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

transientSimpleFoam - SIMPLE with time derivatives

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

Like Tree4Likes
  • 2 Post By wyldckat
  • 1 Post By alberto
  • 1 Post By wyldckat

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 14, 2015, 11:21
Default transientSimpleFoam - SIMPLE with time derivatives
  #1
Senior Member
 
shereez234's Avatar
 
M Sereez
Join Date: Jan 2014
Location: England
Posts: 352
Blog Entries: 1
Rep Power: 13
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: http://www.cfd-online.com/Forums/ope...implefoam.html ]

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
 
M Sereez
Join Date: Jan 2014
Location: England
Posts: 352
Blog Entries: 1
Rep Power: 13
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: 1,912
Rep Power: 36
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 (current status: http://albertopassalacqua.com/?p=1541)
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
 
M Sereez
Join Date: Jan 2014
Location: England
Posts: 352
Blog Entries: 1
Rep Power: 13
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
Member
 
W.T
Join Date: Oct 2012
Posts: 35
Rep Power: 13
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
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,974
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
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 and sourav90 like 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: 1,912
Rep Power: 36
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 (current status: http://albertopassalacqua.com/?p=1541)
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
 
M Sereez
Join Date: Jan 2014
Location: England
Posts: 352
Blog Entries: 1
Rep Power: 13
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
 
M Sereez
Join Date: Jan 2014
Location: England
Posts: 352
Blog Entries: 1
Rep Power: 13
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

Old   August 24, 2018, 16:54
Default
  #10
gu1
Senior Member
 
Guilherme
Join Date: Apr 2017
Posts: 216
Rep Power: 9
gu1 is on a distinguished road
Hi,

I edited the original code for OpenFOAM 5.0. Is attached.
I kindly ask them to verify the code (Bruno?), since I did not test them and feedback would be extremely important.
Attached Files
File Type: zip transientSimpleFoam.zip (3.8 KB, 1 views)
gu1 is offline   Reply With Quote

Old   August 24, 2018, 18:26
Default
  #11
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,974
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quick answer: Sorry, but... I already provided the port of this utility for OpenFOAM 5, roughly 30 minutes before your post above, also as an answer to your associated request on that thread:
Quote:
Originally Posted by wyldckat View Post
Greetings Guilherme,

I've now finished porting the code to OpenFOAM 2.3.x, 2.4.x, OpenFOAM 3.0.x, 4.x, 5.x and 6, instructions provided on the front page of the repository: https://github.com/wyldckat/transientSimple

I've updated the wiki section accordingly: https://openfoamwiki.net/index.php/M..._get_the_files

Best regards,
Bruno
So I'm not sure what you want me to look at, given that I already provided the instructions on how to use the updated code with OpenFOAM 5 as well...
wyldckat is offline   Reply With Quote

Old   August 25, 2018, 08:31
Default
  #12
gu1
Senior Member
 
Guilherme
Join Date: Apr 2017
Posts: 216
Rep Power: 9
gu1 is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
Quick answer: Sorry, but... I already provided the port of this utility for OpenFOAM 5, roughly 30 minutes before your post above, also as an answer to your associated request on that thread:

So I'm not sure what you want me to look at, given that I already provided the instructions on how to use the updated code with OpenFOAM 5 as well...
NICE! Very nice !!! I did the update just because I did not find it. And I asked you to check the code because I have not tested it yet ... I'm afraid I'll spread something inefficient.

About the code, I realized that it's a mix between SIMPLE and PISO codes, correct?!
Would it be possible to create a SIMPLE(C) with discretization of time?! Without the PISO loop...
gu1 is offline   Reply With Quote

Old   August 25, 2018, 09:14
Default
  #13
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,974
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quote:
Originally Posted by gu1 View Post
Would it be possible to create a SIMPLE(C) with discretization of time?! Without the PISO loop...
Quick answer: I have no idea, but in principle it should be possible, although I'm not sure if the 'Consistent' mechanisms for SIMPLE are compatible with transient simulations or not.
You will have to study the solvers in more detail to see that for yourself, as well as look for information online about SIMPLEC in general.
wyldckat is offline   Reply With Quote

Old   August 26, 2018, 12:33
Default
  #14
gu1
Senior Member
 
Guilherme
Join Date: Apr 2017
Posts: 216
Rep Power: 9
gu1 is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
Quick answer: I have no idea, but in principle it should be possible, although I'm not sure if the 'Consistent' mechanisms for SIMPLE are compatible with transient simulations or not.
You will have to study the solvers in more detail to see that for yourself, as well as look for information online about SIMPLEC in general.
Bruno,

I have a question and maybe you can help me understand,... I was studying both codes (transientSimpleFoam and simpleFoam) and both contain the term ''p.storePrevIter( )''.
The code (simpleFoam) compiled in current versions of OF does not contain this term... but I think they are included, as this would misrepresent the model of both.
Could you tell where this variable is in the current codes?
gu1 is offline   Reply With Quote

Old   September 1, 2018, 15:08
Default
  #15
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,974
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quick answer:
  • "solutionControl::storePrevIterFields()" e.g. for OpenFOAM 3.0: https://cpp.openfoam.org/v3/a02365.h...b04483ba6a1e2b - called from "simpleControl::loop" and "pimpleControl::loop".
  • It then seems to rely on a semi-automagical methodology that is done in the method "Foam::singleRegionSolutionControl::storePrevIterT ypeFields()" at:
    Code:
    $FOAM_SRC/cfdTools/cfdTools/general/solutionControl/solutionControl/singleRegionSolutionControl/singleRegionSolutionControlTemplates.C
    in OpenFOAM 6.
    • In other words, if I'm seeing this correctly: if each field that is stored on-memory is also being relaxed when solving (see relaxation factors in fvSolution), then if it's being relaxed, then it should also be stored between time steps.
gu1 likes this.
wyldckat is offline   Reply With Quote

Reply

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
[Other] refineWallLayer Error Yuby OpenFOAM Meshing & Mesh Conversion 2 November 11, 2021 12:04
decomposePar problem: Cell 0contains face labels out of range vaina74 OpenFOAM Pre-Processing 37 July 20, 2020 06:38
Floating point exception error lpz_michele OpenFOAM Running, Solving & CFD 53 October 19, 2015 03:50
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 05:35


All times are GMT -4. The time now is 07:07.