|
[Sponsors] |
Using a variable (increasing) inlet to get an easy convergence/initialization ? |
|
LinkBack | Thread Tools | Search this Thread | 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: 249
Rep Power: 17 |
Dear all,
I'm running some simulations with rhoSimplecFoam (k-epsilon, 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 2.15e-1; k: type fixedValue; value uniform 1.6e-2; 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 2.15e-1; value uniform 2.15e-1; k: type inletOutlet; inletValue uniform 1.6e-2; value uniform 1.6e-2; 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 2.15e-1; k: type compressible::kqRWallFunction; value uniform 1.6e-2; 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 2.15e-1; k: value uniform 1.6e-2; 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: 272
Rep Power: 18 |
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: 134
Rep Power: 18 |
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: 249
Rep Power: 17 |
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: 249
Rep Power: 17 |
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, 07:22 |
|
#6 |
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 272
Rep Power: 18 |
hello,
You may try to modify the outlet BC: -p : totalPressure - U pressureInletOutletVelocity (or pressureInletVelocity / pressureDirectedInletVelocity / ...) regards, olivier |
|
April 2, 2013, 10:02 |
|
#7 |
Senior Member
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 249
Rep Power: 17 |
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, 09:01 |
|
#8 |
Member
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 13 |
is it possible to use such table options for the SRF or MRF - options in order to increase the rotational speed?
|
|
April 9, 2014, 10:35 |
|
#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_; |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
OpenFoam-1.6-ext Allwmake compilation error - one last barrier | Pat84 | OpenFOAM Installation | 15 | July 25, 2012 22:49 |
Turbulent flow through a pipe with variable inlet velocity | lobstar | OpenFOAM Running, Solving & CFD | 8 | March 28, 2012 12:15 |
Validation 12.1 vs 6.3, Difference in Reported Inlet Total Pressure | jola | FLUENT | 1 | May 5, 2011 15:33 |
Inlet table in STAR-CD | Sachin | Siemens | 1 | March 26, 2008 11:22 |
Variable velcity at inlet | John | FLUENT | 1 | April 7, 2003 12:34 |