[sunnysun]

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

[mattijs]

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.

[sunnysun]

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

[johndeas]

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.

[sunnysun]

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

[mattijs]

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

[sunnysun]

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

[mattijs]

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'.

[sunnysun]

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

[mattijs]

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.

findTimes.C

[sunnysun]

Hi, Mattijs,

It is working now, thank you very much!

Vivien

[johndeas]

Thanks Mattijs, now I am stuck with creating the timeVaryingMappedFixedValue on another thread, but will test it as soon as possible !

[mmmn036]

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