Floating point Error

lorf · August 16, 2010, 06:47

Hi!

Beforehand - sorry that I repeat the often named error message:

ERROR #001100279 has occurred in subroutine ErrAction.

Floating point exception: Overflow

I tried to solve that with many advices from this forum but nothing help so I describe my problem.

I have an airflow-simulation through ramified pipe and the simulation function as long as I take the boundary conditions inlet- velocity / outlet static-pressure but the results aren't useful so I change the boundary conditions to inlet - total pressure & outlet massflow. Now at the 12 iteration the error (see ahead) comes. It is an steady state simulation.

I tried the following:
Change:
1. Turbulencemodel from k-epsilon to SST and BSL.
2. Reference pressure from 0 Pa to 8 Pa.
3. Fluid timescale factor from 1 to 2 & 5.
4. tried a transient simulation
5. change the mesh size (refine and coarse)

but no change

I have no more ideas so I would be glad to hear some other ideas to solve that problem.

Thanks
lorf

DukeLeto · August 17, 2010, 14:39

CFX can be fairly senstitive to initial conditions. Make sure you are setting something reasonable.

If your problem is violent in nature (i.e. supersonic or transonic) you should most likely ramp up the total pressure from a low to a final value over perhaps 100 iterations. The number of iterations is available for use in expressions. See the CFX documentation.

ghorrocks · August 17, 2010, 18:57

Overflow errors mean your numerics have diverged big-time. Your model is too unstable and you need to improve the stability.

Some hints, in approximate order you should try them:
* Check the simulation setup is correct.
* Start the simulation with very small timesteps and only increase them back to normal values once it is converging consistently.
* Use the double precision solver.
* Switch to upwinding for the spatial differencing and first order time differencing if transient (but note this is inaccurate and you should go back to accurate differencing for the final run to convergence).
* Ramp the boundary conditions up to make the startup easier.
* Improve mesh quality
* Do an initial run on a coarse mesh and interpolate this to a finer mesh for an initial condition.

August 16, 2010, 06:47	Floating point Error	#1
lorf New Member Join Date: Aug 2010 Posts: 1 Rep Power: 0	Hi! Beforehand - sorry that I repeat the often named error message: ERROR #001100279 has occurred in subroutine ErrAction. Floating point exception: Overflow I tried to solve that with many advices from this forum but nothing help so I describe my problem. I have an airflow-simulation through ramified pipe and the simulation function as long as I take the boundary conditions inlet- velocity / outlet static-pressure but the results aren't useful so I change the boundary conditions to inlet - total pressure & outlet massflow. Now at the 12 iteration the error (see ahead) comes. It is an steady state simulation. I tried the following: Change: 1. Turbulencemodel from k-epsilon to SST and BSL. 2. Reference pressure from 0 Pa to 8 Pa. 3. Fluid timescale factor from 1 to 2 & 5. 4. tried a transient simulation 5. change the mesh size (refine and coarse) but no change I have no more ideas so I would be glad to hear some other ideas to solve that problem. Thanks lorf

August 17, 2010, 14:39	Floating Point	#2
DukeLeto New Member Dr. Richard R. Lange Join Date: Jun 2010 Location: Pittsburgh Posts: 5 Rep Power: 15	CFX can be fairly senstitive to initial conditions. Make sure you are setting something reasonable. If your problem is violent in nature (i.e. supersonic or transonic) you should most likely ramp up the total pressure from a low to a final value over perhaps 100 iterations. The number of iterations is available for use in expressions. See the CFX documentation.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
CGNS Compiling	Diego	Main CFD Forum	17	December 21, 2014 01:40
attach/detach (valve opening/closing)	phsieh2005	OpenFOAM Running, Solving & CFD	2	March 21, 2009 05:18
DecomposePar links against liblamso0 with OpenMPI	jens_klostermann	OpenFOAM Bugs	11	June 28, 2007 17:51
Floating point Error message	Jonathan	FLUENT	2	January 16, 2007 04:07
user subroutine error	CFDUSER	CFX	2	December 9, 2006 06:31

August 17, 2010, 18:57		#3
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	Overflow errors mean your numerics have diverged big-time. Your model is too unstable and you need to improve the stability. Some hints, in approximate order you should try them: * Check the simulation setup is correct. * Start the simulation with very small timesteps and only increase them back to normal values once it is converging consistently. * Use the double precision solver. * Switch to upwinding for the spatial differencing and first order time differencing if transient (but note this is inaccurate and you should go back to accurate differencing for the final run to convergence). * Ramp the boundary conditions up to make the startup easier. * Improve mesh quality * Do an initial run on a coarse mesh and interpolate this to a finer mesh for an initial condition.