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

LinkBack  Thread Tools  Display Modes 
March 28, 2013, 03:32 
Using a variable (increasing) inlet to get an easy convergence/initialization ?

#1 
Senior Member
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 237
Rep Power: 10 
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, 10:04 

#2 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 265
Rep Power: 11 
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, 14:54 

#3 
Senior Member
Jose Rey
Join Date: Oct 2012
Posts: 131
Rep Power: 10 
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 15:24. 

March 29, 2013, 04:23 

#4 
Senior Member
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 237
Rep Power: 10 
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, 06:00 

#5 
Senior Member
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 237
Rep Power: 10 
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: 265
Rep Power: 11 
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: 237
Rep Power: 10 
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: 5 
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  
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 11:22 
Variable velcity at inlet  John  FLUENT  1  April 7, 2003 11:34 