[s_baghalian]

hi
i have a 90 degree bend with circular section.
straight length in before the bend is 35 m and after the bend is 100 m.
curvature radius is 9 m and radius of section is 1.5 m. flow is 2 phases with depth of water 0.66m.
i modeled it with ICEM and i want to run it with CFX.
how are boundary conditions in this model?
how should i define volume fraction in this model?

[ghorrocks]

See the tutorial example free surface flow over a bump for how to set this up.

[s_baghalian]

i ran it but in iteration 980, an error has occurred.
this error is :
ERROR #001100279 has occurred in subroutine ErrAction. Message:
Floating point exception: Overflow
i reduced physical timescale but error didn't remove.

i don't know what is this error and what should i do?

[ghorrocks]

The tutorials should complete without error. You have almost certainly set something up wrong. Do it again, our use the already completed files.

[s_baghalian]

i run the tutorial and a channel with rectangular section and lower length, without any error. but my model that i defined (channel with circular section) have error.
i have not any problem in tutorial, i have problem in my model.

[michael_owen]

Originally Posted by s_baghalian

hi
i have a 90 degree bend with circular section.
straight length in before the bend is 35 m and after the bend is 100 m.
curvature radius is 9 m and radius of section is 1.5 m. flow is 2 phases with depth of water 0.66m.
i modeled it with ICEM and i want to run it with CFX.
how are boundary conditions in this model?
how should i define volume fraction in this model?

How have you set up the boundary conditions? Are you running in steady state or transient? What is the mesh resolution? Are you running in double precision?

[s_baghalian]

regime of flow is steady so i ran it steady.

in inlet boundary:
mass and momentum: option: normal speed

turbulence : option: intensity and length scale
fractional intensity: 0.05
eddy length scale: UpH
fluid values: air: upvfair
water: upvfwater
regime of flow is steady so i ran it steady.

in outlet boundary:
flow regime: subsonic

mass and momentum: option: static pressure
relative pressure: down press

in wall boundary:
mass and momentum: no slip wall

in initial conditions, all of options are automatic.

Expressions:
DenH 998 [kg m^-3]
DownH 1.66 [m]
DownPres DenH*g*DownVFWater*(DownH-y)
DownVFAir step((y-DownH)/1[m])
DownVFWater 1-DownVFAir
UPH 1.66 [m]
UpPres DenH*g*UpVFWater*(UpH-y)
UpVFAir step((y-UpH)/1[m])
UpVFWater 1-UpVFAir

i don't think that mesh have problem.
i ran it again and again and i saw results before the error was created, volume fraction and contours of velocity are correct but i don't know why there is an error!!!

[michael_owen]

in initial conditions, all of options are automatic.

This may be a problem. I'm unsure of how well the automatic initialization can initialize the volume fractions and pressure field from the boundary conditions.

Also, what is the exact error, and what does the convergence graph look like before the crash?

[s_baghalian]

thank you very much for attention to me.
if no problem for you,please send to me your email till i send to you CFX-pre file.
in initialization option, i select automatic with value for fluid setting.
air: volume fraction: UPVFAir
water: volume fraction :upvfwater
graph have high fluctuations.

[michael_owen]

Originally Posted by s_baghalian

thank you very much for attention to me.
if no problem for you,please send to me your email till i send to you CFX-pre file.
in initialization option, i select automatic with value for fluid setting.
air: volume fraction: UPVFAir
water: volume fraction :upvfwater
graph have high fluctuations.

You need to initialize the Pressure with the hydrostatic pressure and also initialize the velocity in the pipe, unless it is still, which I can't imagine. If you still have problems converging, reduce the timescale factor. Are you using a homogenous flow field? If not, do so.

I don't have time to review your cfx pre case.

[s_baghalian]

i ran it with all of the things that you say too.i reduced physical timescale. i ran it with 0.000001 physical time scale, but unfortunately an error exist.
how many can i reduce physical timescale?

[michael_owen]

Originally Posted by s_baghalian

i ran it with all of the things that you say too.i reduced physical timescale. i ran it with 0.000001 physical time scale, but unfortunately an error exist.
how many can i reduce physical timescale?

What is the exact error?

[s_baghalian]

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Floating point exception: Overflow |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| Writing crash recovery file |
+--------------------------------------------------------------------+

Details of error:-
----------------
Error detected by routine POPDIR
CRESLT = ILEG

Current Directory : /FLOW/NAMEMAP

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX solver exited with return code 1. No results file |
| has been created. |
+--------------------------------------------------------------------+

End of solution stage.

[michael_owen]

There is an Expert Parameter under IO Controls to Write a Backup at Start. Turn this on, and then post process the .bak file. And make sure the initialization looks correct. Pay particular attention to the pressure. Do you have the hydrostatic pressure gradient alligned correctly for the bouyancy gravity vector you have specified, etc.

[s_baghalian]

in domain option>fluid models>free surface model>option, i selected none instead of standard. i correct it, i think that this is affective, isn't it?