CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Free surface flow in counter current limitation (http://www.cfd-online.com/Forums/cfx/116344-free-surface-flow-counter-current-limitation.html)

j.zamorano April 17, 2013 09:57

Free surface flow in counter current limitation
 
Hello, I am trying to do a simulation of 2 flows (water and air) flowing counter currently in a horizontal hot leg. I have problems of convergence with steady state, so now I am trying a transient one. I have defined constant velocity inlets for both water and air, an outlet for the water with pressure condition, and an opening for the air. Even with the transient simulation, it is becoming really hard to get convergence. Can you give me any advice? I have selected a 1ms timestep. Thanks.

ghorrocks April 17, 2013 18:48

Please post an image of what you are modelling and the CCL or output file.

j.zamorano April 22, 2013 03:52

http://www.subirimagenes.com/otros-f...-8398648.html]http://s2.subirimagenes.com/otros/pr...48facility.jpg[/URL]

Left: air constant velocity inlet
Bottom: water constant velocity inlet
Bottom: water outlet (pressure difference 0 Pa)
Up: air opening (dinamic pressure 0 Pa)

Solver control:
Transient, 1 sec total time, 1 ms timestep, Upwind, second order backward euler, 1E-04 residual target.

Free surface model: air and water continuous fluids, 2F model for drag coefficient, homogeneous turbulence, k-epsilon model

j.zamorano April 22, 2013 03:57

Is this enough information? If you need the output file or the CCL please give me your e-mail, and I will send it to you.

Thanks

ghorrocks April 22, 2013 09:00

Why have you chose a 1ms time step? Unless you have actually done a sensitivity analysis on that time step size and determined it is what you need then it is bound to be wrong.

So let the solver work the time step out for you. Use adaptive timestepping, homing in on 3-5 coeff loops per iteration.

Are you using surface tension?

Why are you using a highly inaccurate spatial discretisation scheme (upwind) but a very accurate temporal scheme (2nd order back eular)? If you just want quick and dirty results then run 1st order in time as well. If you want an accurate answer you will need to run a better spatial discretisation than that.

RicochetJ April 22, 2013 09:28

If you let the solver work out the time step via adaptive time stepping I've found the time step it selects is usually prohibitively small, such as 1e-8 s (that is if you converge to 3-5 loops).

ghorrocks April 22, 2013 18:25

That is because it needs small time steps! There are very few simulations where this does not find the correct time step.

The only exception to this is when you are happy to sacrifice accuracy to just "muddle" through a tricky bit of the simulation and don't care about accuracy. An example could be when you first start the simulation up, or when an aggressive action occurs which you do not care about the details (eg a fast combustion event).

If this slows the simulation too much then
* Check that your mesh is not too fine
* Check your convergence is not too tight
* Get a faster computer
* Get more computers and run parallel.

j.zamorano April 24, 2013 09:34

I am new in CFX, What parameters should I take to make adaptive timestepping? Max Courant number?

ghorrocks April 25, 2013 07:04

No. Courant number only has a tenuous link to convergence in CFX as it is an implicit solver.

The recommended approach for adaptive time stepping is homing in on 3-5 coeff loops per iteration.

j.zamorano April 25, 2013 10:31

I am not using surface tension forces, should I? I think the diameter is too big and this forces are too small (0.05 m). I am using free surface model, should I change it to mixture model?

Thank you so much

ghorrocks April 25, 2013 18:49

Only use surface tension if it is important for the flow you are modelling. It is an expensive model and will slow you down a lot, so only use it if you have to.

j.zamorano April 26, 2013 06:33

http://www.subirimagenes.com/imagen-...-8405900.html]http://s2.subirimagenes.com/imagen/p...5900error2.png[/URL]

This is happening to me when I try to do a transient simulation. Does anyone know what happen? The program says something about overflow

ghorrocks April 26, 2013 07:23

This is a floating point error (which then caused lots of other errors including crashing the parallel run) - this is an FAQ: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

j.zamorano April 30, 2013 06:44

I am having quite good results with steady state simulations. Now, I am doing transient ones. I want to reach the second state of the picture by improving the gas velocity. But, although the function for the gas velocity inlet is well defined, when I plot the results it shows everytime the first state (left). Can be this because problems of convergence? What should I do?

http://www.subirimagenes.com/otros-t...-8411961.html]http://s2.subirimagenes.com/otros/pr...transition.jpg[/URL]

ghorrocks April 30, 2013 19:32

I do not understand your problem. What are you seeing and what do you expect to happen?


All times are GMT -4. The time now is 14:31.