CFD Online Logo CFD Online URL
Home > Forums > OpenFOAM Running, Solving & CFD

No flow through periodic (cyclic) boundaries in impeller with foam-extend-3.1

Register Blogs Members List Search Today's Posts Mark Forums Read

LinkBack Thread Tools Display Modes
Old   November 7, 2014, 03:57
Default No flow through periodic (cyclic) boundaries in impeller with foam-extend-3.1
New Member
Antti Heino
Join Date: Mar 2014
Location: Finland
Posts: 3
Rep Power: 3
anttiad9000 is on a distinguished road
Hello dear foamers!

I am calculating an imcompressible flow in centrifugal pump impeller using simpleFoam (MRFSimpleFoam) and rotational periodicity. First I was using OpenFOAM 2.2.2 and cyclicAMI for interfaces. When I did some comparison to CFX results and measurements I saw that it provided good enough results in some cases but as the mass flow through the impeller is decreased also the results seem diverge more. From this I concluded that the problem may be in the interface treatment because as the mass flow decreases the meridial velocity component decreases and tangential component increases. This means that the recirculation is higher on lower flow rates and the flow goes back and forth the cyclicAMI interface which makes the interface treatment very important.

Due to the reason above I changed to foam-extend-3.1 as it has GGI, which is used in CFX, instead of AMI. Using GGI I got a similiar pump curve as with CFX but head, circumferential velocity and torque where 5-10 % higher. I was certain that these values were not right and tried to find the cause for them. It seemed as if there were additional blades and another problem arose. I looked at the flow (phi) through periodic boundaries (IMPELLER_PER) using patchIntegrate and realized it was very small (around 1E-13). Which means they are like thin surfaces (additional blades) and increase the values above. I then calculated the same case with full non-periodic mesh and the results matched near perfectly to CFX and measurements. The reason for strange results was indeed the cyclic boundary. I would still like to use the periodic boundaries as they greatly decrease the computational load. Here is a quickly drawn picture to clarify the situation for those not that familiar with pumps:

I used both cyclic and cyclicGgi boundary types and the results were the same. Using the same mesh with cyclicAMI there was phi through the cyclic boundaries so this problem only exists when I use foam-extend-3.1. The mesh is created with TurboGrid and converted first with ICEM to Fluent format and then with fluent3DMeshToFoam.

Has anyone had any similiar problems before and if so what was the solution? I started from zero with OpenFOAM six months ago and now I believe this is the final problem I have left for a good and accurate impeller calculation with OpenFOAM. I added some attachments (boundary, fvSchemes, fvSolution, createPatchDict, MRFZones, log.checkMesh) which may be relevant to the solution. I very much appreciate all the help :)

Best regards,

TLDR: I have no flow going through periodic boundaries (IMPELLER_PER) in impeller computation using GGI and foam-extend-3.1.
Attached Files
File Type: zip (4.1 KB, 21 views)

Last edited by anttiad9000; November 7, 2014 at 05:27.
anttiad9000 is offline   Reply With Quote

Old   November 8, 2014, 06:29
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
I was looking at one of those 2 weeks ago - it turned out to be a user error. Please try cyclicGGI and set up the transform correctly. If your transform is wrong, you will get a report from lots of uncovered cases.

Please let me know how you get on,

Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting:
hjasak is offline   Reply With Quote

Old   November 10, 2014, 05:43
New Member
Antti Heino
Join Date: Mar 2014
Location: Finland
Posts: 3
Rep Power: 3
anttiad9000 is on a distinguished road
Thank you Hrv for answering,

I guess it was the transform problem as you said. When I tried cyclicGgi before i used changeDictionary to change the boundary file. Now I used createPatch to recreate all the boundaries. It seems to have fixed the issue. Thanks again for helping with the problem.

anttiad9000 is offline   Reply With Quote


cyclic, foam-extend-3.1, ggi, impeller, mrfsimplefoam

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
How to define to right point for locationInMesh Mirage12 OpenFOAM Native Meshers: snappyHexMesh and Others 4 April 10, 2014 10:12
simpleFoam parallel AndrewMortimer OpenFOAM Running, Solving & CFD 10 November 12, 2013 18:03
channelFoam for a 3D pipe AlmostSurelyRob OpenFOAM 3 June 24, 2011 13:06
Import gmsh msh to Foam adorean Open Source Meshers: Gmsh, Netgen, CGNS, ... 24 April 27, 2005 08:19
fluid flow fundas ram Main CFD Forum 5 June 17, 2000 21:31

All times are GMT -4. The time now is 16:25.