# Fatal overflow in linear solver (RSM)

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 July 13, 2005, 15:09 Fatal overflow in linear solver (RSM) #1 Luis 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 k-epsilon 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 k-epsilon 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 test 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 auto-tiestepping in steady solution. Regards, test

 July 14, 2005, 10:46 Re: Fatal overflow in linear solver (RSM) #3 Luis 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 CFX-post, 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, steady-state 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 test 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 Luis 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: 8 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: 10,797 Rep Power: 84 There is an FAQ about linear solver overflow now: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

 July 9, 2012, 11:45 #8 Senior Member   Julio Mendez Join Date: Apr 2009 Location: Greensboro, U.S.A Posts: 104 Rep Power: 8 Dear friend, read thoroughly because, K-E 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!! zobekenobe likes this.

May 23, 2013, 10:43
#9
Member

Sebastian
Join Date: Apr 2013
Posts: 31
Rep Power: 4
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 8-12 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 1e-6 to 1e-12) 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)
Attached Images
 sonotrode.jpg (21.1 KB, 36 views)

 May 24, 2013, 06:19 #10 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,797 Rep Power: 84 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 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 Argen OpenFOAM 3 October 10, 2011 01:17 ztdep Main CFD Forum 7 May 24, 2007 14:14 zaidun CFX 3 June 9, 2006 09:12 hagupta CFX 5 March 24, 2006 11:17 Yangang Bao Main CFD Forum 1 October 25, 1999 04:22

All times are GMT -4. The time now is 07:15.

 Contact Us - CFD Online - Top