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/)
-   -   [ANSYS Meshing] Problem with structured meshing pipe elbow (http://www.cfd-online.com/Forums/ansys-meshing/105103-problem-structured-meshing-pipe-elbow.html)

Kirjain July 23, 2012 07:45

Problem with structured meshing pipe elbow
 
2 Attachment(s)
Hi all,

I am having problems with generating a structured mesh on a pipe with a 90-degree bend. I am using Ansys Meshing and don't have any access to other applications.
Otherwise things would be going fine but just at the bending point the mesh breaks apart into something well peculiar: Random 3D ripples form on the side of the pipe mesh no matter what sort of sizing options I have chosen. I added a few pictures so you can see the abnormality. What am I doing wrong or is it really just a quirk in the software?

Gweher July 23, 2012 08:03

If you could add your mesh file and .agdb geometry that I could have a look. But it may be related to your edge sizing or the way you created the sweep method. I don't know in which order you mesh your different subparts, or if you applied a automatic (default) or a manual "source and target" within the sweep method options.

Anyway, by looking at your pictures, i don't see any mapped face method, this will also improve your mesh quality. Again I don't have lot of information to help you out but if you share your .agdb file I can have a quick look.

Also you can relate to this topic regarding the mesh generation inside a U-bend (180 elbow)

flotus1 July 23, 2012 08:05

Try the advice I gave a few hours ago in a similar thread.

Quote:

Originally Posted by flotus1 (Post 372952)
First of all, you should apply a "structured mesh" to all the surfaces.
This will eliminate the unstructured mesh at the inlet faces.

In the second step, you could try to reset your mesh data (right-click on the mesh, choose "clear generated data")
This often helps when the Ansys mesher seems to ignore your input when
creating the mesh.
Additionally, you should deactivate the "use advanced size functions" option.
Afterwards, you can generate the mesh anew.

When applying sizing on edges, you should always choose "hard" as behaviour. Otherwise the ansys mesher does whatever it wants, but won't create the mesh you have in mind.

Hope this helps.

BTW: the biasing in wall-normal direction looks a bit hard. The volume jump is definitely too high.


Kirjain July 24, 2012 01:32

Hi Gweher could you please give me your email address and I would be happy to send you my meshing and geometry files! I tried the mapped face method as well but it seems to amount to nothing! I'm confused with the generated mesh because only one side of the pipe shows abnormalities whilst meshing even though it is clearly a symmetrical case.

Gweher July 24, 2012 03:36

1 Attachment(s)
For those who are curious, the problem was solved by selecting "manual source and target" under "sweep method" and specifying the source and target faces.

Kirjain July 24, 2012 06:05

Weird results in Fluent
 
1 Attachment(s)
Thank-you, this really helped me. The problem went away after inserting a few face mappings as well, even though the orthogonal quality wasn't as good.

Could I still ask you for a tad more help with the results I get out of Fluent? I'm using the post-processing software in Workbench and the vector plots I obtain are well confusing..! I've attached a picture of both the vector plot for velocity in the pipe bend and the original mesh as a thumbnail for you to see. It seems as if the walls of the pipe weren't there as the velocity vectors happily go through them! Have I just missed something in the pre-calculation process? Is there a way to make the walls imprenetable? Or is this just a quirk in the post-processing programme? I do have all the wall surfaces defined as a named selection etc. so the problem doesn't derive from that.

flotus1 July 24, 2012 06:39

Normalize the vector size or make the vectors smaller, this will solve the confusing display type.
Since there are velocity vectors pointing towards the surfaces in cells which are a little bit away from the wall, the vectors seem to penetrate the wall if they are too long.

atheresia February 7, 2014 10:30

Quote:

Originally Posted by Kirjain (Post 373131)
Hi Gweher could you please give me your email address and I would be happy to send you my meshing and geometry files! I tried the mapped face method as well but it seems to amount to nothing! I'm confused with the generated mesh because only one side of the pipe shows abnormalities whilst meshing even though it is clearly a symmetrical case.

Hi! Any chance you could send me the files as well? I am having similar problems.
Do let me know and I will inbox you my email address:)
Many thanks in advance!

atheresia February 7, 2014 11:05

Quote:

Originally Posted by Gweher (Post 373154)
For those who are curious, the problem was solved by selecting "manual source and target" under "sweep method" and specifying the source and target faces.

Hi!

Any chance you would be able to help me in meshing my geometry as below?
Many thanks in advance!
http://oi62.tinypic.com/10pauxz.jpg


All times are GMT -4. The time now is 14:45.