[saidc.]

Hi,

I'm simulating a natural convection turbulent flow in a box geometry. Inside the box I've a stl file. I cannot share my all mesh but for better understanding HERE there've a quick draw. Case folder and log files have atteched without stl file.

I was working with Foundation v8, but since there is no "heatTransferCoefficient" function there, I decided to work with ESI. With Foundation I haven't got any error. My case works fine. But in ESI I'm getting this error while decomposePar.

Create time

Decomposing mesh region0

Create mesh

Calculating distribution of cells
Selecting decompositionMethod hierarchical [4]

Finished decomposition in 2.88 s

Calculating original mesh data

Distributing cells to processors

Distributing faces to processors

Distributing points to processors

Constructing processor meshes
Reading hexRef8 data : cellLevel
Reading hexRef8 data : pointLevel
Reading hexRef8 data : level0Edge

Processor 0
    Number of cells = 788380
    Number of faces shared with processor 1 = 8091
    Number of faces shared with processor 2 = 7646
    Number of faces shared with processor 3 = 9
    Number of processor patches = 3
    Number of processor faces = 15746
    Number of boundary faces = 174765

Processor 1
    Number of cells = 788380
    Number of faces shared with processor 0 = 8091
    Number of faces shared with processor 3 = 7864
    Number of processor patches = 2
    Number of processor faces = 15955
    Number of boundary faces = 162934

Processor 2
    Number of cells = 788380
    Number of faces shared with processor 0 = 7646
    Number of faces shared with processor 3 = 7911
    Number of processor patches = 2
    Number of processor faces = 15557
    Number of boundary faces = 162985

Processor 3
    Number of cells = 788381
    Number of faces shared with processor 0 = 9
    Number of faces shared with processor 1 = 7864
    Number of faces shared with processor 2 = 7911
    Number of processor patches = 3
    Number of processor faces = 15784
    Number of boundary faces = 152356

Number of processor faces = 31521
Max number of cells = 788381 (9.51318e-05% above average 788380)
Max number of processor patches = 3 (20% above average 2.5)
Max number of faces between processors = 15955 (1.2341% above average 15760.5)

Time = 0
AMI: Creating addressing and weights between 10800 source faces and 10800 target faces
--> FOAM Warning : 
    From void Foam::advancingFrontAMI::checkPatches() const
    in file AMIInterpolation/AMIInterpolation/advancingFrontAMI/advancingFrontAMI.C at line 71
    Source and target patch bounding boxes are not similar
    source box span     : (0 80 240)
    target box span     : (0 80 240)
    source box          : (-40 -40 -120) (-40 40 120)
    target box          : (120 -40 -120) (120 40 120)
    inflated target box : (107.351 -52.6491 -132.649) (132.649 52.6491 132.649)
AMI: Patch source sum(weights) min:0.999999 max:1 average:1
AMI: Patch target sum(weights) min:0.999999 max:1 average:1
AMI: Creating addressing and weights between 10800 source faces and 10800 target faces
--> FOAM Warning : 
    From void Foam::advancingFrontAMI::checkPatches() const
    in file AMIInterpolation/AMIInterpolation/advancingFrontAMI/advancingFrontAMI.C at line 71
    Source and target patch bounding boxes are not similar
    source box span     : (80 0 240)
    target box span     : (80 0 240)
    source box          : (-40 -40 -120) (40 -40 120)
    target box          : (-40 120 -120) (40 120 120)
    inflated target box : (-52.6491 107.351 -132.649) (52.6491 132.649 132.649)
AMI: Patch source sum(weights) min:0.999999 max:1 average:1
AMI: Patch target sum(weights) min:0.999999 max:1 average:1

Processor 0: field transfer
Processor 1: field transfer
Processor 2: field transfer
Processor 3: field transfer

End

After decomposePar is over I tried run the case and the output is:

AMI: Creating addressing and weights between 10800 source faces and 10800 target faces
--> FOAM Warning : 
    From void Foam::advancingFrontAMI::checkPatches() const
    in file AMIInterpolation/AMIInterpolation/advancingFrontAMI/advancingFrontAMI.C at line 71
    Source and target patch bounding boxes are not similar
    source box span     : (0 80 240)
    target box span     : (-2e+150 -2e+150 -2e+150)
    source box          : (-40 -40 -120) (-40 40 120)
    target box          : (1e+150 1e+150 1e+150) (-1e+150 -1e+150 -1e+150)
    inflated target box : (8.26795e+149 8.26795e+149 8.26795e+149) (-8.26795e+149 -8.26795e+149 -8.26795e+149)
--> FOAM Warning : 
    From bool Foam::advancingFrontAMI::initialiseWalk(Foam::label&, Foam::label&)
    in file AMIInterpolation/AMIInterpolation/advancingFrontAMI/advancingFrontAMI.C at line 132
    5760 source faces but no target faces
AMI: Patch source sum(weights) min:0 max:0 average:0
AMI: Patch target sum(weights) min:0 max:0 average:0
AMI: Creating addressing and weights between 10800 source faces and 10800 target faces
--> FOAM Warning : 
    From void Foam::advancingFrontAMI::checkPatches() const
    in file AMIInterpolation/AMIInterpolation/advancingFrontAMI/advancingFrontAMI.C at line 71
    Source and target patch bounding boxes are not similar
    source box span     : (80 0 240)
    target box span     : (-2e+150 -2e+150 -2e+150)
    source box          : (-40 -40 -120) (40 -40 120)
    target box          : (1e+150 1e+150 1e+150) (-1e+150 -1e+150 -1e+150)
    inflated target box : (8.26795e+149 8.26795e+149 8.26795e+149) (-8.26795e+149 -8.26795e+149 -8.26795e+149)
--> FOAM Warning : 
    From bool Foam::advancingFrontAMI::initialiseWalk(Foam::label&, Foam::label&)
    in file AMIInterpolation/AMIInterpolation/advancingFrontAMI/advancingFrontAMI.C at line 132
    5760 source faces but no target faces
AMI: Patch source sum(weights) min:0 max:0 average:0
AMI: Patch target sum(weights) min:0 max:0 average:0

I think I'm missing something because geometry isn't complicate for cyclicAMI.

For quick look Allrun script

runApplication blockMesh
runApplication snappyHexMesh -overwrite
runApplication createPatch -overwrite

runApplication decomposePar
runParallel $(getApplication)
runApplication reconstructPar

Threads used as reference
Error on decomposePar with cyclicAMI
Problems using reconstructPar on a case involving AMI

I'm open any advice.
Kind Regards,
Said.

[TurbulatorTobi]

Hello Said,

You need to change the sign of the separationVector in your createPatchDict. The separationVector is one of the things that ist defined differently depending on the variant and version of OpenFOAM.

You can see this in the warning. The source box is the given patch and the target box the transformed neighbourPatch. So the target box should have the same values as the source box. In the first warning the x-coordinates are 80 above the values of the neighbourPatch leading to 120. So changing the sign of the separationVector will lead to the correct values.

[saidc.]

Originally Posted by TurbulatorTobi

Hello Said,

You need to change the sign of the separationVector in your createPatchDict. The separationVector is one of the things that ist defined differently depending on the variant and version of OpenFOAM.

You can see this in the warning. The source box is the given patch and the target box the transformed neighbourPatch. So the target box should have the same values as the source box. In the first warning the x-coordinates are 80 above the values of the neighbourPatch leading to 120. So changing the sign of the separationVector will lead to the correct values.

Hi Tobias,
I tried your advice and it worked well for me. As you said I just change the sign of the separationVector. Thanks a lot for your reply.

Kind Regards,
Said.

[sinatahmooresi]

Originally Posted by TurbulatorTobi

Hello Said,

You need to change the sign of the separationVector in your createPatchDict. The separationVector is one of the things that ist defined differently depending on the variant and version of OpenFOAM.

You can see this in the warning. The source box is the given patch and the target box the transformed neighbourPatch. So the target box should have the same values as the source box. In the first warning the x-coordinates are 80 above the values of the neighbourPatch leading to 120. So changing the sign of the separationVector will lead to the correct values.

Hello Tobias,

I am not able to find a certain clear definition for separationVector. I am trying to make a fully developed flow in a nozzle before it exits the outlet into a tank. I want to simulate the nozzle with cyclic boundary condition and get the error as discussed above. How one can determine the separationVector for each case?



Thanks,

Sina