
[Sponsors] 
Using a variable (increasing) inlet to get an easy convergence/initialization ? 

LinkBack  Thread Tools  Search this Thread  Display Modes 
March 28, 2013, 02:32 
Using a variable (increasing) inlet to get an easy convergence/initialization ?

#1 
Senior Member
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 238
Rep Power: 13 
Dear all,
I'm running some simulations with rhoSimplecFoam (kepsilon, Air) and I encounter some convergence / initialization problems. I mostly run my case at Mach 0.3 and 0.4 and I often get divergence even with simple geometries such as Naca Airfoils or Cylinders. I tried different techniques:  initialize the flow with a potentialFoam  initialize the velocity internalField at different speed (0 to 80m/s)  play with the under relaxation numbers ...  using upwind scheme  use different meshes (structured, unstructured, yPlus from 0.1 to 30,...) After many tries, I found that a good way to avoid divergence and get convergence is to slowly increase the inlet velocity value ! For example, I start at 2m/s, then 5m/s, then 10m/s and so on until the actual velocity. However, this technique is "slow" and requires some manual change. First, is this "initialization" ok ? I mean, I didn't see anybody using such a technique, maybe there is a problem I don't know about. Second, is there a way to make this automatically ? I found this link but it looks old and unusable in OF2: http://www.idurun.com/?p=512 My inlet is: Code:
alphat: type calculated; value uniform 0; epsilon: type fixedValue; value uniform 2.15e1; k: type fixedValue; value uniform 1.6e2; mut: type calculated; value uniform 0; p: type zeroGradient; T: type fixedValue; value uniform 281.4; U: type fixedValue; value uniform (81.02 0 0); Code:
alphat: type calculated; value uniform 0; epsilon: type inletOutlet; inletValue uniform 2.15e1; value uniform 2.15e1; k: type inletOutlet; inletValue uniform 1.6e2; value uniform 1.6e2; mut: type calculated; value uniform 0; p: type fixedValue; value uniform 95650; T: type inletOutlet; inletValue uniform 281.4; value uniform 281.4; U: type inletOutlet; inletValue uniform (81.02 0 0); value uniform (81.02 0 0); Code:
alphat: type alphatWallFunction; value uniform 0; epsilon: type compressible::epsilonWallFunction; value uniform 2.15e1; k: type compressible::kqRWallFunction; value uniform 1.6e2; mut: type mutkWallFunction; value uniform 0; p: type zeroGradient; T: type zeroGradient; U: type fixedValue; value uniform (0 0 0); Code:
alphat: value uniform 0; epsilon: value uniform 2.15e1; k: value uniform 1.6e2; mut: value uniform 0; p: value uniform 95650; T: value uniform 281.4; U: value uniform (81.02 0 0); 

March 28, 2013, 09:04 

#2 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 272
Rep Power: 14 
hello,
Which field is diverging ? My guess would be turbulence model : => try turbulentIntensityKinetics... for k, and turbulentMixingLenght... for epsilon, and relax k,epsilon (if steady solver). If you would to use a ramped velocity inlet, take a look at flowRateInletVelocity or uniformFixedValue, and specify a velocity changing in time (or iteration), like: Code:
type uniformFixedValue; uniformValue table ( (0 (0 0 0)) (100 (100 0 0)) ); regards, olivier 

March 28, 2013, 13:54 

#3 
Senior Member
Jose Rey
Join Date: Oct 2012
Posts: 134
Rep Power: 14 
Look at the motorbike tutorial (Allrun), which uses potentialFoam to get the fields initially, then it runs the actual solver. Would this work for you?
MY BAD: You alread tried this. Last edited by JR22; March 28, 2013 at 14:24. 

March 29, 2013, 03:23 

#4 
Senior Member
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 238
Rep Power: 13 
Thx Olivier for your advices.
0) the diverging field is most of the time the pressure that leads to a Floating Point Exception (caused by the thermo model). 1) I've tried to change my k and epsilon settings (inlet and relax number) but it doesn't change anything. 2) The technique of the Table works well but I need many steps to reach my final velocity. 3) I've also tried to use the flowRateInletVelocity inlet but it also often diverge after only 2 or 3 iterations (the pressure starts to diverge first). Moreover, using this kind of Inlet, I get some strange oscillation of the pressure/density through my domain. It's like a wave going from the inlet to the outlet and coming back (once my pressure inlet > pressure outlet and then two iteration later it is pressure inlet < pressure outlet and so on). 

March 29, 2013, 05:00 

#5 
Senior Member
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 238
Rep Power: 13 
To make the things simple, here is my current case (3.8 MB) :
http://www.fredo490.fr/public/rhoSim...der_Vinlet.zip It is a structured 4 inch cylinder at 81.02m/s (95650 Pa and 8.2°C). 

April 2, 2013, 06:22 

#6 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 272
Rep Power: 14 
hello,
You may try to modify the outlet BC: p : totalPressure  U pressureInletOutletVelocity (or pressureInletVelocity / pressureDirectedInletVelocity / ...) regards, olivier 

April 2, 2013, 09:02 

#7 
Senior Member
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 238
Rep Power: 13 
thx for your advice.
For those who want, I found a good source for the table inlet: http://www.openfoam.org/version2.1.0...conditions.php Also, I found that using a "Laplacian schemes linear limited 0.5" helps a lot. 

April 9, 2014, 08:01 

#8 
Member
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 9 
is it possible to use such table options for the SRF or MRF  options in order to increase the rotational speed?


April 9, 2014, 09:35 

#9 
Senior Member

Well,
in case of MRF you can do it cause omega is defined as follows: Code:
// Angular velocty (rad/sec) autoPtr<DataEntry<scalar> > omega_; Code:
// Revolutions per minute scalar rpm_; 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
OpenFoam1.6ext Allwmake compilation error  one last barrier  Pat84  OpenFOAM Installation  15  July 25, 2012 21:49 
Turbulent flow through a pipe with variable inlet velocity  lobstar  OpenFOAM Running, Solving & CFD  8  March 28, 2012 11:15 
Validation 12.1 vs 6.3, Difference in Reported Inlet Total Pressure  jola  FLUENT  1  May 5, 2011 14:33 
Inlet table in STARCD  Sachin  Siemens  1  March 26, 2008 10:22 
Variable velcity at inlet  John  FLUENT  1  April 7, 2003 11:34 