# cfx strange error

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

 December 23, 2011, 14:30 cfx strange error #1 Senior Member   Join Date: Jan 2010 Posts: 110 Rep Power: 7 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.

 December 23, 2011, 14:37 #2 Senior Member   Join Date: Jan 2010 Posts: 110 Rep Power: 7 -at the top boundary I have choosed the entrainment option

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

 December 26, 2011, 13:56 #4 Senior Member   Join Date: Jan 2010 Posts: 110 Rep Power: 7 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%)..

 December 27, 2011, 06:07 #5 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,803 Rep Power: 85 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.

 December 27, 2011, 06:13 #6 Senior Member   Join Date: Jan 2010 Posts: 110 Rep Power: 7 Well seen.

 December 27, 2011, 06:24 #7 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,803 Rep Power: 85 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.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post sebastian OpenFOAM Running, Solving & CFD 53 April 10, 2014 05:45 bkubicek OpenFOAM 13 May 26, 2011 05:48 Chrisi1984 OpenFOAM Installation 0 December 31, 2010 07:42 allenzhao OpenFOAM Installation 127 January 30, 2009 20:08 jens_klostermann OpenFOAM Bugs 11 June 28, 2007 17:51

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