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

TimeVaryingUniformFixedValue BC in foam 15

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

Like Tree1Likes
  • 1 Post By louisgag

Reply
 
LinkBack Thread Tools Display Modes
Old   July 17, 2008, 17:32
Default Hi Guys: I am running foam
  #1
Member
 
Ning Yang
Join Date: Mar 2009
Location: University Park, PA, USA
Posts: 85
Rep Power: 8
nzy102 is on a distinguished road
Hi Guys:

I am running foam 1.5 with a timeVaryingUniformFixedValue BC. Here is the format I used in my bc:

type timeVaryingUniformFixedValue;
fileName "time-series";
boundAction clamp; // (error|warn|clamp|repeat)

i tried both relative path and complete path for the "time-series" file. And the format of the file is consistent with the old version 1.4.1, and it is something like:

{
t0 p0
t1 p1
t2 p2
....
}

when I ran my stuff, I got an error:

================================================== =
Reading transportProperties

Reading field p

Reading field U



keyword outOfBounds is undefined in dictionary "/home/nzy102/OpenFOAM/nzy102-1.5/run/tutorials/icoFoam/pediatric_aorta_4-e_test mesh_pulsatile_resistancenewbc_zeroGradU/0/U::inlet"

file: /home/nzy102/OpenFOAM/nzy102-1.5/run/tutorials/icoFoam/pediatric_aorta_4-e_testm esh_pulsatile_resistancenewbc_zeroGradU/0/U::inlet from line 61 to line 63.

From function dictionary::lookupEntry(const word& keyword) const
in file db/dictionary/dictionary.C at line 213.

FOAM exiting
================================================== =

Anybody here has a clue what is wrong?

Thank you.

Ning
nzy102 is offline   Reply With Quote

Old   July 18, 2008, 02:53
Default Try something like this:
  #2
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
olesen will become famous soon enough
Try something like this:

fileName "$FOAM_CASE/time-series";
outOfBounds clamp;

It looks like the docs are slightly out-of-sync.
olesen is offline   Reply With Quote

Old   July 30, 2008, 13:57
Default Using the openfoam 1.5 package
  #3
Senior Member
 
louisgag's Avatar
 
Louis Gagnon
Join Date: Mar 2009
Location: Québec, QC, Canada
Posts: 200
Rep Power: 9
louisgag is on a distinguished road
Send a message via ICQ to louisgag
Using the openfoam 1.5 package, I had to manually set the $FOAM_CASE variable before running paraFoam to avoid an error that would cause it to exit before any rendering could be done. (That is in the case of a time varying inlet velocity).
louisgag is offline   Reply With Quote

Old   July 31, 2008, 02:39
Default I've reported this and it's al
  #4
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
olesen will become famous soon enough
I've reported this and it's already been fixed for the next release.
If you are willing to patch the source a bit, the changes to vtkPV3Foam.C are quite simple:

In the Foam::vtkPV3Foam::vtkPV3Foam constructor
you need these lines:

// avoid argList and get rootPath/caseName directly from the file
fileName fullCasePath(fileName(FileName).path());

if (!dir(fullCasePath))
{
return;
}
if (fullCasePath == ".")
{
fullCasePath = cwd();
}

// Set the case as an environment variable - some BCs might use this
if (fullCasePath.name().find("processor", 0) == 0)
{
setEnv("FOAM_CASE", fullCasePath.path(), true);
}
else
{
setEnv("FOAM_CASE", fullCasePath, true);
}
olesen is offline   Reply With Quote

Old   July 31, 2008, 11:12
Default Thank you Mark. By adding
  #5
Senior Member
 
louisgag's Avatar
 
Louis Gagnon
Join Date: Mar 2009
Location: Québec, QC, Canada
Posts: 200
Rep Power: 9
louisgag is on a distinguished road
Send a message via ICQ to louisgag
Thank you Mark.

By adding

// Set the case as an environment variable - some BCs might use this
if (fullCasePath.name().find("processor", 0) == 0)
{
setEnv("FOAM_CASE", fullCasePath.path(), true);
}
else
{
setEnv("FOAM_CASE", fullCasePath, true);
}



after

fileName fullCasePath(fileName(FileName).path());

if (!dir(fullCasePath))
{
return;
}
if (fullCasePath == ".")
{
fullCasePath = cwd();
}



my problem was solved.
mm.abdollahzadeh likes this.
louisgag is offline   Reply With Quote

Old   August 19, 2008, 08:08
Default Hello Guys, Just for comple
  #6
Member
 
Tobias Holzinger
Join Date: Mar 2009
Location: Munich, Germany
Posts: 46
Rep Power: 8
woody is on a distinguished road
Hello Guys,

Just for completion of this thread: I tried to restart my simulation with the new Version.
There seemed to be a change in the file Format of the TimeVaryingUniformFixedValue BC, at least for varying velocities. My old file looked like:
(
t1 U1
t2 U2
t3 U3
...
)

The new file has to look like:

(
(t1 (Ux1 Uy1 Uz1))
(t2 (Ux2 Uy2 Uz2))
(t1 (Ux3 Uy3 Uz3))
...
)

Obviously somebody managed to change the Velocitydescription from normal to cartesian...
would be nice if such things are posted somewhere....

Hope this helps anyone who starts with this BC
__________________
Tobias Holzinger

Chair of Thermodynamics, TU München
woody 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
TimeVaryingUniformFixedValue holger_marschall OpenFOAM Running, Solving & CFD 4 August 10, 2013 14:47
TimeVaryingUniformFixedValue with sonicLiquidFoam Bugs amp Fixes chnrdu OpenFOAM Bugs 1 May 21, 2008 09:52
TimeVaryingUniformFixedValue does not work as a pressureInlet with sonicLiquidFoam nishant_hull OpenFOAM Running, Solving & CFD 5 May 21, 2008 08:54
TimeVaryingUniformFixedValue boundary condition liu OpenFOAM Running, Solving & CFD 1 October 12, 2007 13:19
FOAM CFDtoy Main CFD Forum 5 September 21, 2004 14:09


All times are GMT -4. The time now is 17:22.