periodic boundaries
 

I want to define two rotational periodic boundaries (the angle between them is 180°). They are identically (equal number of faces, equal geometry).

/grid/modify-zones> make-periodic Periodic zone [()] 5 Shadow zone [()] 7 Rotational periodic? (if no, translational) [yes] yes Create periodic zones? [yes] yes

zone 5: matched 13596 out of 15234 faces. zone 7: matched 13596 out of 15234 faces.

Error: Failed to make zones periodic. Error Object: #f

Can someone help me ??

Re: periodic boundaries
 

can u specify the details of the geometry, then we can discuss about the problem - thanks!

Re
 

I'm now face the same problem
could any one pls, tell me how to fix this problem

Re: periodic boundaries
 

Has anyone determined a solution to this problem in Fluent? I also am working on simulations that require rotational periodicy. Occasionally I am able to create the periodic zones, but sometimes I receive the errors: "Error: Failed to make zones periodic. Error Object: #f"

I believe that I am not doing anything different when I create the periodic zone successfully. I am always ensuring that the rotational axis is aligned with the z-axis of the geometry and I am using match control in meshing for the two faces of the periodic zone. Any ideas of what may casue this?

yes i solved it before,
Type in Fluent command Window
>Mesh
>mp if doesn't work try to type the following and change number
>Mesh
>Mz
>Mt "change value (limit is 0.5)"

i faced the same problem. maybe u shoud make periodic in your meshing software ，then export the grid，at last import into FLUENT、、、、、、、which meshing software you are useing？？ICEM CFD can do it.

*I know I am late but, you must have the axis of rotation in the global z-direction for rotational periodicity. It may also be true that translational periodicity must be orthogonal across z as well.

Use /mesh/rotate in the interpreter and set your point of origin and axis of mesh rotation so that the global z-axis is parallel with the axis of periodicity

use /mesh/mz/make-periodic in the interpreter and move on as usual. You can also invoke periodicity in your meshing software (* Z-axis and axis of periodicity must be parallel) and Fluent should take care of it from there.

If there is a way to make the stored axis something other than (0 0 1) or any other vector, none of the above would matter.

Hi
The default tolerance can be problematic in small meshes

just use the text command
grid/modify-zone/mt
and specify smaller tol's untill all nodes are matched up and then you're good to go
I had to reduce from 0.1 to 1e-6

I was facing the same problem and I solved it by changing the rotation axis on the "cell zone condition" tab. My geometry was rotationally periodic along x axis but standard fluent settings use the z axis as the rotation axis.

I hope this helps!

Cheers,

Rob

This is problem of mesh, if you not mesh same cell size and division on periodic boundaries, Fluent through this error, If you want to avoid

1.Remesh,with match control.

2.If it irregular geometry then use periodic interface in fluent ( interface option defining boundaries as interface )

wdxgd
 

It is useful,thanks:)

I faced the same problem and just swapped the shadow region with periodic region and the periodic zone was successfully created.

Hi everyone,

in my case I have resolved the problem making higher the tolerance (from 0.05 to 0.1).
I think the problem comes from the CAD geometry. If the periodic domains from the CAD software are not clean (that means, there are overlapping between the periodic elements), fluents doesn´t like it and appears the error.
If you increase the tolerance value (grid/modify-zone/mt), fluent doesn´t take into account this ovelapping.

Bye

luiscssz

Hello, I followed your command and I got
warnning : your interfaces may adversely affected by the periodic creation..
what should I do?
Thanks

This is my impeller and I want to make periodicity in fluent..Thanks

How to do that in ICEM CFD?

Hello, try this technique easier than ICEM, Thanks!

https://youtu.be/eD0nxctN_yw

I followed your suggestion,but the fluent is still failing to create the periodicity. Do you have any further suggestions? My analysis is on 2D rotor-stator translational simulation as seen in the png. files below.

thanks in advance

Is your flow direction axis defined correctly in your "Cell Zone Conditions". If your direction axis is wrong, fluent wont be able to create a periodic boundary condition.



Hint: If your mesh is periodic, fluent should detect it on it's own.

In ANSYS R 18.2 for translational cyclic boundary condition I used
the command line of Fluent to create it, following the description of
https://www.researchgate.net/post/Ho...actually_means

/mesh/modify-zones> make-periodic
Periodic zone [()] 25
Shadow zone [()] 26
Rotational periodic? (if no, translational) [yes] no
Create periodic zones? [yes] yes
Auto detect translation vector? [yes] no
x-direction (m) [0] 0
y-direction (m) [0] -0.0273
z-direction (m) [0] 0

translation deltas: 0.000000 -0.027300 0.000000
zone 26 deleted

created periodic zones.

Hint: Fluent tried to compute the delta in y-direction itself but calculated a value of -0.02731. The creation of the periodic zones failed during auto detect. Hence, I just entered the correct offset myself (Auto detect translation vector? [yes] no) and it worked.

I'll try it and hope it'll work! thanks a lot!

Hi dear lukasf,

Following the link you gave, I only found the solutions with auto detect translation vector as "yes". I just wonder how you set the value as "-0.0273" and why on y direction. My geometry is a little complicated. how can I define the value and the direction? You can see my geometry in the attached files. My problem is 2D, the fluid flows x direction and the peridicity is y direction. Thanks in advance.

I used the value of -0.0273 m in the y-direction because of my geometry.


I have a rectangular channel. The patches on the left and right side of my channel which are supposed to become cyclic have a distance of -0.0273 m in the y-direction. It is a translational distance. Thus, I am using "Rotational periodic? (if no, translational) [yes]" no


From your images I can see that you are trying to calculate a flow in a turbine. Here you should actually use Rotational periodic YES, in my opinion.

hi dear friends,

I have solved my problem and overcame the periodicity problem. It was caused due to the creating names for the edges in meshing. I had created the periodic names for the all length of the edges which was incorrect as seen in the photo "incorrect name selection". I have changed the name selections making blade profiles as wall, you can see in the photo " correct name selection". Aften then, I was able to see the velocity vectors in the results.

Thanks your helps

I just demand some literature articles about 2D or 3D turbomachinary axial water or air flow analysis using Fluent. If you have some articles about it, it will be very helpful for me to decide blade chord length, inlet velocity/pressure, turbulent viscosity values selected on Fluent.

best regards

hey, i think i did the same thing like you, if you dont mind. would you like share ur TUI ? cause i just did like what u said, but mine is still cant work

I am using corrugated wall geometry and wants to apply periodic boundary condition and face the problem that number of elements are not same on both zones.... how to resolve it ??? and also tell how can make periodic before mesh import to fluent using ansys workbench

Hello everyone
i am working with 3d geometry with corrugated wall meshing by patch conforming method and facing a problem with periodic boundary condition that num of elements not same on both zones and also use match tolerance using minimum edge length shown in meshing... tell me is this the tolerance value that i am using?? or something else?
if using non conformal meshing then can anybody guide me how to create interface zones for periodic boundary zones???????

Solution of error object "f"
 

Dear friends,

I have also encountered the same problem very often. This problem is not common when you use ICEM for mesh. But when I started using Fluent Meshing, I encountered this problem quite often. Solution:

> mesh
> modify-zones
> mz
> Zone (1) (()) Write your zone ID
> Zone (2) (()) Write your zone ID
> Zone (3) (()] If it is not exist, skip with enter button

merged zones into periodic_wall_right. 1.