CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Problem calculating forces on blades 2 (for finding forces)

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

Like Tree6Likes
  • 1 Post By bye bye my blue
  • 4 Post By Tobi
  • 1 Post By wyldckat

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 20, 2016, 12:20
Default Problem calculating forces on blades 2 (for finding forces)
  #1
Member
 
bye bye my blue
Join Date: Sep 2016
Posts: 37
Rep Power: 5
bye bye my blue is an unknown quantity at this point
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
libs
(
"libincompressibleTurbulenceModel.so"
"libincompressibleRASModels.so"
);
application pimpleDyMFoam;

startFrom latestTime;

startTime 0;

stopAt endTime;

endTime 3.15;

deltaT 1e-3;

writeControl adjustableRunTime;

writeInterval 0.01;

purgeWrite 0;

writeFormat ascii;

writePrecision 6;

writeCompression off;

timeFormat general;

timePrecision 6;

runTimeModifiable true;

adjustTimeStep yes;

maxCo 20.0;



functions
(
forces_blade
{
type forces;
functionObjectLibs ("libforces.so");
patches (blades);
CofR (0 0 0);
//pName p;
//UName U;
//verbose true;
rhoName rhoInf;
rhoInf 1.225;
//factor 19.7363;
outputControl timeStep;
outputInterval 100;
}
);


// ************************************************** *********************** //
--> FOAM FATAL IO ERROR:
'functions' entry is not a dictionary

file: /home/pcl/OpenFOAM/pcl-4.0/run/OpenFOAM-2D-VAWT-master/system/controlDict from line 18 to line 75.

From function bool Foam::functionObjectList::read()
in file db/functionObjects/functionObjectList/functionObjectList.C at line 555.

FOAM exiting

this message appeared... -0-;;

how can i solve it ?
ordinary likes this.
bye bye my blue is offline   Reply With Quote

Old   October 20, 2016, 12:58
Default
  #2
Member
 
Geir Karlsen
Join Date: Nov 2013
Location: Norway
Posts: 59
Rep Power: 10
gkarlsen is on a distinguished road
Use different brackets {}. See http://cfd.direct/openfoam/user-guid...ction-objects/
gkarlsen is offline   Reply With Quote

Old   October 20, 2016, 21:49
Default Problem calculating forces on blades 2 (for finding forces)
  #3
Member
 
bye bye my blue
Join Date: Sep 2016
Posts: 37
Rep Power: 5
bye bye my blue is an unknown quantity at this point
in contolDict,

functions
{
forces_blade
{
type forces;
functionObjectLibs ("libforces.so");
patches (blades);
CofR (0 0 0);
//pName p;
//UName U;
//verbose true;
rhoName rhoInf;
rhoInf 1.225;
//factor 19.7363;
outputControl timeStep;
outputInterval 100;
}
};


--> FOAM FATAL ERROR:
Could not find rho

From function void Foam::functionObjects::forces::initialise()
in file forces/forces.C at line 197.

FOAM exiting


how can I solve it ?? why this message occurs?????????
bye bye my blue is offline   Reply With Quote

Old   October 24, 2016, 08:01
Default
  #4
Member
 
Emre
Join Date: Nov 2015
Location: Izmir, Turkey
Posts: 94
Rep Power: 7
ordinary is on a distinguished road
Quote:
Originally Posted by bye bye my blue View Post
in contolDict,

functions
{ -------------------------- >This must be (
forces_blade
{
type forces;
functionObjectLibs ("libforces.so");
patches (blades);
CofR (0 0 0);
//pName p;
//UName U;
//verbose true;
rhoName rhoInf;
rhoInf 1.225;
//factor 19.7363;
outputControl timeStep;
outputInterval 100;
}
}; ---------------------------------------------->This must be )


--> FOAM FATAL ERROR:
Could not find rho

From function void Foam::functionObjects::forces::initialise()
in file forces/forces.C at line 197.

FOAM exiting


how can I solve it ?? why this message occurs?????????
I think the red parentheses must be ( and )
ordinary is offline   Reply With Quote

Old   October 24, 2016, 23:01
Default it didn't work..
  #5
Member
 
bye bye my blue
Join Date: Sep 2016
Posts: 37
Rep Power: 5
bye bye my blue is an unknown quantity at this point
Quote:
Originally Posted by ordinary View Post
I think the red parentheses must be ( and )
your red parentheses are not answer.


it had been previous problem and already solved.

i still don't know...
bye bye my blue is offline   Reply With Quote

Old   November 7, 2016, 02:55
Default
  #6
New Member
 
Ben
Join Date: Oct 2016
Posts: 25
Rep Power: 6
bentkj is on a distinguished road
I have the exact same error, but for a 2D airfoil case (with reference to the airfoil2D tutorial). It would be great if someone could provide a solution to this.

Thank you,
Ben
bentkj is offline   Reply With Quote

Old   November 17, 2016, 17:53
Default Same here / FOAM FATA ERROR: Could not find rho
  #7
New Member
 
Tom D.
Join Date: Nov 2016
Posts: 7
Rep Power: 6
piroshki is on a distinguished road
I am getting the exact same problem, and I don't understand why since I have triple-checked for typos, and I am using what others have claimed works online...

Might this be a bug? Anyone ever managed to solve this one?
piroshki is offline   Reply With Quote

Old   November 18, 2016, 13:10
Default "Could not find rho" - problem with forces output
  #8
New Member
 
Tom D.
Join Date: Nov 2016
Posts: 7
Rep Power: 6
piroshki is on a distinguished road
Hello all,

I've been researching this issue for 2 days now, and can't seem to figure out what I am doing wrong. I am attempting to record the forces on a particular item in my simple icoFoam run. (A streamlined bulbous shape in a simple water "tunnel").

The issue I hit is I when the solver tries to write the output to a file I get the error "could not find rho". If I have writeInterval = 1 then I will get this error after the first timestep is complete. If I have writeInteral = 5 then it happens after 5 timesteps.

--> FOAM FATAL ERROR:
Could not find rho

From function void Foam::functionObjects::forces::initialise()
in file forces/forces.C at line 196.



I also tried to run the run with no force output and then do a -postProcess and I get the exact same error, immediately after loading the mesh.


forces forces:
Not including porosity effects
Time = 0

Reading fields:
volScalarFields: p
volVectorFields: U

Executing functionObjects


--> FOAM FATAL ERROR:
Could not find rho

From function void Foam::functionObjects::forces::initialise()
in file forces/forces.C at line 196.

FOAM exiting




Here is my "forces" file:

forces
{
type forces;
functionObjectLibs ("libforces.so");
writeControl timeStep;
writeInterval 5;
patches (bulb_sd8020);
rhoName rhoInf;
CofR (0 0 0);
pName p;
UName U;
log yes;
verbose true;
rhoInf 1025;
}


I am getting to grips with OpenFoam and wish I could figure this out for myself, but I am stuck...

Thanks for any pointers!

Tom.
piroshki is offline   Reply With Quote

Old   November 21, 2016, 08:06
Post
  #9
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Augsburg
Posts: 2,478
Blog Entries: 6
Rep Power: 46
Tobi has a spectacular aura aboutTobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
I do not know which OpenFOAM version you are using but the rhoName is wrong if you use the latest one. Also your message tells you that you cannot find the entry rho So finally you should do it like:
Code:
rho          rhoInf;
rhoInf      1000;
See also, tutorials/incompressible/simpleFoam/motorBike/system/forceCoeffs


By the way ... you should use code - tags for your posts.
Cheers.
__________________
Keep foaming,
Tobias Holzmann
Tobi is offline   Reply With Quote

Old   November 21, 2016, 15:52
Default
  #10
New Member
 
Tom D.
Join Date: Nov 2016
Posts: 7
Rep Power: 6
piroshki is on a distinguished road
Hello Tobias,
Many thanks for such a quick response. It is much appreciated. I saw the rhoName variable so often in examples it never occurred to me the solution would be so simple...! Your comments are also duly noted with regards to quoting text!
Kind regards,
Tom.
piroshki is offline   Reply With Quote

Old   November 22, 2016, 09:47
Default
  #11
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,959
Blog Entries: 45
Rep Power: 122
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Greetings to all,

This has come to my attention, thanks to the following bug report: http://bugs.openfoam.org/view.php?id=2347

Unfortunately, no one in this thread provided detailed steps on how to reproduce the same error, therefore I'm going to focus on the bug report, until this is fixed or at least understood.

edit: Wait, sorry, bentkj did mention which tutorial can be used, namely the airfoil2D case.



edit 2: OK, I've noticed just now what the problem is and here is what I wrote on the bug report:
Quote:
OK, I then looked in more detail and the problem is that the settings have changed. If you look at the documentation: http://cpp.openfoam.org/v4/a00866.html#details - you'll see that the '*Name' entries have been changed to this:
Code:
      rho rhoInf;
      p p;
      U U;
Please try this and let us know if it solves the problem.

edit 3: the previous 3 posts from another thread, given these are all in the same topic.

Best regards,
Bruno
__________________

Last edited by wyldckat; November 22, 2016 at 18:11. Reason: see "edit:", "edit 2:" and "edit 3:"
wyldckat is offline   Reply With Quote

Old   November 22, 2016, 11:23
Default Problem solved using the suggested changes
  #12
New Member
 
Mukul
Join Date: Nov 2016
Posts: 6
Rep Power: 6
mukul92 is on a distinguished road
Okay, I confirm that making the above changes solves the issue.
Moving to OF-4 just helped us get around some bug which was crashing parallel runs of pimpleDyMFoam.
Thank you very much!
mukul92 is offline   Reply With Quote

Old   November 22, 2016, 12:28
Default
  #13
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Augsburg
Posts: 2,478
Blog Entries: 6
Rep Power: 46
Tobi has a spectacular aura aboutTobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
It is the third topic about that "rho"

No one uses the search engine ! :P
__________________
Keep foaming,
Tobias Holzmann
Tobi is offline   Reply With Quote

Old   November 22, 2016, 18:17
Default
  #14
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,959
Blog Entries: 45
Rep Power: 122
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quote:
Originally Posted by Tobi View Post
It is the third topic about that "rho"
Hopefully I've merged the remaining other thread onto this one that was on this topic.


Quote:
Originally Posted by Tobi View Post
No one uses the search engine ! :P
Ironically, the problem was that people used the search engine and found the outdated information...
purnp2 likes this.
wyldckat is offline   Reply With Quote

Old   November 23, 2016, 11:00
Default
  #15
New Member
 
Tom D.
Join Date: Nov 2016
Posts: 7
Rep Power: 6
piroshki is on a distinguished road
Yup - plenty of examples of rhoName all over the place, not too many showing just rho... In any case this thread will be a useful reference. Perhaps the error message could be amended - "could not find rho (rhoName has been deprecated)"? Thanks much to the fast responses.
piroshki is offline   Reply With Quote

Old   January 10, 2017, 11:45
Default
  #16
New Member
 
Zhenlan GAO
Join Date: Oct 2015
Location: France
Posts: 17
Rep Power: 7
tubois is on a distinguished road
I just had the same problem. It comes with the Visual CFD case set up.
I haven't experienced this problem when I run the motobike example by coping the tutorials, but have this error when I use Visual CFD for the case set up. Maybe it should be told to ESI GROUP.

Quote:
Originally Posted by wyldckat View Post
Hopefully I've merged the remaining other thread onto this one that was on this topic.



Ironically, the problem was that people used the search engine and found the outdated information...
tubois is offline   Reply With Quote

Old   April 19, 2018, 11:48
Default Solved it.
  #17
New Member
 
jan tore
Join Date: Mar 2018
Posts: 1
Rep Power: 0
jan2re is on a distinguished road
Quote:
Originally Posted by Tobi View Post
I do not know which OpenFOAM version you are using but the rhoName is wrong if you use the latest one. Also your message tells you that you cannot find the entry rho So finally you should do it like:
Code:
rho          rhoInf;
rhoInf      1000;
See also, tutorials/incompressible/simpleFoam/motorBike/system/forceCoeffs


By the way ... you should use code - tags for your posts.
Cheers.
Thanks this solved the problem for me.
jan2re is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Rotating blades fan problem Luk FLUENT 1 June 27, 2006 10:56
a problem in calculating pressure drop in Fluent? yu chun FLUENT 1 May 18, 2004 04:40
Problem in calculating drag coefficient Sohail Ahmed FLUENT 2 March 18, 2004 01:40
2d foil pressure forces problem mayor FLUENT 4 December 1, 2003 04:57
Valve Forces in CFdesign Mike Clapp Main CFD Forum 3 March 8, 2001 15:09


All times are GMT -4. The time now is 07:21.