Regarding unbounded alpha values -interFoam

phani45 · July 31, 2017, 07:13

Dear Foamers,

I'm using interFoam for flow over flat plate. Over the course of time I see the alpha values increasing beyond 1. With refined mesh , with all schemes including upwind.

. Can anyone of you help me to overcome this issue

I'm attaching fvschemes,fvsolution and p_rgh files for your perusal.fvSchemes.txt

fvSolution.txt

p_rgh.txt

floquation · July 31, 2017, 07:56

You can use a limited scheme as convective scheme for the alpha equation, for example:

Code:

    div(phi,alpha)  Gauss limitedVanLeer 0 1; //vanLeer;
    div(phirb,alpha) Gauss limitedLinear 0 1; //linear;

Use the banana trick to find out what limited schemes exist in OpenFOAM.

santiagomarquezd · August 25, 2017, 20:29

Hello, the MULES integrator mostly overrides the fluxes computed by the limiters, therefore the whole thing is related to MULES. Try to reduce your time-step or using more nAlphaSubCycles.

Regards.

Elham · July 5, 2018, 04:32

Quote:

Originally Posted by santiagomarquezd

Hello, the MULES integrator mostly overrides the fluxes computed by the limiters, therefore the whole thing is related to MULES. Try to reduce your time-step or using more nAlphaSubCycles.

Regards.

Hi,

As my alpha was unbounded I used the following expression.

Code:

        alpha1=max(scalar(0.0),min(alpha1,scalar(1.0)));

I don't know if there is any issue with it that nobody uses.

Cheers,

Elham

Mahmoud_aboukhedr · March 6, 2019, 08:05

Quote:

Originally Posted by Elham

Hi,

As my alpha was unbounded I used the following expression.

Code:

        alpha1=max(scalar(0.0),min(alpha1,scalar(1.0)));

I don't know if there is any issue with it that nobody uses.

Cheers,

Elham

Where exactly you added this equation ??

santiagomarquezd · March 6, 2019, 09:06

Hello, that method is non-conservative and should be avoided.

Regards

Mahmoud_aboukhedr · March 6, 2019, 09:34

Quote:

Originally Posted by santiagomarquezd

Hello, that method is non-conservative and should be avoided.

Regards

Thanks for your reply, however increasing the nAlphaSubCycles and decreasing the time step does not solve the problem.
Currently, I see an increase in my alpha value due to the unbounded alpha max and min

redTo · May 14, 2020, 11:10

Hi Mahmoud, did you solve this problem? I'm saving the same problem right now with my simulation.

Regards

chivaee · September 25, 2021, 06:05

It may be a little late to give an answer here, but have you tried isoAdvectors i.e., interIsoFoam? It gives bounded alpha.water fields

July 31, 2017, 07:13	Regarding unbounded alpha values -interFoam	#1
phani45 Member Phanindra Join Date: Jan 2013 Posts: 39 Rep Power: 13	Dear Foamers, I'm using interFoam for flow over flat plate. Over the course of time I see the alpha values increasing beyond 1. With refined mesh , with all schemes including upwind. . Can anyone of you help me to overcome this issue I'm attaching fvschemes,fvsolution and p_rgh files for your perusal.fvSchemes.txt fvSolution.txt p_rgh.txt

July 31, 2017, 07:56		#2
floquation Senior Member Kevin van As Join Date: Sep 2014 Location: TU Delft, The Netherlands Posts: 252 Rep Power: 20	You can use a limited scheme as convective scheme for the alpha equation, for example: Code: div(phi,alpha) Gauss limitedVanLeer 0 1; //vanLeer; div(phirb,alpha) Gauss limitedLinear 0 1; //linear; Use the banana trick to find out what limited schemes exist in OpenFOAM.

August 25, 2017, 20:29		#3
santiagomarquezd Senior Member Santiago Marquez Damian Join Date: Aug 2009 Location: Santa Fe, Santa Fe, Argentina Posts: 452 Rep Power: 23	Hello, the MULES integrator mostly overrides the fluxes computed by the limiters, therefore the whole thing is related to MULES. Try to reduce your time-step or using more nAlphaSubCycles. Regards. floquation, SHUBHAM9595, Lorenzo210 and 1 others like this. __________________ Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC) - CONICET/UNL Tel: 54-342-4511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe - Argentina. http://www.cimec.org.ar

March 6, 2019, 09:06		#6
santiagomarquezd Senior Member Santiago Marquez Damian Join Date: Aug 2009 Location: Santa Fe, Santa Fe, Argentina Posts: 452 Rep Power: 23	Hello, that method is non-conservative and should be avoided. Regards erinsam likes this. __________________ Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC) - CONICET/UNL Tel: 54-342-4511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe - Argentina. http://www.cimec.org.ar

September 25, 2021, 06:05		#9
chivaee New Member Hamid Join Date: Mar 2012 Posts: 20 Rep Power: 14	It may be a little late to give an answer here, but have you tried isoAdvectors i.e., interIsoFoam? It gives bounded alpha.water fields Michalis_Loukas likes this.

May 14, 2020, 11:10		#8
redTo New Member Liz Join Date: Apr 2020 Location: Germany Posts: 10 Rep Power: 6	Hi Mahmoud, did you solve this problem? I'm saving the same problem right now with my simulation. Regards

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
interFoam vs. simpleFoam channel flow comparison	DanM	OpenFOAM Running, Solving & CFD	12	January 31, 2020 15:26
Mapping values from 2D mesh to 3D mesh boundary during runtime	benk	OpenFOAM Programming & Development	1	June 13, 2014 02:39
InterFoam - Dambreak - alpha	erncyc	OpenFOAM	0	July 4, 2012 11:18
Bounded scheme gives unbounded solution	su_junwei	OpenFOAM Running, Solving & CFD	3	November 18, 2011 02:35
Alpha to be phased out	Heiko Gerhauser	Main CFD Forum	17	July 25, 2001 14:40