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

boundary condition icofoam: how to make a ramp

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

Like Tree1Likes
  • 1 Post By cfd-noob

Reply
 
LinkBack Thread Tools Display Modes
Old   January 6, 2012, 06:22
Default boundary condition icofoam: how to make a ramp
  #1
New Member
 
Join Date: Jan 2012
Location: Germany
Posts: 9
Rep Power: 5
cfd-noob is on a distinguished road
hey,
I hope I am in the right forum here.
I want to change the icofoam case in the tutorial in a way that the upper wall doesn't has the speed of "1" at the beginning.

So I need "timeVaryingUniformFixedValue". But to use that type I need to write "EXE_LIBS = -lcfdTools" into the Make/options file and than recompile it. (This is what I have read so far).

First of all, ist that true?
And second, I am using Ubuntu. So with "sudo gedit" I was able to change the file in "opt/openfoam210/applications/solvers"...
But how do I recompile it from there? Or am I doing everything wrong here :-(

Thanks for every answer
cfd-noob is offline   Reply With Quote

Old   January 6, 2012, 11:40
Default
  #2
Senior Member
 
Join Date: Mar 2011
Posts: 174
Rep Power: 6
anon_a is on a distinguished road
Hello

In order to apply different boundary conditions you don't need to compile anything, you just have to modify the files in the directory 0 (please read the manual :-) ).

In general, in order to apply timeVaryingUniformFixedValue you would do the following:

i) open 0/U with an editor and change the field
movingWall
{
type timeVaryingUniformFixedValue;
fileName "time-series";
outOfBounds clamp;
}

ii) create a file in the main directory of the case called "time-series" and place the time and velocity values like this
(
(0. (0 0 0))
(1. (1 0 0))
)

More information on this BC
TimeVaryingUniformFixedValue BC in foam 15
TimeVaryingUniformFixedValue b.c.
timeVaryingUniformFixedValue
error about timeVaryingUniformFixedValue

Compilation is performed with "wmake" or "wmake libso" (again, read the manual).
But you don't really need this right now.

Regards,
S.P.
anon_a is offline   Reply With Quote

Old   January 6, 2012, 15:40
Default
  #3
New Member
 
Join Date: Jan 2012
Location: Germany
Posts: 9
Rep Power: 5
cfd-noob is on a distinguished road
Thank you very much, but it doesn't work.

Here is the problem:

Quote:
FOAM FATAL IO ERROR:
Unknown patchField type timeVaryingUniformFixedValue for patch type wall

Valid patchField types are :

59
(
SRFFreestreamVelocity
SRFVelocity
activeBaffleVelocity
activePressureForceBaffleVelocity
advective
calculated
codedFixedValue
codedMixed
cyclic
cyclicAMI
cyclicSlip
cylindricalInletVelocity
directionMixed
empty
fixedGradient
fixedInternalValue
fixedNormalSlip
fixedValue
flowRateInletVelocity
fluxCorrectedVelocity
freestream
inletOutlet
mapped
mappedField
mappedFixedInternalValue
mappedFixedPushedInternalValue
mappedFlowRate
mappedVelocityFlux
mixed
movingWallVelocity
nonuniformTransformCyclic
oscillatingFixedValue
outletInlet
outletMappedUniformInlet
partialSlip
pressureDirectedInletOutletVelocity
pressureDirectedInletVelocity
pressureInletOutletParSlipVelocity
pressureInletOutletVelocity
pressureInletUniformVelocity
pressureInletVelocity
pressureNormalInletOutletVelocity
processor
processorCyclic
rotatingPressureInletOutletVelocity
rotatingWallVelocity
sliced
slip
supersonicFreestream
surfaceNormalFixedValue
swirlFlowRateInletVelocity
symmetryPlane
timeVaryingMappedFixedValue
translatingWallVelocity
turbulentInlet
uniformFixedValue
waveTransmissive
wedge
zeroGradient
)
The Problem is, icoFoam does not have the type "timeVaryingUniformFixedValue". To use this type, I have to modify icoFoam e.g. putting the library cfdtools in it. And than I have to compile it, so that icoFoam has the library can can use this type.

And I don't know how to do that.
cfd-noob is offline   Reply With Quote

Old   January 6, 2012, 15:57
Default
  #4
Senior Member
 
Join Date: Mar 2011
Posts: 174
Rep Power: 6
anon_a is on a distinguished road
Ok, now your problem is much clearer!
I didn't realize there were such changes in v2.1.0.

Here, take a look at this:
http://www.openfoam.org/version2.1.0...conditions.php
"uniformFixedValue" is what you are looking for
(I guess it's the part with the "table")
anon_a is offline   Reply With Quote

Old   January 6, 2012, 18:19
Default
  #5
New Member
 
Join Date: Jan 2012
Location: Germany
Posts: 9
Rep Power: 5
cfd-noob is on a distinguished road
Thank you very much.

I didn't realize that the new version can't work with the old tutorials.
This is how I solve it now:
Quote:
movingWall
{
type uniformFixedValue;
uniformValue tableFile;
tableFileCoeffs
{
fileName "$FOAM_CASE/ramp"
outOfBounds clamp;
}

}
No recompilation was necessary.
saba_saeb likes this.
cfd-noob 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
Boundary Conditions Thomas P. Abraham Main CFD Forum 20 July 7, 2013 05:05
SymmetryPlane Boundary Condition raytracer OpenFOAM Running, Solving & CFD 0 July 11, 2008 17:04
CFX Solver : Sudden crash Hervé CFX 2 June 16, 2008 06:40
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55


All times are GMT -4. The time now is 05:21.