[dai549592484]

Dear All,

when simulate a DFBI case with wave, motion of the structure radiate wave to the inlet, and the inlet will reflect the radiated wave to the structure. so,
does any one know how to eliminate the wave reflection from the inlet?

Thanks in advance.

[me3840]

You need to dampen the wave near the BC. There's a setting for this, check the user guide.

[dai549592484]

Originally Posted by me3840

You need to dampen the wave near the BC. There's a setting for this, check the user guide.

Hi me3840, thank you for your answer. I know the reflection from the outlet can be dampened by setting damping. But my question is the reflection from the inlet. If a damping zone is set between the inlet and the structure, the incident wave will never reach the structure.

[me3840]

Hm. I don't think that's possible. Under what circumstance would the wave not reflect in real life?

[dai549592484]

the problem is the real life do not have a "domain". Reflection is caused by ''domain'' effect.

[Roman]

Damping zone is a poor solution if you are sending in waves through it. If you have large problems with reflection then your domain is probably to small in the first place. Could you perhaps increase the distance from the inlet and dampen all the other walls?

[dai549592484]

Originally Posted by Roman

Damping zone is a poor solution if you are sending in waves through it. If you have large problems with reflection then your domain is probably to small in the first place. Could you perhaps increase the distance from the inlet and dampen all the other walls?

Hi Roman

Thank you for your answer. Yes, it is ture that we can relief the reflection from inlet by extending the domain. However, extending the domain will cause 2 problems. 1) computation resource will increase extensively. 2) wave decay caused by mesh.

It is a solution but not good enough.

[ping]

you will get almost zero wave decay if you follow the guidelines for capturing waves well like 20 cells trough to peak and 40-80 per wave length using good anisotropic refinement with the trimmer mesher and to save cells use very wide cells until you get near your structure

and use second order time and ensure the courant number is below 1 in the wave by getting the time step low enough

and the little decay you do get can be adjusted by making the wave a little larger at inlet

[Roman]

1. Very true, however, by creating smart grid refinements this should not be extremely computationaly expensive.

2. AS for grid goes, I'm unsure if you are simulating on VOF wave or not. If you do:

Set your Z size to about 1/20th of the wave amplitude.

Set your second order unsteady solver time step relatively to the wavelength division chosen, using the following equation: if the dx chosen was 1/80th, then use (wave period) / (2.4 * 80), if it was 1/90th, use (wave period) / (2.4 * 90), and so forth. Be careful to not create unrealistically steep waves. For example, the 1st order wave theory applies to waves with amplitudes to wave length of around 1:100.

Shorter times steps are required in some steep wave cases where the turbulent kinetic energy might diverge.

EDIT: ping beat me to it

[dai549592484]

Hi ping, thank you for your answer. Yes I know that. However, I don't belive you can get almost zero decay in wave tank direction. Of course for time history, there's almost no decay when close to the inlet.

BTW, to use second order time you need to make sure the courant number is smaller than 0.5 rather then 1.

[dai549592484]

Thanks Ping, Roman. I am waitting for an anwser like "EOM" method. Which is far more efficient than the current solution. Do you guys know about it?

[Roman]

Could you elaborate a little further? What are you trying to simulate, is it a boat in waves and you are trying to analyze response? I agree with ping, cases with little to no grid damping are possible, it's a mater of computational cost.

[ping]

we have several cases with essentially no decay after more than 10 wave passes so it is possible with care and i suggest you create a one cell wide model to show this youself

oem stands for euler overlay method i think and i have heard that this will be added to the software to allow efficient creation of much larger domains together with a better wave damping method using a solution forcing technique but i have no idea when

[Roman]

Originally Posted by ping

oem stands for euler overlay method i think and i have heard that this will be added to the software to allow efficient creation of much larger domains together with a better wave damping method using a solution forcing technique but i have no idea when

They mentioned that "forcing technique" will come in version that will be released this summer.

[dai549592484]

Are you sure? This will be fantastic

[dai549592484]

Do you mean 10 wave lengths away from the velocity inlet or at a certain point which is close to the inlet experienced 10 waves?

[tms120]

Originally Posted by Roman

1. Very true, however, by creating smart grid refinements this should not be extremely computationaly expensive.

2. AS for grid goes, I'm unsure if you are simulating on VOF wave or not. If you do:

Set your Z size to about 1/20th of the wave amplitude.

Set your second order unsteady solver time step relatively to the wavelength division chosen, using the following equation: if the dx chosen was 1/80th, then use (wave period) / (2.4 * 80), if it was 1/90th, use (wave period) / (2.4 * 90), and so forth. Be careful to not create unrealistically steep waves. For example, the 1st order wave theory applies to waves with amplitudes to wave length of around 1:100.

Shorter times steps are required in some steep wave cases where the turbulent kinetic energy might diverge.

EDIT: ping beat me to it

@Roman:
Hi Roman, I am able to generate my desired wave (steepness 1/20), but when I put the body in waves, the turbulent energy and dissipation rates diverging. Apparently it seems like I may have to use very small timestep than the one I used to generate waves or first order temporal may work which reduces the wave height. Any suggestion will be appreciated.

[sriram9127]

I was running a simulation, the power went off but the system was backed up by UPS. I saved the simulation after some time the file is not opening and it pops up the message "Apparently, the original save action did not terminate successfully". How to retrieve my simulation???? Any ideas?