CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLOW-3D (http://www.cfd-online.com/Forums/flow-3d/)
-   -   sloshing- mean kinetic energy not constant (http://www.cfd-online.com/Forums/flow-3d/89897-sloshing-mean-kinetic-energy-not-constant.html)

satellite_control June 24, 2011 18:02

sloshing- mean kinetic energy not constant
 
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

MuxaB June 27, 2011 20:13

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?

satellite_control June 29, 2011 04:32

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!

MuxaB June 29, 2011 20:08

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.

satellite_control June 30, 2011 05:57

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.

MuxaB July 1, 2011 17:51

Quote:

Originally Posted by satellite_control (Post 314201)
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.


All times are GMT -4. The time now is 15:10.