CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Floating point Error (http://www.cfd-online.com/Forums/cfx/79194-floating-point-error.html)

lorf August 16, 2010 06:47

Floating point Error
 
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

Floating Point
 
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.


All times are GMT -4. The time now is 04:43.