View Issue Details

IDProjectCategoryView StatusLast Update
0001106OpenFOAM[All Projects] Bugpublic2015-05-01 16:47
ReporterfeymarkAssigned Tohenry 
PriorityhighSeveritymajorReproducibilityalways
Status resolvedResolutionfixed 
PlatformArch LinuxOSOS Version
Product Version 
Fixed in Version 
Summary0001106: meshPhi not written
DescriptionmeshPhi doesn't get written during pimpleDyMFoam run creating big pressure jumps when restarting simulation.
Steps To ReproduceRun movingCone tutorial, analyse the data and use common sense.
Additional InformationIf this is not a bug then please explain to me why there should be a pressure jump from -7 to -9, in the first time step, when restarting without meshPhi.
TagsNo tags attached.

Activities

feymark

2013-12-10 12:47

reporter  

henry.zip (683,022 bytes)

henry

2013-12-10 13:06

manager   ~0002678

Have you changed the code to dump and read meshPhi? What difference do you see by doing this? I see no need to dump and read meshPhi when running with first-order in time.

feymark

2013-12-10 13:19

reporter   ~0002679

Look at the two cases I have attached, they are exactly the same apart from the meshPhi file. Run them with your pimpleDyMFoam, it will run for one time step starting from t=0.0002. Open up ParaView and see the difference between the two cases at t=0.000205. The pressure field for the case with meshPhi is more or less the same as at t=0.0002. The case without meshPhi, however, exhibits a pressure drop from -7 to -9.

feymark

2013-12-10 13:23

reporter   ~0002680

This of course confirms that meshPhi is read when present.

henry

2013-12-10 13:54

manager   ~0002681

Thanks for the details. The problem with using meshPhi from the previous time-step is that it needs to be mapped following tompology change. To avoid this I have been changing the solvers to operate on intensive properties only thus avoiding the need to read and write meshPhi. This new approach is much more general and reliable and will be used in all the "DyM" solvers in the next release. Some of the changes for topology change have been back-ported to OpenFOAM-2.2.x which is why meshPhi is not written but not all the changes to support this -- appologies for confusion and the bug.

I will revert the fvMesh code in OpenFOAM-2.2.x to write meshPhi again which will be sufficient for mesh-morphing cases but is not ideal for topology change. All this will be fixed in the next release.

henry

2013-12-10 15:06

manager   ~0002683

Resolved by commit cde97091ebaba91cbb15d57da65793c4d30d6a17

Issue History

Date Modified Username Field Change
2013-12-10 12:47 feymark New Issue
2013-12-10 12:47 feymark File Added: henry.zip
2013-12-10 13:06 henry Note Added: 0002678
2013-12-10 13:19 feymark Note Added: 0002679
2013-12-10 13:23 feymark Note Added: 0002680
2013-12-10 13:54 henry Note Added: 0002681
2013-12-10 15:06 henry Note Added: 0002683
2013-12-10 15:06 henry Status new => resolved
2013-12-10 15:06 henry Resolution open => fixed
2013-12-10 15:06 henry Assigned To => henry