CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Post-Processing

postProcess Utility: icoFoam -noFunctionObjects Why?How?

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

Like Tree1Likes
  • 1 Post By wyldckat

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 4, 2016, 06:04
Default postProcess Utility: icoFoam -noFunctionObjects Why?How?
  #1
New Member
 
Teresa
Join Date: Nov 2015
Posts: 22
Rep Power: 5
TeresaT is on a distinguished road
Dear Forum Users,

my goal is to get the wallShearStress of my icoFoam (openFoam 4.0) case. For simpleFoam it is documented in the Userguide:

simpleFoam -postProcess -func wallShearStress

So I tried this:

icoFoam -postProcess -func wallShearStress

Outcome:
Quote:
--> FOAM FATAL ERROR:
Wrong number of arguments, expected 0 found 1
Invalid option: -postProcess
Invalid option: -func
Using: icoFoam -postProcess -help
I get this
Quote:
-noFunctionObjects do not execute functionObjects
Okay, my bad, i should not try to execute functionObjects with icoFoam but how else can I get the wallShearStress of an icoFoam case?

Any Ideas?
Kind regards,
Teresa
TeresaT is offline   Reply With Quote

Old   November 5, 2016, 03:21
Default
  #2
Member
 
Arsalan
Join Date: Jul 2014
Posts: 74
Rep Power: 7
arsalan.dryi is on a distinguished road
Simply run application

Code:
wallShearStress
Regards,
Arsalan.
arsalan.dryi is offline   Reply With Quote

Old   November 5, 2016, 03:34
Default
  #3
New Member
 
Teresa
Join Date: Nov 2015
Posts: 22
Rep Power: 5
TeresaT is on a distinguished road
Hi Arsalan,

this application does not exist in openFoam 4.0.

This is what you get if you try it:
Quote:
$ wallShearStress
wallShearStress has been superceded by the '-postProcess' solver command-line option, e.g.
simpleFoam -postProcess -func wallShearStress
Regards,
Teresa
TeresaT is offline   Reply With Quote

Old   November 13, 2016, 12:42
Default
  #4
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,936
Blog Entries: 42
Rep Power: 119
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 lightwyldckat is a glorious beacon of light
Quick answer: For situations where the solver isn't needed for post-processing, there is the postProcess utility, e.g.:
Code:
postProcess -func wallShearStress
The problem is that icoFoam only handles laminar flow and wallShearStress requires a turbulence model to be used.

The closest would be to switch to pisoFoam, for which you need to update "fv*" files in "system" and add "turbulenceProperties" in the folder "constant".
__________________
wyldckat is offline   Reply With Quote

Old   November 13, 2016, 13:32
Default
  #5
New Member
 
Teresa
Join Date: Nov 2015
Posts: 22
Rep Power: 5
TeresaT is on a distinguished road
Thank you for you help.

I have one more question regardning you tipp: Should I calculate the hole case again oder just use pisofoam for postprocessing the icofoam case?

Kind regards,
Teresa
TeresaT is offline   Reply With Quote

Old   November 13, 2016, 16:07
Default
  #6
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,936
Blog Entries: 42
Rep Power: 119
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 lightwyldckat is a glorious beacon of light
Quick answer: It should work without having to simulate everything again... although I am a bit concerned about the value you've used for "nu" in the "transportProperties" file.

I say this because the icoFoam solver is mostly a simple/basic solver for demonstrating how things work and it doesn't account for all of the physics... which may lead to people to not properly adjust the "nu" value either and instead use the default values from the tutorial cases.
wyldckat is offline   Reply With Quote

Old   November 14, 2016, 03:43
Default
  #7
New Member
 
Teresa
Join Date: Nov 2015
Posts: 22
Rep Power: 5
TeresaT is on a distinguished road
Thanks again!

What physics are you are thinking of? I chose icoFoam because my case has a transient, laminar flow of an incompressible fluid. I usually use normalization so I change the kinematic velocity to reflect the Reynolds-Number.

Greetings,
Teresa
TeresaT is offline   Reply With Quote

Old   November 14, 2016, 17:10
Default
  #8
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,936
Blog Entries: 42
Rep Power: 119
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 lightwyldckat is a glorious beacon of light
Quote:
Originally Posted by TeresaT View Post
What physics are you are thinking of? I chose icoFoam because my case has a transient, laminar flow of an incompressible fluid. I usually use normalization so I change the kinematic velocity to reflect the Reynolds-Number.
Quick answer: Ah, OK, I'm relieved to read that you've made the decision based on facts, therefore I don't see any problems. Just don't forget to set the model in "turbulenceProperties" to use "laminar", so that it's still in reference to the same base modelling strategy as used with icoFoam.

If you only want to calculate wall shear stress, it should work just fine. Because from what I've looked up on the old code in 2.3.x, wall shear stress is essentially:
Code:
const volSymmTensorField Reff(-nu()*dev(twoSymm(fvc::grad(U_))));

        wallShearStress.boundaryField()[patchI] =
        (
           -mesh.Sf().boundaryField()[patchI]
           /mesh.magSf().boundaryField()[patchI]
        ) & Reff.boundaryField()[patchI];
This to say that there are no divergence operators, in which case things could get a big tricky.

Essentially my concern is that if you needed to calculate other properties that depend on how the flow was modelled, pisoFoam accounts for more details that icoFoam doesn't. If you compare the source code of the two solvers, you'll see what I mean.
randolph 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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
icoFoam floating point exception (8) leizhao512 OpenFOAM Running, Solving & CFD 7 November 1, 2018 11:43
postProcess functionality in openFOAM 4 bullmut OpenFOAM Post-Processing 23 July 21, 2017 09:11
Something doens't work with wallHeatFlux utility or externalWallHeatFluxTemperat BC!! zfaraday OpenFOAM Post-Processing 0 February 5, 2015 16:47
[Other] Contribution a new utility: refine wall layer mesh based on yPlus field lakeat OpenFOAM Community Contributions 57 February 1, 2015 08:25
Kubuntu uses dash breaks All scripts in tutorials platopus OpenFOAM Bugs 8 April 15, 2008 07:52


All times are GMT -4. The time now is 16:35.