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

transientSimpleFoam - SIMPLE with time derivatives

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

Like Tree2Likes
  • 1 Post By wyldckat
  • 1 Post By alberto

Reply
 
LinkBack Thread Tools Display Modes
Old   December 14, 2015, 11:21
Default transientSimpleFoam - SIMPLE with time derivatives
  #1
Senior Member
 
shereez234's Avatar
 
shereez
Join Date: Jan 2014
Location: England
Posts: 200
Rep Power: 5
shereez234 is on a distinguished road
The explanation in the top of the source file in this solver says " For non-Newtonian fluid'' which questions me. Was this Solver really built for Non-Newtonian fluids Bruno?

[ Moderator note: Moved from this thread: transient simpleFoam ]

Last edited by wyldckat; December 28, 2015 at 16:25. Reason: see "Moderator note:"
shereez234 is offline   Reply With Quote

Old   December 26, 2015, 14:01
Default transientSimpleFoam - SIMPLE with time derivatives
  #2
Senior Member
 
shereez234's Avatar
 
shereez
Join Date: Jan 2014
Location: England
Posts: 200
Rep Power: 5
shereez234 is on a distinguished road
Hello Everyone;

Hope every one is doing great !

Has any one used this solver which is supposed to be SIMPLE but with time derivatives so ( unsteady simple foam).

My only concern is it says that it is for non- newtonian flow in the source file.
Is this true?

Here is the link:
https://github.com/wyldckat/transien...ientSimpleFoam

I saw a post where Prof Jasak said that transientSimple algorithm can be used for large courant number flows. So I am really keen to use this solver. Furthermore has any one coded SIMPLEC or SIMPLER for transient ?

Regards and have a good day!!

Shereez
shereez234 is offline   Reply With Quote

Old   December 26, 2015, 23:13
Default
  #3
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 27
alberto will become famous soon enoughalberto will become famous soon enough
You can use pimpleFoam instead.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats.
OpenQBMM - An open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   December 27, 2015, 11:05
Default
  #4
Senior Member
 
shereez234's Avatar
 
shereez
Join Date: Jan 2014
Location: England
Posts: 200
Rep Power: 5
shereez234 is on a distinguished road
Quote:
Originally Posted by alberto View Post
You can use pimpleFoam instead.
Dear alberto;

Many thanks for the reply. I have had previous tries trying to run pimpleFoam for cases. The thing is I am running airfoil vortex shedding cases and depending on the strouhal number some of the Time periods are 0.2 seconds, 1 seconds or even 5 seconds.

And pimpleFoam stability blows up above any courant number 20 not even menioning about the accuracy of the solution. however the transient Simple Foam I have compiled can handle and converge any courant number. My only concern is that it says in the source file description that it is for non- newtonian flows which I don't understand why.

But once again, many thanks for your suggestion.

Regards

Shereez
shereez234 is offline   Reply With Quote

Old   December 28, 2015, 04:00
Default
  #5
New Member
 
W.T
Join Date: Oct 2012
Posts: 19
Rep Power: 6
dybuk is on a distinguished road
In transportProperties file yuo can chose any single phase transport model, including nonNewtonian and IMO thats is a reason.
dybuk is offline   Reply With Quote

Old   December 28, 2015, 13:56
Default
  #6
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,748
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
Greetings to all!

@Shereez:
Quote:
Originally Posted by shereez234 View Post
The explanation in the top of the source file in this solver says " For non-Newtonian fluid'' which questions me. Was this Solver really built for Non-Newtonian fluids Bruno?
According to the source code, it was designed in a way that can work with Newtonian and Non-Newtonian fluids. If you check the contents of the file "createFields.H": https://github.com/wyldckat/transien...teFields.H#L37 - you will find these lines near the end:
Code:
    singlePhaseTransportModel laminarTransport(U, phi);

    //autoPtr<incompressible::RASModel> turbulence
    autoPtr<incompressible::turbulenceModel> turbulence
    (
        //incompressible::RASModel::New(U, phi, laminarTransport)
        incompressible::turbulenceModel::New(U, phi, laminarTransport)
    );
This means that the file "transportProperties" will be loaded by the object "laminarTransport" and subsequently used by the "turbulence" (model) object. This means that the dynamic viscosity "nu" will be loaded from "transportProperties" file and the respective transport model will be used, may it be Newtonian or Non-Newtonian.

How do I know it is the file "transportProperties" that is loaded? Check the file pointed out by this command:
Code:
echo $FOAM_SRC/transportModels/incompressible/singlePhaseTransportModel/singlePhaseTransportModel.C
You can also see it online for 3.0.x: https://github.com/OpenFOAM/OpenFOAM...ortModel.C#L33

Best regards,
Bruno
shereez234 likes this.
__________________

Last edited by wyldckat; December 28, 2015 at 16:26. Reason: edited the header to greet everyone, not just Shereez
wyldckat is offline   Reply With Quote

Old   December 28, 2015, 14:31
Default
  #7
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 27
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by shereez234 View Post
Dear alberto;

Many thanks for the reply. I have had previous tries trying to run pimpleFoam for cases. The thing is I am running airfoil vortex shedding cases and depending on the strouhal number some of the Time periods are 0.2 seconds, 1 seconds or even 5 seconds.

And pimpleFoam stability blows up above any courant number 20 not even menioning about the accuracy of the solution. however the transient Simple Foam I have compiled can handle and converge any courant number. My only concern is that it says in the source file description that it is for non- newtonian flows which I don't understand why.

But once again, many thanks for your suggestion.

Regards

Shereez
If your are interested in having a time-resolved simulation, your Courant number should be less than 1. Using anything larger would not be appropriate.

For what I know transientSimpleFoam is not part of OpenFOAM either...
shereez234 likes this.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats.
OpenQBMM - An open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   December 28, 2015, 16:20
Default
  #8
Senior Member
 
shereez234's Avatar
 
shereez
Join Date: Jan 2014
Location: England
Posts: 200
Rep Power: 5
shereez234 is on a distinguished road
Quote:
Originally Posted by alberto View Post
If your are interested in having a time-resolved simulation, your Courant number should be less than 1. Using anything larger would not be appropriate.

For what I know transientSimpleFoam is not part of OpenFOAM either...
Dear Alberto. Yes I am aware that courant number needs to be limited to 1 for piso or if I am interested in small time scale unsteadiness.

But for instance consider a case like this :

A vortex shedding case for which Force convergence has a periodic solution which has a Frequency of 4Hz : --> so Time period = 1/4 = 0.25 seconds.

Let's assume that this case is for reynolds number = 1 million. Which means to have a courant number of 1 or below I will need a DT = 1e-05 seconds or lower. So one complete wave length of the force curve can be computed using 20,000 time steps. Which is computationally expensive.

One of my professors pointed out to me that if I can place 100 or 200 points in one time period ( One wave length) then this should lead to a good estimate of the periodic shedding pattern that we are interested in.

So I believe if I can have a DT = 0.002 seconds I should still be able to capture the unsteadiness that I am interested in. Or not Well, I will see.

Best Regards

Shereez
shereez234 is offline   Reply With Quote

Old   December 29, 2015, 08:20
Default
  #9
Senior Member
 
shereez234's Avatar
 
shereez
Join Date: Jan 2014
Location: England
Posts: 200
Rep Power: 5
shereez234 is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
Greetings to all!

@Shereez:

According to the source code, it was designed in a way that can work with Newtonian and Non-Newtonian fluids. If you check the contents of the file "createFields.H": https://github.com/wyldckat/transien...teFields.H#L37 - you will find these lines near the end:
Code:
    singlePhaseTransportModel laminarTransport(U, phi);

    //autoPtr<incompressible::RASModel> turbulence
    autoPtr<incompressible::turbulenceModel> turbulence
    (
        //incompressible::RASModel::New(U, phi, laminarTransport)
        incompressible::turbulenceModel::New(U, phi, laminarTransport)
    );
This means that the file "transportProperties" will be loaded by the object "laminarTransport" and subsequently used by the "turbulence" (model) object. This means that the dynamic viscosity "nu" will be loaded from "transportProperties" file and the respective transport model will be used, may it be Newtonian or Non-Newtonian.

How do I know it is the file "transportProperties" that is loaded? Check the file pointed out by this command:
Code:
echo $FOAM_SRC/transportModels/incompressible/singlePhaseTransportModel/singlePhaseTransportModel.C
You can also see it online for 3.0.x: https://github.com/OpenFOAM/OpenFOAM...ortModel.C#L33

Best regards,
Bruno

Bruno;

I did not see your reply until now. that's great news. thanks very much

Regards

shereez
shereez234 is offline   Reply With Quote

Reply

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
decomposePar problem: Cell 0contains face labels out of range vaina74 OpenFOAM Pre-Processing 27 November 2, 2015 18:04
Floating point exception error lpz_michele OpenFOAM Running, Solving & CFD 53 October 19, 2015 02:50
refineWallLayer Error Yuby OpenFOAM Meshing & Mesh Conversion 0 April 27, 2015 18:25
pisoFoam with k-epsilon turb blows up - Some questions Heroic OpenFOAM Running, Solving & CFD 26 December 17, 2012 04:34
calculation diverge after continue to run zhajingjing OpenFOAM 0 April 28, 2010 04:35


All times are GMT -4. The time now is 11:12.