so your problem is the periodicity and not the mesh? How did you setup periodicity?

I can read the other parts of my geometry, this is the only one I cannot read.
For all the other parts, I have periodicity problem: all the periodic zones are considered as translational, I can change in Fluent to rotational but then the angle is equal to 0 and I don't find where I can give Fluent the real value of the angle.

I couldn't read your file (Far) since some files are missing. Or can I use mine to complete (*.uns..)?

Rodriguez: I don't have this message, when it starts to read the mesh, appear the message I've posted before. Can you explain me how you deal with periodicity in Fluent?

I am working on Linux, Fluent in parallel.

sorry, I didn't see this post before replying.
For periodicity I did :
Mesh/Global Mesh Setup, then Set-up periodicity (basis 0.0.0, axis 1.0.0 and angle 45)
Blocking/Edit block, then Periodic Vertices

Then in Output/Boundary Conditions, I give the periodic conditions to the surfaces

Instead of default method choose "vector option and select two points of axis of rotation (make these points by yourself). Also when you apply Y-block every thing goes away like edge mesh parameters, association and even periodicity. So you have to again associate, again define periodic vertices and again specify edge mesh parameters (This is bug I think in R14.5) and then you are done.

PS. 1. Files I have uploaded are saved in R14.5. Are you able to open .tin and .blk if yes then you can get generate mesh yourself.

2. I am attaching a sample project done for you where periodicity is applied.

In Icem: You just need to give some name to each surface you want to become periodic, such as "front" and "back" or whatever. Export your mesh.
In Fluent: Go to the "Cell Zone Conditions" and click on each of the surfaces. Note the "ID" number, that is shown in the tab. Then, go to the fluent terminal and type: "mesh" then "modify-zones" then "make-periodic". Follow the instructions. Fluent will then delete one of the zones an the other one will be left under "Cell Zone Conditions". If you click on that surface a "periodic conditions" button will appear, where you can set up things such as pressure drop along the periodic zones.

I showed in one the posts that you can output one periodic boundary condition in ICEM to Fluent easily (your case has single periodicity) and whereas for double periodicity you should define one in ICEM and other in Fluent

Ok found it http://www.cfd-online.com/Forums/ans...ty-fluent.html


Here we go for more

http://www.cfd-online.com/Forums/ans...ification.html

http://www.cfd-online.com/Forums/flu...-geometry.html

http://www.cfd-online.com/Forums/ans...h-overlap.html

Oups, quite hard to understand...I look at it now.

In the meantime, I've generated the mesh from your file and this time, Fluent could read it. But as for the other parts, the periodicity is set to translational.
So I tried to do what Rodriguez wrote, but the strange thing is that when imported in Fluent, I have just 1 periodic surface, no shadow, so maybe Fluent just see 1 surface instead of 2 and that's why he puts directly an angle of 0 when I tell him to use rotational. mean, if considering your file, in Fluent, I just have per1, no per2, but on the display, when I clic on per1, I have the 2 surfaces (Fluent puts per1+per2 in per1)

This is how periodic works in Fluent. You will have only one entity for two periodic surfaces .

I really don't understand: I've created a part with NO PERIODICITY (no periodic mesh, no vertex periodic...no boundary condition with periodicity in ICEM)... but it's not read in Fluent and I've a message telling that 2 zones have inappropriate zone type (periodic)...but I didn't specify ANY periodic zone in ICEM !!!
I'm getting really mad now.

but so, how do I give Fluent the 45 degree value?

Did you free all the points in ICEM from beeing periodic? Did you recreate the premesh and re-convert to unstructured mesh?

yes I did.
But the names of surfaces were "periodic_dx" and "periodic_sx", I didn't change that...they are just...names...but this time, I named them : "titi" and "toto"...and Fluent read them as separate surfaces (maybe putting the word "periodic" in the name gives automatically to Fluent the "idea" of periodicity ), no problem for check grid...WUNDERBACH :-) .... but impossible to create the periodicity in Fluent, following your advices....

sorry if you already read that post : ok for periodicity, I just forgot to change the axis in Fluent. It's ok now. So, it seems that a name shouldn't contain "key" words. But why do I have to do it like this? Periodicity in ICEM should be ok!

If you want to specify it in Fluent via TUI, Fluent should automatically determine angle

yes, he did it :-) (45 degrees)
But I still don't understand why I have to cancel all periodicity in ICEM. Isn't there any risk that creating mesh in ICEM with no periodic conditions, leads to an "non-periodic" mesh? I mean, a mesh that would not correspond cell by cell on the 2 surfaces?

Yes it should do as want to do. But for that you need to understand how ICEM periodic function works. You have to specify that at two places. One in mesh panel and second in blocking (making all corresponding vertices periodic)

As far as I understand it, you have to ensure that by yourself. Also, I think that marking nodes as "periodic" won't do that for you. But maybe I am wrong.
ps: great that you did it!

hi Far, Rodriguez,

well, about periodicity in ICEM, except the fact that I was using the "user defined by angle" instead of "vector", where am I wrong?

I was doing this:

Mesh/Global Mesh Setup then set-up periodicity
Blocking/Edit Block , then Periodic Vertices (selecting the pair of periodic vertices, respecting the same orientation each time)
Output/ Boundary Conditions , then giving periodic to the periodic surfaces

you're right Rodriguez, I'm happy it's quite done, but it's not automatic to cancel the periodic vertices, sometimes when doing Pre-Mesh and loading the mesh, everything is going wrong...so I have to cancel blocking and do it again....taking a lot of time.
The good point is that I'm learning a lot like this.

Another question, when doing block, the points and curves must not be included really? only surfaces and body? maybe I'm wrong with this from the beginning.

Thank you so much to all of you; I wouldn't have done it without you. It's not completely finished, but I hope big problems are over now.

I haven't used it lately. But difference is that with user defined angle, it is assumed that you have axis of rotation is on any three of principal axis. So if you have offset then you cannot use it. Instead use "vector option and choose two points which lies on axis of rotation.

Just cancel the periodicity in the same panel where you have created.

For 3d case, you just need surface for boundary conditions and material for interior. For 2d case you need curves for boundary conditions and no need of material (or body) for interior.

Hello again !!!

I've meshed all the different parts, merged everything in Fluent. It was ok, but when running simulations, results were really strange, I think I had too many interfaces. So I've been trying to mesh again in 1 piece... I've done it maybe 10 times!!! and everytime, there is something wrong.
I send you the last try. Could someone tell me why the mesh is coming like this (at the upper right "corner" ) ? sometimes, this part comes ok but with other problems and sometimes not. I always do the same thing so I really don't understand.

Hi, there is a .zipx file inside the zip file. Can you uplaod a "common" file format? Such as just .zip ?

the file is too big if *.zip, how else can I send it?

ok, I've tried AGAIN.
Now I have another problem of
"Cell Centroid is xc 35.776754 yc 6.767326 zc 0.400559
WARNING: no face with given nodes. Thread 16, cell 10995"
I read on-line that it could be a problem of meshing.

So I opened again the file and got what is on the picture !!! what is it????
I don't know anymore what to do with ICEM !!!!
Everytime I have a different kind of error. Are there some bugs or I don't know?

@yorelchr: topology is not great.

what do you mean? what do all these blue lines mean?

blue lines show internal edges. You have made several y blocks even in the areas where they are not needed

I have just done Y-blocks for the part down the geometry and the upper-right part. I have done that maybe 30 times, always starting from the geometry (not canceling existing blocks) and it is the first time I get that.
I am really getting mad. It's been exactly 2 weeks I've been trying and I know now that everytime, I will have a different error (interior parts seen as wall, error on cells without mesh like the previous one, mesh not read for I don't know which reason...).

Quality > 0.8
Angle > 45

I didn't check it in fluent. Just finished blocking and uploaded here. Please check blocking and let me know if something is missing...
https://dl.dropboxusercontent.com/u/...nozzle_Far.zip



http://imageshack.us/a/img4/4300/a001ou.jpg
http://imageshack.us/a/img195/8517/a002x.jpg
http://imageshack.us/a/img856/998/a003b.jpg

More pics
 

http://imageshack.us/a/img441/3064/a004z.jpg
http://imageshack.us/a/img211/565/a005ha.jpg
http://imageshack.us/a/img825/9423/a006r.jpg

Thank you very much for this!
I see that I was doing wrong with my Y-blocks.
There were 2 problems when I generated the mesh, maybe because I have not all the files. For one it was ok, I could fix it. For the other, I send you a picture of it.
And I was wrong also since I was trying to avoid the small cells (coming from the beginning) all through the chamber.

Corrected files...


https://dl.dropboxusercontent.com/u/...-2013_Far2.rar

PS: Wait at least one hour so that files get uploaded on dropbox.

I can't get the files, I have :
Error (404)
We can't find the page you're looking for. Check out our Help Center and forums for help, or head back to home.

now check link. it is working

Far, in this triangle shaped geometry, where you have the three blocks: Is there a way to tell ICEM to make the angle of the three edges in the middle equal (each 120°)? Or do you have to estimate it by hand?
Attachment 21295

It is done by ICEM. If you adjust everything in place and make the Y block, each angle would measure 120. But once you have changed it, there is no way to ensure it.

Hi Far,

sorry for replying so late but I had to work on something else. I'm now back on this job.
Thank you very much for what you have posted. There is just a problem with periodicity. I've "rebuild" the parts (lato_sx and lato_dx) but the problem remains. So yesterday, AGAIN, I tried by myself and this time all was ok, at least, it seemed. Fluent read without problem, ok also for periodicity, but I encountered a new problem (!!!). I send you the picture. When I go back to ICEM, in the menu on the left, under mesh, I have some shells and the problem seems to be there. However I'm running the case with Fluent and it seems ok but I don't know if the results will be influenced by this...the problem lies at the main inlet : the inlet mesh takes a part of the wall mesh, the wall-ogiva takes a part of wall-inlet...I don't know why I have this situation. When running the case, I import profile at the inlet, so, only cells in the profile are concerned, so maybe the calculations can be ok, but still....why?

everything seems alright. I am not able to understand where problem lies :o

well, maybe I was not really clear in my explanations :-)
the inlet should be just the vertical "blue" part and in fact, when displaying it, I also have a part of the wall.

delete that block only.

create new block with eight vertices. four are there, and click on four locations approximately.

Associate edges to curves and vertex to point and you are done.

ok, I'll try that, I'm just afraid that maybe the face between the 2 bocks will be seen as wall in Fluent, already had this problem ... I'll tell you
Thanks again!

No , it will not happen. don't make any face to surface association