[vince60270]

hello everyone,
I am new on star ccm+ and for a Project, i simulated a multiphase flow (water/air) 50/50 with eulerian multiphase and fifth order waves around a boat. Everything went perfectly with regular velocity values for the current and wind. But now i want to see how the boat behave with a velocity increasing from 0 to 28 m/s. So to do this i created a time dependant table, imported it, setted the current and wind to Zero for the model and for inlets i setted velocity profiles to Composite linked to the table. Everything seems good but the Problem is that the full iso surfaces Cells ar not updating at each time step ( the inlet "pushes" the other cells) creating a huge wave and destroying the Simulation...I tried many things but as i am not confident enough with the Software i am Kind of blocked. If someone know how to help me it would be really really nice.
Sorry if my english is poor,
Vince.

[vince60270]

To be more precise what i want to do is simulate a boat accelerating from 0 to 28m/s in 3 s for and then stay at 28m/s for 7s on water with small waves (5cm) or flat water and be able to study its free motions ( Rotation and Translation).
thanks

[ping]

think about what you have done - all the rest of the water is still stationary and you have applied a new velocity at one boundary so it does what i would expect and creates a wave

there are two ways to get around this

set the wave to zero speed and use a translating moving preference frame for the region and make this move that the required input speeds

or accelerate the whole fluid domain at the same rate as your inlet is increasing by using a momentum source or add gravity in the horizontal direction

[vince60270]

thank you very much for your answer. I totally understand that what i got as results is in Agreement with what i asked with my BC as soon as i didn't know how to update evry cells...Could you explain to me more precisely how to do one or anaother solution ( the easier if possible) because i am not confident enough with this Software to do it by myself.
It would be great.

[ping]

i have not done the reference frame method for some time but here we go

set the flat wave to zero since you dont want the water to move

down in tools create a new rotating and translating reference frame

set its translation velocity in the hulls motion axis to a constant or some equation of time or to a more complex user defined field function ramping up for example and the latter can be interpolated from a table of course use the table field function

in the regions physics values under motion set the reference frame to the one created above

thats it

[ping]

i just checked this by taking the completed boat in waves tutorial case and

changed the wave to 0 velocity and height of .0001m
created a new reference frame with -2.5m/s x velocity
in the regions physics values under motion set the reference frame to the one created above
added a velocity vector scene and use the field relative velocity to view vectors

it gives the same results as running the tutorial as completed with a height of .0001m

[vince60270]

thank you for your help, i am not sure i totally understand the Explanation but i am going to try and give you Feedbacks ASAP.

[vince60270]

So i did what you explained but for the rotating and translating Frame we can only define constant velocity, it's not possible to link the velocity to a table (time) dependant velocity Profile... What i would like to do is to have the velocity increasing by itself during the Simulation

[me3840]

You don't need to do a moving reference frame.

Create a translating motion on the single region, and move that region relative to the wave. This will accelerate all of the water simultaneously.

Essentially you have a wave and you will be moving the computational domain through the wave.

[vince60270]

i went to tool/Motion and created a Translation Motion but then i went to Region isosurface to set it to the Motion but i am lost i am really not good enough to do it could you be more precise ? If it can help you i followed with accuracy the DFBI boat in head waves tutorial but now instead of having a constant Speed i want to have velocity Profile linked to a time dependant table . thank you for your help

[vince60270]

Nobody could help me ? Please..

[ping]

you did not follow my guidance - my easy method is that you do need to create a new reference frame and not a new motion since you need to keep using the dfbi motion physics for the motion setting

as I have explained this method works very well for what you need to do so please follow my guide for using it on the completed boat in waves tutorial

and to do more than a constant value of velocity see my post above on May 9, 2014 13:59 where I explained several ways beyond a constant value

[vince60270]

i followed your steps and every times got the Problem i had before crashing the Simulation that's why i am still asking for help. I don't say your method doesn't work but i assume i missed something in your Explanation that's why i am asking for more precise Explanation.

[vince60270]

for example when i create the moving reference Frame for Rotation and Translation the velocity Definition Option is only a constant velocity, i have no Option to select table time or field function or whatever so how would it be possible to update the velocity if it is a constant?

[ping]

as i have mentioned above...

in most menus in starccm+ where there is a constant input you can actually put in an equation or a field function eg in your case $Time * 0.123 will work but the 0.123 will need to be different of course and will give you a simple ramp

add an if statement so as to level it out at say 10s and you have what a good step forward

but it can also be set to a more complex user defined field function ramping up for example and the latter can be interpolated from a table of course use the table field function

so i suggest you go and read the full help on field functions including the special table ones which do exactly what you want from imported velocities

and read Using STAR-CCM+ > Setting Conditions and Values > Setting Values Using an Expression for details of putting equations in place of constants - it even has an example of doing it for motion

[vince60270]

hello,
Thank you for this more detailed Explanation i read what you said and managed to set the translating Frame with the time variable as i wanted but i think i have to Change some Parameters in my regions/boundary conditions because with the boat in wave tutorial if i complete it i set the velocity and Motion spec to field function vof waves model for inlet and wall (velocity inlet) which is Zero and for the pressure outlet also to pressure outlet field function hydrostatic pressure of waves so i can see my Frame updating but the boudary stay at Zero as i expected and i have reversed flow at the outlet... i don't know what i have to Change for this in order to have a fully moving and working Frame ...But thank you reading the Topics you pointed was very useful even for my understanding

[ping]

the normal velocity field will be zero since the water is now not moving ie it is actually more like a real hull moving in stationary water

so as I said in an earlier post you need to instead use the field called relative velocity

[vince60270]

yeah it s okay now for the updating and stuff but do you have any clue about the reversed flow at the outlet ? and also an idea of how many inner Iteration i should choose to have a good convergence because with 0.01s time step, 10 inner iterations and 10 s real time the convergence is really poor

[vince60270]

thank you very much for your help i managed to solve my Problems, at least for the Moment... :-) i hope it will work and if not, I'll be back. Thanks again

[ping]

5 inner iterations is what is normally recommended for all hull cfd and then get the timestep okay for a reasonable courant number

you can test these yoursefl and see how different your resulting waves, forces etc are