CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Why the generated waves disappear when moving away from the wavemaker?

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

Like Tree1Likes
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 10, 2021, 19:51
Post Why the generated waves disappear when moving away from the wavemaker?
  #1
Member
 
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 51
Rep Power: 3
pashazanousi is on a distinguished road
I simulated a NWT to study an elastic plate vibration fixed on the tank floor exposed to group waves. but the generated waves disappear before reaching the plate.
I used ANSYS CFX with VOF model and Laminar flow model.

NWT.PNG
__________________
Best regards

Saeed Pashazanousi
Urmia University
Tel: 0098 936 811 864
What's App: 0098 936 811 8647
Email: st_s.pashazanousi@urmia.ac.ir
pashazanousi is offline   Reply With Quote

Old   July 11, 2021, 19:58
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,871
Rep Power: 132
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I have no idea what a NWT is. Please do not assume people know what your acronyms mean.

But the answer to your question is you have too much dissipation. This is probably due to a poor simulation setup, possibly things like:
* Mesh too coarse
* Not converging tight enough
* Not high enough order advection scheme
* Other numerics too diffusive (interpolation schemes on other variables)
* Unsuitable advection scheme on VOF equation (should use compressive)
* Time step too large
* Need double precision numerics
aero_head likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   July 18, 2021, 22:30
Post
  #3
Member
 
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 51
Rep Power: 3
pashazanousi is on a distinguished road
Thanks, ghorrocks

Sorry for late reply
You're right. I'm sorry for that mistake.
The NWT is the abbreviation for Numerical Wave tank.

Let's back to my problem:
The excitation period is about 2.96 sec and I considered the timestep equal to 0.01 sec.
My computational mesh is 100 per wavelength and 21 per wave height in the free surface area. The free surface area height is about two-wave height.
I used RMS residual target with 1E-4. Max. Coefficient loop of 200 used in CFX-pre and Max 20 Iteration for the coupling solver.
Simulation Time=180 sec
I selected these parameters according to recommendations in references and papers.
What is your idea about these parameters?
__________________
Best regards

Saeed Pashazanousi
Urmia University
Tel: 0098 936 811 864
What's App: 0098 936 811 8647
Email: st_s.pashazanousi@urmia.ac.ir
pashazanousi is offline   Reply With Quote

Old   July 18, 2021, 22:35
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,871
Rep Power: 132
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Max coeff loops of 200 sounds way too high. 10 is more like what you want.

Coupling solver? What does this mean? What coupling solver? Are you doing this as a FSI simulation? If so, why?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   July 18, 2021, 22:45
Default
  #5
Member
 
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 51
Rep Power: 3
pashazanousi is on a distinguished road
Thanks for your quick reply
I'm working on vibration of an elastic plate exposed to some group waves.
I need to validate with a paper results.
The paper used non-dimensional parameters. It's made it hard to validate for me!
I think the 2 way FSI is the right solution!
Do you have an other idea?
__________________
Best regards

Saeed Pashazanousi
Urmia University
Tel: 0098 936 811 864
What's App: 0098 936 811 8647
Email: st_s.pashazanousi@urmia.ac.ir
pashazanousi is offline   Reply With Quote

Old   July 18, 2021, 23:01
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,871
Rep Power: 132
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I would get this model working accurately as a CFD only simulation before adding FSI. Putting it another way, there is no point doing the FSI model when the CFD sub-model is inaccurate.

So just do a CFD only model and get it working accurately. Then add the FSI bits.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   July 18, 2021, 23:13
Default
  #7
Member
 
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 51
Rep Power: 3
pashazanousi is on a distinguished road
You mean at first I should do a simulation with 1 way FSI or a simple numerical wave tank with rigid plate?
I simulated an empty tank to validate Wavemaker theory! The results were in agreement with the theory!
Please explain more if you can!
Thanks ghorrocks!
__________________
Best regards

Saeed Pashazanousi
Urmia University
Tel: 0098 936 811 864
What's App: 0098 936 811 8647
Email: st_s.pashazanousi@urmia.ac.ir

Last edited by pashazanousi; July 19, 2021 at 05:52.
pashazanousi is offline   Reply With Quote

Old   July 19, 2021, 00:13
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,871
Rep Power: 132
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
A simple numerical wave tank with a rigid plate sounds like a good next step.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   July 19, 2021, 05:51
Default
  #9
Member
 
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 51
Rep Power: 3
pashazanousi is on a distinguished road
Thanks, ghorrocks
I will try it and share the results here
__________________
Best regards

Saeed Pashazanousi
Urmia University
Tel: 0098 936 811 864
What's App: 0098 936 811 8647
Email: st_s.pashazanousi@urmia.ac.ir
pashazanousi is offline   Reply With Quote

Old   July 19, 2021, 08:07
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,871
Rep Power: 132
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
You don't have to share it. What I describe is just good engineering practise: If you have a complex system of many parts and it does not work, then what is wrong? It is hard to fix as it is so complex.

So separate out all the individual component systems and get them working properly by themselves. Time spent doing this at the beginning means that when the complex system fails to work (like it always does first time around) then you know the problem has to be the interaction between the systems, because all the systems by themselves work OK.

This applies to any engineering system, not just CFD.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   July 19, 2021, 08:50
Default
  #11
Member
 
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 51
Rep Power: 3
pashazanousi is on a distinguished road
Thank you for your generosity ghorrocks
You are so good and right is yours.
I will do as you said.
__________________
Best regards

Saeed Pashazanousi
Urmia University
Tel: 0098 936 811 864
What's App: 0098 936 811 8647
Email: st_s.pashazanousi@urmia.ac.ir
pashazanousi is offline   Reply With Quote

Old   July 20, 2021, 19:24
Default
  #12
Member
 
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 51
Rep Power: 3
pashazanousi is on a distinguished road
Hi ghorrocks
I'm using a Desktop PC with these configurations:
CPU: Intel 10600 corei5
Ram: 16 GB ram
SSD & HDD: 240 GB+ 4 TB
I want to set up a MPI Local Parallel but I don't know how should I do it.
__________________
Best regards

Saeed Pashazanousi
Urmia University
Tel: 0098 936 811 864
What's App: 0098 936 811 8647
Email: st_s.pashazanousi@urmia.ac.ir
pashazanousi is offline   Reply With Quote

Old   July 20, 2021, 20:12
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,871
Rep Power: 132
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Setting up parallel simulations is all described in the installation manual.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   July 20, 2021, 20:53
Default
  #14
Member
 
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 51
Rep Power: 3
pashazanousi is on a distinguished road
Thank you ghorrocks
I study the manual about how set up a MPI Local parallel but honestly I understand almost nothing!

But I defined a MPI Parallel Partition for CFX Solver with specified direction(1,0,0) and High Priority! I set 2 for allocated factor!
I don't know are they the correct settings or not but Now the system is running well with 4 core (Max allowed partitions for free student version of Ansys).

Thank you for your attention and the time you spent
pashazanousi is offline   Reply With Quote

Old   August 19, 2021, 15:51
Default
  #15
Member
 
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 51
Rep Power: 3
pashazanousi is on a distinguished road
Hi ghorrocks
I set the coupling residual equal to 0.01 (default value) and maximum coupling iteration equal to 20.
Does this setting lead to a good result?
__________________
Best regards

Saeed Pashazanousi
Urmia University
Tel: 0098 936 811 864
What's App: 0098 936 811 8647
Email: st_s.pashazanousi@urmia.ac.ir
pashazanousi is offline   Reply With Quote

Old   August 19, 2021, 18:19
Default
  #16
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,871
Rep Power: 132
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
If you have parameters which you do not know if they are set correctly then do a sensitivity analysis to find out if they are important. Try coupling residuals of 0.001, 0.01 and 0.1 and see if it makes any difference. Likewise try max coupling iterations of 10, 20 and 40.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   August 19, 2021, 21:01
Default
  #17
Member
 
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 51
Rep Power: 3
pashazanousi is on a distinguished road
Thank you ghorrocks
OK, I got it! I will do it!
But I want to know what is the meaning of residual target in the coupling regions!
For example for mesh transfer data from transient structural to CFX, I choose 0.01! It means 0.01 m as residual target? Or for Force Data transfer, 0.01 for residual target means 0.01 Newton?
I need the residual target equal to 0.0001 m for the mesh displacement!
I can't anything about that in Ansys help or other documents!
__________________
Best regards

Saeed Pashazanousi
Urmia University
Tel: 0098 936 811 864
What's App: 0098 936 811 8647
Email: st_s.pashazanousi@urmia.ac.ir
pashazanousi is offline   Reply With Quote

Old   August 19, 2021, 21:06
Default
  #18
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,871
Rep Power: 132
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I don't know the exact definition of that residual target. All I can say is to look in the documentation.

If you do a sensitivity analysis and show that you have set it tight enough that it is not affecting results then it does not matter what the exact definition is. It just means you have set it tight enough that your results are accurate (for that parameter at least).
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Reply

Tags
ansys cfx, freesurface, fsi 2-way coupling, transient analisys, water waves

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
HELP - Moving car simulation in fluent Brad Wells FLUENT 7 January 4, 2018 20:55
2D selective mesh generation Durga Sravan ANSYS 17 February 5, 2014 01:56
Weird representation of generated waves stonescar STAR-CCM+ 2 June 21, 2013 11:19
CFD Animations of waves, ships, and turbulence---- Douglas Dommermuth Main CFD Forum 23 January 8, 2008 13:41
Will compression waves overtake a moving shock? GRA Main CFD Forum 2 October 19, 2006 01:24


All times are GMT -4. The time now is 04:51.