CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

simpleWindFoam-tutorial

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   December 7, 2010, 13:41
Default simpleWindFoam-tutorial
  #1
Member
 
inginer's Avatar
 
Ovidiu Michiu
Join Date: Apr 2010
Location: Ingolstadt, Germany
Posts: 52
Rep Power: 7
inginer is on a distinguished road
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
inginer is offline   Reply With Quote

Old   February 22, 2011, 05:46
Default
  #2
New Member
 
siri
Join Date: Apr 2010
Location: Norway
Posts: 16
Rep Power: 7
snippsnuske is on a distinguished road
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
snippsnuske is offline   Reply With Quote

Old   May 21, 2011, 11:46
Default
  #3
New Member
 
Hanan Einav-Levy
Join Date: May 2011
Posts: 10
Rep Power: 6
hananfoam is on a distinguished road
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?
hananfoam is offline   Reply With Quote

Old   July 11, 2011, 05:45
Default
  #4
New Member
 
Join Date: May 2011
Posts: 8
Rep Power: 6
rgarcia is on a distinguished road
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...
rgarcia is offline   Reply With Quote

Old   July 12, 2011, 05:44
Default
  #5
New Member
 
Tom
Join Date: Mar 2011
Posts: 11
Rep Power: 6
tidal_Tom is on a distinguished road
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
tidal_Tom is offline   Reply With Quote

Old   July 12, 2011, 05:59
Default
  #6
New Member
 
Join Date: May 2011
Posts: 8
Rep Power: 6
rgarcia is on a distinguished road
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
rgarcia is offline   Reply With Quote

Old   September 4, 2012, 09:09
Default
  #7
New Member
 
Carlos Peralta
Join Date: Aug 2011
Posts: 6
Rep Power: 5
cperalta is on a distinguished road
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
cperalta is offline   Reply With Quote

Old   September 4, 2012, 15:25
Default
  #8
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
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:
Code:
upRho*diskArea_*mag(upU)
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:
Code:
scalar T = 2.0*upRho*diskArea_*mag(upU)*a*(1 - a);

    forAll(cells, i)
    {
        Usource[cells[i]] += ((Vcells[cells[i]]/V())*T*E) & upU;
    }
It does the inner product with upU as a last operation... which would probably do the operation you're expecting.

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   September 5, 2012, 03:39
Default
  #9
New Member
 
Carlos Peralta
Join Date: Aug 2011
Posts: 6
Rep Power: 5
cperalta is on a distinguished road
Thank you heaps, Bruno!

Best regards,

Carlos
cperalta is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Tutorial for subcooled nucleate boiling Asghari FLUENT 34 September 27, 2013 04:58
Problem on Fluent Tutorial: Horizontal Film Boilig Feng FLUENT 2 April 13, 2013 05:34
2D Mesh Generation Tutorial for GMSH aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 04:52
STAR-CD Tutorial shekhar aryal STAR-CD 4 March 22, 2010 04:25
Rotor/stator tutorial, and how to... gilberto CFX 5 January 21, 2002 10:41


All times are GMT -4. The time now is 16:17.