CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

cfx strange error

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 23, 2011, 14:30
Default cfx strange error
  #1
Senior Member
 
Join Date: Jan 2010
Posts: 110
Rep Power: 7
antonio is on a distinguished road
I am trying to simulate the propagation of particles in the last few meters of a reservoir (incluind the dam section) using the algebraic slip model and I am receiving the following error message:
+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine FPX: c_fpx_handler |
|

Does anyone knows what causes this?
I have defined the following boundary conditions:
- at inlet velocity and the mass fraction;
-at the outlet a smooth no slip wall;
-at the bottom and the lateral parts of the model a rough no slip wall
-in the top of my domain I have specified an opening boundary with the following features:
-relative pressure equal to the height of the flow that is above of my domain
-pressure option assigned to opening pressure
-low turbulence intensity
-mass fraction equal to zero
In doing so, I am trying to model not the entire height of the dam but just a few meters from the bottom (where the sediments will be accumulated). Furthmore, I have defined the reference pressure equal to the pressure correponding to the height of the flow above the domain, velocities equal to zero, an hydrostatic pressure distribution, and mass fraction equal to zero as initial conditions.

What can be wrong in this approach?Many thanks.
antonio is offline   Reply With Quote

Old   December 23, 2011, 14:37
Default
  #2
Senior Member
 
Join Date: Jan 2010
Posts: 110
Rep Power: 7
antonio is on a distinguished road
-at the top boundary I have choosed the entrainment option
antonio is offline   Reply With Quote

Old   December 24, 2011, 05:38
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Is it a floating point error? If so then this means your simulation has diverged. Need to improve numerical stability.
ghorrocks is offline   Reply With Quote

Old   December 26, 2011, 13:56
Default
  #4
Senior Member
 
Join Date: Jan 2010
Posts: 110
Rep Power: 7
antonio is on a distinguished road
It is a floating point error and a little bit surprisingly (at least for me) by changing the initial level of turbulence in domain the error disappears. I had k=epsilon=0 and now I have low level of turbulence (I=1%)..
antonio is offline   Reply With Quote

Old   December 27, 2011, 06:07
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You cannot have epsilon = 0. It leads to a divide by zero error on the turbulent viscosity - ie a floating point error This does not sound surprising at all to me.
ghorrocks is offline   Reply With Quote

Old   December 27, 2011, 06:13
Default
  #6
Senior Member
 
Join Date: Jan 2010
Posts: 110
Rep Power: 7
antonio is on a distinguished road
Well seen.
antonio is offline   Reply With Quote

Old   December 27, 2011, 06:24
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Well, the e based turbulence model cannot have epsilon=0 as the turbulent viscosity goes undefined. This is a key failing of these models and is why they cannot model low Re flows or transitional flows. This is one of the key advantages of omage based turbulence models, and why the omega turbulence models are used in the vast majority of these sort of flows.

So not so much a "well seen" as an example of a well known fundamental failing of epsilon based turbulence models.
ghorrocks 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
polynomial thermophysical properties II sebastian OpenFOAM Running, Solving & CFD 53 April 10, 2014 05:45
OpenFOAM install on Ubuntu Natty 11.04 bkubicek OpenFOAM 13 May 26, 2011 05:48
ParaView for OF-1.6-ext Chrisi1984 OpenFOAM Installation 0 December 31, 2010 07:42
OpenFOAM on MinGW crosscompiler hosted on Linux allenzhao OpenFOAM Installation 127 January 30, 2009 20:08
DecomposePar links against liblamso0 with OpenMPI jens_klostermann OpenFOAM Bugs 11 June 28, 2007 17:51


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