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

Velocity components residuals are missing when running with interDyMFoam

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

Like Tree3Likes
  • 1 Post By wyldckat
  • 1 Post By wyldckat
  • 1 Post By kmefun

Reply
 
LinkBack Thread Tools Display Modes
Old   October 16, 2015, 12:37
Smile Velocity components residuals are missing when running with interDyMFoam
  #1
New Member
 
vsammartano's Avatar
 
Vincenzo
Join Date: Oct 2012
Location: Palermo (IT)
Posts: 11
Rep Power: 6
vsammartano is on a distinguished road
Send a message via Skype™ to vsammartano
Hi there,
I'm quite new to OpenFOAM and I am working on a CFD simulation of a Cross-Flow water Turbine. I have created the OpenFOAM case and the simulation seems to work fine. BUT, during the simulation, in the terminal I can't read the residual of the velocity components. I know that the solver computes those unknowns, I want see these residuals during the simulation.
How can I do that!?
Thanks in advance!
PS: I am using the interDyMFoam solver
vsammartano is offline   Reply With Quote

Old   October 17, 2015, 05:37
Default
  #2
Senior Member
 
Join Date: Jun 2012
Posts: 103
Rep Power: 6
Bazinga is on a distinguished road
how do you start the solver? I just tried a tutorial and the residuals and simulation information were shown in the terminal after I just typed the solver name.
Bazinga is offline   Reply With Quote

Old   October 17, 2015, 14:18
Default
  #3
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,749
Blog Entries: 39
Rep Power: 103
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Quick answer: Check the file "system/fvSolution", search for the block "PIMPLE" and check if this line exists:
Code:
momentumPredictor no;
If you have it defined like this, then this means that the velocity (momentum) equation isn't solved directly.
vsammartano likes this.
wyldckat is offline   Reply With Quote

Old   October 18, 2015, 05:55
Smile ...easy solution!! finally!
  #4
New Member
 
vsammartano's Avatar
 
Vincenzo
Join Date: Oct 2012
Location: Palermo (IT)
Posts: 11
Rep Power: 6
vsammartano is on a distinguished road
Send a message via Skype™ to vsammartano
Quote:
Originally Posted by wyldckat View Post
Quick answer: Check the file "system/fvSolution", search for the block "PIMPLE" and check if this line exists:
Code:
momentumPredictor no;
If you have it defined like this, then this means that the velocity (momentum) equation isn't solved directly.
Dear Bruno, I'm so grateful to you for helping me out! I was stucked! it was such an easy solution ... tomorrow I'll modify the fvSolution file as you told me! YEP!
thank you again!
vsammartano is offline   Reply With Quote

Old   October 18, 2015, 06:05
Smile
  #5
New Member
 
vsammartano's Avatar
 
Vincenzo
Join Date: Oct 2012
Location: Palermo (IT)
Posts: 11
Rep Power: 6
vsammartano is on a distinguished road
Send a message via Skype™ to vsammartano
Quote:
Originally Posted by Bazinga View Post
how do you start the solver? I just tried a tutorial and the residuals and simulation information were shown in the terminal after I just typed the solver name.
Dear Bazinga, thank you for your suggestion. Obviously I started the solver typing the name of the solver in the terminal. I think this is the only way to start a simulation in OpenFOAM.
In my case the problem was that in the fvSolution file, located in the system folder, the momentum equation was not solved directly...thus I caould not find the residuals of the velocity components.

Thank you again!
cheers!
vsammartano is offline   Reply With Quote

Old   October 19, 2015, 07:37
Default
  #6
New Member
 
vsammartano's Avatar
 
Vincenzo
Join Date: Oct 2012
Location: Palermo (IT)
Posts: 11
Rep Power: 6
vsammartano is on a distinguished road
Send a message via Skype™ to vsammartano
Dear Bruno, I modified the fvSolution file as you suggested....it works! Could you please suggest me some reference where I can read how does this solver work? Thank you again,
cheers!
vsammartano is offline   Reply With Quote

Old   October 24, 2015, 13:20
Default
  #7
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,749
Blog Entries: 39
Rep Power: 103
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Quote:
Originally Posted by vsammartano View Post
Could you please suggest me some reference where I can read how does this solver work?
Quick answer: Unfortunately I'm not familiar with any reference documentation for interDyMFoam.
Nonetheless, there is some about interFoam: https://openfoamwiki.net/index.php/InterFoam
The "DyM" part means "Dynamic Mesh" and is a mechanism that is mostly common to all solvers that have this tag in their name. Google:
Code:
OpenFOAM dynamic meshing explained
vsammartano likes this.
wyldckat is offline   Reply With Quote

Old   September 10, 2016, 00:54
Default
  #8
Member
 
carno
Join Date: Mar 2009
Posts: 33
Rep Power: 9
Carno is on a distinguished road
I also have exact same problem. My velocity components are not getting printed on screen to monitor. Here is a log,
Code:
Create time

Create mesh for time = 0


SIMPLE: convergence criteria
    field p      tolerance 0.0001
    field U      tolerance 0.0001
    field "(k|omega|epsilon)"    tolerance 0.0001

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model kOmegaSST
Selecting patchDistMethod meshWave
kOmegaSSTCoeffs
{
    alphaK1         0.85;
    alphaK2         1;
    alphaOmega1     0.5;
    alphaOmega2     0.856;
    gamma1          0.55555556;
    gamma2          0.44;
    beta1           0.075;
    beta2           0.0828;
    betaStar        0.09;
    a1              0.31;
    b1              1;
    c1              10;
    F3              false;
}

Creating MRF zone list from MRFProperties
    creating MRF zone: MRF1
Creating porosity model list from porosityProperties

Porosity region porosity1:
    selecting model: DarcyForchheimer
    creating porous zone: rad
Using pressure implicit porosity
No finite volume options present


Starting time loop

Time = 1

GAMG:  Solving for p, Initial residual = 1, Final residual = 0.0229096, No Iterations 1
time step continuity errors : sum local = 0.16611452, global = -0.013244094, cumulative = -0.013244094
smoothSolver:  Solving for omega, Initial residual = 0.0074746818, Final residual = 1.6552667e-005, No Iterations 1
smoothSolver:  Solving for k, Initial residual = 1, Final residual = 0.0020565579, No Iterations 1
ExecutionTime = 393.767 s  ClockTime = 394 s

Time = 2

GAMG:  Solving for p, Initial residual = 0.99980948, Final residual = 0.028042093, No Iterations 1
time step continuity errors : sum local = 1373.7404, global = -115.04725, cumulative = -115.06049
smoothSolver:  Solving for omega, Initial residual = 0.001862281, Final residual = 2.6651327e-006, No Iterations 1
smoothSolver:  Solving for k, Initial residual = 0.99999977, Final residual = 0.00054471924, No Iterations 1
bounding k, min: -30136.2 max: 40949627 average: 31.478273
ExecutionTime = 547.618 s  ClockTime = 548 s
The part of my fvSolution is as below,
Code:
SIMPLE
{
    residualControl
    {
        p               1e-4;
        U               1e-4;
        "(k|omega|epsilon)" 1e-4;
    }
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;
    nUCorrectors    2;
    momentumPredictor   yes;

}
Kindly help..I am using porousSimpleFoam solver
Carno is offline   Reply With Quote

Old   September 11, 2016, 10:31
Default
  #9
Member
 
Kaufman
Join Date: Jul 2013
Posts: 52
Rep Power: 5
kmefun is on a distinguished road
Quote:
Originally Posted by Carno View Post
I also have exact same problem. My velocity components are not getting printed on screen to monitor. Here is a log,
Code:
Create time

Create mesh for time = 0


SIMPLE: convergence criteria
    field p      tolerance 0.0001
    field U      tolerance 0.0001
    field "(k|omega|epsilon)"    tolerance 0.0001

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model kOmegaSST
Selecting patchDistMethod meshWave
kOmegaSSTCoeffs
{
    alphaK1         0.85;
    alphaK2         1;
    alphaOmega1     0.5;
    alphaOmega2     0.856;
    gamma1          0.55555556;
    gamma2          0.44;
    beta1           0.075;
    beta2           0.0828;
    betaStar        0.09;
    a1              0.31;
    b1              1;
    c1              10;
    F3              false;
}

Creating MRF zone list from MRFProperties
    creating MRF zone: MRF1
Creating porosity model list from porosityProperties

Porosity region porosity1:
    selecting model: DarcyForchheimer
    creating porous zone: rad
Using pressure implicit porosity
No finite volume options present


Starting time loop

Time = 1

GAMG:  Solving for p, Initial residual = 1, Final residual = 0.0229096, No Iterations 1
time step continuity errors : sum local = 0.16611452, global = -0.013244094, cumulative = -0.013244094
smoothSolver:  Solving for omega, Initial residual = 0.0074746818, Final residual = 1.6552667e-005, No Iterations 1
smoothSolver:  Solving for k, Initial residual = 1, Final residual = 0.0020565579, No Iterations 1
ExecutionTime = 393.767 s  ClockTime = 394 s

Time = 2

GAMG:  Solving for p, Initial residual = 0.99980948, Final residual = 0.028042093, No Iterations 1
time step continuity errors : sum local = 1373.7404, global = -115.04725, cumulative = -115.06049
smoothSolver:  Solving for omega, Initial residual = 0.001862281, Final residual = 2.6651327e-006, No Iterations 1
smoothSolver:  Solving for k, Initial residual = 0.99999977, Final residual = 0.00054471924, No Iterations 1
bounding k, min: -30136.2 max: 40949627 average: 31.478273
ExecutionTime = 547.618 s  ClockTime = 548 s
The part of my fvSolution is as below,
Code:
SIMPLE
{
    residualControl
    {
        p               1e-4;
        U               1e-4;
        "(k|omega|epsilon)" 1e-4;
    }
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;
    nUCorrectors    2;
    momentumPredictor   yes;

}
Kindly help..I am using porousSimpleFoam solver
Hi
you can set nUCorrectors 0;
to use pressure explicit porosity and then it will go through the block that solving momentum equation. More details can be referred to the files createPorousZones.H and UEqn.H which located at applications/solvers/incompressible/simpleFoam/porousSimpleFoam/
Hope this could help you.
Carno likes this.

Last edited by kmefun; September 11, 2016 at 22:19.
kmefun is offline   Reply With Quote

Old   September 12, 2016, 11:39
Default
  #10
Member
 
carno
Join Date: Mar 2009
Posts: 33
Rep Power: 9
Carno is on a distinguished road
Thanks ... It works
Carno is offline   Reply With Quote

Reply

Tags
openfoam, residuals, u components

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Calculate velocity components from shear stress Arnoldinho OpenFOAM Running, Solving & CFD 0 August 29, 2011 12:07
ATTENTION! Reliability problems in CFX 5.7 Joseph CFX 14 April 20, 2010 15:45
velocity components at blade tip Sridevi CFX 1 January 9, 2006 02:59
Variables Definition in CFX Solver 5.6 R P CFX 2 October 26, 2004 02:13
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 09:11


All times are GMT -4. The time now is 04:23.