CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > REEF3D

Breaking waves in FNPF

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

LinkBack Thread Tools Search this Thread Display Modes
Old   October 2, 2022, 00:00
Post Breaking waves in FNPF
New Member
Felix Daddo
Join Date: Aug 2022
Location: Sydney, Australia
Posts: 25
Rep Power: 3
FelixD is on a distinguished road
Hey REEF3D users,

I have been playing around with simulating breaking waves in the fnpf module. This is based off tutorial 8.3: Wave breaking over a mild slope.

I found that I was getting an N 61 error (exceeding critical velocities) when using the tutorial files exactly as they were. I found two ways to work around this issue and thought I'd share them in case anyone else has the same issue and if there is anything wrong with what I've done, hopefully someone can point that out too. The files I have used are exactly as in the tutorial except for the changes made below:

Workaround 1: reduce the cfl number (N 47)
This works but it must be made quite low which slows the simulation It also may not stop the issue from arising if the simulation time is increased.

Workaround 2: increase the length of the coastal relaxation zone (A 341)
In the tutorial this is only 2 cells. I increased it to 10 and was able to run the entire simulation with the original cfl number

Thanks, Felix
FelixD is offline   Reply With Quote

Old   October 4, 2022, 03:50
Senior Member
Arun Kamath
Join Date: Nov 2014
Location: Trondheim, Norway
Posts: 265
Rep Power: 13
kamath is on a distinguished road
Hi Felix,

In general, an N 61 error points at something going wrong in the simulation causing the CFL number to go out of bounds and resulting in a crash.

I would highly suggest using paraview to identify the location at which the crash occurs. This can help a lot.

Having said that, with or without doing the above, you did arrive at two good bandaids to avoid the crash.

1. Reducing N 47- controlling the CFL to lower values will result in more control over the velocities going out of bounds, at the cost of a slower simulation as you noticed. However, this approach may not always work.

2. This approach also helps avoid the crash but what it covers over is the possible problems near the coastline. You introduce a longer "dead zone" than necessary.

However, your approach did point to where the problem was
(And possibly points to a bug that might have creeped in, so we are looking into it)

If you use the original files and look at the Paraview output, you will notice that there is a stray "free surface line" at the end of the flume. You will also notice that at the time of the crash, the free surface seems to "go under" the solid slope.
The latter points to a wrong calculation of the coastline, i.e it seems like the coastline is not detected where it is supposed to be (at the water-solid boundary) and possibly at the end of the 32 m slope (where a speck of water was seen at the beginning)

So an appropriate solution would be to cut the flume to 20 m and set the height to 0.4047 m and at the same time the grid focus point in z to be at 0.4047 m.
The simulation runs to completion.

Finally, we are looking into a possible problem with initialisation of the water level for FNPF simulations with emergent objects. Thank you for bringing this to our notice.
X years with REEF3D
kamath is offline   Reply With Quote

Old   October 9, 2022, 07:14
Super Moderator
Hans Bihs
Join Date: Jun 2009
Location: Trondheim, Norway
Posts: 377
Rep Power: 17
valgrinda is on a distinguished road
Hi Felix,

could you share your cases setups for testing? Thanks!
Hans Bihs
valgrinda is offline   Reply With Quote

Old   October 12, 2022, 01:42
New Member
Felix Daddo
Join Date: Aug 2022
Location: Sydney, Australia
Posts: 25
Rep Power: 3
FelixD is on a distinguished road
Originally Posted by valgrinda View Post
Hi Felix,

could you share your cases setups for testing? Thanks!
Thanks Hans,

I will attach the files for the fnpf simulation. I am trying to use HDC to model the breaking wave with CFD once the waves reach the domain. I am able to successfully do this for this case.

The other part of my studies is incorporating the sediment transport model, however whenever I change the solid to a topo to model sediment transfer the simulation crashes due to high velocity at the foot of the bed. I've been trying for days but have had no success with it at all.
Attached Files
File Type: zip fnpf (1.3 KB, 7 views)
File Type: zip cfd files - sediment (1.2 KB, 3 views)
File Type: zip cfd files - breaking wave (no sediment transfer).zip (663 Bytes, 2 views)
FelixD is offline   Reply With Quote


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
Breaking Waves in REEF3D SFLOW, A 246 vs A 248 pjoynt REEF3D 3 March 22, 2022 06:22
Animations of Ship Waves and Breaking Waves Dommermuth Main CFD Forum 1 August 15, 2011 12:10
CFD Animations of breaking waves Dommermuth Main CFD Forum 0 June 17, 2009 11:47
Breaking Water Waves Erik Wickley-Olsen Main CFD Forum 9 May 18, 2007 10:50
Breaking Water Waves Erik Wickely-Olsen FLUENT 0 May 4, 2007 12:44

All times are GMT -4. The time now is 22:26.