|
[Sponsors] |
[mesh manipulation] "moveDynamicMesh -checkAMI" problem |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
October 30, 2014, 08:04 |
"moveDynamicMesh -checkAMI" problem
|
#1 |
Member
chen long
Join Date: Dec 2012
Posts: 32
Rep Power: 13 |
Hi Foamers
I try to use OF 2.3.0 the tutorial file propeller to simulate the flow around tidal turbine. When I try to type moveDynamicMesh-checkAMI It shows Code:
--> FOAM FATAL ERROR: request for volVectorField U from objectRegistry region0 failed available objects of type volVectorField are 0() From function objectRegistry::lookupObject<Type>(const word&) const in file /home/opencfd/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198. FOAM aborting #0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::error::abort() in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libdynamicFvMesh.so" #3 Foam::Q::execute() in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libutilityFunctionObjects.so" #4 Foam::OutputFilterFunctionObject<Foam::Q>::execute(bool) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libutilityFunctionObjects.so" #5 Foam::functionObjectList::execute(bool) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #6 Foam::Time::run() const in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #7 Foam::Time::loop() in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #8 in "/opt/openfoam230/platforms/linux64GccDPOpt/bin/moveDynamicMesh" #9 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #10 in "/opt/openfoam230/platforms/linux64GccDPOpt/bin/moveDynamicMesh" Aborted (core dumped) |
|
November 1, 2014, 14:21 |
|
#2 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128 |
Quick answer: The "U" field is not loaded automatically when using the mesh-only solver moveDynamicMesh. You can try using the function object "readFields" to forcefully load the "U" file: http://openfoamwiki.net/index.php/Ti...loading_fields - section "3.3 Force loading fields"
|
|
November 3, 2014, 03:22 |
|
#3 |
Member
chen long
Join Date: Dec 2012
Posts: 32
Rep Power: 13 |
Hi Bruno Santos
Thanks for you reprly. However, my of is 2.3.0. and the readfield is a separate file under system.The error remains. |
|
November 17, 2014, 15:47 |
|
#4 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128 |
Hi Jackie Chen,
Sorry for the late reply, but I finally managed to give a quick look into this. The tutorial "incompressible/pimpleDyMFoam/propeller" has in its "system/controlDict" these lines: Code:
functions { #include "readFields" #include "Q" #include "surfaces" #include "forces" } I looked better into the error output you got and it states that it was in fact the "Q" utility function that crashed. In addition, the script "Allrun.pre" has these lines near the end: Code:
# - create the inlet/outlet and AMI patches runApplication createPatch -overwrite # - test by running moveDynamicMes #runApplication moveDynamicMesh -checkAMI # - set the initial fields cp -rf 0.org 0 It takes too long to generate this mesh in my machine, so I haven't tried this yet, but my suggestion is that you place the call for moveDynamicMesh to after the copy is made, namely: Code:
# - create the inlet/outlet and AMI patches runApplication createPatch -overwrite # - set the initial fields cp -rf 0.org 0 # - test by running moveDynamicMesh runApplication moveDynamicMesh -checkAMI ----------------- edit: OK, the mesh is now finished generating and I still got the same crash. I managed to get it working if I comment out the line for "Q" in "system/controlDict", namely: Code:
functions { #include "readFields" // #include "Q" #include "surfaces" #include "forces" } Best regards, Bruno Last edited by wyldckat; November 17, 2014 at 15:54. Reason: see "edit:" |
|
August 12, 2015, 21:46 |
|
#5 | ||
Member
Werner
Join Date: Jul 2015
Location: West Lafayette, USA
Posts: 34
Rep Power: 10 |
Hi Bruno,
Thanks for your help, I commented the line for Q and the program seemed to work for the first 10 timesteps (0.1 to 1) but crashed at 1 , at the first writing time with this error: Quote:
Quote:
regards, Werner |
|||
August 13, 2015, 07:50 |
|
#6 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128 |
Quick answer: You will have to comment out the "surfaces" entry as well:
Code:
functions { #include "readFields" // #include "Q" // #include "surfaces" #include "forces" } |
|
August 13, 2015, 13:41 |
Understanding issue with velocity U.
|
#7 | |
Member
Werner
Join Date: Jul 2015
Location: West Lafayette, USA
Posts: 34
Rep Power: 10 |
Thank you Bruno !
Once more that made it work Could you explain what we disabled there disabling Q and Surfaces ? In each step I could read "Did not find volVectorField U Not updating Uboundary conditions." Is there any way of solving this ? I think that solving this would be useful becuase when I run the application pimpleDyMFoam a get a floating point exception related to division by 0 in the process of reading speed U. I paste here the error ... I apreciate very much your help Quote:
|
||
August 13, 2015, 14:04 |
|
#8 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128 |
Quick answer:
|
|
August 13, 2015, 15:00 |
|
#9 |
Member
Werner
Join Date: Jul 2015
Location: West Lafayette, USA
Posts: 34
Rep Power: 10 |
Hi Bruno,
1. Ok! yeah, you're right , with a speed of 158 rad/s the turbine rotated 90 degrees between each step. Now I set the deltaT to 0.001 for 9 degrees between each step, is that fine. I'm still getting the FPE (Floating point exception). Do you know a current post where I can get further advise for this issue ? 2. In that sense should we enable Q and Surfaces to get the full results when we run the solver ? |
|
August 13, 2015, 15:35 |
|
#10 | |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128 |
Quick answers:
Quote:
I can't remember any specific threads on this topic. I believe those two entries are mostly demonstrations of features that OpenFOAM provides for co-processing which the solver is running, i.e. post-processing on-the-fly.
__________________
|
||
August 13, 2015, 16:05 |
|
#11 |
Member
Werner
Join Date: Jul 2015
Location: West Lafayette, USA
Posts: 34
Rep Power: 10 |
Hi Bruno,
I set deltaT to 1e-5 , as it was in the propeller tutorial, and the issue was solved :P Thanks a lot once more |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[Other] engineFoam new mesh problem | ayhan515 | OpenFOAM Meshing & Mesh Conversion | 5 | August 10, 2015 08:45 |
UDF compiling problem | Wouter | Fluent UDF and Scheme Programming | 6 | June 6, 2012 04:43 |
Gambit - meshing over airfoil wrapping (?) problem | JFDC | FLUENT | 1 | July 11, 2011 05:59 |
natural convection problem for a CHT problem | Se-Hee | CFX | 2 | June 10, 2007 06:29 |
Adiabatic and Rotating wall (Convection problem) | ParodDav | CFX | 5 | April 29, 2007 19:13 |