simpleWindFoam-tutorial
 

hello,

did somebody used simpleWindFoam solver from the tutorials to run turbineSiting case?

i'm typing the simpleWindFoam but i receive a error like this

"Selecting model type actuationDiskSource
Source:disk1
-selecting cells using cellSet actuationDisk1
-->FOAM FATAL IOERROR:
cannot openfile.

file:/home/openfoam/OpenFOAM/openfoam-1.7.0/run/projects/TRAINS/SimpleWindFoam/turbineWind/4/polyMesh/sets/actuationDisk1 at line 0

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 61.

FOAM exiting."


What is the point of makeZones file?

best,
Ovidiu

I have run it and made it workd. Let me know if you are still strugling with it (since your post is from december). Would be nice to get in contact with you if you are still working on this case.
Siri

Hello,

I am having a problem running the simpleWindFoam tutorial in parrallel,
i get this error:

[0] --> FOAM FATAL ERROR:
[0] Illegal content 102401 of set:actuationDisk1 of type cellSet
Value should be between 0 and 60123

I used the simple method for decomposing the mesh. Is this the source of the problem?

Hi everybody!

I'm currently running simpleWindFoam to simulate the actioan of an actuator disk in a flat terrain to study the wake. I can run the case in one single processor, eventhough the results are not very satisfying. Now, when I try to run simpleWindFoam in parallel I 've several problems. I'm trying it with metis and simple methods and the error I've got is:

[3]
[3]
[3] --> FOAM FATAL ERROR:
[3] Unormal = 7.18296e-310 not found in dictionary
[3]
[3] From function actuatorDisk::actuatorDiskTemplates
[3] in file actuatorDiskTemplates.C at line 74.
[3]
FOAM parallel run exiting
[3]
--------------------------------------------------------------------------
MPI_ABORT was invoked on rank 3 in communicator MPI_COMM_WORLD
with errorcode 1.

NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes.
You may or may not see output from other processes, depending on
exactly when Open MPI kills them.
--------------------------------------------------------------------------
[2]
[2]
[2] --> FOAM FATAL ERROR:
[2] Unormal = 1.42174e-312 not found in dictionary
[2]
[2] From function actuatorDisk::actuatorDiskTemplates
[2] in file actuatorDiskTemplates.C at line 74.
[2]
FOAM parallel run exiting
[2]
[1]
[1]
[1] --> FOAM FATAL ERROR:
[1] Unormal = 1.42174e-312 not found in dictionary
[1]
[1] From function actuatorDisk::actuatorDiskTemplates
[1] in file actuatorDiskTemplates.C at line 74.
[1]
FOAM parallel run exiting
[1]


Even changing the code and imposing Cp = Ct = 0 for wind speed lower than 4 m/s.
I don't have this problem with just one processor...

I though that maybe doing the decompose, it breaks the actuator disk in two different zones. But then, I don't understand why this error!

could you tell me what you think about it?


@ hananfoam: Did you do the cellSet and the setsToZones after doing your changes? It looks like if your trying to use the actuator disk in you current grid using an old grid with more cells...

Hi all,

I have been using this solver for investigating turbine wakes in a circulating water channel. I have managed to achieve good agreement with experimental data.

However there is a problem when running in parallel.

I have had the same errors you report rgarcia, but it will run sometimes in parallel. I think the problem arises as follows.

If the decomposition of the mesh cuts the actuator disc region so that some parts of the actuator disc are split across different processors then the results become incorrect.

I think this is because when the total actuator disc volume is calculated (see the source code - actuationDiskSourceTemplates.H), only the volume of actuator disc in that processor is used - it does not add the regions from all the processors. Therefore the total disc volume used is smaller, and different on each processor resulting in non-uniform force of too greater magnitude.

I haven't got around to editing the code yet to take this into account but I think there was some advice on this forum about computing the volume of a cellZone in parallel runs.

My work around (as I needed results) was to ensure the actuator disc was on a single processor.

Tom

Hi all,

Thank you very much for your answer Tom! I will check the blogs about computing the volume of a cellZone in parallel runs! ;)

Roger

Hello,
I was wondering if this problem was solved in a more recent version of OF. Otherwise, is there a simple way to ensure the disk is on a single processor?

Additionally, I was looking at the equations in the actuationDiskSourceTemplates.C and I see
scalar T = 2.0*upRho*diskArea_*mag(upU)*a*(1 - a);
but shouldn't it be upU^2?
scalar T = 2.0*upRho*diskArea_*mag(upU)*mag(upU)*a*(1 - a);

thanks for any help.

Carlos

Greetings Carlos,

In OpenFOAM 2.1.1 and 2.1.x this doesn't seem to be a problem, because the tutorial "incompressible/simpleFoam/turbineSiting" runs in parallel by default and doesn't seem to have any problems (at least not in 2.1.x). It doesn't even have any explicit indication of isolating disks on a single processor...


As for the code, this:
gives you the mass flow rate. So why would you want to multiply by magU once again? ... then again, if you look at the code below it:
It does the inner product with upU as a last operation... which would probably do the operation you're expecting.

Best regards,
Bruno

Thank you heaps, Bruno!

Best regards,

Carlos