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

No Wall pressure from OpenFOAM 2.2.0

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 24, 2013, 16:55
Default No Wall pressure from OpenFOAM 2.2.0
  #1
Senior Member
 
musaddeque hossein
Join Date: Mar 2009
Posts: 307
Rep Power: 9
musahossein is on a distinguished road
Dear all:
I am running sloshing tank 2D in interDyMFoam. I have the following controlDict file to capture pressures from the left and right walls. In the previous version of OpenFOAM this ran without any problem and gave output. However since I have upgraded to OpenFOAM 2.2.0 and Ubuntu 12.10, it creates the time folders and the sub folders, but they are blank. Also I noted that whereas before the time folders were directly output to the sloshingTank2D directory, the output is now sent to a subfolder called "Post Processing". Any help in this regard would be greatly appreciated.

Thanks!
---------------------------------------------------------------------------------------------------------------------------
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application interDyMFoam;

startFrom startTime;

startTime 0;

stopAt endTime;

endTime 4.00;

deltaT 0.001;

writeControl adjustableRunTime;

writeInterval 0.020;

purgeWrite 0;

writeFormat ascii;

writePrecision 6;

writeCompression compressed;

timeFormat general;

timePrecision 6;

runTimeModifiable yes;

adjustTimeStep yes;

maxCo 0.5;
maxAlphaCo 0.5;

maxDeltaT 1;

functions
{
wallPressure
{
type surfaces;
functionObjectLibs ("libsampling.so");
outputControl outputTime;
outputInterval 5;
surfaceFormat raw;
interpolationScheme cell;

fields ( alpha1
p
);
surfaces
(
leftwalls
{
type patch;
patches (leftWall);
interpolate true;
triangulate false;
}
rightwalls
{
type patch;
patches (rightWall);
interpolate true;
triangulate false;
}
);

} // end functions
musahossein is offline   Reply With Quote

Old   March 25, 2013, 22:55
Default Post processing wont write at intervals in Controldict
  #2
Senior Member
 
musaddeque hossein
Join Date: Mar 2009
Posts: 307
Rep Power: 9
musahossein is on a distinguished road
Dear all;
Here is another question. I have set the writeinterval to 0.02. So shouldnt there be an output folder 0.02, 0.04..... etc? However, postprocessing only gives output at 0.1, 0.2 etc..Any ideas. Other than controldict, is there any other dictionary files where the interval needs to be modified or revised? I cant seem to find one.

Thanks
musahossein is offline   Reply With Quote

Old   March 25, 2013, 23:09
Default post processing pressure file does not occur at writeInterval in controlDict
  #3
Senior Member
 
musaddeque hossein
Join Date: Mar 2009
Posts: 307
Rep Power: 9
musahossein is on a distinguished road
I have the writeInterval in the controlDict file in solshingTank2d file set at 0.02. However, I do not get outputs at 0.02, 0.04, 0.06 etc - rather the files (post processing) are 0.1, 0.2, 0.3 etc. Can anyone tell me why this is happening? Thanks. The file is appended below. Does the outputInterval have anything to do with it? Thanks.

application interDyMFoam;

startFrom startTime;

startTime 0;

stopAt endTime;

endTime 40;
//endTime 0.02;

//deltaT 0.01;
deltaT 0.001;

writeControl adjustableRunTime;

//writeInterval 0.05;
writeInterval 0.02;

purgeWrite 0;

writeFormat ascii;

writePrecision 6;

writeCompression compressed;

timeFormat general;

timePrecision 6;

runTimeModifiable yes;

adjustTimeStep yes;

maxCo 0.5;
maxAlphaCo 0.5;

maxDeltaT 1;

functions
{

wallPressure
{
type surfaces;
functionObjectLibs ("libsampling.so");
outputControl outputTime;
outputInterval 5;
surfaceFormat raw;
interpolationScheme cell;

fields ( alpha1
p
);
surfaces
(
leftwalls
{
type patch;
patches (leftWall);
interpolate true;
triangulate false;
}
rightwalls
{
type patch;
patches (rightWall);
interpolate true;
triangulate false;
}
);
musahossein is offline   Reply With Quote

Old   April 1, 2013, 12:45
Default
  #4
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Musaddeque,

Since you didn't mention that you've made changes to the patches, then the reason for no values in the sub-folders of "postProcessing/wallPressure" is because the patches "leftWall" and "rightWall" do not exist.
You can confirm this by running:
Code:
patchSummary  -time 0
As for the time issue, it's simple:
  1. "writeInterval" is defined to "0.02".
  2. But in the function object you have:
    Code:
    outputInterval  5;
  3. 5*0.02 = 0.1 - which is the time interval you are getting in the output.
Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   April 4, 2013, 19:05
Default
  #5
Senior Member
 
musaddeque hossein
Join Date: Mar 2009
Posts: 307
Rep Power: 9
musahossein is on a distinguished road
Thankyou very much. I didnt realize that and thought they were two independent items.
musahossein is offline   Reply With Quote

Old   July 25, 2013, 08:15
Default Wallpressure computation in sampleDict
  #6
Senior Member
 
musaddeque hossein
Join Date: Mar 2009
Posts: 307
Rep Power: 9
musahossein is on a distinguished road
Dear all:

I am running sloshingTank2d in OpenFoam for a rectangular tank and the tank is partially filled with water. I am using sampleDict to obtain wall pressure. My question is the wall pressure values that I get, are they the pressure due to the water only? I cannot find documentation on how this quantity is calculated in OpenFOam. Any help will be appreciated. A segment of the sampledict output is provided below (X is in/out of the paper; Y is parallel to the paper and Z is vertically up. The origin is at the middle of the fluid phase and gas phase interface:

X Y Z alpha P
0 0.45 0.256061 0 99997.1
0 0.45 0.24596 0 99997.2
0 0.45 0.235859 0 99997.3
0 0.45 0.225758 0 99997.4
0 0.45 0.215657 0 99997.5
0 0.45 0.205556 2.38699e-308 99997.6
0 0.45 0.195455 1.16744e-297 99997.7
0 0.45 0.185354 1.98218e-285 99997.8
0 0.45 0.175253 4.45133e-264 99997.9
0 0.45 0.165152 1.63685e-243 99998
0 0.45 0.155051 1.3369e-223 99998.1
musahossein is offline   Reply With Quote

Old   July 29, 2013, 19:53
Default dynamic and static pressure
  #7
Senior Member
 
musaddeque hossein
Join Date: Mar 2009
Posts: 307
Rep Power: 9
musahossein is on a distinguished road
Dear all:

I have a question about how OpenFOAM calculates pressure. In the sloshingTank2D problem, if I sample the wall pressure - is the pressure the total pressure (dynamic + static) or only the dynamic pressure? How can I find out. Also if it is the total pressure then what can I do in the dictionary files to get the dynamic pressure only?

Suggestions will be greatly appreciated!

Thanks.

Musa
musahossein is offline   Reply With Quote

Old   August 31, 2013, 15:27
Default can inerdymfoam give static pressure?
  #8
Senior Member
 
musaddeque hossein
Join Date: Mar 2009
Posts: 307
Rep Power: 9
musahossein is on a distinguished road
Can anyone tell me if OpenFoam can provide static pressure at each point? I am running Openfoam 2.2.1 , interdymfoam, sloshingtank2d and trying to get pressure against the wall. Openfoam gives total pressure P from which I need to subtract pRef and also static pressure so I can get the dynamic pressure. Is there any way that the solver (interdymfoam) can give me the static pressure at each point where it outputs p?

Thanks
musahossein is offline   Reply With Quote

Old   August 31, 2013, 15:33
Default
  #9
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Musaddeque,

There is a function object that might help you, named "pressureTools": http://foam.sourceforge.net/docs/cpp...5.html#details

There is a thread on this topic here: pressureTools postProcessing function objects in 2.2.0
You'll have to read the whole thread, because the information is spread across various posts

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   October 1, 2013, 07:05
Default
  #10
New Member
 
JUN HONG
Join Date: Nov 2012
Posts: 4
Rep Power: 4
Junhong is on a distinguished road
Hi Musaddeque,

I put the function (below) in controlDict, there is no data files produced in each folder (timestep). It works well in the earlier versions. Did you encounter such problem and how to solve it ?

Thanks!

Junhong

-----------------------------------------------------
left-wheel
{
type surfaces;
functionObjectLibs ( "libsampling.so" );
enabled true;
outputControl timeStep;
outputInterval 2;
surfaceFormat raw;
interpolationScheme cell;
fields
( p );
surfaces
(
left-wheel
{
type patch;
patches (left-wheel);
}
);
}
-----------------------------------------------
Junhong is offline   Reply With Quote

Old   October 1, 2013, 12:16
Default
  #11
Senior Member
 
musaddeque hossein
Join Date: Mar 2009
Posts: 307
Rep Power: 9
musahossein is on a distinguished road
Your output interval is 2. what is your data write interval? since the output data is output interval * the data write interval, there may be a problem there. Check that.
musahossein is offline   Reply With Quote

Old   October 1, 2013, 14:08
Default
  #12
New Member
 
JUN HONG
Join Date: Nov 2012
Posts: 4
Rep Power: 4
Junhong is on a distinguished road
Thanks!
the version 2.2.0_b2 used. same as the bug described
http://www.openfoam.org/mantisbt/view.php?id=813


startFrom latestTime;
startTime 0;
stopAt endTime;
endTime 6.0;
deltaT 5e-6;
writeControl timeStep;
writeInterval 250;


type surfaces;
// Where to load it from
functionObjectLibs ( "libsampling.so" );
// Write at same frequency as fields
enabled true;
outputControl timeStep;
outputInterval 1;
surfaceFormat vtk; //vtk,raw,something else?
interpolationScheme cell;
Junhong is offline   Reply With Quote

Reply

Tags
controldict, openfoam 2.2.0, slosingtank2d, wallpressure

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
Radiation interface hinca CFX 15 January 26, 2014 18:11
An error has occurred in cfx5solve: volo87 CFX 5 June 14, 2013 17:44
pressure wall boundary condition in CFX murx CFX 4 October 9, 2012 06:50
New OpenFOAM Forum Structure jola OpenFOAM 2 October 19, 2011 06:55
natural convection mehrdadeng CFX 10 February 25, 2011 06:25


All times are GMT -4. The time now is 05:10.