View Issue Details
|ID||Project||Category||View Status||Date Submitted||Last Update|
|0001379||OpenFOAM||[All Projects] Bug||public||2014-08-22 09:08||2015-03-17 22:46|
|Fixed in Version|
|Summary||0001379: Weird artificial flow in twoPhaseEulerFoam|
|Description||In a stagnant simulation case of an air loop reactor an artificial flow forms when the domain has an inclined bottom.|
|Steps To Reproduce||Mesh and run the attached to cases and compare results. The setup of the two cases is equal except for the mesh. One case has a flat bottom and the bottom of the other case is chamfered.|
|Tags||No tags attached.|
StagnantAirLift.tar.gz (75,850 bytes)
StagnantBubbleColumn_curvedBottom.tar.gz (3,418 bytes)
I created an even simpler test case, see the file StagnantBubbleColumn_curvedBottom.tar.gz. I took the injection tutorial case from the twoPhaseEulerFoam tutorials, removed the file fvOptions and added this lines to blockMeshDict:
arc 0 1 (0.075 -0.025 0.0)
arc 4 5 (0.075 -0.025 0.1)
Now the 2D bubble column has a curved bottom. If you run the case, you will see strange things are happening.
As the fvOptions are removed, there are no sources. Only gravity is acting and nothing should happen.
However, a strong circulation develops.
|I observed basically the same problem. See http://www.cfd-online.com/Forums/openfoam-solving/148146-bad-momentum-source-vortice-direction-twophaseeulerfoam-non-ortho-meshes.html for a full description!|
@projectionist, Im interested into this,and I try to figure it out but failed.
BTW, I downloaded ur curveBottom case, I saw the dispersed phase's initial value is 0.293239, is this value getting down during in your simulation?
I have twoPhaseEulerFoam running with a p_rgh formulation consistent with the way this is done in interFoam and compressibleInterFoam which completely removes the spurious currents in the lower part of the vessel but surface currents remain. The issue is that subtracting the hydrostatic part of the pressure only solves the problem of the interaction between the buoyancy force and non-orthogonality in regions of uniform density; at the interface the density gradient is VERY large and the forces do not achieve an equilibrium.
I have a few more test to do before pushing this change but the likelyhood is that if you need cases with a free-surface to converge to 0 flow at least the mesh surrounding the surface will need to be orthogonal.
Resolved by commit 50b2edbedc4c36390d6cfccbf295b840990cc4da
in OpenFOAM-dev: https://github.com/OpenFOAM/OpenFOAM-dev
|2014-08-22 09:08||projectionist||New Issue|
|2014-08-22 09:08||projectionist||File Added: StagnantAirLift.tar.gz|
|2014-09-09 09:01||projectionist||File Added: StagnantBubbleColumn_curvedBottom.tar.gz|
|2014-09-09 09:09||projectionist||Note Added: 0003228|
||Note Added: 0003689|
|2015-02-11 04:50||sharonyue||Note Added: 0003747|
|2015-03-11 14:32||henry||Note Added: 0004084|
|2015-03-17 22:46||henry||Note Added: 0004148|
|2015-03-17 22:46||henry||Status||new => resolved|
|2015-03-17 22:46||henry||Resolution||open => fixed|
|2015-03-17 22:46||henry||Assigned To||=> henry|
|2015-03-24 00:17||liuhuafei||Issue cloned: 0001602|