CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

simpleFoam crashes without error messages

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 1 Post By jenc24
  • 1 Post By ufocfd

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 22, 2023, 01:18
Default simpleFoam crashes without error messages
  #1
Member
 
Giles Richardson
Join Date: Jun 2012
Location: Cambs UK
Posts: 98
Rep Power: 13
ufocfd is on a distinguished road
simpleFoam crashes (during 1st iteration) without error messages. It just stops running after the 3 momentum equation lines, and before the pressure equation, without any indication what the problem is.

The case is an MRF case using 2 zones connected with cyclicAMI interface, although the crash is probably related to a mesh error. I will have to run checkMesh again and scrutinise the output for any problems.

I had a similar issue a while back and it was related to cells not connected to the main mesh properly, or just connected by one node. I will add a reply when the problem is fixed.
ufocfd is offline   Reply With Quote

Old   March 22, 2023, 02:31
Default
  #2
New Member
 
Join Date: Nov 2022
Location: Slovenia
Posts: 10
Rep Power: 3
jenc24 is on a distinguished road
I encountered a similar issue (crash without error), when I had too large mesh and too little memory (RAM) to work with such mesh.

I don't know if this is the case with you, I just thought it might help someone.

Regards!
ufocfd likes this.
jenc24 is offline   Reply With Quote

Old   March 22, 2023, 06:29
Default
  #3
Member
 
Giles Richardson
Join Date: Jun 2012
Location: Cambs UK
Posts: 98
Rep Power: 13
ufocfd is on a distinguished road
thanks - got it running eventually...

I think the problem was because I had the wrong zone name in the MRFProperties file (it was zone1 and should have been zone0). But at the same time I remeshed both zones after removing the linkage geometry between the blades and fuselage - giving a nice clean gap, so there is no geometry on the cyclic interface. So the problem could have been caused by either of those 2 things.

I have attached some notes which is what I use to help set up an MRF case.

======================
MRF case setup for AMI
======================

requires:

-2 mesh directories
- topoSetDict (to create inner MRF and outer mesh zones)
- createPatchDict (to create cyclicAMI boundaries)
- MRFProperties (to specify the rotation)

start with cylinder, fuselage and blades geometry - cylinder is cyclic interface

generate 2 seperate case directories - 1 for inner mesh, and 1 for outer mesh

using snappyHexMesh
- move point location for inner mesh (inside cylinder)
- move point location for outer mesh (outside cylinder and fuselage in freestream)
(move both dir 2 to 0)

NOTE: check both boundary files have cyl-inner and cyl-outer as surface names

use topoSetDict to create "zone0" *** for inner mesh

use topoSetDict to create "zone1" *** for outer mesh

then go above both case directories and use mergeMeshes <dir1> <dir2>

this creates a new "1" dir in the <dir1>, so then move this "1" to "0"

can use paraview with "read zones" toggled ON, to check the inner zones.

====

use createPatch to make the cyclicAMI boundaries for cyl-inner and cyl-outer
- check that it says cyclicAMI in the createPatchDict file
- check that it has the right surface names too

then check that you have c1 aand c2 defined as cyclicAMI in boundary file

check that there are 2 cell zones in cellZones file

update the boundary files p U k omega nut with cyclicAMI (for c1 and c2)

create or modify the MRFProperties file in "constant" dir to set omega (speed)
- check you have got the right zone names
- and check right surfaces in the MRF file

run in simpleFoam as normal (fingers crossed)
jenc24 likes this.
ufocfd is offline   Reply With Quote

Old   March 22, 2023, 14:11
Default
  #4
Member
 
Giles Richardson
Join Date: Jun 2012
Location: Cambs UK
Posts: 98
Rep Power: 13
ufocfd is on a distinguished road
PS. I also found some mesh errors that needs fixing...

There were non-manifold points, which can be found by using:
foamToVTK -pointSet nonManifoldPoints

and some problem with edgefaces, when using checkMesh -allTopology
foamToVTK -faceSet edgeFaces

also some nonOrthogonalFaces on the cyclicAMI inner boundary,
foamToVTK -faceSet nonOrthoFaces !!! (cause immediate crash)

Then you can load them into Paraview and see where they are.

https://twitter.com/garcfd/status/16...345152/photo/1

(twitter image)

Last edited by ufocfd; March 23, 2023 at 14:17.
ufocfd is offline   Reply With Quote

Old   March 26, 2023, 14:36
Default
  #5
Member
 
Giles Richardson
Join Date: Jun 2012
Location: Cambs UK
Posts: 98
Rep Power: 13
ufocfd is on a distinguished road
PS. I have since learnt that its much quicker and simpler to mesh the (both inner and outer parts) at the same time and then setup without any cyclic AMI, you just add couple of lines in the snappyHexMeshDict, and then the MRF is ready to go (you don't even need to merge 2 separate meshes). The only thing you need to do is put the cellZone name (below) into the MRF properties file.

cellZone cell-inner-volume;
faceZone face-inner-volume;
mode inside;
ufocfd is offline   Reply With Quote

Reply

Tags
crash, simplefoam

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
simpleFoam crashes after a few iterations - mesh issue? NiklasH108 OpenFOAM 11 July 29, 2020 11:19
simpleFoam crashes Sean95 OpenFOAM Running, Solving & CFD 11 March 15, 2018 05:07
cyclicAMI + simpleFoam crashes in parallel jmf OpenFOAM Running, Solving & CFD 6 June 28, 2017 15:30
SimpleFoam crashes after restarting simulation fedez91 OpenFOAM Running, Solving & CFD 18 September 4, 2016 08:59
potentialFoam & simpleFoam crashes after snappyhexmesh [parallel execution] pilot320 OpenFOAM Running, Solving & CFD 10 November 12, 2015 16:56


All times are GMT -4. The time now is 06:12.