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

rhoSimpleFoam div(phi,k/K) 2.1.x 2.0.x

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 31, 2013, 10:09
Default rhoSimpleFoam div(phi,k/K) 2.1.x 2.0.x
  #1
Member
 
Martin
Join Date: Nov 2011
Posts: 30
Rep Power: 5
wernsen is on a distinguished road
Dear Foamers,

I am having trouble with a rhoSimpleFoam case which is running under 2.0.x without a problem. If I try to run this case under 2.1.x I am gettin the Fatal Error:

Code:
--> FOAM FATAL IO ERROR: 
keyword div(phi,K) is undefined in dictionary
What is the capital K and why do I need it since in 2.0.x it is not necessary?

thx
martin
wernsen is offline   Reply With Quote

Old   January 31, 2013, 10:24
Default
  #2
Senior Member
 
Join Date: Nov 2009
Location: Michigan
Posts: 135
Rep Power: 7
doubtsincfd is on a distinguished road
something is missing in fvSchemes

It might also be a missing comma or a {

Try giving a default scheme for div
doubtsincfd is offline   Reply With Quote

Old   January 31, 2013, 10:42
Default
  #3
Member
 
Martin
Join Date: Nov 2011
Posts: 30
Rep Power: 5
wernsen is on a distinguished road
my fvSchemes::divSchemes looks like that:

Code:
divSchemes
{
   default            none;
   div(phi,U)                     Gauss upwind;
   div(phi,h)                     Gauss upwind;
   div(phi,k)                     Gauss upwind;
   div(phi,epsilon)               Gauss upwind;
   div(phi,omega)                 Gauss upwind;
   div(U,p)                     Gauss linear;
   dic(phi)              Gauss linear;
   div((muEff*dev2(T(grad(U)))))  Gauss linear;
}
so I already have a scheme for the div(phi,k) but not for div(phi,K) which confuses me. So what is the K?
wernsen is offline   Reply With Quote

Old   January 31, 2013, 11:06
Default
  #4
Member
 
Join Date: Jun 2012
Posts: 67
Rep Power: 5
maHein is on a distinguished road
The formulation of the energy equation has changed from 2.0.x to 2.1x. In the later one, the divergence on the kinetic energy K is part of it. That's why you need div(phi,K) in your fvSchemes. See line 8 of the hEqn.H file:

Code:
- fvc::div(phi, 0.5*magSqr(U), "div(phi,K)")
By the way, I noticed considerable differences between results from both versions. I tested both for turbomachinery simulation and the 2.1.x resulted in negative isentropic efficiencies. So make sure to compare both results and see if they are reasonable.
maHein is offline   Reply With Quote

Old   February 4, 2013, 03:43
Default
  #5
Member
 
Martin
Join Date: Nov 2011
Posts: 30
Rep Power: 5
wernsen is on a distinguished road
Thank You very much "maHein"!
wernsen is offline   Reply With Quote

Old   February 20, 2015, 10:12
Default
  #6
New Member
 
Eugen
Join Date: Sep 2014
Posts: 18
Rep Power: 2
estang is on a distinguished road
Quote:
Originally Posted by maHein View Post
The formulation of the energy equation has changed from 2.0.x to 2.1x. In the later one, the divergence on the kinetic energy K is part of it. That's why you need div(phi,K) in your fvSchemes. See line 8 of the hEqn.H file:

Code:
- fvc::div(phi, 0.5*magSqr(U), "div(phi,K)")
By the way, I noticed considerable differences between results from both versions. I tested both for turbomachinery simulation and the 2.1.x resulted in negative isentropic efficiencies. So make sure to compare both results and see if they are reasonable.
I use Version 2.3.0 and i do not understand why the angledDuctExplicitFixedCoeff tutorial for rhoSimpleFoam runs with
Code:
div(phi,k)      bounded Gauss upwind;
and the same fvSchemes file doesn't work with my case.

I get the following errormessage:
Quote:
--> FOAM FATAL IO ERROR:
keyword div(phi,K) is undefined in dictionary "/home/estang/OpenFOAM/estang-2.3.0/run/2_fluid_Testcase_comp_heat_transfer/system/fvSchemes.divSchemes"

file: /home/estang/OpenFOAM/estang-2.3.0/run/2_fluid_Testcase_comp_heat_transfer/system/fvSchemes.divSchemes from line 30 to line 40.

From function dictionary::lookupEntry(const word&, bool, bool) const
in file db/dictionary/dictionary.C at line 437.

FOAM exiting
i just want to understand
estang is offline   Reply With Quote

Old   February 20, 2015, 11:01
Default
  #7
Member
 
Join Date: Jun 2012
Posts: 67
Rep Power: 5
maHein is on a distinguished road
It is a capital "k" in your warning: div(phi, K).
maHein is offline   Reply With Quote

Old   February 23, 2015, 02:20
Default
  #8
New Member
 
Eugen
Join Date: Sep 2014
Posts: 18
Rep Power: 2
estang is on a distinguished road
Quote:
Originally Posted by maHein View Post
It is a capital "k" in your warning: div(phi, K).
That's why i'm asking here in this thread. I copied the fvSchemes without any edit from the tutorial. I can run the tutorial but when i try to run my own case with the same fvSchemes the solver complains. Shouldn't the same message appear with running the tutorial case?
estang is offline   Reply With Quote

Old   February 24, 2015, 04:32
Default
  #9
Member
 
Join Date: Jun 2012
Posts: 67
Rep Power: 5
maHein is on a distinguished road
You have to check whether you use sensibleEnthalpy or sensibleInternalEnergy in your thermodynamicProperties. This changes the form of the energy equation and thus introduces different terms such as div(phi,K).
maHein is offline   Reply With Quote

Old   February 24, 2015, 04:52
Thumbs up
  #10
New Member
 
Eugen
Join Date: Sep 2014
Posts: 18
Rep Power: 2
estang is on a distinguished road
Thank you very much.

Bad that i didn't see the difference in my thermophysical Properties before.

I should have a look to the different formulations.
estang 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
Pressure instability with rhoSimpleFoam philipp. OpenFOAM 7 July 27, 2015 09:31
transsonic nozzle with rhoSimpleFoam Unseen OpenFOAM Running, Solving & CFD 7 April 16, 2014 03:38
Installation on Ubuntu 12.04 LTS samiam1000 OpenFOAM Installation 11 May 26, 2012 05:54
Transonic rhoSimpleFoam Equations eric.m.tridas OpenFOAM 3 January 25, 2012 11:52
Problem with rhoSimpleFoam mecbe2002 OpenFOAM 3 April 11, 2010 00:54


All times are GMT -4. The time now is 02:05.