Problem with cyclic boundaries in Openfoam 1.5
 

Hello,

I have a really annoying problem concerning cylic boundaries with OpenFoam 1.5. The mesh generator is Gambit and I convert the mesh with fluentMeshToFoam and for cyclic boundaries is use the createPatch utility. With a simple channel everything works fine but the thats not what I am interested in. My focus lies on a circular cylinder with perodic boundary in spanwise direction. Gambit exports the mesh without any problems and my periodic boundary is defined as "wall". FluentMeshToFoam converts the mesh and I have to change in constants/polymesh/boundary the wall entry of my perodic boundary to cyclic. In createPatchDict I have to define every periodic patch, a matchingTolerance and if I want to have a synchronisation of coupled points. I set matchingTolerance to 1E-3 and Sync to true. And this is what I get after using createPatch utility:

face 0 area does not match neighbour 2520 by 188.925% -- possible face ordering problem.
patch:p_z15 my area:0.00822951 neighbour area:0.000234351 matching tolerance:0.001
Mesh face:914248 vertices:4((1.37852 1.44903 4) (1.25963 1.32406 4) (1.29225 1.29225 4) (1.41421 1.41421 4))
Neighbour face:916768 vertices:4((0.428847 0.450783 4) (0.418304 0.439701 4) (0.429136 0.429136 4) (0.439952 0.439952 4))
Rerun with cyclic debug flag set for more information.

From function cyclicPolyPatch::calcTransforms()
in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 150.

Increasing the matchingTolerance produces the same error, exept if it becomes greater than 2, than it works ... but I dont trust the periodic boundary, because 2 seems to be a little bit to high for a tolerance? Where is my mistake? I dont have any idea. Please help :(

Change write precision
 

Try changing your write precision in your controlDict to 10 before you convert your mesh. If it is 3D try using the fluent3DMeshToFoam command. Also, make sure you have linked your edges correctly in Gambit. I had a similar problem a few weeks ago.

Dan

Thx for your quick help, but this doesn't work. :-/
1) I tested the writePrecision but nothing changed ... I still have this anoying error. I guess this was a major problem of earlier OpenFoam versions and should be fixed in 1.5.
2) fluent3DMeshToFoam produces a segmentation fault:
Creating cellZone 0 name: fluid type: fluid
#0 Foam::error::printStack(Foam::Ostream&)
#1 Foam::sigSegv::sigSegvHandler(int)
...
Segmentation fault
3) During my test with the channel I recognized, that linking the faces of the periodic boundary produces an error in createPatch and without linking everything is fine.
For my cylinder mesh I tried first without linking, which produces the error above. Now due to your reply I linked every face of my perodic boundary (I have to decompose my boundary in serveral parts to help gambit with meshing) and the error above is still the same.

I dont have any idea what to do. The cylinder test case is just a simplification of my real problem and I need this periodic boundaries and Gambit for meshing (blockMesh utility is no option). I am open for any idea which could fix my problem. If anybody needs my mesh-files, please tell me I will upload them.

Thx,
fs82

Try posting your mesh and let me know what patches are cyclic. If you have a .jou file to go with it so I can generate the mesh myself that would be great. I had this problem a few months ago and it was incredibly annoying. I found some posts on the message board that helped.

Dan

This would be great if you could try it. I have no more idea, what to try next :/
I uploaded the files to my webaccount. If you klick on the link below, you will find a zip-archiv with all neccesary gambit files included and my createPatchDict. I think I named everything in english, except the file name :D Periodic are all "p_z<number>" patches.

Thanks a lot.

Fabian

http://wwwpub.zih.tu-dresden.de/~fschleg/cylinder.zip

still not sure
 

I took a look at your mesh file and imported the mesh with no problems. I did however get the same problem that you have. I would make sure of a few things.

1. Make sure that you liked the faces correctly. I had a similar problem and I wasn't linking the faces correctly and reversing the direction correctly. Make sure that you pick the mirror image of the vertex on opposing sides and the arrows that leave the opposing vertices are going the same direction. Since your mesh is nice, it may be hard to tell if you have the right direction. If you use a tet mesh the mesh becomes twisted and its obvious that its going the wrong direction. I suspect that this is it.

2. Make sure you change the write precision. Once i fixed my mesh linking problem, that was another problem. I think that this problem was pointed out in:
http://www.cfd-online.com/Forums/ope...-boundary.html

3. Try making the the periodic boundaries as separate faces in GAMBIT (after the edges/faces have been linked and volume meshed), then check to make sure that the number of points and cells match. After that you can make them into cyclic patches in OF.

Thats all I can think of right now. Try some of those and if it doesn't work, then go back to a simple geometry and try that until you have the method down.

Dan

Yeah I found the problem. For everyone who is dealing with the same problem concerning cyclic boundaries in OpenFoam try the following:

1) as mentioned above from chegdan, make sure that you have linked all your faces correctly (Reverse orientation switch in Gambit have to be ON)

2) if you have split your perodic boundaries into parts to help gambit for meshing, put every part of your periodic boundary into one patch. Do not put both faces which should be periodic into the same boundary patch. They have to be separate patches.

3) export mesh with Gambit

4) use fluentMeshToFoam

5) create a CreatePatchDict dictionary in system/ folder and combine your separate perodic patches to one. For type use cyclic. Do not touch constant/polymesh/boundary for this step.

Example:
{
name pz_1;
type cyclic;
constructFrom patches;
patches (pz_1 pz_1shadow);
set f0;
}

6) run createPatch utility. This will combine the periodic patches to one and renumber it for OpenFoam.

7) open constant/polymesh/boundary and change wall to cyclic for your periodic boundaries. Do not forget to change your createPatchDict, because you have combined two patches to one right before.

8) rerun createPatch for making your boundaries perodic

This should work und looks good for me. I guess the problem ist Gambit, which numbers the faces without any order if you put both parts of your perodic boundary into one patch. I think fluent does not care about the numbering of the boundary faces but OpenFoam (CreatePatch) does. So for me it works :-D

Thx chegdan for your help.

Fabian

Edit: If you still have Problems: Make sure you have set WritePrecision in controlDict to a value greater than 10. Also try to remove functions from controlDict (comment them out).

glad I could help
 

Glad I could help.

I still have another problem with periodic boundaries. I tried another Gambit mesh to convert it to OpenFoam. This is a simple channel with two periodic boundaries. With the steps I described above I get a error during the second run of createPatch:

Synchronising points.
--> FOAM Warning :
From function syncTools<class T, class CombineOp>::syncPointList(const polyMesh&, UList<T>&, const CombineOp&, const T&, const bool)
in file /home/dm2/henry/OpenFOAM/OpenFOAM-1.5/src/OpenFOAM/lnInclude/syncToolsTemplates.C at line 1047
There are decomposed cyclics in this mesh with transformations.
This is not supported. The result will be incorrect
Points changed by average:0.00458973012292 max:7.02481475253

I am not really sure what synchronisation of points does, but if I turn it of everything works fine. Is this problem due to my TWO periodic boundaries? May be the converter is not able to distinguish between the two periodic patches?

Fabian

I've had similar problem before. It turned out that I set the write tolerance too small (it was initially set as 1e-6 or something, now it's happily staying at 2e-2 and works great.) I'll try and see if I can get your grid working when I get back into my lab later today, though (that's where I have openfoam installed,I'm still trying to figure out how to scp a file on a windows machine to a linux machine.)

________

EDIT:

Yeah, I just realized that I do have X windows on my current workstation and downloaded your file through firefox. Anyway, I think there's a few problem with your setup.

First of all, I don't think the createPatchDict are setup to handle more than two patches, so you should probably group all the faces on the RHS into a boundary patch called sidewall_right and the faces on LHS into sidewall_left (they should be in the same order when you assign the faces to BC in Gambit, e.g. top to down, front to back or something similar). Hope that helps.

If you need more than one patch on each wall, create the cyclic sets on a 1 to 1 basis just to make sure the face order does not get messed up.

Thx for having a look to my mesh. Linux offers you a nice little tool called dos2unix which converts Linux files for usage in a microsoft environment. By default is is not installed but you can simple download it via your package manager.
So my cyclinder is now working fine with the process discribed some posts before. Which variable have you set to 2e-2? WritePrecision or matchingTolerance ? I know the easiest way to get createPatch work is adjusting the matchingTolerance, but for my cylinder mesh I have to set the matchingTolerance to a value greater than 2. So if you try my way with two times createPatch, first to combine the two boundaries which should be periodic into one patch and second to make this patch periodic, this works ... that was what I thought until yesterday.
I need a channel mesh, so I created one with Gambit and tried my way to get periodic/cyclic boundaries in flow and crossflow direction. But this does not work and I get the error mentioned one post before.
The solution was to turn of syncronisation of points for the last run of createPatch. So for me it would be interesting what synconisation really does and why it sometimes works and sometimes not. It is not satisfying do figure out a special way of creating periodic boundaries for every new mesh.
While having a closer look to the channel395 tutorial I also noticed another mystery. In this tutorial the cyclic boundaries are in several patches for every side. So one patch for left side, one for right side, one for inflow and one for outflow. I thought you have to have one patch for every perodic boundary, for this example one patch in- and outflow and one patch left and right ... if I try this for my channel I get the annoying possible face ordering problem. I dont know where is my problem?

I don't really understand the whole process of channel395 either, but from observation I've concluded that the boundary setup they used for that case only works if the boundary is meshed uniformly.

I've never looked further into the problem since I've managed to get the cyclic patch working by grouping each side of the wall with one patch and combining the two using createPatch, and since I deal more with airfoil simulation instead of channel flow, I guess I never felt the need to look further into the issue. Hope that helps.

I get the problem ... try and error and a hint in a thread. I have the situation of two periodic boundaries which are orthogonal to each other and this is a problem. CreatePatch is not able to synchronize the nodes which are situated along the corner egde which connect both boundaries. This is because of a different transformation tensor for the same node belonging to several patches. For one the synchronization works but not for both. The nice thing is - may be only for my channel - that the mesh with and without synchronization is the same, so it doesn't mather (a diff on all files in polymesh shows no difference). This could be a result of my writePrecision of 12 but I am not sure. So if you have two periodic boundaries which are connected and lie on different planes turn off pointSync and it will work!
Thx for help
P.S.: May be anybody know what pointSync really does I guess it adjusts the point coordinates?

creating cyclic boundary condition,
 

Hi, I am having difficulty in creating cyclic boundary condition, I have done it this way:
1- I created a mesh in Gambit (Quarter of a cylinder) and I called the two planes symmetrya and symmetryb. and I set them to be symmetry for periodic bc.
2-set the writePrecision in system/controlDict to 12.
3-In the end of *.msh file I saw
(0 "Cells:")
(12 (0 1 5eb78 0))
(12 (2 1 5eb78 1 4))

(0 "Zones:")
(45 (2 fluid fluid)())
(45 (3 mass-flow-inlet ariinlet2)())
(45 (4 symmetry symmetryb)())
(45 (5 symmetry symmetrya)())
(45 (6 pressure-outlet outlet)())
(45 (7 wall wall)())
(45 (8 mass-flow-inlet airinlet1)())
(45 (9 mass-flow-inlet fuelinlet)())
(45 (11 interior default-interior)())

I did not change anything here, and leave it as it is.
3-then I ran fluentMeshTofoam *.msh :

Building boundary and internal patches.
Creating patch 0 for zone: 3 start: 1 end: 25 type: mass-flow-inlet name: ariinlet2
Creating patch 1 for zone: 4 start: 26 end: 10345 type: symmetry name: symmetryb
Creating patch 2 for zone: 5 start: 10346 end: 20665 type: symmetry name: symmetrya
Creating patch 3 for zone: 6 start: 20666 end: 23898 type: pressure-outlet name: outlet
Creating patch 4 for zone: 7 start: 23899 end: 34233 type: wall name: wall
Creating patch 5 for zone: 8 start: 34234 end: 34263 type: mass-flow-inlet name: airinlet1
Creating patch 6 for zone: 9 start: 34264 end: 34306 type: mass-flow-inlet name: fuelinlet
Creating patch 7 for zone: 11 start: 34307 end: 1181033 type: interior name: default-interior
Adding new patch ariinlet2 of type patch as patch 0
Adding new patch symmetryb of type symmetryPlane as patch 1
Adding new patch symmetrya of type symmetryPlane as patch 2
Adding new patch outlet of type patch as patch 3
Adding new patch wall of type wall as patch 4
Adding new patch airinlet1 of type patch as patch 5
Adding new patch fuelinlet of type patch as patch 6
Patch default-interior is internal to the mesh and is not being added to the boundary.

Default patch type set to empty

Writing mesh... to "constant/polyMesh" done.


End


4-It creates in the constant/polymesh ---> boundary :

7
(
ariinlet2
{
type patch;
nFaces 25;
startFace 1146727;
}
symmetryb
{
type symmetryPlane;
nFaces 10320;
startFace 1146752;
}
symmetrya
{
type symmetryPlane;
nFaces 10320;
startFace 1157072;
}
outlet
{
type patch;
nFaces 3233;
startFace 1167392;
}
wall
{
type wall;
nFaces 10335;
startFace 1170625;
}
airinlet1
{
type patch;
nFaces 30;
startFace 1180960;
}
fuelinlet
{
type patch;
nFaces 43;
startFace 1180990;
}
)


5-then I define the createPatchDict in /system and within that I have:
matchTolerance 1E-3;
pointSync true;
patches
(
{
name symmetrya;

type cyclic;

constructFrom patches;

patches (symmetrya symmetryb);
}
);

6-then I ran createPatch, this was the outcome:
Create time

Reading createPatchDict.

Using relative tolerance 0.001 to match up faces and points

Create polyMesh for time = 0


Moving faces from patch symmetrya to patch 2
Moving faces from patch symmetryb to patch 2

Doing topology modification to order faces.

Synchronising points.
Points changed by average:0 max:0

Removing patches with no faces in them.

Removing empty patch symmetryb at position 1
Removing patches.
Writing repatched mesh to 1

End
7-It creates a folder /1/polyMesh and within that:
[]$ ls
boundary cellZones faces faceZones neighbour owner points pointZones

8-vi boundary :
6
(
ariinlet2
{
type patch;
nFaces 25;
startFace 1146727;
}
symmetrya
{
type symmetryPlane;
nFaces 20640;
startFace 1146752;
}
outlet
{
type patch;
nFaces 3233;
startFace 1167392;
}
wall
{
type wall;
nFaces 10335;
startFace 1170625;
}
airinlet1
{
type patch;
nFaces 30;
startFace 1180960;
}
fuelinlet
{
type patch;
nFaces 43;
startFace 1180990;
}
)

8-I copy all the contents of this folder to constant/polymesh/

9- I did changed the symmetryplane type now to cyclic for symmetrya

10-I did the simpleFoam and I received this error:

Create time
Create mesh for time = 0
face 0 area does not match neighbour 10320 by 21.8435% -- possible face ordering problem.
patch:symmetrya my area:0.000277 neighbour area:0.000344925 matching tolerance:0.001
Mesh face:1146752 vertices:4((0 0 0.1123) (0.05 0 0.1123) (0.05 0 0.11784) (0 0 0.11784))
Neighbour face:1157072 vertices:4((0 0.043315 0) (0 0.0502135 0) (0.05 0.0502135 0) (0.05 0.043315 0))
Rerun with cyclic debug flag set for more information.

From function cyclicPolyPatch::calcTransforms()
in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 150.

FOAM exiting



Can anyone help me with this problem?

This looks pretty good, but while reading your post I figured out two possible problems.

1) When you define your boundary conditions in gambit use "wall" not "periodic" or something else. But make sure that you link all your periodic faces.

2) After your step 9 you have to use createPatch again and you will get another directory like in step 7 with a new polymesh (remove the directory from step 7 before you start createPatch again)

Try this and hopefully this will work.

creating cyclic boundary condition
 

Hi

I did what you told me but I still have problems,.....

You still get the error you posted a view days ago? May be you could upload your mesh anywhere? I would try to convert it to OpenFoam for myself.

cyclic bc problem
 

I have the exact same problem with cyclic BCs and mesh exported from Gambit/Fluent. I followed the procedures described above and still cannot make it work. Did you guys find what the problem was? I'm running out of ideas of how to fix this problem. Thanks

Aha! I figure it out. I did what mcjicpm2 did above, however, i used Fluent3DtoFoam instead of FluenttoFoam and that made all the difference. Make sure that the faces are properly linked in Gambit though.

hi fabian
that realy worked, thanks a lot!!

Dear Fabian,
I created my mesh by blockMesh, snappyHexmesh, but still have the problem
"face 391 area does not match neighbour 791 by 0.0136179% -- possible face ordering problem."
I also set writeprecision as 10..
Could you please give some suggestion? Thank you so much!
Aqua

Dear aqua,

In "createPatchDict" file from the applications/utilities/mesh/manipulation folder, you will see the following...

// 2. Correct incorrect cyclic:
// This will usually fail upon loading:
// "face 0 area does not match neighbour 2 by 0.0100005%"
// " -- possible face ordering problem."
// - in polyMesh/boundary file:
// - loosen matchTolerance of all cyclics to get case to load
// - or change patch type from 'cyclic' to 'patch'
// and regenerate cyclic as above

So, you can loosen matchTolerance of your cyclics to get it to work or change the patch type to patch from cyclic and use createPatch to make your cyclic. Hope this helps, let me know.

Dear vishalsacharya,
Thank you so much for your kind reply. I knew the matchTolerance, so I tried to give it a big value, even 3. but it still didn't work.
For me the interesting thing was:
I could create the cyclic in OF2.0 with a matchTolerance of 0.001;
But I couldn't create the cyclic in OF 1.6-ext even the matchTolerance was 3...

So I assumed that OF1.6ext has something not that right...

cheers!

Aqua

hi

I found out that PointWise dont need these steps such as Gambit. is this true ?

problem with fan and createPatch
 

Hi everyone,

I am having trouble dealing with cyclic boundary conditions, namely with the fan boundary condition since I want to simulate a jump pressure between two parts of my system.

First I will describe a little bit my case. I have two different tubes. At the outlet of the first tube I want to simulate a pressure drop of 0,2bar before the flow continues through the other tube (see picture 1 attached).

My problem is that the patches "a and b" do not match each other ( the error says "area does not match neighbour 2520 by...") after mesh-conversion to OF. Therefore the createPatch utility must be run.

The process I´ve carried out so far is:

1. Mesh-generation/export with ANSYS

2. Coversion with fluent3DMEshtoFOAM

3. Creation of createPatchDict to combine the separated periodic patches to one (a und b to a)

4. Run createPatch utility. Folder /1/polyMesh is created

5. Copy of the contents of /1/polyMesh to constant/polymesh/

6. Change wall type to cyclic for the new created "a" patch

7. Now I need the NeighbourPatch for the new created "a" patch... What should I do here?

Fabian says that createPatch directory should be changed and then createPatch re-run again. I do know how this new createPatchDict should look like... I mean, what should be written there in order to get the right second patch?

Another way I came up with would be to use cyclicAMIs instead of cyclics one. On this way, the createPatch-process would be avoided but then the fan b.c. could not be used (the error "attempt to cast type cyclicAMI to type cyclic" appears)..

Other possibility would be to use groovyBC... but I am not sure about it.

I am running out of ideas anklöäd I would really appreciate any kind of help in this topic.

I wish you a nice Thursday,
José.

Hi Josè. What OF version are you using? you did not mention it in your post.

mad

Hi Maddalena,

I am using OF 2.1.1.

Regards,
José.

Then this is not the right place where to look for infos... Cyclic definition has changed since OF 2.1. You can find something more here: http://www.cfd-online.com/Forums/ope...aries-21x.html

Thank you Maddalena!

I went through this post (and the post inside it) and I am still having some trouble after modifying my case.
I will be post my case there. I will be very grateful if you could take a look at it.

Greets,
José.

problem in creation of Cyclic Boundaries
 

Hi ,

I have followed the steps mentioned above to create cyclic boundaries but i am getting following error
Anybody know whats the problem ?

problems with Cyclic and simpleSRFFoam in OF-ext 3.0
 

Hi,
I think that I have a problem with cyclic interface. I'm running a pump blade passage in simpleSRFFoam in foam-extend 3.0 The mesh is fully hexahedral made with a commercial software and the cyclic interface has been created with create patch. The checkMesh is OK and my BC are

Boundary

Urel

p


the simulation diverges really quickly:

But if I use wall instead of cyclic it runs.

Do you have any suggestion?

Regards,
Ale

Hi,

Floating point error is bad because you can not get and error which is occurring while solving the problem.
Few things to check...
1. How many no of passages you have ( according to your input i can see there are 7 passages ) if not please correct accordingly.
2. Check your initial values for all fields are appropriate .
3. Most importantly your cyclic definition in commercial package while meshing should be very appropriate i.e point to point connection between the nodes.

Regards,
Sangamesh Hosur

Thank you for your reply.

1: The number of blade passage is correct
2: I think they are. But I will check it again.
3: The meshes on the cyclic boundary is conformal.

Seeing how fast it's diverging I think that the error has to be something evident but I couldn't find it yet.

Hi,

Check your k-omega BC's. Which are the major culprits for this floating point error .

by the way how have you evaluated k-omega values ?

Regards,
Sangamesh Hosur

the first time I calculated my k omega and epsilon with standard formula using the inlet velocity, the second time I took it from the results of the simulation that I'm using as benchmark and then I tried to run it as laminar with a reduced velocity but the results don't change that much. While setting the cyclic BC as wall the simulation runs with both sets of turbulent BC.
for example my k dictionary looks like:

Yesterday I ran the complete impeller with the same BC and initial field and the results are fine, so I'm sure that my problem is related to cyclic BC.
I found a topic about problems of cyclic BCs applied to curved surface.

http://www.cfd-online.com/Forums/ope...-boundary.html

Mattijs

"Hi Håkan,

cyclics have to be planar for automatic matching (couplePatches, createPatch) to work since both transformation tensor and face-face correspondence have to be determined.

If they are non-planar you'll have to get your mesh generator to output the patch faces in the correct order. "

As far as I know the new definition of the cyclic BC (OF 2.1x), don't have anymore this limitation. I saw that the utility createPatch in OF-ext-3.0 is taken from OF-ext-1.6 and if I'm not wrong it uses the old cyclic definition, consequently I start to think that it can be the reason why my simulation diverges. Am I wrong?
Can you suggest me how can I check if my cells are in the correct order?

Regards,
Alessandro

Hi

I am using terrain block mesher to mesh my terrain .The problem with this tool is that it cannot generate cyclic boundary conditions.I therefore had to use the createPatchDict utlity to create the cyclic patches. the problem is that I have north,south east west patches as neighbours and I cannot combine them into two as you did for your case as each. I am attaching the boundary and createPatchDict and would appreciate if you can kindly suggest a solution to my problem.