
[Sponsors] 
July 13, 2005, 15:09 
Fatal overflow in linear solver (RSM)

#1 
Guest
Posts: n/a

Hi
I have a two cylinders model connect between them using a small hole (as a domain interface). The objective is using a tangential velocity create a small tornado through the hole. The simulation with the kepsilon model works well, but the model is not able to reproduce good enough the highly turbulence zone inside the vortex. Hence, I switch to the Reynolds stress model with the kepsilon model as initial conditions, but until now no matter what I do, the simulation crash in a fatal overflow in linear solver. What could I do? 

July 14, 2005, 08:28 
Re: Fatal overflow in linear solver (RSM)

#2 
Guest
Posts: n/a

Hi,
After how many iterations does the case crash? When you use higher order turbulence models, you would need to use a smaller time step (steady/trans). Just check if you are using autotiestepping in steady solution. Regards, test 

July 14, 2005, 10:46 
Re: Fatal overflow in linear solver (RSM)

#3 
Guest
Posts: n/a

Hi
I have used a physical timestep of 1x10^5 s. The simulation crash on the 12th iteration. I made a backup on the 11, I checked in the CFXpost, and I found high velocities, around 20,000 m/s (a singularity) in some points. Another thing to mention is that I can't run the simulation using RSM from the beginning because it doesn't start. I need to use a turbulence control with transient factor of 5, which helps the code to run the first iteration as laminar model, the next one as zero eq., and so on, until it gets to the RSM. Finally, I have tried both modes, steadystate and transient, same results. Thank you P.S. Using lower timesteps just make the simulation crash later, for example at the 25. 

July 14, 2005, 23:48 
Re: Fatal overflow in linear solver (RSM)

#4 
Guest
Posts: n/a

Hi,
Difficult to point out the issue without looking at your problem setup, geom and mesh. I can suggest the following though: # Since the problem is crashing very early it can be the issue with the boundary condition. # Try using local timescale factor of about 2 for steady runs. # Test the case with a coarse mesh which will make the solution diffusive. Just need to find out where the error comes from.. Regards, Ananth 

July 18, 2005, 17:27 
Re: Fatal overflow in linear solver (RSM)

#5 
Guest
Posts: n/a

I found the problem, it was the domain interface. Hence, I managed to make a big assembly, and the RSM worked. Thank you for your help guys.


July 7, 2012, 04:42 

#6 
New Member
zoheb
Join Date: Mar 2009
Location: india, mumbai
Posts: 24
Rep Power: 9 
What did you exactly manage to do


July 8, 2012, 07:28 

#7 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,094
Rep Power: 94 
There is an FAQ about linear solver overflow now: http://www.cfdonline.com/Wiki/Ansys...do_about_it.3F


July 9, 2012, 11:45 

#8 
Senior Member

Dear friend, read thoroughly because, KE has some limitations!! and one of them is that is based on eddy viscocity assumption.. and this yield that it can not handle "well" the anysotropy of the field!!
Take a look on the books!! 

May 23, 2013, 10:43 

#9 
Member
Sebastian
Join Date: Apr 2013
Posts: 31
Rep Power: 5 
Hi, I didnt want to make a new thread on this since I have a similar problem.
I attached a picture of the geometry. What I try to do:  The longer cylinder is moving in an oscillating way  the complete room is filled with water  I expect cavitation because of the motion My problem:  fatal overflow in linear solution at around 812 coefficient loop of the very first iteration step  the motion itself works but as soon as I put in a second fluid (water vapour) and enable cavitation I get this problem in the very first timestep. => I tryed to go down with timescale (from 1e6 to 1e12) but it didnt work. The Mesh is refined in the area where the cavitation is expected edit: I try to simplify the problem as much as possible, so I have no turbulence modell and adiabatic walls. (heat transfer: total energy) 

May 24, 2013, 06:19 

#10 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,094
Rep Power: 94 
Combining a FSI and cavitation simulation is always going to be difficult. You should expect convergence difficulties in a simulation like this.
Why are you modelling heat transfer? Most people most cavitation as isothermal. The cavitation model in CFX assumes isothermal behaviour. Have a look at the cavitation example in the CFX, cavitating flow over a hydrofoil. And: Removing the turbulence model does NOT simplify the problem! It causes problems and makes it harder to converge  this itself might explain your convergence difficulties! If the flow is turbulent you need a turbulence model to get sufficient dissipation for the model to converge. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Linear Solver  Argen  OpenFOAM  3  October 10, 2011 01:17 
free C code for large sparse matrix linear solver  ztdep  Main CFD Forum  7  May 24, 2007 14:14 
Fatal overflow in linear solver error. Why?  zaidun  CFX  3  June 9, 2006 09:12 
Solver: Fatal Bounds error detected  hagupta  CFX  5  March 24, 2006 11:17 
solver for linear system with large sparse matrix  Yangang Bao  Main CFD Forum  1  October 25, 1999 04:22 