
[Sponsors] 
September 27, 2013, 15:01 
Fatal overflow in linear solver

#1 
Senior Member
ali
Join Date: Oct 2009
Posts: 288
Rep Power: 11 
Hi,
I am simulating air flow around a turbine blade. I can obtain the solution when turbulence model is set to Kepsilon and KOmega. When I want to run the case with SST, I receive the following error message. The solver crashes in the very first iteration. The simulation is steady state. I have reduced the timescale factor to 1e6 and moved the boundaries away from the blade and also increased the memory allocation factor. p, li { whitespace: prewrap; } ++  ERROR #004100018 has occurred in subroutine FINMES.   Message:   Fatal overflow in linear solver.  ++ Any suggestions? Thanks 

September 28, 2013, 13:27 

#2 
Member
Mohamad Alagheband
Join Date: Oct 2012
Posts: 41
Rep Power: 7 
if your mesh is quite fine ,try changing relaxation factors.
I've got this problem,different case ,after changing relaxation factors in expert parameter it started to run 

September 30, 2013, 09:42 

#3 
Senior Member
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 13 
Did you try with local timescales?


September 30, 2013, 18:21 

#4 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 14,088
Rep Power: 109 
This is an FAQ: http://www.cfdonline.com/Wiki/Ansys...do_about_it.3F


October 9, 2013, 02:39 

#5 
Senior Member
ali
Join Date: Oct 2009
Posts: 288
Rep Power: 11 
Thanks,
I fixed that issue for steady state case. Now that I want to solve the case for transient case I receive the exact same error again. Now what I can do? I have tried decreasing time step size and used the steady case solution for initializing the domain. Generally what should one do when encountered by this error in transient simulations? We do not have physical timescales any more to play with to overcome this error and obtain solution. 

October 9, 2013, 02:49 

#6  
Senior Member
ali
Join Date: Oct 2009
Posts: 288
Rep Power: 11 
Quote:
Thanks. I solved this issue for steady case but still have problem in unsteady case. Where in expert parameters I can set underrelaxation factor? I cannot find it. Btw what is the difference between underrelaxation factor and physical timescale for steady simulation? Thanks 

October 9, 2013, 05:39 

#7  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 14,088
Rep Power: 109 
Quote:
Quote:


February 19, 2016, 05:05 
Fatal over flow error

#8 
New Member
Join Date: Feb 2012
Posts: 14
Rep Power: 7 
Hi,
I am trying to simulate an axial flow turbine rotor in CFX. I used Meshing tool to generate mesh. A fully hexagonal mesh has been generated. In CFX Solver, after 2025 iterations simulation diverges giving "fatal over flow error in linear solver." A steady state analysis, and I used SST turbulence model. I tried different time scales, but could not overcome the the divergence problem. Also, I tried to improve mesh quality. With different mesh spesifications, I got the same error. Any suggestions? Thanks 

February 19, 2016, 05:23 

#9  
Senior Member
Maxim
Join Date: Aug 2015
Location: Germany
Posts: 389
Rep Power: 5 
Have you tried all the other things mentioned here?
Quote:


February 19, 2016, 05:56 
Fatal

#10 
New Member
Join Date: Feb 2012
Posts: 14
Rep Power: 7 
Hi Maxim,
I have checked and tried most of them but transient simution. I will run a transient simulation in order to determine an appropriate time scale. Then I will let you know. In my previous studies the simulations converged. When I changed the tip clearance of squealer geometry, I encoundered this divergence problem. I checked if it is related to the geometry, but I havent found anything related to the geometry. Thanks 

February 26, 2016, 05:49 
Fatal over flow error

#11 
New Member
Join Date: Feb 2012
Posts: 14
Rep Power: 7 
Hi Maxim,
I tried different time scales and meshes for the calculations. I thought it may be due to min value of "Orthog. Angle", therefore I tried to improve the mesh. Min "Orthog. Angle" has been increased up to 32 deg. However, it did not help to converge. Then I used various physical time steps. I ended the analysis before it diverges to see what is wrong. Max value of the Courant number is too high. I have read that there is o requier Courant number to be small. But, I reduced the time scale considerably to reduce the Courant number. After that I noticed that run diverges later. After some runs, I had a solution without energy equation to see the results were acceptable. Generally the results are ok but some total pressure distributions are not physically acceptable. I carried on the run. (By the way, the number of elements in my cases are quite high to keep the y plus values at acceptable levels) Do you think it is all about Courant number for a steady state analysis? thanks 

February 26, 2016, 05:57 

#12  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 14,088
Rep Power: 109 
Quote:
If you have: * Checked your simulation is valid and correctly set up * Made the time step very small * Got the best mesh you can * Tried double precision * Use the best initial conditions you can (these are all listed in the FAQ, of course) If you have done all those things and it is still not converging then your only real option is to do a transient simulation and march it to steady state in a time resolved model. This is much slower, but convergence is much more reliable. Use adaptive time stepping homing in on 35 coeff loops per iteration so the solver can find its own time step size. Don't guess a time step size, you will invariably get it wrong  and don't limit the time step size the solver can use, if it needs a very big or small time step let it. 

February 26, 2016, 06:16 

#13 
New Member
Join Date: Feb 2012
Posts: 14
Rep Power: 7 
Hi Maxim,
I think I did the all steps. I tried to get a thinner boundary layer since very high velocity values near the suction side, at singular points. I also tried transient simulations. With a few trials I achieved to reduce Courant number to acceptable levels which are given in CFX tutorials. But I could not get a solution. I will run some transient solutions. Thanks 

February 26, 2016, 06:39 

#14 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 14,088
Rep Power: 109 
Don't use Courant number as a guide. As I said, Courant number does not have a major effect on implicit solvers. Use convergence and accuracy considerations instead.


February 26, 2016, 07:18 

#15 
Senior Member
Maxim
Join Date: Aug 2015
Location: Germany
Posts: 389
Rep Power: 5 
It seems that I am late to the party now  Glenn already pointed out the ideas/suggestions I would have had, too.
As far I as know, the Courant Number ideally should be below 30 but since it corresponds directly to your selected timestep, it doesn't help as a criteria for convergence. I found some training material slides from ansys in the www  I hope I'm allowed to link it here. They talk about the Courant number and suggest typical values of 210. But as Glenn said, the Courant number isn't important for steadystate simulations. Maybe you can post your ccl and out files and we could have a look. I'm sure you started with Auto Timescale for your steadystate calculation and tried different factors? 

February 26, 2016, 07:44 

#16 
New Member
Join Date: Feb 2012
Posts: 14
Rep Power: 7 
Thanks Glenn.
I will run a transient simulation considering your suggestions. Maxim, I started from auto time scale then tried various time scales. I just ended a simulation. The simulation didnt diverge. A good point. But this time physical time scales is lower. Now, I will do some post process to see whether the results are acceptable or not. thanks 

February 26, 2016, 09:03 
Fatal over flow error

#17 
New Member
Join Date: Feb 2012
Posts: 14
Rep Power: 7 
Hi,
I am sending one of the out files. Physical time scale was 0.001 in this case. Thanks 

February 27, 2016, 04:26 

#18 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 14,088
Rep Power: 109 
You have some translational periodic interfaces. What are they doing? This seems unusual in a rotating machine simulation. Can you show your domain so I know where these periodic interfaces are located?
You should probably make your reference pressure 100000 [Pa]  3595 [Pa], and use 0 [Pa] for your outlet pressure. This might reduce round off error. 

February 28, 2016, 08:24 

#19 
New Member
Join Date: Feb 2012
Posts: 14
Rep Power: 7 
Hi Glenn,
The outpuy file I sent belongs to a linear cascade arrangement, not annular cascade. In order to define flow direction, I used cylindrical coordinates. I got the velocity components from a rotating cascade to have an idea, not for a comparison. CFX makes the transformation of the components. You can find the computational domain in the attachment. I will try your suggestion. Thanks for your consideration 

February 28, 2016, 17:50 

#20 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 14,088
Rep Power: 109 
Are you sure you have that right? Why is the inlet using cylindrical coordinates to define the inlet flow when it is a linear blade cascade?
Does it converge when you run it entirely in cartesian coordinates? This is looking like the XY problem: http://xyproblem.info/ 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Fatal overflow in linear solver error. Why?  zaidun  CFX  7  August 11, 2016 05:59 
what exactly does the linear solver do?  alpha754293  CFX  20  May 25, 2016 08:23 
time consuming of the linear solver  luckycfd  OpenFOAM Programming & Development  3  September 23, 2013 05:29 
Use "bounded" in scheme or not to use?  immortality  OpenFOAM PreProcessing  0  June 11, 2013 16:20 
solution diverges when linear upwind interpolation scheme is used  subash  OpenFOAM  0  May 29, 2010 01:23 