CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   multiphase model, water in air? (http://www.cfd-online.com/Forums/main/71325-multiphase-model-water-air.html)

bugra December 25, 2009 11:28

multiphase model, water in air?
 
hi everybody,

i study on a multiphase flow model. jet water flow flows from a nozzle into air (g force applied), i want to simulate it with fluent, for a cross section 2D model, all the multiphase model (vof, eulerian and multiphase) work and give a result, but when i try for 3D model, the continuty diverges.

it has unstructured mesh and take the courant number default as 0,25.

i want to see only the distance that the water goes in air.

is there anybody studied this before?

thanks for your helps...

Bugra

bugra December 25, 2009 11:29

And the model is very large, 20 meter length and 15 meter wide, 10 meter height.

Bugra

CFDtoy December 30, 2009 23:57

modeling multiP jets
 
hi there,
the problem is not difficult...make sure you tune your solution controls properly ..if you require only the dispersion angle etc..try running SIMPLE with PRESTO scheme for pressure, first order upwinded variables etc...this should give you pretty decent results..

let me know when and where you diverge..what is the error listed?

/cfdtoy
http://cfdtoy.blogspot.com


Quote:

Originally Posted by bugra (Post 240922)
And the model is very large, 20 meter length and 15 meter wide, 10 meter height.

Bugra


bugra January 1, 2010 11:12

hi,

thank you for your reply, after 15 iteration, the problem begins to diverge, and contnty is going up, if i let it go, it goes 1e12 and higher, actually, it doesn't give an error, it only runs, but not converges,

bugra
[IMG]file:///C:/DOCUME%7E1/bugra/LOCALS%7E1/Temp/moz-screenshot-1.png[/IMG]

bugra January 1, 2010 11:12

so i couldn't add convergence picture, don't mind the link above

bugra January 1, 2010 11:28

the error is that;

Error: > (greater-than): invalid argument [2]: wrong type [not a number]
Error Object: 1.#inf

at 102. iteration

Bugra

CFDtoy January 1, 2010 15:55

MP divergence
 
Hello bugra,
good that you were able to spot divergence immediately. Now, are you running steady or unsteady model? what kind of multiphase model are you running - VOF or eulerian-eulerian or mixture model? what are your initial conditions? is there turbulence added? what are your solution control settings?

Hopefully, we can get something out from here.

/CFDtoy
Visit http://cfdtoy.blogspot.com


Quote:

Originally Posted by bugra (Post 241228)
hi,

thank you for your reply, after 15 iteration, the problem begins to diverge, and contnty is going up, if i let it go, it goes 1e12 and higher, actually, it doesn't give an error, it only runs, but not converges,

bugra
[IMG]file:///C:/DOCUME%7E1/bugra/LOCALS%7E1/Temp/moz-screenshot-1.png[/IMG]


bugra January 1, 2010 18:10

hello again,

it's unsteady model (i'm not sure if i use steady, it gives true solution for only dispersion of water in air), i tried steady model too, but it diverged too. i use VoF model, turbulance k-epsilon, water in the pipe is at 1-5 bars static pressure, the upper surface is pressure inlet for air, the outer surface is pressure outlet for air, as i read from tutorials, piso algorithm, all of underrelaxation factors are 1, pressure is "body force weighted", momentum first order, volum fraction "Geo-Reconstruct", tke is first order, and tdr is first order.
in addition to this, it' s unstrucured grid.

the problem is that, water comes in a pipe to a nozzle and here, it enters into air. water in pipe has between 1 and 5 bars pressure. i wanna to see only the distance that water has gone and the angle of going out from nozzle.

thanks
Bugra

CFDtoy January 1, 2010 21:38

divergence
 
From the log file check which quantity is diverging? continuity, xvel, y vel, k , epsilon, etc...which one is not converging?

Anyways, other thing to try: keep piso

under relaxation - pressure = 0.4
under relaxation - momentum = 0.4
body force 1

turbulent knetic energy 0.4
turbulent dissip rate 0.4

for pressure-velocity coupling - presto
first order upwind for others

hope you are running unsteady model - check the model : 2D or 3D - steady or unsteady..

for unsteady : go to solve -> iterate

variable time step and fix courant number to 0.5

min and max time steps can be like 1e-09 to 1e-03 ...i dont know your grid size so cant say much here.

initialize - from inlet and iterate..

Let me know if it works...btw have you run Fluent VOF model before?

Regargds,

CFDtoy
http://cfdtoy.blogspot.com



Quote:

Originally Posted by bugra (Post 241246)
hello again,

it's unsteady model (i'm not sure if i use steady, it gives true solution for only dispersion of water in air), i tried steady model too, but it diverged too. i use VoF model, turbulance k-epsilon, water in the pipe is at 1-5 bars static pressure, the upper surface is pressure inlet for air, the outer surface is pressure outlet for air, as i read from tutorials, piso algorithm, all of underrelaxation factors are 1, pressure is "body force weighted", momentum first order, volum fraction "Geo-Reconstruct", tke is first order, and tdr is first order.
in addition to this, it' s unstrucured grid.

the problem is that, water comes in a pipe to a nozzle and here, it enters into air. water in pipe has between 1 and 5 bars pressure. i wanna to see only the distance that water has gone and the angle of going out from nozzle.

thanks
Bugra


bugra January 2, 2010 11:41

hi,

the continuity was diverging. the others (k, epsilon ...) are almost constant (less than 1e-3). i meaned that while saying "(i'm not sure if i use steady, it gives true solution for only dispersion of water in air)", i said that, i already run unsteady, but if i use steady, in your opinion, does it be true for this problem, does the steady solution be true?

i tried the parameters you wrote above, it runs at the moment, it doens't diverge. i had used vof model before, but the problem was easier than this, and mesh was quad. there was no problem with convergence. but here, there are tangential edges and the bad trihedral meshes on this surfaces, minimum mesh size is 3mm, tetrahedral cells.

thanks
Bugra

CFDtoy January 2, 2010 14:09

convergence
 
Hi,
Continuity divergence is kinda expected ...your relaxation was too high and with the time step you use, the parameters i suggested above takes care of the variable update. Even with PISO if you use higher time steps, you may want to lower your relaxtion factors so that variable update remains under control.

The simulation should run just fine now. Next time, when you get divergence..first place to see is solution controls, pressure momentum and turb settings !

/CFDtoy
Visit http://cfdtoy.blogspot.com



Quote:

Originally Posted by bugra (Post 241302)
hi,

the continuity was diverging. the others (k, epsilon ...) are almost constant (less than 1e-3). i meaned that while saying "(i'm not sure if i use steady, it gives true solution for only dispersion of water in air)", i said that, i already run unsteady, but if i use steady, in your opinion, does it be true for this problem, does the steady solution be true?

i tried the parameters you wrote above, it runs at the moment, it doens't diverge. i had used vof model before, but the problem was easier than this, and mesh was quad. there was no problem with convergence. but here, there are tangential edges and the bad trihedral meshes on this surfaces, minimum mesh size is 3mm, tetrahedral cells.

thanks
Bugra



All times are GMT -4. The time now is 00:25.