|
[Sponsors] |
foam-extend lacking rhoCentralDyMFoam - what to do? I need ggi BC |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
November 27, 2018, 03:55 |
foam-extend lacking rhoCentralDyMFoam - what to do? I need ggi BC
|
#1 |
Member
Martin
Join Date: Aug 2018
Posts: 33
Rep Power: 8 |
I want to use density-based solver to solve rotating case (turbomachinery) so I chose solver rhoCentralDyMFoam. I successfully ran the simulation and it took 25 hours on 1 core. Geometry is periodic so now I want to simulate only one period of it. I tried with cyclicAMI boundary condition on periodic patches, but it didn't work.
Looks like I need to use ggi, I mean cyclicGgi BC. The problem is that original Openfoam doesn't have ggi BCs so I installed foam-extend - but this one lacks rhoCentralDyMFoam, it only has rhoCentralFoam. I tried to use rhoCentralFoam with dynamicMeshDict but it didn't work. Is there any possibility to use rhoCentralDyMFoam with ggi BCs? What else can I do? |
|
December 11, 2018, 16:26 |
|
#2 |
Senior Member
Peter Baskovich
Join Date: Jul 2014
Posts: 127
Rep Power: 12 |
Let's jump back to your original case with rhoCentralDyMFoam on "original openfoam".
I think we can fix the cyclicAMI. Can you share more information? If the case is not secret and isn't too big, can you archive the whole thing and share it. Otherwise can you share the 0 and system folders and the boundary file from constant. A diagram or dimensioned drawing of the geometry/mesh would also be super useful. Also please let us know exactly which version you are running -Peter |
|
December 18, 2018, 09:34 |
|
#3 | |
Member
Martin
Join Date: Aug 2018
Posts: 33
Rep Power: 8 |
Quote:
So there are 3 cellZones, the main one is called rotor, it is rotating in the middle of other two zones which are stationary. I did "createPatch" successfully so I have some cyclic patches which are correctly linked (I need cyclic because mesh is just one period (1/7) of impeller). I also have 2 pairs of cyclicAMI patches - one pair is located where "inlet zone" is connected to rotor and another pair where rotor is connected to "outlet zone". If you look at the file "boundary", cyclicAMI patches are at the bottom and there is this setting: Code:
transform noOrdering; The original setting I had was Code:
transform rotational; If you want to see the mesh in Paraview, you need to rename folder 0 to 0_, otherwise Paraview crashes. Attaching picture of mesh and picture of second cyclicAMI pair. As you can see, faces are not exactly the same, number of faces is slightly different as well, but patches are similar enough for AMI to work, in my opinion. |
||
December 19, 2018, 04:13 |
cyclicRepeatAMI !!
|
#4 |
Member
Martin
Join Date: Aug 2018
Posts: 33
Rep Power: 8 |
Apparently cyclicAMI boundary condition does not support transient simulation of cyclic (periodic) geometries. It lacks ability to connect faces from one side of geometry to faces on other side. This was implemented only recently in Openfoam 6 with new type of BC - cyclicRepeatAMI. More info about it: https://github.com/OpenFOAM/OpenFOAM...29439fac374a60
Now my case finally runs past that time 3.2e-6 Edit: If you want to run my case, change U/massFlowRate to 0.005 (0.035 is appropriate for whole 360° geometry, so 0.005 for 1/7 period) and dynamicMeshDict/omega to 4294 (41000 RPM) |
|
Tags |
foam-extend, foam-extend-4.0, ggi, rhocentraldymfoam, rhocentralfoam |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
error with reactingFoam | BakedAlmonds | OpenFOAM Running, Solving & CFD | 4 | June 22, 2016 03:21 |
[blockMesh] error message with modeling a cube with a hold at the center | hsingtzu | OpenFOAM Meshing & Mesh Conversion | 2 | March 14, 2012 10:56 |
[blockMesh] BlockMesh FOAM warning | gaottino | OpenFOAM Meshing & Mesh Conversion | 7 | July 19, 2010 15:11 |
[blockMesh] Axisymmetrical mesh | Rasmus Gjesing (Gjesing) | OpenFOAM Meshing & Mesh Conversion | 10 | April 2, 2007 15:00 |
[Gmsh] Import gmsh msh to Foam | adorean | OpenFOAM Meshing & Mesh Conversion | 24 | April 27, 2005 09:19 |