CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (https://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [GAMBIT] odel the stirred tank in GAMBIT (https://www.cfd-online.com/Forums/ansys-meshing/108056-odel-stirred-tank-gambit.html)

 jamalf64 October 13, 2012 12:30

odel the stirred tank in GAMBIT

Hi dear friends

Im MSc student in material science. I want to model the stirred tank in GAMBIT for use sliding mesh in fluent.
Can everybody any help me in creating it?

thanks

 -mAx- October 15, 2012 01:32

 jamalf64 October 15, 2012 03:18

1 Attachment(s)
Quote:
pictures of my problem is below.
units in cm
depth of groove: 3mm
how I do model inner&outer zone for sliding mesh in my problem?
thanks

 -mAx- October 15, 2012 03:30

is your sliding mesh relating to rotation of impeller?
I saw a domain with air. Does it mean you are also solving multiphase?

 jamalf64 October 15, 2012 03:34

Quote:
 Originally Posted by -mAx- (Post 386618) is your sliding mesh relating to rotation of impeller? I saw a domain with air. Does it mean you are also solving multiphase?
dear max
exactly. you understand correctly

 -mAx- October 15, 2012 03:44

ok
First, you need to split your domain.
I talk now about multiphase: if the height of yoru domain is 26.5cm, then you create and move a plane and you split the volume for having 2 volumes in respect of your picture (height 21.5 & 5)
You should be able to select either water volume, or air volume.

Second, the sliding zone: for that you will create a cylinder with a radius 5,6 7 or waht you want (radius has to be greater thant max radius from impeller). Move the the cylinder in such way that it will be coaxial to the impeller.
Split your water volume with the cylinder, and delete the cylinder. Check if you can select the impeller zone (rotor). If yes, copy this volume with any translation's vector.
Delete the original impeller volume. Now you have an hollow in the water domain. Select the cylindric surface from stator domain, and define it as interface.
Select the cylindric surface from rotor (copy), and define it as interface.
Now move the rotor (copy) back , with opposite translation's vector.
That's it..............

 jamalf64 October 15, 2012 03:53

Quote:
 Originally Posted by -mAx- (Post 386621) ok First, you need to split your domain. I talk now about multiphase: if the height of yoru domain is 26.5cm, then you create and move a plane and you split the volume for having 2 volumes in respect of your picture (height 21.5 & 5) You should be able to select either water volume, or air volume. Second, the sliding zone: for that you will create a cylinder with a radius 5,6 7 or waht you want (radius has to be greater thant max radius from impeller). Move the the cylinder in such way that it will be coaxial to the impeller. Split your water volume with the cylinder, and delete the cylinder. Check if you can select the impeller zone (rotor). If yes, copy this volume with any translation's vector. Delete the original impeller volume. Now you have an hollow in the water domain. Select the cylindric surface from stator domain, and define it as interface. Select the cylindric surface from rotor (copy), and define it as interface. Now move the rotor (copy) back , with opposite translation's vector. That's it..............
I contact with you, tonight
tnx

 jamalf64 October 15, 2012 07:34

thanks
What is the size of the inner cylinder (sliding mesh zone)and the its exact location?

 -mAx- October 15, 2012 07:36

the radius is up to you, but the cylinder should englobe the impeller.
Cylinder's axis hast to be the same than impeller
This split will generate the rotor zone

 jamalf64 October 15, 2012 07:47

1 Attachment(s)
Quote:
 Originally Posted by -mAx- (Post 386660) the radius is up to you, but the cylinder should englobe the impeller. Cylinder's axis hast to be the same than impeller This split will generate the rotor zone
This is the new image:

 -mAx- October 15, 2012 08:06

yes; now copy your cylinder anywhere and apply interfaces.
In your case you will need to also apply interfaces on top and bottom from cylinder.
And now I wonder if it would be more easy to extrude your cylinder in air-domain.
Thus, you will also have sliding mesh in air-domain

 jamalf64 October 15, 2012 08:19

I need to define moving zone (zone and not boundary condition)?
If it is needed, where it should be defined?

 -mAx- October 15, 2012 08:22

both: zone and boundary conditions
Then if your sliding mesh is successfull you can add complexity with multiphasis

 jamalf64 October 15, 2012 08:47

1 Attachment(s)
Quote:
 Originally Posted by -mAx- (Post 386669) both: zone and boundary conditions I would recommand you to start without multiphase. Then if your sliding mesh is successfull you can add complexity with multiphasis
Now we have 3 volume that their pictures attached below.
How to be define the zones?

 -mAx- October 15, 2012 08:55

as I said I would split your first zone (first picture) with the same plane (air-water), and then delete the air-domain (2nd picture) and also the rest of first zone.
That means only water.
Before deleting, save as another name for being able to pick this dbs later.

For the zone, you only need to define rotor as another fluid domain (say rotor). But the most important is interfaces.
For that your both volumes (stator and rotor) has to be disconnected (as I previously described). To check if they are, try to move (not copy) the rotor anywhere. If it is successfull, then both volumes are disconnected

 jamalf64 October 15, 2012 15:03

Hi dear Max
are you sure that inner cylinder must be deleted?
when I delete the inner cylinder, fluent shows below error:
" Grid Check
Domain Extents:
x-coordinate: min (m) = -1.200000e+001, max (m) = 1.200000e+001
y-coordinate: min (m) = -1.199330e+001, max (m) = 1.199330e+001
z-coordinate: min (m) = 0.000000e+000, max (m) = 2.650000e+001
Volume statistics:
minimum volume (m3): 3.673007e-003
maximum volume (m3): 9.045283e-001
total volume (m3): 1.159029e+004
Face area statistics:
minimum face area (m2): 4.027711e-002
maximum face area (m2): 1.069187e+000
Checking number of nodes per cell.
Checking number of faces per cell.
Checking number of cells per face.
Checking face cells.
Checking bridge faces.
Checking right-handed cells.
Checking face handedness.
Checking face node order.
Checking element type consistency.
Checking boundary types:
Checking face pairs.
Checking periodic boundaries.
Checking node count.
Checking nosolve cell count.
Checking nosolve face count.
Checking face children.
Checking cell children.
WARNING: Unassigned interface zone detected for interface 6
WARNING: Unassigned interface zone detected for interface 7
Checking storage.
Done.

WARNING: Grid check failed."

What do I have to do?

 -mAx- October 16, 2012 01:26

basically you only delete the inner cylinder you used for the split.
The other inner cylinder (with impeller) is deleted BUT replaced by its own copy.
So you are not suppose, at the end, having a hole at place of rotor.
The warnings are ok since you didn t define the grid interfaces

 jamalf64 October 16, 2012 17:26

Dear Max

Do I need to subtract impeller volume from inner cylinder?

thank you so much

 -mAx- October 17, 2012 00:47

yes.
So in you case:
*copy volume 3 (translaction vector (0 0 0)) --> it generates a volume 5
*unite volumes 2 & 3
*substract volume 2 with 1
*split volume 2 with 5
*delete impeller volume (6) --> here this volume should be deleted with substract tool, but I don't know why it is not the case
*copy volume 5 with (0 0 50) --> it generates a volume 7
*delete volume 5
*assign all the interfaces on volume 2 & 7
*move volume 7 with (0 0 -50)
That's it!

 jamalf64 October 17, 2012 02:30

Quote:
 Originally Posted by -mAx- (Post 386983) yes. So in you case: *copy volume 3 (translaction vector (0 0 0)) --> it generates a volume 5 *unite volumes 2 & 3 *substract volume 2 with 1 *split volume 2 with 5 *delete impeller volume (6) --> here this volume should be deleted with substract tool, but I don't know why it is not the case *copy volume 5 with (0 0 50) --> it generates a volume 7 *delete volume 5 *assign all the interfaces on volume 2 & 7 *move volume 7 with (0 0 -50) That's it!
Is that volume 1=impeller, volume 2=inner cylinder & volume 3= large cylinder?

All times are GMT -4. The time now is 14:36.