CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

My simulation stops before last time step (endTime) rhoCentralFoam

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

Like Tree1Likes
  • 1 Post By shock77

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 22, 2021, 10:49
Default My simulation stops before last time step (endTime) rhoCentralFoam
  #1
New Member
 
Rafael Antonio Meņaca Cabrera
Join Date: Jul 2020
Posts: 2
Rep Power: 0
RafaelAMC is on a distinguished road
Hi foamers,

I'm using rhoCentralFoam as solver in order to carry out a simulation of a discharge of air (air flowing through a small space).

The simulation starts without problems but stops before the endTime.

I don't understand why, because it is a transient simulation and it should run the time that I set.

The only reason I can think is maybe occurs a complete discharge of air and the control volume does not have work fluid.

What can I do?

Thanks.
RafaelAMC is offline   Reply With Quote

Old   February 23, 2021, 08:15
Default
  #2
Senior Member
 
anonymous
Join Date: Jan 2016
Posts: 417
Rep Power: 11
simrego is on a distinguished road
Hi!


Include controlDict, log, error message, or something.
Based on this description noone can help you.
simrego is offline   Reply With Quote

Old   February 23, 2021, 11:55
Default
  #3
New Member
 
Rafael Antonio Meņaca Cabrera
Join Date: Jul 2020
Posts: 2
Rep Power: 0
RafaelAMC is on a distinguished road
Sure simrego...

Thanks for your reply.


Boundary conditions:

p
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v1912                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 1e5;

boundaryField
{
    INLET
    {
        type            uniformFixedValue;
		uniformValue table
		(
			(0 3000000)
			(9.26e-05 3000000)
			(0.0001852 3000000)
			(0.0002 3000000)
		);
	}
	
	OUTLET
    {
        type            fixedValue;
		value			uniform 101325;
    }

    SYMMETRY
    {
        type            symmetry;
    }

	WALLS
    {
        type            zeroGradient;
    }

    frontAndBack
    {
        type            empty;
    }
}

// ************************************************************************* //
T

Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v1912                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 1 0 0 0];

internalField   uniform 1;

boundaryField
{
    INLET
    {
        type            uniformFixedValue;
		uniformValue table
		(
			(0 500)
			(9.26e-05 600)
			(0.0001852 550)
			(0.0002 500)
		);
    }
	
	OUTLET
    {
        type            fixedValue;
		value			uniform 300;
    }

    SYMMETRY
    {
        type            symmetry;
    }

	WALLS
    {
        type            zeroGradient;
    }

    frontAndBack
    {
        type            empty;
    }
}


// ************************************************************************* //
U

Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v1912                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    INLET
  
	{
		type pressureInletOutletVelocity;
		value uniform (0 0 0);
	}
    
	
	OUTLET
    {
        type            inletOutlet;
		inletValue		uniform (0 0 0);
		value uniform	(0 0 0);
    }

    SYMMETRY
    {
        type            symmetry;
    }

	WALLS
    {
        type            slip;
    }

    frontAndBack
    {
        type            empty;
    }
}


// ************************************************************************* //
controlDict

Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v1912                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     rhoCentralFoam;

startFrom       startTime;

startTime       0;

stopAt          endTime;

endTime         10000;

deltaT          9.25e-8;

writeControl    adjustable;

writeInterval   9.25e-8;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression off;

timeFormat      general;

timePrecision   6;

runTimeModifiable true;

adjustTimeStep  yes;

maxCo           1;

maxDeltaT       1;


// ************************************************************************* //
The simulation stops without mistakes:

diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal: Solving for rhoUx, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal: Solving for rhoUy, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal: Solving for rhoE, Initial residual = 0, Final residual = 0, No Iterations 0
ExecutionTime = 19.7 s ClockTime = 34 s

Mean and max Courant Numbers = 0.149261 0.407854
deltaT = 9.25e-08
Time = 0.00020091

diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal: Solving for rhoUx, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal: Solving for rhoUy, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal: Solving for rhoE, Initial residual = 0, Final residual = 0, No Iterations 0
ExecutionTime = 19.72 s ClockTime = 34 s

:~/OpenFOAM/OpenFOAM-v1912/proyectos/crevice/crevicesNeue$

Finally, the computational domain (top: inlet; bottom: outlet; and some walls with one side of symmetry)
Attached Images
File Type: png domain.png (14.6 KB, 7 views)
RafaelAMC is offline   Reply With Quote

Old   February 23, 2021, 14:03
Default
  #4
Senior Member
 
Michael Alletto
Join Date: Jun 2018
Location: Bremen
Posts: 524
Rep Power: 10
mAlletto is on a distinguished road
Hello did you notice that the number of iterations are zero. This happens normally if the initial condition of a fluid at rest is consistent with the applied boundary conditions.
Best

Michael
mAlletto is offline   Reply With Quote

Old   February 23, 2021, 16:56
Default
  #5
Senior Member
 
Join Date: Aug 2015
Posts: 494
Rep Power: 12
clapointe is on a distinguished road
I'm not immediately sure why the simulation might stop (is there an error printed at all?), but zero iterations is not uncommon for a rhoCentralFoam case (when diagonal solvers are used -- you can check this by running e.g. the shockTube tutorial. There are some threads on this, e.g. rho residual always zero, why? sonicFoam, OF 5.x) and is not necessarily a cause for alarm.

Caelan
clapointe is offline   Reply With Quote

Old   April 29, 2021, 08:12
Default
  #6
New Member
 
Jason Bavosky
Join Date: Apr 2021
Location: Mumbai
Posts: 12
Rep Power: 2
Jay22kar is on a distinguished road
Hello,

I am facing the same issue although I noticed that the solution runs if you reduce the Courant number.

In your controlDict, reduce the maxCo to 0.5 or 0.25 & then try.
Jay22kar is offline   Reply With Quote

Old   April 30, 2021, 06:36
Default
  #7
Senior Member
 
Join Date: Dec 2019
Posts: 188
Rep Power: 3
shock77 is on a distinguished road
Interestingly I see no real error message. But your boundary conditions are weird.


1. Why do you set your temperature to 1K? Solving the energy equation that way is very troublesome.

2. Dont use fixedValue for p at the inlet and outlet, its very unstable. Use rather totalPressure at the inlet and fixedPressure at the outlet.


3. The stability limit of rhoCentralFoam is Co = 0.5. You should rather use Co = 0.3 or 0.4 with low order schemes or 0.1 and 0.2 for high order schemes.
giovanni.medici likes this.
shock77 is offline   Reply With Quote

Reply

Tags
rhocentralfoam, solvers, timesteps

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
AMI speed performance danny123 OpenFOAM 21 October 24, 2020 05:13
Setting up Lid driven Cavity Benchmark with 1M cells for multiple cores puneet336 OpenFOAM Running, Solving & CFD 11 April 7, 2019 01:58
Extrusion with OpenFoam problem No. Iterations 0 Lord Kelvin OpenFOAM Running, Solving & CFD 8 March 28, 2016 12:08
AMI interDyMFoam for mixer nu problem danny123 OpenFOAM Programming & Development 8 September 6, 2013 03:34
How to write k and epsilon before the abnormal end xiuying OpenFOAM Running, Solving & CFD 8 August 27, 2013 16:33


All times are GMT -4. The time now is 19:01.