CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

cyclicAMI "bounding boxes are not similar" error

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

Like Tree1Likes
  • 1 Post By TurbulatorTobi

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 5, 2021, 17:07
Post cyclicAMI "bounding boxes are not similar" error
  #1
Member
 
Said CATALBAS
Join Date: Feb 2020
Location: Türkiye
Posts: 58
Rep Power: 4
saidc. is on a distinguished road
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.

Code:
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:

Code:
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
Code:
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.
Attached Files
File Type: zip NC_LES.zip (16.3 KB, 31 views)
File Type: txt logblockMesh.txt (2.4 KB, 4 views)
File Type: txt logsnappyHexMesh.txt (111.6 KB, 5 views)
File Type: txt logcreatePatch.txt (3.1 KB, 18 views)
File Type: txt logbuoyantPimpleFoam.txt (5.5 KB, 1 views)
saidc. is offline   Reply With Quote

Old   April 9, 2021, 16:51
Default change the sign of the separationVector
  #2
New Member
 
Tobias
Join Date: Apr 2021
Posts: 1
Rep Power: 0
TurbulatorTobi is on a distinguished road
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. likes this.
TurbulatorTobi is offline   Reply With Quote

Old   April 9, 2021, 17:08
Post
  #3
Member
 
Said CATALBAS
Join Date: Feb 2020
Location: Türkiye
Posts: 58
Rep Power: 4
saidc. is on a distinguished road
Quote:
Originally Posted by TurbulatorTobi View Post
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.

Last edited by saidc.; April 11, 2021 at 10:25.
saidc. is offline   Reply With Quote

Reply

Tags
cyclicami, natural convectin

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
DPM udf error haghshenasfard FLUENT 0 April 13, 2016 07:35
[swak4Foam] GroovyBC the dynamic cousin of funkySetFields that lives on the suburb of the mesh gschaider OpenFOAM Community Contributions 300 October 29, 2014 19:00
OpenFOAM without MPI kokizzu OpenFOAM Installation 4 May 26, 2014 10:17
Ansys Fluent 13.0 UDF compilation problem in Window XP (32 bit) Yogini Fluent UDF and Scheme Programming 7 October 3, 2012 08:24
DecomposePar links against liblamso0 with OpenMPI jens_klostermann OpenFOAM Bugs 11 June 28, 2007 18:51


All times are GMT -4. The time now is 20:59.