CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   Link faces meshes for periodic BC with ANSYS WORKBENCH (http://www.cfd-online.com/Forums/ansys-meshing/74973-link-faces-meshes-periodic-bc-ansys-workbench.html)

mawi01 April 13, 2010 10:28

Link face meshes for periodic BC with ANSYS WORKBENCH
 
Hello everybody !

I try to attach periodic BC to my geometry to receive an equal number of mesh elements on 4 specific surfaces. Usually, I used GAMBIT with its "link face meshes " function, which worked without any problems. Due to new version of ANSYS I am working with WORKBENCH (Physics Preference : CFD . Solver Preference : FLUENT) to mesh geometries. Unfortunatly, the ANSYS WORKBENCH doesn 't provide the function "link face meshes " anymore, which has been replaced by the "match control " function.
To simplify my geometry, consider it as an cuboid (or ashlar ? ). The front and back surface as well as both sides should be linked for periodic BC. Only the bottom and top surface remain as "walls". So , I used the "match control" function for the front and back surface and it worked. Next, I did the same for both side surfaces and an error occured telling me, that "The combination of different match controls causes conflicts. The conflicts will be at the intersection of the highlighted entities."

I have read through ANSYS Help to find a solution for my problem, but can't find a hint. I hope that you can solve my problem ! If you need more specific information just let me know !

Thank you very much!

Kind regards,

Martin

PSYMN April 16, 2010 14:56

Temporary Limitation...
 
Sorry, this is a documented limitation at 12.1...

( see the help, 3rd bullet under "Keep the following information in mind when using the match control feature: " )

Sorry, we are working on it...:o

wildli February 1, 2011 16:00

have you solved the problem?
 
Quote:

Originally Posted by PSYMN (Post 254993)
Sorry, this is a documented limitation at 12.1...

( see the help, 3rd bullet under "Keep the following information in mind when using the match control feature: " )

Sorry, we are working on it...:o

Simmon, have you solved the problem? I am encountering the same problem now. please let me know if your ansys has solved it or not, I am currently using ANSYS 12.0 and not sure if this version has the bug fixed or not.
thanks.

nvarma April 9, 2015 16:42

and it still is a limitation?

JoeKal September 20, 2015 16:46

Periodic boundary for multiple faces - ANSYS Meshing (Workbench14.5)
 
There maybe a way to deal with this. In ANSYS Meshing, add a Symmetry object to ur main problem tree. In the symmetry option, insert Periodic. Now u can choose multiple faces for the periodic boundary on ur problem. Remember that the co-ordinate system needs to be cylindrical otherwise it will not work.
There is also a linear periodic option in the Symmetric option under Symmetry object. But I haven't explored this yet.

Hope this helps.

villager March 13, 2016 14:10

Quote:

Originally Posted by JoeKal (Post 564886)
There maybe a way to deal with this. In ANSYS Meshing, add a Symmetry object to ur main problem tree. In the symmetry option, insert Periodic. Now u can choose multiple faces for the periodic boundary on ur problem. Remember that the co-ordinate system needs to be cylindrical otherwise it will not work.
There is also a linear periodic option in the Symmetric option under Symmetry object. But I haven't explored this yet.

Hope this helps.

As I found, Periodic and Cyclic Symmetry create rotated mesh, as for Rotational Periodic. Linear periodic creates a mesh that suits for Translational Periodic.
If the mesh contains two peridoic boundaries with the common edge that differ in translation direction, Symmetry would not help too. Checked in ANSYS v 162. There's still a limitation on mesh generation with multiple as it is pointed out in Meshing Help.

There same holds for Match Control.
Also to note, Match Control with Automatic/Tet Mesh did not worked for me in ANSYS v 162 at all - it creates mesh that causes "Number of nodes read (...) does not match number referenced (...). Resetting counter to match the number referenced." warning in FLUENT. Then the mesh quality is equal to 0, and skewness is 1, that results in impossibility of any solution. Mesh repair/improve does not help in this case too. I hope this bug would be fixed in next versions.


All times are GMT -4. The time now is 11:23.