Wall-resolved RANS with interFoam
5 Attachment(s)
Hi All,
TLDR: When I run RANS with interFoam and k-omega SST and a wall-resolved grid I get terrible problems at the free surface which leads to divergence in most cases. How to get past this? Usually when I run calculations of ship flows I use wall functions due to high Re and never had any issues (well, I had plenty but not like this). Recently I wanted to benchmark my set-up in OpenFOAM 3.0 on a 1 m long Wigley hull and could not justify using a wall function at Re under 1 million. That's when issues started. I meshed the case both using snappyHexMesh and Pointwise (structured hexahedral) with y+<1 and used standard low-Re BC's (fixedValue nut 0, fixedValue k 0, omegaWallFunction). I have used very similar, wall-resolved grids with interPhaseChangeFoam (as well as simple/piso/pimpleFoam) and never had any issues but for this particular case I get very bad smearing at the interface which leads to non-physical results and most cases diverge. I ran the snappy case with nutUSpaldingWallFunction as is and re-meshed the Pointwise grid with y+ 50 and switched on the wall function, both worked very well and gave good results. I then tried modifying the low-Re cases by switching on interface compression, adding surface tension and changing BCs to avoid using the variableHeightFlowRate and outletPhaseMeanVelocity outlet BCs but the results stayed the same. I checked the mesh quality and in both cases it's fine. The allTopology allGeometry option reports some bad quality tet faces and undetermined cells but these are pretty much the same for the grid with wall function so I don't see why they would make the difference. I've attached the case set-up below and will appreciate any hints. Cheers, Artur Pointwise case with y+<1: https://www.dropbox.com/s/hsfc6ukvhe...igley.zip?dl=0 Pointwise y+ 1 checkMesh -allTopology -allGeometry: Code:
Mesh stats Code:
solvers Code:
ddtSchemes Attachment 49915 Attachment 49916 Attachment 49917 Attachment 49918 |
Hi Artur, have you made progress on this?
To my knowledge the interface compression scheme should cause trouble when using high aspect ratio cells at the interface. That means increasing the cell number in longitudinal direction may help, if you still need to fully resolve boundary layers. Anyway, what about the 2 mesh errors that you posted? Are these from the pointwise mesh? /Stefan |
Hi,
Thanks for the reply. I haven't resolved the issue yet because this is a side project and I had to put it on halt for a while due to other commitments. The mesh errors are from the Pointwise mesh, yes, but they only appear when you use the -allGeometry option. I see them on most of my grids and never had any issues (the low determinant is a different symptom of the high aspect ratio as far as I understand). I tried increasing the number of cells along the waterline but I'll try to push it a bit more. My thoughts were also that the interface compression scheme would cause issues in this situation hence I ran a few cases without it but it didn't make much of a difference. If you have any other comments they'll be most welcome :) All the best A |
Solved
2 Attachment(s)
To anyone who's interested, here's the solution:
Following Stefan's suggestion, I switched off the interface compression in fvSolution by setting Code:
cAlpha 0; Happy foaming A |
All times are GMT -4. The time now is 09:51. |