[mehdiman]

Hi
I'm currently doing a simulation of a large plate floating on sea,and i want to calculate the vertical displacement of plate in a regular wave,for this,i use Star ccm+ coupling with Abaqus co-simulation,it works but the answers are False,for example for a 0.5 m wave height ,and 100 m wave length ,the result of vertical displacement in abaqus shows over than 15 m. and these are my inputs :
rectangular plate properties : 2*300*60 m
Enabled Models
Three-Dimensional (Selected automatically)
Gradients (Selected automatically)
Time
Implicit Unsteady
Material
Eulerian Multiphase
Multiphase Model
Volume of Fluid (VOF)
Viscous Regime
Turbulent
Reynolds-Averaged Turbulence
K-Epsilon Turbulence
Optional Models
Gravity
VOF Waves
if someone can help me,please contact with this email: booymeister@gmail.com

[me3840]

Is the plate deforming? Why are you using abaqus?

Are you sure the size of the model is correct? Check that the plate is sized correctly, your answer seems very large considering the inputs.

[Roman]

Sounds like your coupling frequency is to low. What timestep do you have in starccm and what is your coupling timestep set to?

[mehdiman]

Originally Posted by me3840

Is the plate deforming? Why are you using abaqus?

Are you sure the size of the model is correct? Check that the plate is sized correctly, your answer seems very large considering the inputs.

Yes,deformed,and i need the deformed shape of plate, using abaqus for better analysis,to reach the displacement of amplitude.

[mehdiman]

Originally Posted by Roman

Sounds like your coupling frequency is to low. What timestep do you have in starccm and what is your coupling timestep set to?

Time step in star ccm and abaqus are 0.01 s

[Roman]

This is also true for the maximum allowable time step in abaqus setup as well?

[me3840]

0.01s is probably far too large for the fluid simulation. Does each timestep converge? The position and deformation as well as the fluid parameters (drag, left, etc) should converge every timestep.

[mehdiman]

thanks dear friends,
when i simulate wave, i see the several wave under whole plate,if i want to model one incident wave moving from the first point to the end point of my plate,what can i do?

[Roman]

I would define a first order VOF wave and set "point of water level" x value to the start position of the plate. When the simulation runs the wave will have a defined velocity at which it propogates to the end point.

[mehdiman]

Originally Posted by Roman

I would define a first order VOF wave and set "point of water level" x value to the start position of the plate. When the simulation runs the wave will have a defined velocity at which it propogates to the end point.

Thnks dear , u said my step time is large,what is the better step time do u think ? For both abaqus and star ccm ?

[mehdiman]

Originally Posted by me3840

0.01s is probably far too large for the fluid simulation. Does each timestep converge? The position and deformation as well as the fluid parameters (drag, left, etc) should converge every timestep.

If i want to change the step time,what is your idea about both abaqus and star timestep? As you know my model has a large dimentions..

[me3840]

Well you want to ensure that the CFL on the interface of the water and air is no greater than 1. You may have to drop the timestep to make that happen. I would suggest starting at 3ms or so.

[mehdiman]

Originally Posted by me3840

Well you want to ensure that the CFL on the interface of the water and air is no greater than 1. You may have to drop the timestep to make that happen. I would suggest starting at 3ms or so.

thanks for ur great help,i have a new problem now,which kind of mesh do you use for this dimensions of fluid domain,and what is the maximum cell size that i can use?

[me3840]

I can't answer what size to use. You must use engineering judgement to choose a mesh size that resolves important gradients while maintaining acceptable accuracy and speed.

As far as what kind of mesh to use, wave calculations like this mean you really only care about 2 of 3 dimensions, so a trim grid with anisotropy near the domain boundaries and more isotropy in the region of interest is usually more efficient.