CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

rotating propeller in stationary baffled vessel

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 10, 2010, 12:21
Default rotating propeller in stationary baffled vessel
  #1
Senior Member
 
raymond
Join Date: Nov 2009
Posts: 149
Rep Power: 7
wlt_1985 is on a distinguished road
I would like to model a rotating propeller inside a stationary baffled vessel with water as the fluid inside. I had a lot of trials. Unfortunately, in all my model, the rotating propeller always rotating with the baffled vessel. I do not know which part I am making wrong. Does anyone how to model the correct model in this case? Please help me. Thanks.
wlt_1985 is offline   Reply With Quote

Old   October 11, 2010, 02:51
Default
  #2
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,972
Rep Power: 30
-mAx- will become famous soon enough
The easiest way would be to treat your problem with sliding mesh.
Basically you need 2 regions which are not connected: rotor and stator, and then define interfaces
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 11, 2010, 03:03
Default
  #3
Senior Member
 
raymond
Join Date: Nov 2009
Posts: 149
Rep Power: 7
wlt_1985 is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
The easiest way would be to treat your problem with sliding mesh.
Basically you need 2 regions which are not connected: rotor and stator, and then define interfaces
Thanks for help. I tried to model with two regions, one is the solid propeller and another is water fluid. When trying to define the interface between this two region, message has been shown as below:

Warning: materials in neighbor cell threads (3 and 4) of interior zone 14 are of different types (aluminum and water-liquid). This problem MUST be fixed before solving!

I totally do not have idea in solving it.

Please help.

Thanks
wlt_1985 is offline   Reply With Quote

Old   October 11, 2010, 03:09
Default
  #4
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,972
Rep Power: 30
-mAx- will become famous soon enough
not like that.
Substract your solid region (you should have empty area instead of solid impeller)
Then if your geometry enables it, draw (split) a circle around your rotor.
You have now 2 regions, the disk which is your rotor, and the outer domain which is your stator.
As I said you need to disconnect your 2 regions, for applying interfaces.
Check online help chapter 11.2 Sliding Mesh Theory
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 11, 2010, 04:23
Default
  #5
Senior Member
 
raymond
Join Date: Nov 2009
Posts: 149
Rep Power: 7
wlt_1985 is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
not like that.
Substract your solid region (you should have empty area instead of solid impeller)
Then if your geometry enables it, draw (split) a circle around your rotor.
You have now 2 regions, the disk which is your rotor, and the outer domain which is your stator.
As I said you need to disconnect your 2 regions, for applying interfaces.
Check online help chapter 11.2 Sliding Mesh Theory
Thanks for your help. If I would like to model the motion behavior of the fluid (initially which is stationary) which is affected by the motion and shape of the solid stirrer inside the stationary baffled vessel, the solution mentioned above still valid for it? Or any modification should be applied?

Really thanks to your help.
wlt_1985 is offline   Reply With Quote

Old   October 11, 2010, 04:30
Default
  #6
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,972
Rep Power: 30
-mAx- will become famous soon enough
what I mentionned above is just the geometry / mesh side (no physics).
How they move, can you explain later in fluent (not in gambit)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 11, 2010, 05:24
Default
  #7
Senior Member
 
raymond
Join Date: Nov 2009
Posts: 149
Rep Power: 7
wlt_1985 is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
what I mentionned above is just the geometry / mesh side (no physics).
How they move, can you explain later in fluent (not in gambit)
Thanks. One more question, if I split my rotor (impeller) by using a geometry which has the same shape but larger size to my rotor (impeller) instead of a circle, does it work for my sliding mesh model?
wlt_1985 is offline   Reply With Quote

Old   October 11, 2010, 05:37
Default
  #8
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,972
Rep Power: 30
-mAx- will become famous soon enough
no.
The split should be a circle.
For undestanding, try to imagine a split like a star. If you rotate your star with 10°, you cannot superpose rotor and stator regions.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 11, 2010, 05:48
Default
  #9
Senior Member
 
raymond
Join Date: Nov 2009
Posts: 149
Rep Power: 7
wlt_1985 is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
no.
The split should be a circle.
For undestanding, try to imagine a split like a star. If you rotate your star with 10°, you cannot superpose rotor and stator regions.
In order to split my rotor (impeller) by using a geometry which has the same shape but larger size to my rotor (impeller) instead of a circle, does it mean that I need to use dynamic mesh?
wlt_1985 is offline   Reply With Quote

Old   October 11, 2010, 05:51
Default
  #10
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,972
Rep Power: 30
-mAx- will become famous soon enough
if you cannot create a circle-split, then yes you will have to handle with dynamic mesh.
Can you quick post a sketch of your rotor-stator?
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 11, 2010, 06:11
Default
  #11
Senior Member
 
raymond
Join Date: Nov 2009
Posts: 149
Rep Power: 7
wlt_1985 is on a distinguished road
Here is my initial gepmetry
Attached Images
File Type: bmp geometry.bmp (90.3 KB, 50 views)
wlt_1985 is offline   Reply With Quote

Old   October 11, 2010, 07:00
Default
  #12
Senior Member
 
raymond
Join Date: Nov 2009
Posts: 149
Rep Power: 7
wlt_1985 is on a distinguished road
Here is my initial geometry to be studied. What should I do in order to have best model of the fluid motion behavior which induced by the solid impeller? Thanks a lot.
Attached Images
File Type: bmp geometry.bmp (90.3 KB, 28 views)
wlt_1985 is offline   Reply With Quote

Old   October 11, 2010, 07:24
Default
  #13
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,972
Rep Power: 30
-mAx- will become famous soon enough
your picture is quite small...
As far as I saw, you can draw a circle (cylinder-surface in 3d) surrounding your impeller.
You can also attach your geometry (*.dbs) if you want
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 11, 2010, 08:20
Default
  #14
Senior Member
 
raymond
Join Date: Nov 2009
Posts: 149
Rep Power: 7
wlt_1985 is on a distinguished road
I would like to attach my dbs file. Unfortunately, it was around 1M and error during attaching. I tried to model as solution provided before and it was work. Thanks for your help. The cylinder should be just created surrounding the impeller or it should be huge enough until close to the stationary baffles?
wlt_1985 is offline   Reply With Quote

Old   October 11, 2010, 08:23
Default
  #15
Senior Member
 
raymond
Join Date: Nov 2009
Posts: 149
Rep Power: 7
wlt_1985 is on a distinguished road
If I would like to model it with dynamic mesh, what should I do to the model setting?
wlt_1985 is offline   Reply With Quote

Old   October 12, 2010, 01:01
Default
  #16
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,972
Rep Power: 30
-mAx- will become famous soon enough
so I received your file.
Do followings:
*delete volume2
*create cylinder (height 0.2 / radius 1=radius 2=0.04 / Axis Location Positive Z)
*split volume1 with the cylinder (volume4)
*delete volume5 (solid) --> should be already deleted (volume2) but it's early this morning, don't want to investigate )
here we are, you have 2 regions: rotor and stator.
*copy volume1 with translation (0.1 0 0) (it generates volume 5), delete volume1
*move copied volume5 with translation (-0.1 0 0)
* The 2 volumes are now disconnected.
Apply interfaces (one for each volume)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 12, 2010, 01:23
Default
  #17
Senior Member
 
raymond
Join Date: Nov 2009
Posts: 149
Rep Power: 7
wlt_1985 is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
so I received your file.
Do followings:
*delete volume2
*create cylinder (height 0.2 / radius 1=radius 2=0.04 / Axis Location Positive Z)
*split volume1 with the cylinder (volume4)
*delete volume5 (solid) --> should be already deleted (volume2) but it's early this morning, don't want to investigate )
here we are, you have 2 regions: rotor and stator.
*copy volume1 with translation (0.1 0 0) (it generates volume 5), delete volume1
*move copied volume5 with translation (-0.1 0 0)
* The 2 volumes are now disconnected.
Apply interfaces (one for each volume)
Thanks for help. Max.
wlt_1985 is offline   Reply With Quote

Old   October 13, 2010, 13:45
Default
  #18
New Member
 
anonymous
Join Date: Oct 2010
Posts: 8
Rep Power: 6
cfd_confuse is on a distinguished road
Hi Max, for the above mixing tank problem, may i know what is the ideal number of cells for both the moving zone and the fluid zone, in a 2.5m tall cylindrical tank?? Also, may i know how to go about setting the boundary condition in fluent?
cfd_confuse is offline   Reply With Quote

Old   October 14, 2010, 01:23
Default
  #19
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,972
Rep Power: 30
-mAx- will become famous soon enough
There is no rule. Just check that you have enough cells where you think there is pressure drops etc...
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   October 14, 2010, 08:14
Default
  #20
New Member
 
anonymous
Join Date: Oct 2010
Posts: 8
Rep Power: 6
cfd_confuse is on a distinguished road
Hi Max, what about the boundary condition to set in fluent? i am not sure about the boundary condition to be use for the mixingtank
cfd_confuse 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
Rotating propeller in a finite freestream velocity asma CFX 9 January 7, 2014 07:14
Counter rotating propeller (propfan) Ball FLUENT 0 August 13, 2008 16:14
Rotating Propeller Nolin FLUENT 1 September 6, 2006 23:07
propeller rotating at zero inflow velocity Ammu FLUENT 1 July 23, 2005 13:36
Solid particles in a rotating vessel with 5.7.1 Sandeep CFX 0 May 17, 2005 10:54


All times are GMT -4. The time now is 19:37.