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

openfoam 2.2 force coefficients 0

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

Like Tree5Likes
  • 1 Post By hakonbar
  • 2 Post By harsha_kulkarni
  • 1 Post By sibo
  • 1 Post By Andela

Reply
 
LinkBack Thread Tools Display Modes
Old   April 1, 2013, 12:23
Default openfoam 2.2 force coefficients 0
  #1
Senior Member
 
Mihai Pruna
Join Date: Apr 2010
Location: Boston
Posts: 191
Blog Entries: 1
Rep Power: 9
mihaipruna is on a distinguished road
The same dictionary worked in previous versions.
The case solves and there should be a net force because pressure integration shows a number greater than 0.
Here is the forceCoeffs dictionary:

Code:
forces

{

    type        forceCoeffs;

    functionObjectLibs ( "libforces.so" );

    outputControl timeStep;

    outputInterval 1;

    patches     (

        "vol1face1"

        "vol1face2"

        "vol1face3"

        "vol1face4"

        "vol1face5"

        "vol1face6"

    );

    pName       p;

    UName       U;

    rhoName     rhoInf;      // Indicates incompressible

    log         true;

    rhoInf      1;           // Redundant for incompressible

    liftDir     (-0.000000 1.000000 0.000000);

    dragDir     (1.000000 0.000000 0.000000);

    CofR        (0.72 0 0);  // Axle midpoint on ground

    pitchAxis   (0 0 1);

    magUInf       100.0000;

    lRef            1.0000;

    Aref            6.0000;

    }
mihaipruna is offline   Reply With Quote

Old   April 1, 2013, 13:14
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,978
Blog Entries: 39
Rep Power: 108
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Hi Mihai,

I haven't tested this, but comparing the tutorial "tutorials/incompressible/simpleFoam/motorBike" between versions:
You'll see that there is a new entry:
Code:
binData
    {
        nBin        20;          // output data into 20 bins
        direction   (1 0 0);     // bin direction
        format      gnuplot;
        cumulative  yes;
    }
In theory, you should have seen in your solver log folder a message indicating the missing entry "binData".


Best regards,
Bruno
__________________
wyldckat is offline   Reply With Quote

Old   April 1, 2013, 14:57
Default
  #3
Senior Member
 
Mihai Pruna
Join Date: Apr 2010
Location: Boston
Posts: 191
Blog Entries: 1
Rep Power: 9
mihaipruna is on a distinguished road
Bruno
I tried to add that part and got an error.
mihaipruna is offline   Reply With Quote

Old   April 1, 2013, 17:45
Default
  #4
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,978
Blog Entries: 39
Rep Power: 108
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Hi Mihai,

Now I'm confused... I've ran just now the same "motorBike" case from 2.1.x, but on 2.2.0 and 2.2.x and it calculated the forces... although I haven't compared the results...

But one thing I noticed in the file "log.simpleFoam" is that it made a lot of complaints about the div schemes:
Code:
--> FOAM Warning : 
    From function gaussConvectionScheme
    in file finiteVolume/convectionSchemes/gaussConvectionScheme/gaussConvectionScheme.H at line 123
    Reading "/home/bmss/OpenFOAM/bmss-2.1.x/run/tutorials/incompressible/simpleFoam/motorBike/system/fvSchemes.divSchemes.div(phi,U)" at line 30
    Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.
    To remove this warning switch off 'boundedGauss' in "/home/bmss/OpenFOAM/OpenFOAM-2.2.x/etc/controlDict"
smoothSolver:  Solving for Ux, Initial residual = 0.226116, Final residual = 0.0133515, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 0.275451, Final residual = 0.0161505, No Iterations 3
smoothSolver:  Solving for Uz, Initial residual = 0.172255, Final residual = 0.0161645, No Iterations 2
GAMG:  Solving for p, Initial residual = 0.106832, Final residual = 0.00781284, No Iterations 2
time step continuity errors : sum local = 0.0152865, global = 0.00268025, cumulative = 0.00268025
--> FOAM Warning : 
    From function gaussConvectionScheme
    in file finiteVolume/convectionSchemes/gaussConvectionScheme/gaussConvectionScheme.H at line 123
    Reading "/home/bmss/OpenFOAM/bmss-2.1.x/run/tutorials/incompressible/simpleFoam/motorBike/system/fvSchemes.divSchemes.div(phi,omega)" at line 32
    Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.
    To remove this warning switch off 'boundedGauss' in "/home/bmss/OpenFOAM/OpenFOAM-2.2.x/etc/controlDict"
smoothSolver:  Solving for omega, Initial residual = 0.00480145, Final residual = 0.000399432, No Iterations 3
--> FOAM Warning : 
    From function gaussConvectionScheme
    in file finiteVolume/convectionSchemes/gaussConvectionScheme/gaussConvectionScheme.H at line 123
    Reading "/home/bmss/OpenFOAM/bmss-2.1.x/run/tutorials/incompressible/simpleFoam/motorBike/system/fvSchemes.divSchemes.div(phi,k)" at line 31
    Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.
    To remove this warning switch off 'boundedGauss' in "/home/bmss/OpenFOAM/OpenFOAM-2.2.x/etc/controlDict"
smoothSolver:  Solving for k, Initial residual = 1, Final residual = 0.0477205, No Iterations 3
ExecutionTime = 12.15 s  ClockTime = 12 s
Are you getting these same messages?

And what was the error you got when you used the "binData" entry?

Best regards,
Bruno
__________________
wyldckat is offline   Reply With Quote

Old   April 1, 2013, 18:54
Default
  #5
Member
 
Dan Kokron
Join Date: Dec 2012
Posts: 33
Rep Power: 6
dkokron is on a distinguished road
Bruno,

I got those same warnings when I converted from 2.1.x to 2.2.x. They are just informational. The numerics didn't change when I re-ran my case with the now recommended 'bounded' schemes. See http://www.openfoam.org/version2.2.0/numerics.php for the details.

Dan
dkokron is offline   Reply With Quote

Old   April 2, 2013, 05:51
Default
  #6
New Member
 
Håkon Bartnes Line
Join Date: Mar 2013
Posts: 27
Rep Power: 6
hakonbar is on a distinguished road
I had the same problem when I upgraded from 2.1 to 2.2. Apparently a bug was introduced in the latest update so that if you record the forces on several surfaces, only those on the last surface in your list will be written to file.

If you define the body on which you wish to measure the forces as a single surface, it'll probably work, but the bug has been fixed in the latest git release.

Read this thread for more info:
http://www.cfd-online.com/Forums/ope...s-airfoil.html
wyldckat likes this.
hakonbar is offline   Reply With Quote

Old   August 7, 2014, 08:22
Default
  #7
Member
 
harshawardhank
Join Date: Mar 2014
Posts: 99
Rep Power: 5
harsha_kulkarni is on a distinguished road
Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.

when I use bounded Gauss it produce following error floating point error

with unbound 'Gauss' it not produce any error
wyldckat and Uyan like this.
harsha_kulkarni is offline   Reply With Quote

Old   January 19, 2017, 11:25
Default Same problem
  #8
New Member
 
sibo
Join Date: Oct 2016
Posts: 22
Rep Power: 2
sibo is on a distinguished road
Hi guys,

how did you solve this problem? I run into the same problem here.

Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.

Although there are many warnings, there is no error. Can we ignore this warning?
I am using the OpenFOAM-3.0.1

Thanks a lot!
Andela likes this.
sibo is offline   Reply With Quote

Old   February 1, 2017, 07:23
Default
  #9
New Member
 
Andela's Avatar
 
Marija Bervida
Join Date: Mar 2016
Location: Slovenia
Posts: 9
Rep Power: 3
Andela is on a distinguished road
Hi Sibo,

I am also using OF 3.0.1., and I got same wqarnings.
After adding in fvSchemes:
div(phi,T) bounded Gauss upwind;
the warnings dissapeared, and the simulation runs without any errors.
sibo likes this.
__________________
*Things are not what they seem; nor are they otherwise.*
Andela is offline   Reply With Quote

Old   February 19, 2017, 09:32
Default
  #10
New Member
 
sibo
Join Date: Oct 2016
Posts: 22
Rep Power: 2
sibo is on a distinguished road
Thanks for your reply!!
sibo 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
Memory protection in OpenFOAM / combinig with FORTRAN botp OpenFOAM Programming & Development 2 February 15, 2016 13:25
ActuatorDiskExplicitForce in OF2.1. Help be_inspired OpenFOAM Programming & Development 8 July 3, 2014 10:54
Obtaining Forces and Force Coefficients ShuToshio OpenFOAM 3 July 25, 2012 00:05
OpenFOAM Foundation Releases OpenFOAM® Version 2.1.1 opencfd OpenFOAM Announcements from ESI-OpenCFD 0 May 31, 2012 09:07
how to set lift and drag coefficients in force mon alagesanj FLUENT 0 November 16, 2008 21:47


All times are GMT -4. The time now is 01:34.