CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Errors with sloshing simulation (http://www.cfd-online.com/Forums/cfx/109312-errors-sloshing-simulation.html)

iamdenis November 14, 2012 15:24

Errors with sloshing simulation
 
1 Attachment(s)
Hello everyone,

sorry for starting another thread on sloshing.. as I have seen many others on this forum.

I am trying to get a sloshing simulation for a coffee cup (using water for now) with an opening at the top. I would like to detect the amount of liquid which leaves the cup due to a periodic motion.

I have done the flow over a bump tutorial and read over some basics on CFX.

If anyone could please assist me with any of these problems I would greatly appreciate it.

1. Since there is no inlet/outlet I am trying to set initial conditions with:

LIBRARY:
CEL:
&replace EXPRESSIONS:
Water height = 5 [ m]
denh = (denwater - denref)
denref = 1.185 [kg m^-3]
denwater = 997 [kg m^-3]
motion = sin(theta) [m/s]
pressure = denh*g*vliquid*((Water height)-y)
vair = 1.0 - vfliquid
vfliquid = (y-(Water height))/y

END
END
END

-but this does not seem to give me a water height of 5m.


2. I have applied symmetry to 2 faces, walls to the bottom and 2 other faces and opening at the top.

I am trying to apply "motion" , a periodic sine motion to the walls but it gives me an error unless I apply it in the W direction. Even then, I do not get any motion in CFD-Post.

Attachment 16970
(using a prism right now for simplicity)

Thank you for the help,
Denis

ghorrocks November 14, 2012 17:31

Use the if-then or step function to give a sharp transition from water to air. This function just linearly adjusts it over a long distance - this is not what you want.

iamdenis November 15, 2012 16:25

Thank you or the tip Glenn!

I made this my CEL code:

LIBRARY:
CEL:
&replace EXPRESSIONS:
Water height = 20 [ cm]
cm = 1 [cm]
denh = (denwater - denref)
denref = 1.185 [kg m^-3]
denwater = 997 [kg m^-3]
motion = 5*sin(t*(360[rad/s])) [cm]
pressure = denh*g*vfliquid*((Water height)-y)
vair = 1.0 - vfliquid
vfliquid = step((Water height - y)/cm)*1.0

END
END
END


I am now getting an error of:

A negative ELEMENT volume has been detected. This is a fatal
error and execution will be terminated. The location of the first
negative volume is reported below.
Volume : -0.6276E-06
Location : ( -0.75701E-01, 0.33485E+00, 0.70440E-01)



I applied "unspecified motion" to the domain, the symmetry walls and the opening. And put in the "motion" expression into X specified displacement for the 3 walls (two sides and the bottom)

Thank you,
Denis

ghorrocks November 15, 2012 17:53

You have not specified your domain motion correctly. If you want the whole thing to oscillate back and forth as a rigid body then you need to apply your motion expression to all boundaries.

To debug mesh motion errors, do a simulation where you output a results file every time step including the mesh. You can also turn off the momentum/energy/turbulence solvers using expert parameters to make it go faster. Then run it and you will see the mesh motion you defined. This allows you to quickly debug the mesh motion.

Also note this model can be done much more simply by changing the gravity vector. This is an approximation which does not precisely model the motion but it might be close enough and it is much easier and faster to run.

iamdenis November 16, 2012 14:28

Hi Glenn,

I fixed the mesh error by reducing mesh element size.

I am now trying to run the simulation in CFD -post but am unable to get the right animation.

I am trying to get something like:
http://www.youtube.com/watch?v=jSs1sFp673o


But my water is just moving back and forth, I am not getting any sloshing.
I set all of the domains to the specified motion, including the water/air domain inside the box.

Sorry for all the questions. I am getting very close and am just missing a few steps!

Thanks again,
Denis

ghorrocks November 17, 2012 20:03

First of all - make sure you get the physics right. Are you simulating a regime where sloshing occurs? If the Reynolds number is too low you will not get sloshing. Also are you correctyl resolving the free surface? If you have excessive diffusion of the surface you will not get sloshing. Is the volume fraction gradient from 0 to 1 resolved over a few elements?

iamdenis November 20, 2012 03:55

Quote:

Originally Posted by ghorrocks (Post 392733)
First of all - make sure you get the physics right. Are you simulating a regime where sloshing occurs? If the Reynolds number is too low you will not get sloshing. Also are you correctyl resolving the free surface? If you have excessive diffusion of the surface you will not get sloshing. Is the volume fraction gradient from 0 to 1 resolved over a few elements?


Thank you for all the help Glenn.
Finally got it working.

-Denis


All times are GMT -4. The time now is 04:23.