Thicken mesh inside circle
 

Hello
I'm projecting intake manifold in gambit and i have huge problem. Automeshing working and it's good for calculations in fluent, but it's not accurate for calculating the flow.
I have tried many options to denisty the mesh inside the circle but none worked. Please help !

can you display any picture of your geometry and your mesh?

i did it by split the circle into 4 90° slices and meshed with quad/tri primitive

but i have another problem
i created 1/4 of torus by sweep face with mesh, but program has created too many elements on the path which i pointed.
How can i reduce congestion of those elemets?
https://scontent-fra3-1.xx.fbcdn.net...a3&oe=5657B150

i solved problem, but have another :(

Fluent crashing when all volumes are not united, what i cant do with this mesh. Can i do something with it?

If you mention Fluent, I understand your mesh is reaedy and you are solving.
Am I right, or did you mean Gambit?
As I see your picture, I see blue topologies, which means you are handling surfaces, and not volumes.
If you want you can provide me your dbs, and I could check exactly what's going on

yes, i meshed all my volumes and tried do solve it in fluent, but it gives me strange results
as velocity outflow i have pointed out two adjacent outlets , where, according to Fluent there is no flow, but instead flow are in the channel , which is not pointed out, i dont know what can i do
my file weight 9mb so i have to use some website to host it
http://www.filedropper.com/siatkazageszczrecznie

ok, I checked your geometry.
You have a connectivity problem between the manifold volume and the "exhausts".
For example look at face 176 & 459 + 467 + 464 + 455
That means you fluid stucks at this face and can't flow further
Here you need to split the face 176 with the 4 others.
Once it is one, you need to connect all faces.
At the end you should see pink surfaces in this area, which means the connectivity is ok.
You have to fix this issue for all your 8 exhausts

If i connect all faces with each other in every exhaust, wont it make my mesh dissapear there?

yes it will.
But your mesh at this moment is useless.
I forgot to mention that you also need to extend your inlet and also your outlets

so, i have to unite all volumes with each other, right? i did it at the beginning and meshed my volume with automesh and results in fluent were good but my project proffesor said, that i have to thicken the mesh inside for better results
a tried to do it 12hours in this program and i still dont have solution to solve this problem :(

if you want to have a quick solution and if you don't want a full hex mesh, then I would go back and handle your geometry with only one volume.
Then you only need to put some size fonctions (for instance at face like face.112) and also a BL.
Mesh then you volume with tet/hexcore

i'm not sure that i understood what u siad, cause i'm rookie in this program and i only want to pass my project lessons on my last semester, but i'll try to do it :) thank very much for your help

Once you have your geometry with only one volume (no split), let me know, I will help you

ok i did it as one volume
http://www.filedropper.com/onevolume

alright, If your teacher only wanted finer mesh, you can pick your volume and mesh it as follow:
Tet/Hybrid (Hexcore) with spacing 1.5 (Remove old mesh & lower mesh).
It will generate a mesh with 1.4millions cells, with hex core.
This is only 5min work
After that you only need to apply your BC

If you want something more specific you can come again and we will work on it

Attachment 43774

Attachment 43775

Attachment 43776

I consulted my project with the teacher and I had to reduce mesh size, then i laid bl 's on the inlet and outlets, teacher said it's ok but i have to many highly skewed elements 0,97>

how can i solve it? here is my model
http://www.filedropper.com/maybeok

in my version I had 0 element which skewness is > 0.97
Try to delete the BL and remesh

you can also try to split all the exhausts.
For instance create surface from edges 236 + 1134 + 1018 + 1131, then split volume with this face. It will isoltate the first exhaust.
Do the same with the other exhausts.
Then mesh all the exhausts, with cooper and spacing 1.
Once it is done create a size function, and pick as source surfaces 462 + 427 + 391 + 355 + 319 + 280 + 241 + 209 + 68 + 64 + 60 + 53 + 100 + 104 + 108 +112
As attachment pick volume with intake.
Start Size 1
Growth rate 1.1
max size 2

If the mesh is still too big for your hardware, then modify the max size in the size function from 2 to 3 , and remesh
and so on....

i understand that without boundary layers i will not have skewed elemets, but my teacher demands boundary layers on outlets and inlets and it makes problem :confused:

BL make only sense if you know the height of your first cell layer (y+>30)
Anyway you can add a BL as your teacher want, but the firxt cell height has to be set according to your Reynolds number (check y+ theory)
Then you can tune your BL with grow factor and number of layers

Wait I checked your model (maybeok) with your BL.
You attached your BL only on edges for inlet, and the other BL for all the outlet edges.
You have to attch the BL on all surfaces except inlet and outlet surfaces.
The aim for the BL is to control the height of the first cell layer. It is important for the turbulence wall function