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/)
-   -   [GAMBIT] Boundary layer mesh & map mesh in rectangular ribbed channel (http://www.cfd-online.com/Forums/ansys-meshing/108779-boundary-layer-mesh-map-mesh-rectangular-ribbed-channel.html)

shayan_mv November 1, 2012 10:44

Boundary layer mesh & map mesh in rectangular ribbed channel
 
Hello
I have a ribbed rectangular channel with two blocks on upper wall as blow:

http://imageshack.us/photo/my-images...hot001rxd.jpg/

I have performed boundary layer mesh as can be seen in the image,but I don't know how to do map mesh for the face!Is it necessary do the mesh for edges first? if so,what will happen for the boundary layer meshes?
How can I have a uniform mesh(with rectangular cells)?

Thanks

shayan

Far November 1, 2012 11:08

don't do this unless you want the hybrid mesh. This geometry is easily mappable. Make few split on the straight line and create edge between vertices. Set the no of nodes on vertical edges, grading scheme and ratio of 1.1-1.2

shayan_mv November 1, 2012 11:29

Quote:

Originally Posted by Far (Post 389693)
don't do this unless you want the hybrid mesh. This geometry is easily mappable. Make few split on the straight line and create edge between vertices. Set the no of nodes on vertical edges, grading scheme and ratio of 1.1-1.2

Thanks for your response.
If i do that,I'll have more than one edge in inlet.So, I should define more than one "inlet velocity" as boundary condition and also the same condition for "pressure outlet". Is this OK?!

-mAx- November 3, 2012 04:57

you can define many edges as part of ONE boundary condition.
Your domain should be automatically set as mappable. If not, follow Far's advice.
If you don't split your domain, enable "internal continuity" option in the boundary layer panel

shayan_mv November 3, 2012 11:52

Quote:

Originally Posted by -mAx- (Post 390008)
you can define many edges as part of ONE boundary condition.
Your domain should be automatically set as mappable. If not, follow Far's advice.
If you don't split your domain, enable "internal continuity" option in the boundary layer panel

Thanks Max
I did what you said,and I got the following result:

http://imageshack.us/photo/my-images...shot002td.jpg/

As you can see in the picture, after "map mesh" the mesh is disorder! I can make it fix by making the interval size smaller,but I don't really need to do that.I just want to have denser mesh near ribs and upper wall and to have the rest of face with larger mesh size! what shall I do now,Max?
thank you

Far November 3, 2012 13:36

Like this?


http://img255.imageshack.us/img255/8478/22767466.png

shayan_mv November 3, 2012 13:50

Quote:

Originally Posted by Far (Post 390060)

exactly.I want this! How did you do? I'm just beginner ,May I ask you to show me the steps that you have done...
Thank you very much

shayan_mv November 3, 2012 14:09

Quote:

Originally Posted by Far (Post 390060)

I know that there are different techniques of doing the mesh,but I am looking for the one that I can reach convergence in acceptable iteration.And also get good results out of that e.g. velocity vectors, Nusselts Number,...

Far November 3, 2012 14:23

First mesh was made in ICEM, which allows me to make the mesh in very few clicks and I just used the O-grid and every thing else is outcome. Whereas the pics below (similar to ICEM mesh) shows the mesh created by Gambit a d requires some geometric operations.

Download gambit file from this link : https://www.dropbox.com/s/05034x33i4...ed_channel.dbs

http://imageshack.us/a/img405/774/83187302.png

http://imageshack.us/a/img826/9830/69265640.png

shayan_mv November 3, 2012 14:41

Quote:

Originally Posted by Far (Post 390066)
First mesh was made in ICEM, which allows me to make the mesh in very few clicks and I just used the O-grid and every thing else is outcome. Whereas the pics below (similar to ICEM mesh) shows the mesh created by Gambit a d requires some geometric operations.

Download gambit file from this link : https://www.dropbox.com/s/05034x33i4...ed_channel.dbs

http://imageshack.us/a/img405/774/83187302.png

http://imageshack.us/a/img826/9830/69265640.png

Thank you so much, I think I should make many faces and mesh each one as I want

regards

Far November 3, 2012 14:44

youtube video being uploaded
 
Youtube clip is currently being processed and will post link, once it is done. Every thing was done in gambit, since you are using gambit

Far November 3, 2012 23:44

Youtube video link :

http://www.youtube.com/watch?v=CfOGD...ature=youtu.be

shayan_mv November 3, 2012 23:58

Quote:

Originally Posted by Far (Post 390111)

Dear Far
The video is not available!

Far November 4, 2012 00:00

Yeah, there was some error in uploading and done again. see this link:

https://www.youtube.com/watch?v=Gub1Kbcup2k

shayan_mv November 4, 2012 08:02

Quote:

Originally Posted by Far (Post 390113)
Yeah, there was some error in uploading and done again. see this link:

https://www.youtube.com/watch?v=Gub1Kbcup2k

Thanks a a lot dear Far. I got nearly good results...

My problem was converged after 1428 iteration! May I ask you that what is the main reason? ( I think it is not acceptable)

Regards

Shayan

Far November 4, 2012 08:07

Quote:

Originally Posted by shayan_mv (Post 390145)
Thanks a a lot dear Far. I got nearly good results...

My problem was converged after 1428 iteration! May I ask you that what is the main reason? ( I think it is not acceptable)

Regards

Shayan

If results are good then why you are not satisfied? Which version of fluent you are using?

shayan_mv November 4, 2012 08:11

Quote:

Originally Posted by Far (Post 390146)
If results are good then why you are not satisfied? Which version of fluent you are using?

Well, in comparison with the previous examples that I have done ,my problems were converged less than 300 iteration !

I use "Fluent 6.3.26"

Far November 4, 2012 08:16

It was the similar case? If not then we cannot compare them!!! This may be due to mesh problem, specially the transition between different blocks (in gambit it is face). So try to make the mesh as smooth as possible and specially at the different faces boundaries there should be slow transition and same cell size on both sides of common edge. Moreover you should make the dense mesh in the regions where you expect the separation and strong gradients.

I also recommend you to make the mesh refinement study by making the successive refined meshes to conclude mesh effects on results.

In short:

1. Mesh should be fine enough

2. Should be smooth as possible

shayan_mv November 4, 2012 08:32

Quote:

Originally Posted by Far (Post 390148)
It was the similar case? If not then we cannot compare them!!! This may be due to mesh problem, specially the transition between different blocks (in gambit it is face). So try to make the mesh as smooth as possible and specially at the different faces boundaries there should be slow transition and same cell size on both sides of common edge. Moreover you should make the dense mesh in the regions where you expect the separation and strong gradients.

I also recommend you to make the mesh refinement study by making the successive refined meshes to conclude mesh effects on results.

In short:

1. Mesh should be fine enough

2. Should be smooth as possible

OK. Thank you very much. you guide very exact. I appreciate that.

I just could not get:
1. "Nusselt Number" plot against "Re or Position"
2. " Friction factor" plot against "Re"

Far November 4, 2012 08:38

Refer to some good reference see where they plotted these values or on which plane or line? Then this can be done in Fluent or CFD-post or techplot!


All times are GMT -4. The time now is 07:04.