|
[Sponsors] |
January 15, 2012, 09:52 |
periodic boundary condition
|
#1 |
Member
Join Date: Nov 2011
Posts: 44
Rep Power: 14 |
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, 10:07 |
|
#2 |
Senior Member
Rick
Join Date: Oct 2010
Posts: 1,016
Rep Power: 26 |
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, 14:16 |
|
#4 |
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,737
Rep Power: 66 |
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, 16:17 |
|
#5 | |
Senior Member
Rick
Join Date: Oct 2010
Posts: 1,016
Rep Power: 26 |
Quote:
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, 17:18 |
|
#6 | |
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,737
Rep Power: 66 |
Quote:
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, 03:25 |
|
#7 | |
Member
Join Date: Nov 2011
Posts: 44
Rep Power: 14 |
Quote:
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, 11:10 |
|
#9 | |
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,737
Rep Power: 66 |
Quote:
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, 04:54 |
|
#10 |
Member
Join Date: Nov 2011
Posts: 44
Rep Power: 14 |
Here it is.
|
|
January 18, 2012, 05:01 |
|
#11 | |
Member
Join Date: Nov 2011
Posts: 44
Rep Power: 14 |
Quote:
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, 05:13 |
|
#12 | |
Senior Member
|
Quote:
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, 05:34 |
|
#13 |
Senior Member
|
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 |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
periodic boundary condition in LES | martor | FLUENT | 3 | April 30, 2022 00:20 |
mixed inflow/outflow downstream boundary condition question | peob | OpenFOAM Running, Solving & CFD | 3 | February 3, 2017 10:54 |
periodic boundary condition (translational) fluent 6.3 | haihek | FLUENT | 3 | January 22, 2014 04:10 |
External Radiation Boundary Condition for Grid Interface | CFD XUE | FLUENT | 0 | July 9, 2010 02:53 |
translational periodic boundary condition | Rola Afify | FLUENT | 2 | September 12, 2006 08:39 |