CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLOW-3D

sloshing- mean kinetic energy not constant

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   June 24, 2011, 18:02
Default sloshing- mean kinetic energy not constant
  #1
New Member
 
Marco S.
Join Date: Oct 2010
Posts: 8
Rep Power: 6
satellite_control is on a distinguished road
Hi,

I am analysing linear sloshing.
I have the problem, that the mean kinetic energy does not get stable.

I use for the momentum advection:second order monotonicity preserving.

Can I also use first order?

What is the difference and how can I get a stable simulation.

I wait for your help!

Thank you
satellite_control is offline   Reply With Quote

Old   June 27, 2011, 20:13
Default
  #2
Senior Member
 
michael barkhudarov
Join Date: Mar 2009
Posts: 331
Rep Power: 9
MuxaB is on a distinguished road
First and second order advection methods should both be fine in this case.

I assume it is the time-average mean kinetic energy that does not settle to a steady-state, right? The instantaneous value would oscillate because of the sloshing movement.

Is the total fluid volume more or less constant?
MuxaB is offline   Reply With Quote

Old   June 29, 2011, 04:32
Default
  #3
New Member
 
Marco S.
Join Date: Oct 2010
Posts: 8
Rep Power: 6
satellite_control is on a distinguished road
Yes that is right. The time averaged mean kinetic energy does not settle to steady state.
I tryed to change a lot of values in Flow. I found out, that the change of the time step controls values brings the simulation to steady state. My values are:

a)
Initial time step: 0.0001
Minimum time step: 0.0000001
Maximum time step: 0.002

With this parameters the simulation do not reach steady state

b)
Initial time step: 0.001
Minimum time step: 0.00001
Maximum time step: 0.05

This values brings the simulation to steady state!
I dont know which values are the best for my simulation.

My simulation is with no-viscosity, no-turbulence, no heat transfer. It refers to the potential theory.


What do you mean by total fluid volume? I have a constant fill level.

I also want to ask, how can I see that my simulation was a succes? By the time aerages mean kinetic energy?

Another question is: I chose SI Units and get for example for the Force 0,0040. Is that Newton? Because that is too small. Normally it has to like 5 Newtons.

Thank you very much for helping me!
satellite_control is offline   Reply With Quote

Old   June 29, 2011, 20:08
Default
  #4
Senior Member
 
michael barkhudarov
Join Date: Mar 2009
Posts: 331
Rep Power: 9
MuxaB is on a distinguished road
Yes, the FLOW-3D force output would be Newtons in SI units. Not sure why it is so small. It should basically be equal to the weight, right?

Adding viscosity would help to reach steady-state.

Even if your fluid level is constant, the total volume may change due to numerical errors. FLOW-3D output the total fluid volume as a function of time. Make sure it is more or less constant. En error of <1% is normal.

To check the correctness of a simulation you can check 2d and 3d plots, forces, slosh amplitude and so on and make sure it makes sense. Other than that, if the solver is converging, no error messages pop up from the solver, then you problably have good results.

using constant time step size may make results more accurate, but using a smaller one does not always make sense. If you do use a smaller time step, make sure to tighten pressure itereation convergence by setting EPSADJ=0.1 or 0.01 (the default is 1.0).

The minimum time step size does not have any effect on the results.
MuxaB is offline   Reply With Quote

Old   June 30, 2011, 05:57
Default
  #5
New Member
 
Marco S.
Join Date: Oct 2010
Posts: 8
Rep Power: 6
satellite_control is on a distinguished road
Hallo,

the Force is in SI Units and I found my mistake :-) It was my density. I had the default setting of 1. And water has 1000kg/m3.

My simulations are now stable. The problem was the too small initial time step size. I had dt=0,00001. Now I have dt=0,0001. I have also change max.time step from 0,002 to 0,01. That works very good.

My question is, does this have a big influence on the results?

My way was by trial and error. I lost 1 week, but now it works great with best results. Everything makes sense.

Both 1st and 2nd Order Momentum advection works fine.

I had another question to the Volume of Fluid advection. I have only water with a free surface. Should I choose Split Lagarngian or One Fluid, with free surface. What do you think?

I thank you a lot.
satellite_control is offline   Reply With Quote

Old   July 1, 2011, 17:51
Default
  #6
Senior Member
 
michael barkhudarov
Join Date: Mar 2009
Posts: 331
Rep Power: 9
MuxaB is on a distinguished road
Quote:
Originally Posted by satellite_control View Post
Hallo,

the Force is in SI Units and I found my mistake :-) It was my density. I had the default setting of 1. And water has 1000kg/m3.

My simulations are now stable. The problem was the too small initial time step size. I had dt=0,00001. Now I have dt=0,0001. I have also change max.time step from 0,002 to 0,01. That works very good.

My question is, does this have a big influence on the results?

My way was by trial and error. I lost 1 week, but now it works great with best results. Everything makes sense.

Both 1st and 2nd Order Momentum advection works fine.

I had another question to the Volume of Fluid advection. I have only water with a free surface. Should I choose Split Lagarngian or One Fluid, with free surface. What do you think?

I thank you a lot.
Nice work! The time step always makes a difference, but it should be insignificant. Regarding the VOF method, both should work fine. I would stick with the default One Fluid with Free Surface, but you can try both to see which one conserves volume better and converges faster.
MuxaB is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Mean Kinetic Energy alastormoody11 STAR-CCM+ 1 January 19, 2011 10:48
How to install CGNS under windows xp? lzgwhy Main CFD Forum 1 January 11, 2011 19:44
question about turbulent kinetic energy junker4236 Main CFD Forum 8 December 24, 2010 04:06
CGNS lib and Fortran compiler manaliac Main CFD Forum 2 November 29, 2010 07:25
ATTENTION! Reliability problems in CFX 5.7 Joseph CFX 14 April 20, 2010 15:45


All times are GMT -4. The time now is 08:49.