Hi, everyone,
I want to use
Hi, everyone,
I want to use timeVaryingMappedFixedValue for my inlet velocities and I set different velocity values for each time step for my simulation (in this case, deltaT = 0.0002 s). I created the directories in constant/boundaryData/inlet/: constant/boundaryData/inlet/points constant/boundaryData/inlet/0/U constant/boundaryData/inlet/0.0002/U constant/boundaryData/inlet/0.0004/U constant/boundaryData/inlet/0.0006/U However, when I run the case(using icoFoam and the time step is set to be 0.0004), I got the following errors: Create time Create mesh for time = 0 Reading transportProperties Reading field p Reading field U Reading/calculating face flux field phi Starting time loop Time = 0.0004 Courant Number mean: 0 max: 0.362781 10061 ( 0 0.0002 0.0004 0.0006 0.0008 0.001 0.0012 0.0014 0.0016 ... ... 3.2 ) In directory "constant/boundaryData/inlet" on patch inlet of field U in file "/vol/isdata8/FIXI-Flow/QiSUN/openfoamtest/Second/ExpeCylinder1uP9/0/U" From function findTime in file fields/fvPatchFields/derived/timeVaryingMappedFixedValue/timeVaryingMappedFixedV alueFvPatchField.C at line 470. FOAM exiting Could anyone help me ? Thank you very much in advance!! sunny |
Switch on the debug flag for t
Switch on the debug flag for the b.c: Set timeVaryingMappedFixedValue to 1 in your ~/OpenFOAM-1.4.1/controlDict.
Have a look at the source ($FOAM_SRC/finiteVolume/lnInclude/timeVaryingMappedFixedValueFvPatchField.C) to see what is happening. |
Hi,Mattijs,
Thanks for the
Hi,Mattijs,
Thanks for the reply! I am really new to this, so...can you explain a bit more how to do this?? Thanks!! Vivien |
There are several controlDict
There are several controlDict in OpenFOAM.
One is located by default in $HOME/OpenFOAM/OpenFOAM-1.4.1/.OpenFOAM-1.4.1 It contains commonly used by all solvers. You have various sections in it, the one of interrest for you would be "DebugSwitches". Set it to 1 for timeVaryingMappedFixedValue. This will force timeVaryingMappedFixedValue to be more verbose in its output, and will help debug. Then, you have a specific controlDict in every case you run, which is only use by the case it belongs to, and contain other infos, but no debugSwitches. |
Hi, John and Mattijs,
I cha
Hi, John and Mattijs,
I changed the DebugSwitches in controlDict and save the changes. But When I run the case, I did not get any more information, ie, the error is exactly the same as I posted before... Any ideas? Thanks!! vivien |
The controlDict file is first
The controlDict file is first looked for in
~/.OpenFOAM-1.4.1/controlDict and then in ~/OpenFOAM/OpenFOAM-1.4.1/.OpenFOAM-1.4.1 |
Hi, Mattijs,
do you mean th
Hi, Mattijs,
do you mean there are two controlDict I need to edit? I only find one in ~/OpenFOAM/OpenFOAM-1.4.1/.OpenFOAM-1.4.1/controlDict and I change the DebugSwitches for timeVaringMappedFixedValue to 1, but I did not see much information after I run the solver. Thanks! Vivien |
Have a look at the sources: $F
Have a look at the sources: $FOAM_SRC/finiteVolume/lnInclude/timeVaryingMappedFixedValueFvPatchField.H
It is the 'TypeName' macro which specifies the name. This is the exact name you should use in the controlDict. In your post you mention 'timeVaringMappedFixedValue' instead of 'timeVaryingMappedFixedValue'. |
Hi, Mattijs,
This is not t
Hi, Mattijs,
This is not the problem... I made a simpler case that there are only 5 time step in constant->boundaryData->inlet(which are 0 0.0002 0.0004 0.0006 0.0008), the geometry is a cylinder and contain 100 points at inlet. After I run icoFoam, I got the following errors and seems the order of files are sorted: Create time Create mesh for time = 0 Reading transportProperties Reading field p Reading field U timeVaryingMappedFixedValue : construct from dictionary timeVaryingMappedFixedValueFvPatchField : Read 100 sample points from "/openfoamtest/NewCase/constant/boundaryData/inlet/points" timeVaryingMappedFixedValueFvPatchField : Used points (0.00138321 0.00138321 0) (0.00154865 0.00111043 0) (0.00167642 0.000812023 0) to define coordinate system with normal (0 0 -1) readSamplePoints : Dumping triangulated surface to triangulation.stl readSamplePoints : Dumping face centres to "/openfoamtest/NewCase/localFaceCentres.obj" timeVaryingMappedFixedValueFvPatchField : In directory "/openfoamtest/NewCase/constant/boundaryData/inlet" found times 5 ( 0.0008 0 0.0002 0.0004 0.0006 ) --> FOAM FATAL ERROR : Cannot find starting sampling values for current time 0 Have sampling values for times 5 ( 0.0008 0 0.0002 0.0004 0.0006 ) In directory "constant/boundaryData/inlet" on patch inlet of field U in file "/openfoamtest/NewCase/0/U" From function findTime in file fields/fvPatchFields/derived/timeVaryingMappedFixedValue/timeVaryingMappedFixedV alueFvPatchField.C at line 470. FOAM exiting Do you know why this is hapening? Many thanks!! Vivien |
Could you try with this findTi
Could you try with this findTimes.C (src/OpenFOAM/db/Time/findTimes.C)?
(It was using this routine to detect the time directories inside constant/boundaryData. There was an assumption in it that the time directories would always have a 'constant') You'll have to rebuild the OpenFOAM library (wmake libso $FOAM_SRC/OpenFOAM) John Deas, this should also fix your problem - couldn't repeat it on your case since it depends on the original file order. http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif findTimes.C |
Hi, Mattijs,
It is working
Hi, Mattijs,
It is working now, thank you very much! Vivien |
Thanks Mattijs, now I am stuck
Thanks Mattijs, now I am stuck with creating the timeVaryingMappedFixedValue on another thread, but will test it as soon as possible !
|
1 Attachment(s)
Hello,
I was trying to use timeVaryingMappedFixedValue bc to get U, k , nuSgs fields value from precursor run to my inlet to have turbulence. I used sample utility to get the field data at precursor run. I added 11 time directory (0,1,2,3.....10) at constant/boundaryData/inlet. Simulation timestep is 0.001. It works fine until the simulation blows out at 2.158 s because of courant no. reaches a huge value. I am adding the log file here. Anyone faces that kind of problem? Any help will be appreciated. Thanks MMMN |
All times are GMT -4. The time now is 15:29. |