View Issue Details Jump to Notes ] Issue History ] Print ]
IDProjectCategoryView StatusDate SubmittedLast Update
0000156OpenFOAM[All Projects] Bugpublic2011-03-04 19:422011-03-04 22:50
Reporterpbryant 
Assigned Tohenry 
PrioritynormalSeverityminorReproducibilityalways
StatusclosedResolutionfixed 
PlatformLinuxOSUbuntuOS Version10.10
Product Version 
Target VersionFixed in Version 
Summary0000156: High viscosity gives wrong result in multiphase problem
DescriptionThe InterFoam solver seems to be giving the wrong answer when the viscosity is large. To demonstrate this I generated a test case called waterDrop which I uploaded as a zip file. It is essentially identical to the damBreak tutorial except that the liquid is now in a rectangular blob suspended above the ground by about 0.218 meters. At t=0 it is dropped and falls down. The expected fall time can be obtained from the usual physics formula: t = sqrt(2*h/g), which in this case is about 0.21 seconds. In the simulation I varied the viscosity of the water, not of the air. It works as expected for low viscosity, but surprisingly the fall time is found to increase when the water viscosity is increased to a large value. As uploaded, the viscosity of the "water" has been increased from 1e-6 to 1e0 and the fall time has increased to about 0.78 seconds. When further increased to 1e2 the water actually floats upwards and disappears out the atmosphere patch!
Steps To ReproduceThe viscosity nu for phase1 is set in the file constant/transportProperties. To run and generate log file, enter the commands: blockMesh, checkMesh, setFields, interFoam | tee log1.
Additional InformationI have tried adjusting most of the parameters in the fvSolution file with little success. Setting momentumPredictor to yes helps somewhat as does increasing nCorrectors but drastically increases the run time and doesn't completely fix the problem. Decreasing Courant number in the controlDict file also has some beneficial effect. I'm hoping that someone will know how to solve this problem, or else can confirm my suspicion that this is a symptom of some kind of bug in the software.
Thanks - Paul
TagsinterFoam, multiphase, viscosity
Attached Fileszip file icon waterDrop.zip [^] (8,315 bytes) 2011-03-04 19:42

- Relationships

-  Notes
(0000276)
henry (manager)
2011-03-04 22:50

Increasing the viscosity ratio increases the stiffness of the problem and in order to converge the velocity in high viscosity region which is accelerating will indeed require an increase in the number of PISO iterations: 10 to 20 are required for a liquid viscosity of 0.1. With a viscosity of 1e2 you may require hundreds of PISO iterations or it may not even converge and you may have to change to PIMPLE and apply under-relaxation, either way it would be EXTREMELY expensive and it is not at all clear that VoF would be appropriate anyway.

- Issue History
Date Modified Username Field Change
2011-03-04 19:42 pbryant New Issue
2011-03-04 19:42 pbryant File Added: waterDrop.zip
2011-03-04 19:47 pbryant Tag Attached: multiphase
2011-03-04 19:47 pbryant Tag Attached: viscosity
2011-03-04 19:47 pbryant Tag Attached: interFoam
2011-03-04 22:50 henry Note Added: 0000276
2011-03-04 22:50 henry Status new => closed
2011-03-04 22:50 henry Assigned To => henry
2011-03-04 22:50 henry Resolution open => fixed