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] New meshing with GAMBIT (http://www.cfd-online.com/Forums/ansys-meshing/84439-new-meshing-gambit.html)

egge24 January 29, 2011 16:56

New meshing with GAMBIT
 
Hi,
I'm new using GAMBIT meshing and I'm having some dificulties.
I'm trying to mesh a porous disc, to create a pressure jump, inside a water tank considering a water-air interface.
  1. I create the geometry of the disc as a face and the tank as a volume. Is this correct or I should create the disc as a volume?
  2. I mesh the disc.
  3. Delete the volume of the tank, leaving the faces behind.
  4. And when I try to create a unique volume, selecting all the faces, gives an ERROR displaying: Unable to create volume because face "disc" is not utuche to the volume.
Hi I can attach the face "disc" into the volume?

Any help will be appreciated.
Regards,
Eduardo

-mAx- January 31, 2011 02:41

*In Gambit-BC you can choose Porous jump, as surface.
In the User Guide, this kind of BC requires: Face Permeability / Porous Medium Thickness /Pressure-Jump Coefficient

*Define your tank as volume, and split it with your disk. Now the disk belongs to your volume

egge24 February 2, 2011 18:30

Thank you -mAx-! I will be back soon with more questions.

egge24 February 2, 2011 21:45

Hi again,

I was able to create a volume including the actuator disc. The actuator disc is only half modelled being attached to a symmetry face, in this case v_face_7. The geometry of the actuator is represented as a face.

I first mesh the actuator disc face using tri element and PAVE type.
But when I`m trying to mesh the whole volume I get an error saying:
"Face v-face 7 contains hard lines and must be meshed using PAVE"

The problem is that in the mesh volume menu I don`t have that option!!

Any suggestions?

Thank yo in advance.

-mAx- February 3, 2011 02:33

post pictures

egge24 February 3, 2011 16:07

Hi -mAx-,
Here are some figures:

Figure 1 - the whole domain; tank and actuator disk.

http://img706.imageshack.us/img706/9199/tanque1.jpg

Figure 2 - v_face 7, includes the symmetry face and the diameter of the actuator disk attached to the symmetry face.

http://img525.imageshack.us/img525/9224/tanque4.png

Figure 3 - Actuator disk using Tri elements and type PAVE.

http://img12.imageshack.us/img12/5334/tanque2.png

If you need any other figure or information let me know.

Thank you.

-mAx- February 4, 2011 02:42

Split your volume
>> Create a (YZ) plane, an place it at the x-coordinate where you disk lies.
Split your volume with this plane.
If you are handling real entities it should be ok, if not I will guide you for doing this in virtual.
Once it is splitted, remesh

egge24 February 7, 2011 17:29

Thanks -mAx-!
It works with the advice you gave me. I gave the plane I created a boundary condition type interior, Is this correct?
I want to ask you a other questions:
  1. Must I mesh the actuator disk before I mesh the volumes or can I mesh both volumes leaving the actuator disk unmesh and give the actuator disk face a boundary condition type of porous jump?
  2. In case I want to model a VOF, water-air interface, for an open channel, Do I have to include a face, BC type interface, along the XZ-plane and mesh both volumes separately before I export the mesh to FLUENT? or can I give this interface condition in FLUENT?
Thanks again.

-mAx- February 8, 2011 02:17

If your splits are correct, you aren't suppose to define the split surfaces as interior. Gambit will detect them automatically as interior, but won't be available in the pre-postprocessing. (will be "merged")
If you want to use, then yes you can define them as interior

1.Mesh and BC are independant. you can apply BC once your mesh is ready (or before meshing, it makes no difference).

2.you have 2 possibilities:
*a> you split your volume into 2 subvolumes, and define each volume as separated fluid volume (fluid 1 and fluid2), then in fluent you can set up your vof model
*b> you don't change your mesh, but you will define the different phase locations within fluent.

I always choosed way a, it is easier.
If you want b, then I think you need to digg around Grid Region Adaptation & Manage Adaptation Registers

cadfemcis February 8, 2011 02:51

Cleaning-Up Geometry for Airplane
 
http://www.youtube.com/watch?v=wmfHHAp55KU

December 28, 2010 Исправление геометрии и построение расчётной сетки для фюзеляжа самолета в среде ANSYS Workbench 2.0 Материал подготовил Колесник В. (Copyright, 2011, ЗАО "КАДФЕМ Си-Ай-Эс").
CADFEM-CIS Tutorial #11-Cleaning-Up Geometry for Airplane.mp4 :cool:

egge24 February 8, 2011 19:44

Thanks again -mAx-! you really help me. Now I'm going to try to set up the model in FLUENT... probably, in the following days, I will be posting a new thread about modelling open channel flow with VOF.
Perhaps, do you know any good tutorial that could guide me to set up and solve my problem in FLUENT?

Kind Regards


All times are GMT -4. The time now is 01:25.