# Using a variable (increasing) inlet to get an easy convergence/initialization ?

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

 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 (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);``` My outlet is: 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);``` My wall is: 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);``` My internalFiel is: 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: 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)) );``` which start with 0 velocity at time 0, then grow to Ux=100m/s at time 100, and stay after that (since outOfBound clamp; is the default). 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   Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,691 Rep Power: 28 Well, in case of MRF you can do it cause omega is defined as follows: Code: ```//- Angular velocty (rad/sec) autoPtr > omega_;``` while in SRF there's no such possibility as RPM is defined as Code: ```//- Revolutions per minute scalar rpm_;``` Surely you can make your own SRFModel where RPM is simillar to omega in MRFModel.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Pat84 OpenFOAM Installation 15 July 25, 2012 21:49 lobstar OpenFOAM Running, Solving & CFD 8 March 28, 2012 11:15 jola FLUENT 1 May 5, 2011 14:33 Sachin Siemens 1 March 26, 2008 11:22 John FLUENT 1 April 7, 2003 11:34

All times are GMT -4. The time now is 18:05.