[liulangdefeng2222]

Thank you very much. I just face the problem. I hope it can help .

[moun139]

Is there a way to implement periodic boundary condition with UDF ? thx

[chaudhry_hashim]

Hi all, I am simulating an axial fan in fluent with inlet and outlet duct for finding the fan curve, I have a confusion regarding the interfaces types should I have to make the interfaces with periodic boundary condition and if yes then what should I consider rotational or translational and how can I calculate the angle if I am considering rotational under the periodic boundary tab.

Thanks in advance

Hashim

[mustafa-uslu]

This was Awesome!!! I just started to understand periodic boundary conditions and in my first shot I succeeded with help of this topic, Thank you very much Peter!

Additional Question: Only a small question, how about boundary condition? I mean for hydraulic diameter, should I assume whole diameter or applying 4*Area/Pwet for 30° slice?

[ghost82]

Originally Posted by mustafa-uslu

This was Awesome!!! I just started to understand periodic boundary conditions and in my first shot I succeeded with help of this topic, Thank you very much Peter!

Additional Question: Only a small question, how about boundary condition? I mean for hydraulic diameter, should I assume whole diameter or applying 4*Area/Pwet for 30° slice?

Whole diameter!

[mustafa-uslu]

Cheers, thats what I've done though

[mustafa-uslu]

Originally Posted by euanw6

I am using a 20 degree segement of a annular cascade of 18 stators. I have followed the steps noted to apply periodic BCs to each side of the 20 degree segment but I get the following error.

zone 11: matched 0 out of 4395 faces.
zone 10: matched 0 out of 4395 faces.
Error: Failed to make zones periodic.
Error Object: #f

Seems like I may have missed something out but I've followed each step.

I created named selections for these two faces and called them interface1 and interface2.

This is also happening to me when I do some changes on geometry/mesh. What I do is each time I double check the periodic faces (if they are still same and matched) and open fluent, having this error and apply same procedure over and over again (mesh/modify/make periodic).

I dont know if there is easier way (to cancel previous selections and apply always new)

[MOHD ZEESHAN]

hi, peter and cfd fellows
i hv encountered a problem in making periodic boundaries in fluent i.e
translation deltas: 0.000000 0.000000 0.003630
zone 27: matched 259 out of 307 faces.
zone 26: matched 259 out of 312 faces.

Error: Failed to make zones periodic.
Error Object: #f
kidly give me somepath for this

thanks
hope 4 ur answer

[shahid nadeem]

Dear Peter I have one very important question. How to define periodicity For Rotor and Stator in ICEM CFD when there are different Number of Blades for Rotor and Different Number of Blades for Stator, since the angle will be different for Each of Them.

Thank You

[Islam Abdelghafar]

Hi Peter,
how can i determine the proper principal axis and the orientation about the principal axis ?

[Monib ur Rehman]

Hi every one.
I am working on CFD using Fluent. i have stuck in the middle. Could anyone please tell me how do i apply periodic boundary condition on walls of sub channel of nuclear reactor? When i apply, i get divergence errors.Please help
Thanks in advance

[rocketeer]

Originally Posted by Peter023

Hello all FLUENT fellows,

recently I encountered a problem with periodic boundaries in fluent (Ansys 13, Workbench+FLUENT) for my rotationally symmetric model, especially how to create them. After some research on this web I found only small pieces of know-how. I figured out the rest myself by experimenting. Here I share the knowledge I've got. I will show how to effectively create a rotational periodic boundary in a short tutorial. Here it comes:

1) Assuming a rotationally symmetric geometry, create a part of your desired model in the Design Modeler. The sketch can be revolved, for example, 30 degrees about any chosen axis, leaving a model of only 1/12th of the full-model volume. This model consists of 2 periodic boundaries. Nothing else needs to be done in DM.

2) a) Go to the Meshing utility. Find the "Model" folder at the top of the tree structure and hit the "Symmetry" button to create a Symmetry folder lower in the tree structure.

b) Expand the "Coordinate systems" and choose your coordinate system. In its properties, change the type to "Cylindrical". Chose the proper value for "Principal axis" and "Orientation about Principal Axis" to get the right direction of rotation indicated by a bent axis arrow.

3) Right click on the "Symmetry" folder created in step 2a and add "Cyclic Region". Go to the settings and complete the required parameters. Choose your cylindrical coordinate system. This row should not light yellow.

Right click on "mesh" and insert "Match Control". Choose the same boundaries as in the "Cyclic Region" keeping the proper order of High and Low... Transformation: cyclic, Coordinate syst.: Global.

Other functions (size fcn, etc.) can be used as well for your mesh.

Generate your mesh by "Update". No error should appear.

4) FLUENT: a) Load your mesh, run "Check". Go to "Cell Zone Conditions -> Edit". Set the proper "Rotation-Axis Direction", If the axis of rotation along the model is X, then set 1 in X direction, leaving 0 in Y and Z.

b) use TUI: mesh/modify-zones/make-periodic choose your periodic boundary IDs as the input. Everything should go well and complete cells match on both sides should be found.

c) run "Mesh -> Check" again. Run "Mesh -> Reorder -> Domain" to reduce the memory bandwidth.

Enjoy your periodic boundaries. :-)

Cheers,
Peter

I think if you only have created a periodic/cyclic symmetry, it would be enough as mentioned in ANSYS meshing guide!

[aero.senthilkumar]

Hi all,
For ICEM users this following link is helpful for doing periodic Boundary condition
https://www.youtube.com/watch?v=HYJcXt0SdMA

[anand.jittanakatti]

In addition you can also get the periodicity in FLUENT by just making some setting in the Display menu
Go to.... Display – Views – Periodic Repeats (define) – translation/rotational

Achieve your desired periodic contours!

Thank you,
Jittanakatti

[villager]

Originally Posted by michel2008

Actually, I think the only difference for a translational one is to define a coordinate system which I did and all the steps worked but this yellow light in the coordinate system prevent to apply right periodic region
[/B]

If you choose Cylindrical coordinate system it should not be yellow, and would work, but it would create mesh as for Rotational Periodic (the same mesh would be obtained with the rotation). If you need Translational Periodic, try using Model -> Symmetry -> Symmetry Region with Linear Periodic type instead. The mesh would be copied by translation, not rotation, which suits for Translational Periodic B.C.

[furqanrk]

Originally Posted by m5edr

Hi Peter
I read the above part carefully and discovered the reason that make FLUENT refused to complete the Periodic B.c of my problem.

Yes , I have two separate Bodies (Domains) and it is not allowed to make one part (the reason: to make each Domain has it is interface face , if i made one part i will got only one interior face)

But Fluent after make periodic B.C successfully ,it told me the periodic operation failed !!

I'm upload My File here ( https://www.dropbox.com/s/4stnm7cm35...%20turbine.rar )
Could you help to solve this

Thanks in advance

Dear expert.. I have to use Superficial gas velocity 0.0016 m/s. But In fluent we have to put Velocity Magnitude at VELOCITY INLET boundary conditions.( INLET VELOCITY) How can I calculate INLET GAS VELOCITY form superficial gas velocity??? ( Reactor dimensions are 20*5*50 cm W*D*L and inlet dimensions are 2.4*1.2 L*D )

[villager]

Originally Posted by furqanrk

Dear expert.. I have to use Superficial gas velocity 0.0016 m/s. But In fluent we have to put Velocity Magnitude at VELOCITY INLET boundary conditions.( INLET VELOCITY) How can I calculate INLET GAS VELOCITY form superficial gas velocity??? ( Reactor dimensions are 20*5*50 cm W*D*L and inlet dimensions are 2.4*1.2 L*D )

It is off topic, you ought to create new post the next time.

Superficial velocity is a velocity that gives the same mass flow rate at any reactor cross-section (or volumetric flow rate, we do not care about density is varying or not - superficial velocity is engineering value based on the mean values). Superficial velocity is just Q/A, i.e. volumetric flow rate / cross-section.
As you have circular cross-section for reactor and inlet, the area A is PI*D^2/4. Q is fixed (to hold continuity principle).
If you have superficial velocity = 0.0016 for reactor (r-r) cross-section, you have to convert it 0.0016*(PI * Dr-r^2 / 4)/(PI * Dinlet^2 / 4) = 0.0016*Dr-r^2/Dinlet^2. Both D values should be put in the same units!
If you have superficial velocity = 0.0016 for inlet, no conversion is needed.

[furqanrk]

Originally Posted by villager

It is off topic, you ought to create new post the next time.

Superficial velocity is a velocity that gives the same mass flow rate at any reactor cross-section (or volumetric flow rate, we do not care about density is varying or not - superficial velocity is engineering value based on the mean values). Superficial velocity is just Q/A, i.e. volumetric flow rate / cross-section.
As you have circular cross-section for reactor and inlet, the area A is PI*D^2/4. Q is fixed (to hold continuity principle).
If you have superficial velocity = 0.0016 for reactor (r-r) cross-section, you have to convert it 0.0016*(PI * Dr-r^2 / 4)/(PI * Dinlet^2 / 4) = 0.0016*Dr-r^2/Dinlet^2. Both D values should be put in the same units!
If you have superficial velocity = 0.0016 for inlet, no conversion is needed.

Dear sir,
First of all sorry to start off topic.. I tried to create new post but unsuccessful. Because in china english website is not easy to open. . .
Second.. your answer is quite good. My problem is solved because of your guidance . thank you..

[Nabeel Abed]

Hi everyone
Is it possible to specify more than one periodic boundary condition in FLUENT?

[1994bm]

Yes. Just create different faces. There shouldn't be overlap.