|
FLUENT Periodic Boundary Condition SOLVED + TUTORIAL
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. :rolleyes: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. :cool:Enjoy your periodic boundaries. :-) Cheers, Peter |
Hi Peter,
That was a good tutorial. Do you by any chance know it it's possible to rotationally link 2 periodic domains to 2 corresponding shadow domains? I'm using the "mesh > modify-zones > make-periodic" command. I tired both methods: a) linking domain1 with domain1' and then domain2 with domain2' or b) linking domain1 and domain2 with domain1' and domain2' They both don't work and give me errors in Fluent. But unfortunately I can't just combine donmain1 with domain2 and domain1' with domain2' when meshing - my meshing strategy doesn't allow me to do that. Any suggestion is most welcome! Dorit |
Hi Dorit,
only one thing comes to my mind at the moment and that is, if your domains are separate bodies in the model, then you must group them as one part. Otherwise, the mesh won't be consistent as continual in both bodies (domains). If so, Fluent cannot process them. Also, I would try to make only two boundaries domain12 and domain12' (if both domains-bodies are grouped in the model, such a named selection should be possible). Would you send some more details about you geometry (picture) or the Fluent command line screen after the make-peri... attempt? Cheers, Peter |
Thanks for your reply.
The primary reason for me to have domain1 and domain2 as 2 separate entities was that one of them is structured and the other is unstructured and as it so happens the structured one is easier to generate in Gridgen while TGrid gives me a much better unstructured mesh. So I couldn't save them under the same name in Gridgen as this wouldn't allow me to only select the unstructured part in TGrid for a new volume generation. Does this make sense? But I now found a way of combining domain1 and domain2 in TGrid after I complete the mesh with the generation of the unstructured part. So I'm effectively linking domain12 with domain12' in Fluent now. As it's the same mesh as before though it should be possible to link them as 2 domains with 2 shadow domains... But thank you for your help :) Dorit |
Quote:
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 Peter023
Thanks for your tutorial. I am trying to apply translational periodic boundaries in the meshing utility, and I am doing your tutorial step by step, but as you mentioned in step 3 , for setting the periodic region details,the light yellow should not be appeared in coordinate system, but it is appeared and I could not be able to solve it, would you please explain me how can I get rid of this problem. Many thanks Michel |
Quote:
this particular example I described is for a rotational symmetry.If you want to use translational you may consider not using the cylindrical coord system.The field is yellow because it requires properly defined cordinate system. |
Dear Peter023
Thanks for your respond. I realized this turial is for a rotational symmetry and you define a cylindrical coordinate system. 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, do you have any suggestion about it? Thanks again Michel |
Dear Michel,
your problem seems to be a bit tricky and will require closer look to the overall setup of the model and the mesh. If your model is composed of several bodies, try to put them into one part. Please analyse your setup thoroughly including all dependencies . Wishing you good luck. Cheers, Peter |
Dear Peter023
Thanks for your consideration and respond. I think maybe it is better to explain more about my problem. Actually, I am trying to simulate micro-cylinders embedded in a rectangular microchannel so I simplified the model with a unit cell which is a square microchannel including a micro-cylinder with an inlet and outlet by apply periodic boundary condition in the inlet and outlet (I used mass-flow rate for inlet boundary condition). The point is when I applied periodic boundary condition in Fluent, an error just appeared before the first iteration calculating solution "divergence detected in AMG solver-pressure correction" . Although I tried to overcome this problem by reducing under relaxation factor and change some parameters in solution control, unfortunately I could not be able to solve it. In the other hand when I want to make periodic region in inlet and outlet in mesh utility, as I wrote the coordinate system light yellow prevent to well define it. I hope you can help me with your experience to solve this problem. I would appreciate if you give me some advices. Thanks again, Michel |
Dear Michel,
thank you for your description. However, I'm not able to provide you with some more help since I didn't have chance to solve the same problem. Perhaps, if the creation of the periodic condition in Fluent went just OK, then the problem is not in the meshing settings but in the solution method in Fluent. You may try to consider using velocity/pressure inlet boundary condition instead of mass rate driven flow. Unfortunatelly, my experience is a bit limited in this field. Good luck. Cheers, Peter |
turbulent fully developed flow in internally finned tube
Hi every one
thanks for all CFX and FLUENT fellows. i have an problem and i need some one who help me to find the solution. i created 3D internally fined tube for one pitch with 20 fins no. in CFX work bench and i mesh this geometry in ICEM CFX then i export this situation to the CFX and FLUENT program. the assumptions for my issue are: 1- steady-state flow water. 2- turbulent fully developed flow (period flow). 3- constant tube wall temperature. the geometry continents from in , out, tube wall(with fins). please can any one who help me to describe the steps in CFX or FLUENT to find the results regards Ali S. B. |
Hi guys,
I have a question, I am trying to move my whole domain in a sinusoidal way. Basically I have a box which is fixed and i am trying to move the whole flow around in a sinusoidal transient way. Which kind of boundary conditions would you suggest me to use. Thanks for your help |
Quote:
It was very helpfull!! |
Thanks a lot!!! This info is very helpful, I didn't know what was wrong in my solution till I introduce periodic boundary conditions after your tutorial
|
Periodic or cyclic boundaries at edges
Hi all, thanks for a great tutorial!
I am trying to model a large tube bundle that I've cut it so it only shows a portion of it. So, I'm trying to apply cyclic or periodic boundaries to the sides, making it take into account the other tubes that are not shown in the model. For some reason my coordinate system always lights up yellow, it's defined as a cartesian "Global Coordinate System". So in the details of the Periodic Region everything is correctly filled out, but the coordinate system always lights up yellow. Is there something I'm missing? You all mentioned to properly define the coordinate system, do I need to do that any further? How do I go about doing this? thanks for all of your help! |
you have to create a new coordinate System with design modeller, because you cannot change the properties of the global coordinate system. ( I guess it is not possible in ansys mesh, but I´m not sure).
Be sure that one axis of this new coordinate system can be used as your rotation axis. Then go back to ansys mesh. Do point 2 b) of the tutorial: " 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." proceed with the further steps of the tutorial. I hope my help is not to late :-) Best regards Tobi |
I have one question:
Is the cyclic region really needed? Isn´t the match control enough? At least it includes all information that is needed! Transformation:cyclic Axis of Rotation: Plane 5, or whatever plane you use for the cylindrical coordinate system! And the high- and low- geometry selection. Without the cyclic region, my mesher seems to generate a good mesh with cyclics, but when I include a Cyclic region to the symmetry folder I get the error message: "the mesher was unable to generate mesh due to [...] incorrect input." I´d be glad for some information and help :-) |
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. |
final result after setting periodic boundary condition
Hi all,
I have to simulate a internal flow in a cylindrical case having both end stator blades and in middle there are rotor blades.There is no outlet and inlet.Atmospheric pressure is maintained initially.I have to calculate torque at different rpm.SO i have cut the whole geometry by 45 degree.and applied periodic boundary condition and used sliding mesh Technic to simulate the physics of flow. I need to know that what is the torque value.Is the torque value = 1/8 of full model value(actual value).As number of rotor blades are 9 and stator blades are 8. Thanks in advance |
| All times are GMT -4. The time now is 01:17. |