CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] How to generate sunstructured "all-tri patch-dependant" surface mesh in ICEM? (http://www.cfd-online.com/Forums/ansys-meshing/82709-how-generate-sunstructured-all-tri-patch-dependant-surface-mesh-icem.html)

jash December 3, 2010 06:18

How to generate sunstructured "all-tri patch-dependant" surface mesh in ICEM?
 
1 Attachment(s)
Hi all,
Typically when I am running alpha-traverse studies, I am creating an unstructured symmetry mesh of my geometry (left half of the geometry, left half of the far field, and a symmetry plane). I have been using patch-independant surface meshing to create the surface mesh, then advancing-front (smooth) + prisms to fill in the volume mesh.

While I am quite happy with the surface mesh on the aircraft, I haven't been happy with the surface mesh generated on the symmetry plane. Since patch-independant surface meshing is using octree to generate the surface triangles, the growth rate on the symmetry plane going from the aircraft to the farfield is very octreeish: aggressive and "boxy". I haven't found a parameter that smooths this out in a nice way. The result is that the advancing-front volume mesh is constrained near the symmetry plane in a way that looks "odd/wrong" when compared to the volume growth away from the symmetry plane (see attached mesh cut-plane, this is looking down the length of the geometry, symmetry plane terminates the mesh on the left side, farfield is off screen on the right side).

I've got a feeling that patch-dependant surface meshing is going to generate a surface mesh on the symmetry plane that is more compatible with the advacing-front volume mesh, but I haven't completely gotten the hang of it. Parts of the surface mesh come out beautiful (just what I am hoping for) and others come out twisted. I've checked my surface normals and they are fine.

So my questions are:
1.)Is there a tutorial describing how to use patch-dependant surface meshing for unstructured meshes (I haven't been able to locate one in the official Ansys tutorials)?
or
2.)Is there an other way to create a surface mesh on the symmetry plane that has a smoother growth ratio going from the aircraft to the farfield?

Thanks for any help!

PSYMN December 4, 2010 14:08

Laplace...
 
There is a tutorial about patch conforming surface mesh on an aircraft, but I always found it more work... (The jist is that you must build topo first and set up sizes on all the curves. Then use the patch dependent surface mesher. You can just mesh a single surface, such as the symmetry plane and then use that when you Octree, or you could mesh the whole thing with patch dependent)

I can dig it up for you if you really want it.

In the mean time, I have another suggestion that is easier to implement...

Generate your Octree Mesh... (no need for Delaunay yet).

Delete all the volume elements (Delete Mesh, then select All volume elements with the selection tool bar). These will be deleted to replace with delaunay eventually, but if you get rid of them now, it is easier to smooth.

Then smooth the heck out of the surface mesh using the Laplace option. Make sure to turn on that laplace checkbox option... Try 50 iterations up to 0.6 or something like that. Laplace tries to smooth out angles between elements and the transition (surface area change) between elements. It ends up looking very "delaunay". But it doesn't focus on individual element quality, so... One more round of regular smoothing (10 iterations up to 0.4) (without Delaunay) to finish up.

Take a look at the surface on the symmetry plane. It should be pretty good.

Then go back to compute mesh => Delaunay to fill the volume and continue on with your regular process...



-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey

jash December 4, 2010 16:23

Excellent, thanks! I've never tried going that extreme on the smoothing options. Looking forward to trying this out on monday.

ok___ko April 19, 2013 07:40

how to generate a mesh
 
Quote:

Originally Posted by PSYMN (Post 286004)
There is a tutorial about patch conforming surface mesh on an aircraft, but I always found it more work... (The jist is that you must build topo first and set up sizes on all the curves. Then use the patch dependent surface mesher. You can just mesh a single surface, such as the symmetry plane and then use that when you Octree, or you could mesh the whole thing with patch dependent)

I can dig it up for you if you really want it.

In the mean time, I have another suggestion that is easier to implement...

Generate your Octree Mesh... (no need for Delaunay yet).

Delete all the volume elements (Delete Mesh, then select All volume elements with the selection tool bar). These will be deleted to replace with delaunay eventually, but if you get rid of them now, it is easier to smooth.

Then smooth the heck out of the surface mesh using the Laplace option. Make sure to turn on that laplace checkbox option... Try 50 iterations up to 0.6 or something like that. Laplace tries to smooth out angles between elements and the transition (surface area change) between elements. It ends up looking very "delaunay". But it doesn't focus on individual element quality, so... One more round of regular smoothing (10 iterations up to 0.4) (without Delaunay) to finish up.

Take a look at the surface on the symmetry plane. It should be pretty good.

Then go back to compute mesh => Delaunay to fill the volume and continue on with your regular process...



-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey

Hi, I just start to learn CFD. Now, I have such a problem, I have already draw a geometry in ICEM, how could I block it and mesh? Could you give me your email address do that I could send you my specific question?
Thanks

star May 30, 2013 11:30

triangular mesh generation
 
Hello friends. I want to make triangular mesh around 2D airfoil. By default it makes quadrilateral. How should I proceed for tri grid? Please help

PSYMN May 30, 2013 14:08

What tool are you using? if ICEM CFD, go to the mesh tab and change the global settings for shell meshing... Or just go to Compute mesh and ask for all tri instead of quad dominant.

star May 31, 2013 06:21

1 Attachment(s)
Thanks PSYMN for your reply.
Yes I am using ICEM. Here I am posting a quick process of mine. I created airfoil and farfield (surface created) curves. Then I changed Shell meshing parameters to "All tri" type. Next, I created block and set some edge parameters under premesh parameters but it still create quad grid.. Also there is no option for 'All tri' under compute mesh... I 'll be really thankful for your help.
Here I attached the type of mesh which I want to generate..

PSYMN May 31, 2013 11:01

Those shell meshing parameters are for shell meshing, not for blocking...

You probably just need unstructured shell meshing which you generate with the mesh tab => Compute mesh. Look for a shell meshing tutorial because you will also need to learn how to set the curve params, 2D inflation, etc.

If you actually want blocking, you can go to edit block to change the block type from mapped to free (mapped is the default). You can also set the free block to any type of unstructured mesh you want... All tri in your case. You probably want the gambit pave all tri for the smoothest mesh. Note, if you are using blocking, you will need to block out the airfoil interactively or use 2D surface blocking if you want it done automatically. Placing a single 2D block will not capture the airfoil.

Best regards,

star May 31, 2013 12:14

Thanks PSYMN for your suggestion. I am now reading tutorial relating to shell meshing. I think for unstructured mesh I will not need blocking. Am I right?


Kind Regards

diamondx May 31, 2013 13:32

Quote:

I think for unstructured mesh I will not need blocking. Am I right?
yes, you are right

star June 1, 2013 03:09

Dear friends Diamondx and PSYMN, I started learning generating unstructured mesh around airfoil ICEM but one initial problem for me is that after computing it gives me some warning that there is hole in domain. I think it assume airfoil as hole because the mesh ignores the airfoil curves as boundaries and also crosses it. How should I specify the airfoil as walls? please help..

Kind Regards

diamondx June 1, 2013 10:56

hello Star,
To specify the airfoil as wall, name those curve "airfoil_wall", then in the output menu specify them as wall. First you have to fix the hole error...
would you mind sharing your project via dropbox. i can take a look at it this weed end...

star June 1, 2013 12:37

1 Attachment(s)
Thanks diamondx for your reply. By wall i mean to make it solid boundary. I think i can go to output after completing my mesh. I am at the initial stage of mesh generation. I posted here photo of my mesh. you can see what I mean. My 2 main questions regarding my requirements are
1) how to make the airfoil as boundary so that the mesh lines couldn't pass it.
2) how to create more/dense mesh near airfoil boundary.

kind Regards

PSYMN June 1, 2013 22:13

2) just set a smaller mesh size on the curves...

1) Delete the surface inside the airfoil and mesh won't generate there.

star June 2, 2013 01:17

Thanks PSYMN, your points were much helpful. I trimmed the surface inside airfoil and now it's better...

handsome June 20, 2013 13:27

Quote:

Originally Posted by PSYMN (Post 431400)
2) just set a smaller mesh size on the curves...

1) Delete the surface inside the airfoil and mesh won't generate there.

hi
how we can delete the surface inside the airfoil in icem cfd?

diamondx June 20, 2013 13:39

it is a very basic step, under the geometry tab, you have options to delete points, curves, and surface, or everything. just click on delete surface... Do some tutorials to learn more about it

handsome June 20, 2013 16:00

Quote:

Originally Posted by diamondx (Post 435089)
it is a very basic step, under the geometry tab, you have options to delete points, curves, and surface, or everything. just click on delete surface... Do some tutorials to learn more about it

hi
thanks a lot for quick reply my friend

let me explain more about my problem

first i import the airfoil from point data(airfoil curves create not have surface now).then i create the farfield boundary for example like square and create surface in the square.
now for shell meshing what can i do?
at the moment icem can't recognize the surface inside and the outside of the airfoil?
how can split the boundary surface by airfoil curve?
i use segment/trim surfaces and select boundary surfaces and airfoil curve but it dose not work and i don't know why?

(i have the surface of the farfield boundary and the airfoil curve now )


Best regards

handsome July 18, 2013 15:45

Geometry (tab) => Geometry Repair => Build Diagnostic Topology. This will trim the surface with the airfoil curves and probably turn them red. You can then delete the surface within the airfoil
this is the key that i dont know

ankur_kr July 23, 2013 18:48

Hi,

I needed a few suggestions regarding meshing in ICEMcfd. Currently I use unstructured tetrahedral mesh with following options, All Tri Shell Meshing, Tetra/Mixed Volume mesh type and Quick Delaunay Volume mesh method. I wanted to know the following

1) My geometry has a rectangular cuboid of dimension 12m X 3m X 3m with a couple of un-meshed cylindrical tubes (12m & 0.15m dia) through it. I entered the maximum size of mesh cell to be 0.3m. I end up getting about 3,000,000 cells!! which really slows down my simulations. [ I do have some inlet/outlet surfaces of dimensions 15 cm over which I applied prism layers of size 3 cm ]. Is there a way I can reduce the no. of cells considerably ?

2) Which one among Delaunay and Octree is better ?

3) Currently I create surface mesh first and the volume and prism together. Is this the correct sequence or directly computing volume mesh without first creating surface mesh is better ?

4) Does structured mesh gives considerable advantage over un-structured mesh ?

Thanks,
Ankur


All times are GMT -4. The time now is 09:36.