[lord_kossity]

Ok, Andras,

your test case works in the way you are describing it using OpenFOAM-1.4.1

Applying the proposed steps to my case always causes problems with the stitchMesh function, normally running into the error

--> FOAM FATAL ERROR : Zero length edge detected. Probable projection error: slave patch probably does not project onto master. Please switch on enriched patch debug for more info#0 Foam::error::printStack(Foam::stream&) in "~/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"

Maybe you can even help me out of this situation!?
I would be really interested in finally solving this problem...

[andras]

Andreas,

I am trying to stitch the faces that make up the surface of a cylinder (to connect inner and outer meshes for Multiple Reference Frame simulations). I can stitch either both pairs of circles or the cylindrical shell but I can't connect the shell patches, when the circles are already stitched.

I have tried creating combined patches and stitching the pairs at once and also stitching them one by one. Either way I run into "projection errors" and other strange errors like you do.

A congruent straight line edge between two or more patches stitches fine. I checked that with another test case. Congruent curved edges seem to be the troublemaker when the patches are not parallel to each other... but this is just a guess.

To cut it short: I'm stuck. Although some people say that stitchMesh is actually working fine I think there are some bugs underneath the carpet (especially concerning more complex geometries).


Andras

[lord_kossity]

Hello Andras,

what I'm trying to stitch are the diffeent mesh resolutions here:

.

As can be seen the Interfaces aren't curvy and the geometry seems quite simple. But not simple enough for stitch Mesh...

I do not even find a starting point were to continue with a new approach of solving that problem.

So any idea for a new starting point is pretty welcome!!

[andras]

Hi Andreas!
You could try creating two final patches using the "createPatch" tool with a createPatchDict that looks like this:

/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.0 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

FoamFile
{
version 2.0;
format ascii;

root "/home/yourUsername/YourCaseRoot";
case "caseName";
instance "system";
local "";

class dictionary;
object createPatcheDict;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

patches
(

{
// Name of new patch
name if0;

// Type of new patch
type patch;

// How to construct: either 'patches' or 'set'
constructFrom patches;

// If constructFrom = patches : names of patches
patches ( face1 face2 face3 ... );

}

{
// Name of new patch
name if1;
...
}

);

Then stitch the combined patches.

Have you already tried my recipe on your mesh with OpenFoam-1.4.1 vanilla?


Best,
Andras

[lord_kossity]

Hello Andras,

well, maybe I did not get the point, but the patches are already defined out of the four faces.

For example if I use
stitchMesh <root> <case> IF_1_inside IF_1_outside,
my aim is to stitch the two patches surrounding the smallest square. What I'm trying to say is that e.g. IF_1_inside consists out of the faces 1, 2, 3, 4, and I do not have to stitch every single face. (As far is I understood the functionality of createPatch is to combine the faces to one single patch!?)


I already tried your recipe on my mesh with OpenFoam-1.4.1 from the opencfd page, but what is the vannila version of that?

Thanks for your time,
Andreas

[andras]

Hi Andreas!
When saying vanilla I mean the standard release without any development patches...
I'm sorry to say I have no further ideas concerning stitchMesh at the moment.


Andras

[mgz1985]

hi,

I do not know if my problem falls in this thread or not but it is kind of strange.

I am trying to mesh a small region between the slot and flap. I define points in sequence but point 3 should be to the right of point 2 but it comes to the left of point 2 no matter what I try.

I am attaching both the image file and the blockMeshDict with this.

Can some one please take a look and help me? I am just trying this patch individually before I put it in my main mesh.

Thanx a lot.

blockMeshDict

[sebastiank]

Hello,
I've tried to get rid of 2 pairs of interfaces in my simulation and did so like Andras Horvarth. But when I run foamMeshToFluent I get the following error message:

--> FOAM FATAL ERROR : edgeFaces_ full at entry:16 for edge 2 0#0 Foam::error::printStack(Foam:stream&) in "/usr/lib64/OpenFOAM/OpenFOAM-1.4.1/lib/libOpenFOAM.so"
#1 Foam::error::abort() in "/usr/lib64/OpenFOAM/OpenFOAM-1.4.1/lib/libOpenFOAM.so"
#2 Foam::cellMatcher::calcEdgeAddressing(int) in "/usr/lib64/OpenFOAM/OpenFOAM-1.4.1/lib/libOpenFOAM.so"
#3 Foam::tetMatcher::matchShape(bool, Foam::List<foam::face> const&, Foam::List<int> const&, int, Foam::List<int> const&) in "/usr/lib64/OpenFOAM/OpenFOAM-1.4.1/lib/libOpenFOAM.so"
#4 Foam::degenerateMatcher::match(Foam::List<foam::fa ce> const&, Foam::List<int> const&, int, Foam::List<int> const&) in "/usr/lib64/OpenFOAM/OpenFOAM-1.4.1/lib/libOpenFOAM.so"
#5 Foam::degenerateMatcher::match(Foam::primitiveMesh const&, int) in "/usr/lib64/OpenFOAM/OpenFOAM-1.4.1/lib/libOpenFOAM.so"
#6 Foam::primitiveMesh::calcCellShapes() const in "/usr/lib64/OpenFOAM/OpenFOAM-1.4.1/lib/libOpenFOAM.so"
#7 Foam::primitiveMesh::cellShapes() const in "/usr/lib64/OpenFOAM/OpenFOAM-1.4.1/lib/libOpenFOAM.so"
#8 Foam::fvSchemes::read() in "/usr/lib64/OpenFOAM/OpenFOAM-1.4.1/applications/bin/foamMeshToFluent"
#9 Foam::objectRegistry::writeData(Foam:stream&) const in "/usr/lib64/OpenFOAM/OpenFOAM-1.4.1/applications/bin/foamMeshToFluent"
#10 __libc_start_main in "/lib/libc.so.6"
#11 Foam::fvMesh::readUpdate() in "/usr/lib64/OpenFOAM/OpenFOAM-1.4.1/applications/bin/foamMeshToFluent"


From function calcEdgeAddressing(const faceList&, const label)
in file meshes/meshShapes/cellMatcher/cellMatcher.C at line 202.

FOAM aborting

Aborted

[obraun]

Hi all,

now I've played around with stitchMesh in a similar configuration than Andreas Dietz, just that it is all hexa. In fact the mesh is generated with ICEM pure hexa in good old block refinement style. When going through unstruct representation in ICEM in order to use fluent format for transfer, there is no connectivity of the non-conformal patches as could have been in Multiblock representation IIRC good old TASCflow times.
SO far so good. So I went to stitch together all the patches and understood I had to do it separately, which means to fiddle around in ICEM to separate the volumes and interface regions ok. (tried the n-squared setting to 1, worked with no complaint but meshCheck complained about degenerate elements, believe he found some elements on opposite sides of the interfaces surrounding a hydrofoil). Got it to have 2x8 patches, pairing each. I put up a little shell script to automate the task. It might be neither bullet-proof neither a tutorial of efficient shell programming but it might be useful for some:

# The pairing patches from ICEM are named e.g. INT_01_E_0 INT_01_E_1 (or _Red _Green)

# The important is that two and only two patches containing the PatchList entry exist

PatchList=( INT_01_E INT_01_W INT_01_N INT_01_S INT_12_W INT_12_E INT_12_N INT_12_S )

echo ${PatchList[@]}

for PatchBase in ${PatchList[@]}; do

rm constant/polyMesh/*Zones
rm constant/polyMesh/meshModifiers
Patches=$(grep $PatchBase constant/polyMesh/boundary)
echo $Patches
stitchMesh ${Patches[0]} ${Patches[1]}

if [ -e 1e-05/polyMesh/ ]
then
rm -r constant/polyMesh/
mv 1e-05/polyMesh/ constant/
rm -r 1e-05
npatch=$(grep -P -m 1 ^[0-9]+$ constant/polyMesh/boundary)
nrm=$(grep -c $PatchBase constant/polyMesh/boundary)
nnew=$(( $npatch - $nrm ))
echo "$npatch $nrm $nnew"
cp constant/polyMesh/boundary tmpbnd
cat tmpbnd | sed "18s/$npatch/$nnew/" | sed "/$PatchBase/,+5d" > constant/polyMesh/boundary
checkMesh

else
exit
fi
done

So far I run into trouble again as soon as stitching a patch neighboring an already stitched patch. Patching N-S and N-S is fine, or E-W and E-W, as soon as a neighbor shall be stitched, I get an error:

Face 1977839 reduced to less than 3 points.
Topological/cutting error B.
Old face: 2(218300 218301) new face: 2(218300 218301)

From function void slidingInterface::coupleInterface(polyTopoChange& ref) const
in file polyMeshModifiers/slidingInterface/coupleSlidingInterface.C at line 1794.

with 1.5-dev (1095)

I ended up following another strategy that seamed more obfuscated at the beginning but showed up to be pretty feasible.

I export just a simple coarse Mesh from ICEM via fluent format into Foam. Then i got the refinement region boundaries as STL files from ICEM, I've slightly blown them up by offset. Use cellSet to define the refinement regions and refineMesh-dict on the cell sets to do the classical Hex-Cutting 2x2x2. This proved to work quite easily and avoids transferring huge fluent format files.

When using embedded refinement regions, have to start with the most outer one, because cells at the 'hanging node interface' become polyhedral and cannot be refined with the standard hex cell cutting.

Hrvoje, as you are apparently working on the invoked routines, I can provide you a more detailed description of what happens.

Cheers

Olivier

[richpaj]

Recently, I happened to be working on stitching together interfaces (tops of boxes in fact) that contain corner points
and initially encountered some of the problems mentioned earlier on this thread cf.

Anita April 21, 2008, 13:27

lord_kossity May 15, 2008, 07:52

To take Anita's outline problem:

------------------------------------
|6......................................5|
|.........................................|
|.........................................|
|1...........................2................|
|==============................|
|10.......................9 || .............|
|............................ ||...............|
|............................ ||...............|
|7....................... 8 || 3.............4|
------------------------------------



stitching 1-2 with 10-9 prevents a similar operation for the pair 9-8 and 2-3. The problem seems
to be related to the projection of nodes from edge 9 to positions along edge 2. These projected nodes appear
as isolated points along edge 2 (when examining the interface 2- 3 in paraView for example)
which do not (necessarily) coincide with the vertices of the faces on the interface 2-3.
The algorithm (in enrichedPatchCutFaces.C) notices this and aborts.

As a possible compromise I used the schema below to resize the patches 9-8
and 2b-3 so that common edge points of (2a - 9 - 2b) are no longer included. After stitching all interfaces
i.e. initially 1 - 2a with 10-9a then 2b-3 with 9b-9 one
is left with a narrow patch one face area wide designated by "*". A "skeletal" patch, if you like, that will
require suitable boundary conditions in order to minimize its impact upon the prevailing flow.


------------------------------------
|6......................................5|
|.........................................|
|.........................................|
|1...........................2a................|
|==============................|
10........................9a *...............|
| .......................9b || 2b.............|
|............................ ||...............|
|............................ ||...............|
|7....................... 8 || 3.............4|
------------------------------------

The dimensions of the flow problem in my case meant that the presence&influence of such a "skeleton" could
be regarded as negligible. This may not always be the case though.


The following is a prescription (using either OpenFoam-1.5.x or OF-1.5-dev) to resize the relevant patches using a
combination of "faceSet" ("pointSet" could be incorporated too if required) and "createPatch" commands:

(
where
interface1 = 1 - 2 - 3
interface2 = 10 - 9 - 8
)

1)

in faceDictInterface1Faces

// Name of set to operate on
name interface1Faces;

// One of clear/new/invert/add/delete|subset/list
action new;

topoSetSources
(

// Patch to faces
patchToFace
{
name interface-1-2-3;
}

);

...issue commands
" cp faceDictInterface1Faces system/faceDict "
"faceSet"

2)

now extract faces whose normals point in the required direction

faceSetDictNormalx


// Name of set to operate on
name interface1-xDirectionFaces;

// One of clear/new/invert/add/delete|subset/list
action subset;

// Actions to apply to pointSet. These are all the topoSetSource's ending
// in ..ToFace (see the meshTools library).
topoSetSources
(

normalToFace
{
normal (1 0 0); // Vector
cos 0.01; // Tolerance (max cos of angle)
}

);

...issue commands
" cp faceSetDictNormalx system/faceDict "
"faceSet"


3)

for each set of faces aligned in a particular direction (or sitting on a component interface plane)
take those that have no vertex lying on the common edge 2-9.


faceSetDictNormalxReduced

// Name of set to operate on
name interface1-xDirectionReducedFaces;

// One of clear/new/invert/add/delete|subset/list
action subset;

// Actions to apply to pointSet. These are all the topoSetSource's ending
// in ..ToFace (see the meshTools library).
topoSetSources
(

// Faces with face centre within box
// Ensure the bounds do *not* include any common edge vertices
boxToFace
{
box (xMin yMin zMin) (xMax yMax zMax);
}

);

...issue commands
" cp faceSetDictNormalx system/faceDict "
"faceSet"


4)


createPatchDictNormalxReduced


// Tolerance used in matching faces. Absolute tolerance is span of
// face times this factor.
matchTolerance 1E-3;


// Do a synchronisation of coupled points.
//pointSync true;
pointSync false;

// Patches to create.
// If no patches does a coupled point and face synchronisation anyway.

patches
(

{
// Name of new patch
name interface1NormalxReduced;

// Type of new patch
type patch;

// How to construct: either 'patches' or 'set'
constructFrom set;

// If constructFrom = set : name of faceSet
set interface1-xDirectionReducedFaces;
}

);

...issue commands
" cp createPatchDictNormalxReduced system/createPatchDict "
"createPatch"



Then repeat steps 1)-4) for all the various interface planes. Finally, "stitchMesh" the 'reduced' interface planes
and apply boundary conditions to the remaining mesh "skeleton".


It's a painful process but might be a useful compromise in some circumstances.
When the surfaces meeting at the corner of an interface are non-planar
then greater use of "boxToFace" ( or similar pointSet directives) will unfortunately be required it seems.

With regard to cylindrical cap interfaces (cylinders with one closed end), it appears that sometimes these
can be stitched directly ( using OF-1.5dev, I didn't extensively check with OF1.5.x) and sometimes not (!). The only
noticeable difference in the two cases being the distribution of interface points along the edges. If points from
both interfaces coincide (to whatever tolerance) along the edge then the stitching process is likely to fail.
In the latter situation decomposing as above, 1) - 4), might be an alternative approach.


I hope this helps,

Richard Kenny.

[aqua]

Hello，Hrv,
I am trying to simulate two cars passing by each other, by moving mesh. so the geometry model is like in the attachment: block1 and block2 are the air parts, icube and ocube are two cars. block1 and block2 will move towards each other by setting their interfaces GGI.
Now, I am trying to mesh it.
I tried to used snappymultiRegionFoam case to create the mesh. so, in triSurface, there are four files: block1.stl, block2.stl, icub.stl, ocube.stl.
without icube and ocube, I got it managed to creat the mesh. Then I added the icube and ocube.
but，during snappyhexmesh, some information is givin like this:
CellZones:
block1 size:7919
block2 size:7737
icube size:0
ocube size:0
FaceZones:
iblock size:0
oblock size:1200
icube size:0
ocube size:0


Could you please help me on this? Is there some other way to creat the mesh i want? Thank you so much!!

Aqua

[Yosmcer]

As this post is related to stichMesh and that I do not use it, I made a new thread:
Merging ege patches