[fferroni]

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

[ghost82]

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

[Far]

if you are modeling as 2d, then go for axisymetric and no need of periodic bc

[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.

[ghost82]

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

[LuckyTran]

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.

[fferroni]

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

[Far]

post a pic of your meshed model and show where you want to apply periodic boudary condition

[LuckyTran]

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.

[fferroni]

Originally Posted by Far

post a pic of your meshed model and show where you want to apply periodic boudary condition

Here it is.

[fferroni]

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

[Far]

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

[Far]

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