower than layernig.
In curvilinear boundary (such as circle) you can use the constant ratio (not constant height) method of layering.

 cfd seeker September 30, 2012 05:17

Quote:
 Originally Posted by grayback87 (Post 384205) Hi, finally i did it ! It moves without problem. But Now I'm doing some benchmarks, I mean, I'm comparing with the literature, Cd vs Re in stationary and other things. I used Remeshing and it works very fine
did you also use smoothing? ?did you also move the boundary layer mesh?

 grayback87 October 3, 2012 04:00

4 Attachment(s)
Quote:
 Originally Posted by cfd seeker (Post 384239) did you also use smoothing? ?did you also move the boundary layer mesh?
Yes I used smoothing. this are some of my mesh's pictures.
The last picture has the statistics of my mesh, number of elements and skewed cells.

I make some dynamic test to my mesh and It works fine, but, I need to make a very good mesh beacuse I have to make a good Cd Vs Re Plot, because the cylinder its only a little part of my final project of my degree in civil engineering.

If someone see anything wrong please make me know it. (sorry, I'm not very skillfull with english language)

All times are GMT -4. The time now is 19:55.