CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (https://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Mesh unable to follow curved geometry (https://www.cfd-online.com/Forums/ansys-meshing/102869-mesh-unable-follow-curved-geometry.html)

Ananthakrishnan June 5, 2012 04:47

Mesh unable to follow curved geometry
 
Hi..
I am trying to mesh a wing with sinusoidal leading edge..
My problem is that the mesh does not follow the profile of the leading edge UNLESS i give very high bunching as seen near the tip of the wing below..

As you move towards the root of the wing, the mesh is less concentrated and it does not follow the profile..

I need a way to make the mesh follow the profile inspite of lesser number of nodes( currently the node spacing near the root is 0.002 and if i have such spacing throughout the span, total elements become more than 10 million which is not reasonable for me..)

https://dl.dropbox.com/u/79881940/files.rar

The above link contains the block and tin files

thanks....

http://img839.imageshack.us/img839/3...ngedgemesh.jpg

Far June 5, 2012 05:03

try option project to b-spline.

Ananthakrishnan June 5, 2012 05:19

i tried it and i dont see any changes :(( ..
let me upload the .blk and .tin files..

Ananthakrishnan June 5, 2012 05:37

https://dl.dropbox.com/u/79881940/files.rar

the block and tetin files are available in the above URL..

@far..To use project to b spline option, i just need to select it and "apply" right?? after this if i recompute the pre mesh i dont see any changes...

PSYMN June 6, 2012 14:52

It is clear that your mesh size along the wing is larger than the features you are trying to capture... You will need much finer mesh (increase the number of nodes) along the wing...

Ananthakrishnan June 7, 2012 02:17

If i try to capture the features by just increasing the nodes, then the mesh size increases drastically (around 8 million). It is practicably not feasible for me at all..
Is there any other way to do it??

PSYMN June 7, 2012 13:57

You may be able to increase the resolution in that area without increasing everywhere (either with clever topology, or with refined blocks (hanging nodes), sub models, or other methods), but you can't expect to capture that trailing edge with mesh that is coarser than the edge...

Ananthakrishnan June 9, 2012 06:48

Thanks a lot..i was able to create the hanging nodes by mesh refinement but the nodes are not getting projected onto the curves..
I have switched on the "project to B splines" option as well..any ideas??

http://img94.imageshack.us/img94/1539/11751626.jpg

diamondx June 11, 2012 15:09

hello ananthakrishnan,

https://dl.dropbox.com/u/35161486/merged.jpg

did you consider a mix of hexa and tri. i tried and ended up with 3M node like the picture above. may be you will need a more refined mesh depending on you flow around the wing.
I attached the project, file size is 150 Mb because of the *.*uns file. What is your computer specs ? can you handle opening 5M-6M. let me know if you can, then you can set up a case file, then share it with me, i can help you perform calculation on a cluster (big cluster i have access to).

the project file: https://dl.dropbox.com/u/35161486/Ananthakrishnan.zip

Far June 11, 2012 15:10

how did u make the hybrid meshing?

diamondx June 11, 2012 15:15

i made a small box around the airfoil, i named all the surfaces of the box "interface". then i meshed inside of the box using blocking and outside of the box with unstructured and giving a very small size to the tri element next to hexa so the merging process can be done well, after that i went to mesh and merged the two of them and selected "interface" as the common part.

Far June 11, 2012 15:19

both meshes need to be identical at interface? If yes, how to ensure this?

diamondx June 11, 2012 15:29

yes they have to be identical, regarding what ? size, i use the measure distance to calculate length of a hexa element. then i copy that length in the tri size.
That's the only way i found and the only way i know for merging two meshes. Then i trust the program in the merging process to do the adequate change in size and merging the node .
Please let me know of another trustful way.

Far June 12, 2012 02:35

wavy wall
 
See this type of topology advance toplogy , Refer to Fig. no. 5d and 5e. Although it is different software, but still you can idea how to proceed without increasing the mesh size.

Ananthakrishnan June 12, 2012 03:26

@diamondx
thats awesome..sorry i was not able to reply immediately (damn exams)...Thnaks for the cluster man...seriously...let me put my comp to acid test first...
tried the hybrid mesh but wasnt sure about the merging at the interface..i ended up having two sets of nodes at the interface one each for structured and unstructured(even though the size was matching)

i am thinking about "merge sheet with block" option...

Far June 12, 2012 04:23

delete line elements at interface (as suggested by Simon as I remember)

Ananthakrishnan June 14, 2012 05:58

Thanks to all i was able to get a decent mesh..But as of now i am unable to merge the two meshes.

What option should i use in "merge nodes" for merging the two meshes.
I initially thought if i create the unstructured mesh by using the existing mesh on the surface of the interface, then the two meshes are automatically merged!!!

https://www.dropbox.com/s/nu3y4ekrll...%20flipper.rar

diamondx June 14, 2012 14:20

are you using icem 14 ? can't open your project
in merge nodes, select merge meshes, leave the default setting and select the surface that the tri and the hexa has in common in the "merge surface mesh parts"

diamondx June 14, 2012 14:40

ok no it's version 13. but when i open the project everything disappear. can you open it and dismiss the scan plane operation then save it again ? thanks

Ananthakrishnan June 14, 2012 15:01

done..It should be working now

diamondx June 14, 2012 16:37

i could merge. i updated the project in dropbox it should be synchronized depending on your internet speed file name is "scaloped flipper_byali"

Ananthakrishnan June 14, 2012 16:51

I tried the same but i got lot of errors.. :( ..Pleaseeee tell me the procedure you followed with values...

Ananthakrishnan June 14, 2012 16:55

I am really sorry..In that project i didnt convert structured mesh to unstructured. I directly used the structured mesh to create unstructured tetra mesh.
Please delete the mesh and convert the pre mesh to unstructured before creating the tetra mesh..
Sorry again...
I think the files got corrupted. If required pls use this
https://www.dropbox.com/s/8lv33j8pp4...fliperwing.rar

mackr July 5, 2012 11:23

Hi,
sorry for posting here, but I have similiar problems with mesh merging. Maybe you can help?
Whenever I make hex mesh, then convert it to unstructered, then i want to make tetra mesh for different part (I set create mesh for only visible parts, and use exisiting mesh from parts with hex unstructered mesh) hex mesh disaapears. Am I doing something wrong?

diamondx July 5, 2012 11:49

i think when you create your mesh, it re meshes everything like a resetting. What i do is separate the parts by surfaces so i don't lose anything. then that surface will be used for merging.

mackr July 6, 2012 03:15

Yes, these regions are seperated by internal wall. But i think I've managed to do this. After using hexa mesh to create tetra on difeerent region, i just convert pre-mesh to unstructured mesh again, and click 'merge' when icem asks me what to do.
Thanks for your help anyway :)
Cheers

Ananthakrishnan July 7, 2012 03:15

mackr,
1. The merge which icem proposes is not the "merge" which was meant in this thread.
2. what you did was just to create "non conformal mesh" ie mesh nodes are not connected at the interface.they are kind of hanging.
3. after you convert the structured mesh you must be having both the meshes. So to have conformal meshes (ie to join the nodes) go to edit mesh and merge nodes.

Ananthakrishnan July 7, 2012 03:15

Just a small note.. I just found out that, if you use fluent you dont have to merge the meshes. Fluent takes care of non conformal meshes as well.
You just have to define the "interface" in "mesh interfaces" in fluent and it will run normally. Even the size of the structured and unstructured elements at the interface does not matter..


All times are GMT -4. The time now is 03:49.