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] Rotating Concentric Cylinder with mech density higher at the edges (http://www.cfd-online.com/Forums/ansys-meshing/108526-rotating-concentric-cylinder-mech-density-higher-edges.html)

rshbhb October 25, 2012 10:57

Rotating Concentric Cylinder with mech density higher at the edges
 
1 Attachment(s)
Dear MAX,

Hello Sir,

I want to make the kind of geometry as shown in the image (attached) in the gambit software. I believe that you can help me.

Awaiting your reply soon.

Thank you.

ghost82 October 25, 2012 12:25

Hi,
1-create the external cylinder (centered in 0,0,0)
2-create the internal cylinder (centered in 0,0,0)
3-subtract the internal cylinder from the external one
4-create the plane y=0
5-split the volume with this plane
6-mesh edges of the lower base of your volume and mesh the two faces with quad map scheme (if you cannot mesh with map scheme change the vertex type to end)
7-mesh the generatrix of the cylinder
8-mesh the volume with hex cooper scheme, choosing as faces bottom and top faces

Daniele

rshbhb October 25, 2012 12:56

Thank you Daniele.

I'll try and inform you.

ghost82 October 26, 2012 02:52

Quote:

Originally Posted by rshbhb (Post 388538)
Thank you Daniele.

I'll try and inform you.

I tried the steps above, the cells of the 2 volumes if meshed with the cooper scheme will be slightly distorted;
so:

1-create the external cylinder (z positive)
2-create the internal cylinder (z positive)
3-subtract the internal cylinder from the external one
4-create the plane y=0 (for example a big square in xz)
5-split the volume with this plane
6-mesh edges of the bases of your 2 volumes and mesh the 4 faces with quad map scheme
7-mesh the generatrix of the cylinder
8-mesh the 2 volumes with hex map scheme

Daniele

rshbhb October 26, 2012 06:10

I tried this too. but the problem I am facing is, I cannot join back the two volumes after meshing.

I tried to merge the two volumes but the two faces (inside the volume of the annulus) still remain . How do I remove them?

If there is any other alternative (like, to give the BC for the interior faces as INTERIOR) then please let me know.

Thank you,

Daniele.

ghost82 October 26, 2012 06:15

Quote:

Originally Posted by rshbhb (Post 388635)
I tried this too. but the problem I am facing is, I cannot join back the two volumes after meshing.

I tried to merge the two volumes but the two faces (inside the volume of the annulus) still remain . How do I remove them?

If there is any other alternative (like, to give the BC for the interior faces as INTERIOR) then please let me know.

Thank you,

Daniele.

Why do you want to merge the volumes?
Internal faces are not treated as walls, and the two volumes are connected as they are a single volume!
Make sure you check "connected" when you split the volume!

rshbhb October 26, 2012 06:26

Thanks again. I thought that internal faces will be counted as walls.

I want to Give boundary conditions as:
Upper faces-2faces as walls (stationary)
Lower faces-2 faces as walls (stationary)
Interior faces (rotating)
exterior faces (stationary)

& the interors volumes as FLuid (liquids)
(Basically I am trying to make a rheometer geometry)

Should I define the internal & external faces as walls too,, in GAMBIT ?

ghost82 October 26, 2012 07:00

Quote:

Originally Posted by rshbhb (Post 388640)
Should I define the internal & external faces as walls too,, in GAMBIT?

Yes, you have to define them as walls

rshbhb October 26, 2012 07:12

:)
Will I have to select any kind of dynamic or sliding mesh OR I can do normal meshing and rotate the inner walls in FLUENT solver ? (I use the 2nd option).

-Awaiting a quick reply. THanks

ghost82 October 26, 2012 07:16

Quote:

Originally Posted by rshbhb (Post 388652)
:)
Will I have to select any kind of dynamic or sliding mesh OR I can do normal meshing and rotate the inner walls in FLUENT solver ? (I use the 2nd option)

-Awaiting a quick reply. THanks


I think you can only set in fluent the inner wall as "moving"->rotational in respect to z axis as in the tutorial "Non-Newtonian Transitional Flow in an Eccentric Annulus" (search google); However, you should better open a new thread in the fluent forum to have other opinions.

Daniele

rshbhb October 26, 2012 07:20

Quote:

Originally Posted by ghost82 (Post 388653)
I think you can only set in fluent the inner wall as "moving"->rotational in respect to z axis as in the tutorial "Non-Newtonian Transitional Flow in an Eccentric Annulus" (search google); However, you should better open a new thread in the fluent forum to have other opinions.

Daniele

I'll open a new thread in the FLUENT forum. But as you are aware of the problem description can you help me out with FLuent simulation too ?

ghost82 October 26, 2012 07:25

Quote:

Originally Posted by rshbhb (Post 388655)
I'll open a new thread in the FLUENT forum. But as you are aware of the problem description can you help me out with FLuent simulation too ?


First try to solve the problem on your own, you will learn lots of things from your mistakes; however if you will get stuck at some point me and other people will help you.

Daniele

rshbhb October 26, 2012 07:34

Quote:

Originally Posted by ghost82 (Post 388656)
First try to solve the problem on your own, you will learn lots of things from your mistakes; however if you will get stuck at some point me and other people will help you.

Daniele

Dear Sir/ Ma'am,

I have tried to solve the problem with simple mesh geometry but the results obtained by them are a bit absurd.

I'll be uploading the images of my simulations in the new thread for my queries... I'll post the link to my thread in this thread too in few minutes...

THank you !

rshbhb October 26, 2012 07:53

Quote:

Originally Posted by rshbhb (Post 388655)
I'll open a new thread in the FLUENT forum. But as you are aware of the problem description can you help me out with FLuent simulation too ?

Below is the link to the new thread:
Please help. :)

Kind Regards,
Rishabh

http://www.cfd-online.com/Forums/flu...tml#post388662


All times are GMT -4. The time now is 13:40.