# periodic boundary condition

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

 January 15, 2012, 10:52 periodic boundary condition #1 Member   Join Date: Nov 2011 Posts: 44 Rep Power: 5 Hello. I'm trying to simulate a fully developed flow of a pipe cross-section. Instead of simulating the whole 3D pipe (which is straight), it'd be more efficient to simulate the 2D cross section. I know one must use periodic boundary conditions, but I don't know how to set this in FLUENT. A previous thread mentioned a TUI command, but I get some errors using that. If someone could kindly walk me through it. Thank you, Regards, F

 January 15, 2012, 11:07 #2 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 899 Rep Power: 15 Hi, assuming that you have your mesh built with corrected boundaries, in fluent, in the boundary condition panel, select the periodic zone and click set and choose "rotational". This is enough to start the computation. For post processing, if you want to view the whole domain instead of a slice, click on display->views, under periodic repeats click define; in periodic type select rotational; if you have 1/4 pipe write -45 in angle, and 4 in number of repeats; in axis direction put 1 as Z (assuming that the axis of the tube is in z direction). Click the set button. Daniele

 January 15, 2012, 11:08 #3 Super Moderator     Sijal Ahmed Memon (turboenginner@gmail.com) Join Date: Mar 2009 Location: Islamabad Pakistan Posts: 3,906 Blog Entries: 6 Rep Power: 38 if you are modeling as 2d, then go for axisymetric and no need of periodic bc

 January 15, 2012, 15:16 #4 Senior Member   Lucky Tran Join Date: Apr 2011 Location: Orlando, FL USA Posts: 594 Rep Power: 11 Use this command (type it into the command window): /define/boundary-conditions/modify-zones make-periodic Then follow the prompts and enter the appropriate values. This is the only way to create a periodic interface in fluent. There is no way to do it on the GUI (yet). Check out the fluent help file for more information on TUI commands.

January 15, 2012, 17:17
#5
Senior Member

Daniele
Join Date: Oct 2010
Location: Italy
Posts: 899
Rep Power: 15
Quote:
 Originally Posted by LuckyTran Use this command (type it into the command window): /define/boundary-conditions/modify-zones make-periodic Then follow the prompts and enter the appropriate values. This is the only way to create a periodic interface in fluent. There is no way to do it on the GUI (yet). Check out the fluent help file for more information on TUI commands.
Hi LuckyTran,
are you stating that

"in fluent, in the boundary condition panel, select the periodic zone and click set and choose "rotational".
This is enough to start the computation."

will not compute the domain as periodic?

Thank you

January 15, 2012, 18:18
#6
Senior Member

Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 594
Rep Power: 11
Quote:
 Originally Posted by ghost82 Hi LuckyTran, are you stating that "in fluent, in the boundary condition panel, select the periodic zone and click set and choose "rotational". This is enough to start the computation." will not compute the domain as periodic? Thank you
My last were comments on how to create a periodic zone since it requires a TUI command. That is, there is no periodic zone in the boundary conditions panel until you have created it.
Once the periodic zone is in the boundary conditions panel. You can do as you have said and that will be enough.

January 16, 2012, 04:25
#7
Member

Join Date: Nov 2011
Posts: 44
Rep Power: 5
Quote:
 Originally Posted by LuckyTran Use this command (type it into the command window): /define/boundary-conditions/modify-zones make-periodic Then follow the prompts and enter the appropriate values. This is the only way to create a periodic interface in fluent. There is no way to do it on the GUI (yet). Check out the fluent help file for more information on TUI commands.
I tried doing that TUI command. However, it asks me things like "shadow zone" and other info that I don't really know the meaning of. I tried to play around with it but it gives me erros.

Perhaps I don't have a correct mesh?

Also, I would like to have a full cross section of the pipe (although square), I would later like to add some thermal asymmetric boundary conditions...

Kind Regards,

Francesco

 January 16, 2012, 05:12 Post a Pic #8 Super Moderator     Sijal Ahmed Memon (turboenginner@gmail.com) Join Date: Mar 2009 Location: Islamabad Pakistan Posts: 3,906 Blog Entries: 6 Rep Power: 38 post a pic of your meshed model and show where you want to apply periodic boudary condition

January 16, 2012, 12:10
#9
Senior Member

Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 594
Rep Power: 11
Quote:
 Originally Posted by fferroni I tried doing that TUI command. However, it asks me things like "shadow zone" and other info that I don't really know the meaning of. I tried to play around with it but it gives me erros. Perhaps I don't have a correct mesh? Also, I would like to have a full cross section of the pipe (although square), I would later like to add some thermal asymmetric boundary conditions... Kind Regards, Francesco
It will ask for the the first zone and then a shadow zone. These are the two zones that will receive the periodic mapping. The solution from the original zone will be mapped directly onto the shadow zone and the velocity profiles will be preserved across these two zones.

For rotationally periodic meshes (the axis of rotation must like on the x-axis) and the entirety of the mesh must lie above the y=0 line (positive y region). Thees are restrictions placed by fluent.

If your axis of rotation is not compatible, it will likely throw an error saying it could match 0 out of ### faces for each zone.

You may need to regenerate your mesh to these restrictions. Also, it is better to create a conformal mesh on the two periodic faces so that additional interpolation steps are not needed during the solution calculation. When you run the TUI command, it will print out how many of the faces could be matched, and if the matching was conformal or not.

January 18, 2012, 05:54
#10
Member

Join Date: Nov 2011
Posts: 44
Rep Power: 5
Quote:
 Originally Posted by Far post a pic of your meshed model and show where you want to apply periodic boudary condition
Here it is.
Attached Images
 Capture.jpg (24.4 KB, 33 views)

January 18, 2012, 06:01
#11
Member

Join Date: Nov 2011
Posts: 44
Rep Power: 5
Quote:
 Originally Posted by LuckyTran It will ask for the the first zone and then a shadow zone. These are the two zones that will receive the periodic mapping. The solution from the original zone will be mapped directly onto the shadow zone and the velocity profiles will be preserved across these two zones. For rotationally periodic meshes (the axis of rotation must like on the x-axis) and the entirety of the mesh must lie above the y=0 line (positive y region). Thees are restrictions placed by fluent. If your axis of rotation is not compatible, it will likely throw an error saying it could match 0 out of ### faces for each zone. You may need to regenerate your mesh to these restrictions. Also, it is better to create a conformal mesh on the two periodic faces so that additional interpolation steps are not needed during the solution calculation. When you run the TUI command, it will print out how many of the faces could be matched, and if the matching was conformal or not.
Hi

I followed your instructions and "all 3200 faces matched for zones 6 and 5". Now instead of having a velocity-inlet and a pressure-outlet, I only have a velocity inlet. I now go to the boundary conditions tab,and since my condition was an initial velocity, I guess I can specify a mass flow rate... However, I'm just wondering what is the Relaxation Factor and the Number of Iterations..?

Kind Regards,

F

January 18, 2012, 06:13
#12
Super Moderator

Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Posts: 3,906
Blog Entries: 6
Rep Power: 38
Quote:
 it'd be more efficient to simulate the 2D cross section.
So you want to model it as 3D not 2D as posted by you earlier? If you are meshing in GAMBIT then you can apply periodic boundary condition there (better method), else you can use the TUI (text user interface) command in Fluent
Enter commands in following sequence
1. define
2. boundary-conditions
3. modify-zones
4. make-periodic
And select two corresponding surfaces with their zone ids

 January 18, 2012, 06:34 #13 Super Moderator     Sijal Ahmed Memon (turboenginner@gmail.com) Join Date: Mar 2009 Location: Islamabad Pakistan Posts: 3,906 Blog Entries: 6 Rep Power: 38 Try 1000 iterations (that's how many times your matrix is solved iteratively) and must specify sufficient no. of iterations so that the target residual level is achieved. At the moment don't play with under relations factor. In simple words these the are values which forces the speed of level of convergence to next iteration (x new = x + urf * xold).http://www.cfd-online.com/Wiki/Fluen..._parameters.3F https://www.sharcnet.ca/Software/Flu...999.htm#170207

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post peob OpenFOAM Running, Solving & CFD 2 August 14, 2014 09:07 haihek FLUENT 3 January 22, 2014 05:10 martor FLUENT 2 April 10, 2012 19:17 CFD XUE FLUENT 0 July 9, 2010 02:53 Rola Afify FLUENT 2 September 12, 2006 08:39

All times are GMT -4. The time now is 20:23.