|
[Sponsors] |
[blockMesh] Floating Point Exception while generating wedge based mesh |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
June 30, 2021, 07:21 |
Floating Point Exception while generating wedge based mesh
|
#1 |
New Member
Jonas Vogler
Join Date: Jun 2021
Posts: 5
Rep Power: 5 |
Dear Folks,
I have absolutely no clue as to what's wrong here, thus I'm not sure if my issue is actually related to the meshing process or if it is a more generic problem. I'll just try to give you the information I think may be neccessary in order to find the root cause of my issues, so please bear with me. I'm working a project as part of a CFD course at university. I'm trying to model natural convection in a cylinder which is heated at the bottom (const. heat flux of 40 kW/mē) but otherwise has adiabatic walls.Initially the cylinder is filled with 20 L of water at 300 K. I'm also using Boussinesq approximation for the buoyancy effects. The OpenFOAM release I'm working with is 8.20201114-1 (openfoam.org) In order to solve this in a reasonable time I'm using a wedge of 10° (I know it's probably a bit large, but that's not the culprit). I followed https://cfd.direct/openfoam/user-guide/v8-blockMesh/ to setup the vertices etc. So everything basically went well, mesh generation, solving with (buoyantPimpleFOAM), only the results weren't exactly physical and also didn't match too well the reference calculations conducted with Ansys Fluent. Anyway that's how I know the blockMeshDict follows the syntax and topology etc. One of the options I came up with was using buoyantBoussinesqPimpleFoam (the incompressible version of buoyantPimpleFoam as far as I understand things, which I deemed to be better suited for this case anyway) which is only available in the openfoam.com version, so I went ahead and tried to install that. Installing that from source actually worked kind of even though the linker reported some errors. Anyway the mesh generation using blockMesh (com version) failed which is why I was unable to start solving anything. As both versions org and com are not available for my distro (Arch Linux) my tutor suggested to go with a docker image. Same behaviour. I tried to go back to openfoam-org v8 which at least generated a proper mesh before but now that's no longer working as well and which is where I finally get to the point of this post. I hope you're still with me. So my blockMeshDict is: Code:
*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 8 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object blockMeshDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // convertToMeters 1; // all values given in m // I understand thats "scale" in .comVersion // geometry parameters V 20.0; // Volume in l V #calc "$V * 1e-3"; // convert to SI units dhRatio 2.335; // diameter-to-height ratio // spatial discreization dr 2.0e-3; // spacial step size in radial direction in mm dz $dr; // spacial step size in axial direction in mm pi #calc "acos(-1.0)"; // PI angle 5.0; // angle in degrees (10 degree wedge means +-5° from neutral plane angleRad #calc "$angle * $pi / 180.0"; // angle in radians // calculate diameter and height from volume an D/H-ratio D #calc "pow(4 * $V / $pi * $dhRatio, 1.0/3.0)"; // diameter in m R #calc "$D / 2.0"; // radius in m H #calc "$D / $dhRatio"; // height in m // Cell counts Nr #calc "round($R / $dr)"; // Number of cells in radial direction Nz #calc "round($H / $dz)"; // Number of cells in z-direction (i.e. top to bot) // domain boundaries xMin 0; xMax #calc "$R * cos($angleRad)"; yMax #calc "$R * sin($angleRad)"; yMin #calc "$R * sin($angleRad) * -1.0"; vertices ( ($xMin $xMin $xMin) // 0,A ($xMax $yMin $xMin) // 1,B ($xMax $yMax $xMin) // 2,C ($xMin $xMin $H) // 3,D ($xMax $yMin $H) // 4,E ($xMax $yMax $H) // 5,F ); blocks ( hex (0 1 2 0 3 4 5 3) ($Nr 1 $Nz) simpleGrading (1 1 1) ); edges ( arc 1 2 (92.67 0 0) arc 4 5 (92.67 0 370.67) ); boundary ( wall { // cylinder outer wall type wall; faces ( (1 2 4 5) ); } // end wall top { // top type wall; faces ( (3 4 5 3) ); }; // end top bottom { // top type wall; faces ( (0 1 2 0) ); }; // end top front { // face pointing clockwise around z-axis type wedge; faces ( (0 1 4 3) ); } // end front back { // face pointing counterclockwise around z-axis type wedge; faces ( (0 2 5 3) ); } // end front axis { // face pointing counterclockwise type empty; faces ( (0 3 3 0) ); } // end front ); Code:
/*---------------------------------------------------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 8 \\/ M anipulation | \*---------------------------------------------------------------------------*/ Build : 8-15ae41985af0 Exec : checkMesh Date : Jun 30 2021 Time : 12:02:41 Host : "Arch" PID : 65248 I/O : uncollated Case : /home/jonas/Studium/tuw/2021S/CFD/Projekt/simulation/validationCase300K_leastSquares nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10) allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh for time = 0 Time = 0 Mesh stats points: 16745 internal points: 0 faces: 33026 internal faces: 16282 cells: 8232 faces per cell: 5.9898 boundary patches: 6 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 8148 prisms: 84 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 0 polyhedra: 0 Checking topology... Boundary definition OK. Cell to face addressing OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces... Patch Faces Points Surface topology wall 84 170 ok (non-closed singly connected) top 98 197 ok (non-closed singly connected) bottom 98 197 ok (non-closed singly connected) front 8232 8415 ok (non-closed singly connected) back 8232 8415 ok (non-closed singly connected) axis 0 0 ok (empty) Checking geometry... Overall domain bounding box (0 -0.0170089 0) (0.194412 0.0170089 0.167156) Mesh has 2 geometric (non-empty/wedge) directions (1 0 1) Mesh has 3 solution (non-empty) directions (1 1 1) Wedge front with angle 5.00002 degrees Wedge back with angle 5.00002 degrees All edges aligned with or perpendicular to non-empty directions. Boundary openness (1.02257e-14 -5.18071e-15 -7.09525e-18) OK. Max cell openness = 3.06561e-16 OK. Max aspect ratio = 2.00621 OK. Minimum face area = 3.44308e-07. Maximum face area = 6.76938e-05. Face area magnitudes OK. Min volume = 6.85157e-10. Max volume = 1.33606e-07. Total volume = 0.00055274. Cell volumes OK. Mesh non-orthogonality Max: 0 average: 0 Non-orthogonality check OK. Face pyramids OK. Max skewness = 0.323205 OK. Coupled point location match (average 0) OK. Mesh OK. End Code:
/*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: v2012 | | \\ / A nd | Website: www.openfoam.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : _7bdb509494-20201222 OPENFOAM=2012 Arch : "LSB;label=32;scalar=64" Exec : checkMesh Date : Jun 30 2021 Time : 12:05:26 Host : DESKTOP-JD8R1M6 PID : 2799 I/O : uncollated Case : /home/jonas/sim/testMesh nProcs : 1 trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20) allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Time = 0 Mesh stats points: 16830 internal points: 0 faces: 33110 internal faces: 16282 cells: 8232 faces per cell: 6 boundary patches: 6 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 8232 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 0 polyhedra: 0 Checking topology... Boundary definition OK. ***Total number of faces on empty patches is not divisible by the number of cells in the mesh. Hence this mesh is not 1D or 2D. Cell to face addressing OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces... Patch Faces Points Surface topology wall 84 170 ok (non-closed singly connected) top 98 198 ok (non-closed singly connected) bottom 98 198 ok (non-closed singly connected) front 8232 8415 ok (non-closed singly connected) back 8232 8415 ok (non-closed singly connected) axis 84 170 ok (non-closed singly connected) Checking faceZone topology for multiply connected surfaces... No faceZones found. Checking basic cellZone addressing... No cellZones found. Checking geometry... Overall domain bounding box (0 -0.0170088 0) (0.194412 0.0170088 0.167156) Mesh has 2 geometric (non-empty/wedge) directions (1 0 1) Mesh has 3 solution (non-empty) directions (1 1 1) Wedge front with angle 4.99999 degrees Wedge back with angle 4.99999 degrees All edges aligned with or perpendicular to non-empty directions. Boundary openness (-1.42018e-14 -2.82449e-16 1.44999e-17) OK. Max cell openness = 2.82981e-16 OK. Max aspect ratio = 2.00621 OK. ***Zero or negative face area detected. Minimum area: 0 <<Writing 84 zero area faces to set zeroAreaFaces Min volume = 6.85153e-10. Max volume = 1.33605e-07. Total volume = 0.000552737. Cell volumes OK. Mesh non-orthogonality Max: 0 average: 0 Non-orthogonality check OK. Face pyramids OK. ***Max skewness = 1.32253e+147, 84 highly skew faces detected which may impair the quality of the results <<Writing 84 skew faces to set skewFaces Coupled point location match (average 0) OK. Failed 2 mesh checks. End Code:
/*---------------------------------------------------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 8 \\/ M anipulation | \*---------------------------------------------------------------------------*/ Build : 8-15ae41985af0 Exec : blockMesh Date : Jun 30 2021 Time : 11:32:48 Host : "Arch" PID : 50013 I/O : uncollated Case : /home/jonas/Studium/tuw/2021S/CFD/Projekt/simulation/testMesh nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10) allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Creating block mesh from "system/blockMeshDict" [...] #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::sigFpe::sigHandler(int) at ??:? #2 ? in "/usr/lib/libc.so.6" #3 Foam::face::centre(Foam::Field<Foam::Vector<double> > const&) const at ??:? #4 Foam::blockDescriptor::check(Foam::Istream const&) at ??:? #5 Foam::blockDescriptor::blockDescriptor(Foam::dictionary const&, int, Foam::Field<Foam::Vector<double> > const&, Foam::PtrList<Foam::blockEdge> const&, Foam::PtrList<Foam::blockFace> const&, Foam::Istream&) at ??:? #6 Foam::block::block(Foam::dictionary const&, int, Foam::Field<Foam::Vector<double> > const&, Foam::PtrList<Foam::blockEdge> const&, Foam::PtrList<Foam::blockFace> const&, Foam::Istream&) at ??:? #7 Foam::block::New(Foam::dictionary const&, int, Foam::Field<Foam::Vector<double> > const&, Foam::PtrList<Foam::blockEdge> const&, Foam::PtrList<Foam::blockFace> const&, Foam::Istream&) at ??:? #8 void Foam::PtrList<Foam::block>::read<Foam::block::iNew>(Foam::Istream&, Foam::block::iNew const&) at ??:? #9 Foam::blockMesh::createTopology(Foam::IOdictionary const&, Foam::word const&) at ??:? #10 Foam::blockMesh::blockMesh(Foam::IOdictionary const&, Foam::word const&) at ??:? #11 ? in "/opt/OpenFOAM/OpenFOAM-8/platforms/linux64GccDPInt32Opt/bin/blockMesh" #12 __libc_start_main in "/usr/lib/libc.so.6" #13 ? in "/opt/OpenFOAM/OpenFOAM-8/platforms/linux64GccDPInt32Opt/bin/blockMesh" [1] 50013 floating point exception (core dumped) blockMesh I don't understand why this fails after reinstallation when I didn't change the blockMeshDict at all (in fact I setup a base case and only always copy that to create a new one). Also note that I get the same behaviour runnun blockMesh on two tutorial cases "freePiston" and "DLR_A_LTS" which also use wedge geometries so I think my blockMeshDict is fine but I have a more serious issue here. Please if you need more info I'm happy to provide it. I hope you made it this far anyway so any help is much appreciated as this is a bit beyond me... Best regards Jonas |
|
July 1, 2021, 15:25 |
|
#2 |
New Member
Jonas Vogler
Join Date: Jun 2021
Posts: 5
Rep Power: 5 |
Okay so after I've grown a some fresh grey hair I figured out that the solver buoyantBoussinesqPimpleFoam doesn't let me specify externalWallheatFlux BC so it's unusable for me anyway.
The remaining issue I'd like to be able to resolve is the floating point exception when running blockMeshDict. |
|
July 2, 2021, 12:44 |
|
#3 |
Senior Member
Herpes Free Engineer
Join Date: Sep 2019
Location: The Home Under The Ground with the Lost Boys
Posts: 931
Rep Power: 13 |
couldn't reproduce the issue with v2106.
might be useful to report the issue into .org bug tracker.
__________________
The OpenFOAM community is the biggest contributor to OpenFOAM: User guide/Wiki-1/Wiki-2/Code guide/Code Wiki/Journal Nilsson/Guerrero/Holzinger/Holzmann/Nagy/Santos/Nozaki/Jasak/Primer Governance Bugs/Features: OpenFOAM (ESI-OpenCFD-Trademark) Bugs/Features: FOAM-Extend (Wikki-FSB) Bugs: OpenFOAM.org How to create a MWE New: Forkable OpenFOAM mirror |
|
July 2, 2021, 12:57 |
|
#4 | |
New Member
Jonas Vogler
Join Date: Jun 2021
Posts: 5
Rep Power: 5 |
Quote:
May I ask, did you check the mesh? i.e. did it produce prisms for you at the axis? as you are on v2106. Anyway thanks for looking at it. I'm reluctant to file a bug report because as mentioned the blockMeshDict used to compile just fine but after reinstalling .org version I got the fpe so I thought it hast to have sth to do with my system setup rather than OF itself. But I'll reconsider this and may setup a proper reproducable case in order to file a bug report. Thanks. |
||
July 2, 2021, 18:52 |
|
#5 |
Senior Member
Herpes Free Engineer
Join Date: Sep 2019
Location: The Home Under The Ground with the Lost Boys
Posts: 931
Rep Power: 13 |
no, I haven't checked the mesh. But checking in terms of what?
__________________
The OpenFOAM community is the biggest contributor to OpenFOAM: User guide/Wiki-1/Wiki-2/Code guide/Code Wiki/Journal Nilsson/Guerrero/Holzinger/Holzmann/Nagy/Santos/Nozaki/Jasak/Primer Governance Bugs/Features: OpenFOAM (ESI-OpenCFD-Trademark) Bugs/Features: FOAM-Extend (Wikki-FSB) Bugs: OpenFOAM.org How to create a MWE New: Forkable OpenFOAM mirror |
|
July 2, 2021, 21:02 |
|
#6 |
Senior Member
Claudio Boezio
Join Date: May 2020
Location: Europe
Posts: 137
Rep Power: 7 |
Hello Jonas,
I tried your blockMeshDict in OF v8 and it works without errors, I've noticed a few things though. Code:
scale 1; The edges of type arc are superfluous if in your y-direction the cell density is only 1, because the edge of a single cell is straight anyway. I tried entering a density of 10 and got an odd looking block: I then changed the arc definition as follows: Code:
edges ( //arc 1 2 (92.67 0 0) //arc 4 5 (92.67 0 370.67) arc 1 2 ($R 0 0) arc 4 5 ($R 0 $H) ); Then I've noticed that the vertex ordering in two faces, bottom and back, had wrong ordering, although blockMesh didn't complain about it. To make definition of faces easier and less prone to errors, there's a simpler way I discovered in one of the blockMesh tutorial cases. Faces for patches can be defined either with a list of vertices, ordered counterclockwise for the face normal pointing outward (right thumb rule), or, by the block name and face number. For the latter blockMesh takes care of correct vertex ordering. So in your case, give the block a name: Code:
blocks ( name Wedge hex (0 1 2 0 3 4 5 3) ($Nr 1 $Nz) simpleGrading (1 1 1) ); Code:
boundary ( wall { // cylinder outer wall type wall; faces ( (Wedge 1) ); } // end wall top { // top type wall; faces ( (Wedge 5) ); }; // end top bottom { // top type wall; faces ( (Wedge 4) ); }; // end top front { // face pointing clockwise around z-axis type wedge; faces ( (Wedge 2) ); } // end front back { // face pointing counterclockwise around z-axis type wedge; faces ( (Wedge 3) ); } // end front axis { // face pointing counterclockwise type empty; faces ( (Wedge 0) ); } // end front ); |
|
July 6, 2021, 14:50 |
|
#7 |
New Member
Jonas Vogler
Join Date: Jun 2021
Posts: 5
Rep Power: 5 |
The .com version of blockMesh does not produce prisms at the axis but highly skewed hex blocks whereas the .org version correctly implements prisms at the axis. So my question was if you also recognized this. |
|
July 6, 2021, 14:54 |
|
#8 | |
New Member
Jonas Vogler
Join Date: Jun 2021
Posts: 5
Rep Power: 5 |
Quote:
Hey Ship Designer, First of all thanks for your dedicated answer. The naming of the block really makes the syntax much more readable. I wasn't really aware of how to use this properly. As for my OpenFOAM v8 installation, I've got a feeling that I messed up with some systemwide installed libraries during the process of compiling installing uninstalling etc so I'm kinda stuck with the docker image for now Best regards, Jonas |
||
July 6, 2021, 18:46 |
|
#9 | |
Senior Member
Mark Olesen
Join Date: Mar 2009
Location: https://olesenm.github.io/
Posts: 1,714
Rep Power: 40 |
Quote:
You may want the older merge points instead of topological merge if you indeed have wedge geometries. Can specify in the blockMeshDict or as a blockMesh option (see blockMesh -help-full). |
||
July 8, 2021, 06:36 |
|
#10 | |
Senior Member
Mark Olesen
Join Date: Mar 2009
Location: https://olesenm.github.io/
Posts: 1,714
Rep Power: 40 |
Quote:
This precedes the refactoring of blockMesh as a library: https://github.com/olesenm/OpenFOAM-...47100e83f77a52 which was largely done in ramp-up for adding a paraview module to display blockMesh layouts: https://github.com/olesenm/OpenFOAM-...b9c370adf38aee |
||
Tags |
blockmeshdict, fpe, openfoam v8 |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
icoFoam - Floating point exception (core dumped) | File | OpenFOAM Running, Solving & CFD | 26 | March 6, 2021 05:26 |
[ANSYS Meshing] can floating point exception correspond to bad mesh quality? | Red Ember | ANSYS Meshing & Geometry | 3 | July 11, 2017 04:41 |
[foam-extend.org] foam-extend 3.2 on Ubuntu 12.04, Floating point exception for tutorials | arsalan.dryi | OpenFOAM Installation | 7 | November 14, 2016 18:33 |
[blockMesh] checkMesh Floating point exception error | daniel.almeida | OpenFOAM Meshing & Mesh Conversion | 0 | July 31, 2015 15:26 |
[blockMesh] error EOF in blockMesh | Ahmed Khattab | OpenFOAM Meshing & Mesh Conversion | 7 | May 17, 2012 01:37 |