CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   cfx strange error (http://www.cfd-online.com/Forums/cfx/95595-cfx-strange-error.html)

antonio December 23, 2011 14:30

cfx strange error
 
I am trying to simulate the propagation of particles in the last few meters of a reservoir (incluind the dam section) using the algebraic slip model and I am receiving the following error message:
+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine FPX: c_fpx_handler |
|

Does anyone knows what causes this?
I have defined the following boundary conditions:
- at inlet velocity and the mass fraction;
-at the outlet a smooth no slip wall;
-at the bottom and the lateral parts of the model a rough no slip wall
-in the top of my domain I have specified an opening boundary with the following features:
-relative pressure equal to the height of the flow that is above of my domain
-pressure option assigned to opening pressure
-low turbulence intensity
-mass fraction equal to zero
In doing so, I am trying to model not the entire height of the dam but just a few meters from the bottom (where the sediments will be accumulated). Furthmore, I have defined the reference pressure equal to the pressure correponding to the height of the flow above the domain, velocities equal to zero, an hydrostatic pressure distribution, and mass fraction equal to zero as initial conditions.

What can be wrong in this approach?Many thanks.

antonio December 23, 2011 14:37

-at the top boundary I have choosed the entrainment option

ghorrocks December 24, 2011 05:38

Is it a floating point error? If so then this means your simulation has diverged. Need to improve numerical stability.

antonio December 26, 2011 13:56

It is a floating point error and a little bit surprisingly (at least for me) by changing the initial level of turbulence in domain the error disappears. I had k=epsilon=0 and now I have low level of turbulence (I=1%)..

ghorrocks December 27, 2011 06:07

You cannot have epsilon = 0. It leads to a divide by zero error on the turbulent viscosity - ie a floating point error :) This does not sound surprising at all to me.

antonio December 27, 2011 06:13

Well seen.

ghorrocks December 27, 2011 06:24

Well, the e based turbulence model cannot have epsilon=0 as the turbulent viscosity goes undefined. This is a key failing of these models and is why they cannot model low Re flows or transitional flows. This is one of the key advantages of omage based turbulence models, and why the omega turbulence models are used in the vast majority of these sort of flows.

So not so much a "well seen" as an example of a well known fundamental failing of epsilon based turbulence models.


All times are GMT -4. The time now is 17:24.