CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[GAMBIT] odel the stirred tank in GAMBIT

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   October 13, 2012, 12:30
Default odel the stirred tank in GAMBIT
  #1
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
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
jamalf64 is offline   Reply With Quote

Old   October 15, 2012, 01:32
Default
  #2
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
if you give more informations, maybe would someone help you
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 15, 2012, 03:18
Default
  #3
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
if you give more informations, maybe would someone help you
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
Attached Files
File Type: zip picture.zip (88.5 KB, 33 views)
jamalf64 is offline   Reply With Quote

Old   October 15, 2012, 03:30
Default
  #4
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
is your sliding mesh relating to rotation of impeller?
I saw a domain with air. Does it mean you are also solving multiphase?
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 15, 2012, 03:34
Default
  #5
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
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
jamalf64 is offline   Reply With Quote

Old   October 15, 2012, 03:44
Default
  #6
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
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..............
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 15, 2012, 03:53
Default
  #7
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
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..............
please send to me your email
I contact with you, tonight
tnx
jamalf64 is offline   Reply With Quote

Old   October 15, 2012, 07:34
Default
  #8
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
thanks
What is the size of the inner cylinder (sliding mesh zone)and the its exact location?
jamalf64 is offline   Reply With Quote

Old   October 15, 2012, 07:36
Default
  #9
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
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
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 15, 2012, 07:47
Default
  #10
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
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:
Attached Images
File Type: jpg new.jpg (29.7 KB, 33 views)
jamalf64 is offline   Reply With Quote

Old   October 15, 2012, 08:06
Default
  #11
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
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
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 15, 2012, 08:19
Default
  #12
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
I need to define moving zone (zone and not boundary condition)?
If it is needed, where it should be defined?
jamalf64 is offline   Reply With Quote

Old   October 15, 2012, 08:22
Default
  #13
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
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
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 15, 2012, 08:47
Default
  #14
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
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?
Attached Files
File Type: zip volume.zip (8.8 KB, 24 views)
jamalf64 is offline   Reply With Quote

Old   October 15, 2012, 08:55
Default
  #15
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
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
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 15, 2012, 15:03
Default
  #16
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
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 thread pointers.
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?
jamalf64 is offline   Reply With Quote

Old   October 16, 2012, 01:26
Default
  #17
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
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
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 16, 2012, 17:26
Default
  #18
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
Dear Max

Do I need to subtract impeller volume from inner cylinder?

thank you so much
jamalf64 is offline   Reply With Quote

Old   October 17, 2012, 00:47
Default
  #19
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
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!
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 17, 2012, 02:30
Default
  #20
Senior Member
 
Jamal Foroozesh
Join Date: Oct 2012
Location: Iran
Posts: 126
Rep Power: 4
jamalf64 is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
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?
jamalf64 is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Meshing stirred tank with gambit. boh_tea FLUENT 13 March 29, 2013 14:29
model the stirred tank in GAMBIT jamalf64 FLUENT 0 October 13, 2012 12:24
Simulation of stirred tank using sliding mesh technique aymneng Main CFD Forum 0 March 3, 2012 13:19
Gambit Meshing of stirred mixing tank shadyenany FLUENT 4 September 15, 2011 12:13
CFX 5.5.1 stirred tank and LES problem Nishant CFX 2 September 13, 2002 07:11


All times are GMT -4. The time now is 05:45.