[raul_xusernamex_]

Hello, I would like to try to simulate the scour in a pipe under conditions of only waves, but the results show me values that do not correspond to the domain.
I would like to know what is wrong since I make sure that all the commands are correct.

However, something goes wrong, I show the jpg file where that information comes out.

Control.txt

C 11 6
C 12 3
C 13 3
C 14 8
C 15 21
C 16 3

B 1 0.01

B 10 -4.4 4.4 0.0 0.01 -0.3 1.0
O 32 0.0 0.1 0.05

M 20 2

M 10 4

ctr.txt

B 10 1
B 50 0.0001
B 90 1
B 93 0.4 1.43
B 98 3
B 99 4

D 10 4
D 20 2
D 30 1

F 30 3
F 35 4
F 40 3
F 42 1.0
F 60 0.40

I 12 1

N 10 18
N 40 3
N 41 60.0
N 47 0.1

M 10 4

S 10 1
S 11 1
S 12 1
S 20 0.00058
S 21 3
S 22 2700
S 24 0.4
S 25 45
S 32 4
S 57 0


P 10 1
P 30 0.1
P 40 1
P 42 1.0

T 10 0

W 22 -9.81

P 52 0.0125
P 53 1
P 55 0.50

P 51 2.50 0.0125
P 51 5.00 0.0125
P 51 15.0 0.0125
P 51 20.0 0.0125

[kamath]

Hi Hernest,
You seem to have invalid values in your domain (seen from the yellow coloured domain that Paraview shows you).

I would suggest these changes first:
in control.txt, use
S 32 in place of O 32

In ctrl

Use N 10 14 , N 11 11 (I am not sure why you use N 10 18, though that should not be problem
Set S 12 0
S 13 1.0
Choose appropriate S 47 and 48 values based on you simulation.
(Idea here is to start the sediment transport after a couple of waves have passed. The "first" two waves are generally transient and can be ignored)
Include S 80 2 and S 90 1.

It would be also handy to add S 73 to introduce a relaxation around the region of sediment transport.

With these recommendations I take you to a base case for sediment transport under waves. We can then see where the problems might be arising from.

Hope this helps

[raul_xusernamex_]

Thank you very much Mr. Kamath for your willingness to answer and support users in the doubts that one needs.
I made the changes that I had but I have problems associated with the "N" parameter this time I think, because in the execution of the REEF3D program it shows this in several iterations:

ERROR detected by Hypre .... BEGIN
ERROR -- hypre_BiCGSTABSolve: IN and/or NaN detected on input.
The user probably put non-numeric data in b.
Returning the error flag +=101. Program not finished.
ERROR detected by Hypre... END

Also I think it is important to notice this message at the beginning of the execution:

Initialize fdm
[LAPTOP-BGLQJA1P:00077] 3 more processes sent a help message help-btl-vader.txt /cma-permission-denied
[LAPTOP-BGLQJA1P:00077] Set the MCA parameter "orte_base_help_aggregate" to 0 to see all help/error messages
starting start
creating objects
Wave tank: no wave specified;
number of cells: 114400
starting diver_ini
initializing solid.....

Where it stands out that there is no wave in the tank, which in the command B 93 0.4 1.43 indicates the opposite.

I would like to show the changes to see if we can detect what problems exist this time.

control.txt

C11 6
C12 3
C13 3
C14 8
C15 21
C16 3

B 1 0.01

B10 -4.4 4.4 0.0 0.01 -0.3 1.0
S32 0.0 0.1 0.05

M 20 2

M 10 4

ctrl.txt

B 10 1
B 50 0.0001
B 90 1
B 93 0.4 1.43
B 98 3
B 99 4

D 10 4
D 20 2
D 30 1

F 30 3
F 35 4
F 40 3
F 42 1.0
F 60 0.40

I 12 1

N 10 14
N 11 11
N 40 3
N 41 60.0
N 47 0.1

M 10 4

S 10 1
S 11 1
S 12 0
S 13 1.0
S 20 0.00058
S 21 3
S 22 2700
S 24 0.4
S 25 45
S 32 4
S 47 0.5
S 48 0.5
S 57 0
S 71 -3.0
S 72 3.0
S 80 2
S 90 1


P 10 1
P 30 0.1
P 40 1
P 42 1.0

T 10 2

W22 -9.81

P 52 0.005
P 53 1
P 55 0.40

P51 -1.0 0.005
P51 0.0 0.005
P51 1.0 0.005
P51 2.0 0.005

The simulation is not yet finished executing to show the results I wanted but as I go studying each command in discussion.
Very grateful for your time.

[kamath]

I still see that the solver receives invalid values.
But first let us solve the no wave specified problem

You have to include a B 92 call.
B 93 input provides the input wave height and period, but these need to go into a theory for the generation of said waves.
Start with say B 92 4 (or calculate from Le Mehuate's chart which theory is valid)

[raul_xusernamex_]

Excellent!! forget that detail, that I must incorporate the entries of the wave theories.
Because Le Méhaute's scheme (1976) requires that the theories meet a certain range of values, I have calculated new input values for incident waves B 93 0.1 1.43 where is the The generated wave is subject to a third-order Stokes theory, but since it is not clearly indicated in the diagram, I am going to adjust it to second-order Stokes theories, that is, B 92 4 .

I had entered again, in an erroneous way, the following wave parameters (I had miscalculated the Le Mehaute diagram)

B 92 5
B 93 0,1 1,43

At least this time I have managed to obtain valid values in the simulation (attached image). However, I have not yet achieved my objective, which is to move sediments, that is, I need to obtain the changes in the bed where the Pipeline is located, to calculate scour.
I was thinking, based on what I studied, to incorporate the following parameters in the code.

S 16 3
S 17 1
S 25 35 (Change this parameter)
S 30 0,11 (Shields parameter, I think this parameter is important to know if there are sediment movements or not. But I still don't know what value would be appropriate for it to work).

S 73 ? (I am not clear how to enter this parameter yet, so I replaced them with S 71 -3.0 y S 72 3.0 )
S 100 1
S 101 2

In short, I need to solve now:
Current problem: I can't move sediments with the current code, I wanted to see if we could check and see if the parameters I propose would work for what I need.

current target: Obtain the changes in the seabed where the pipe representing the scour is located. I am working on the paper "Numerical modeling of pipeline scour under the combined action of waves and current with free-surface capturing$ , in section 3.2.1 Pipeline scour under waves

I attach the image, which is what I have been able to achieve so far, with the "B" parameters that I modified at the beginning, and right now I am correcting.

Very grateful for your kindness
Greetings...

[Ronja]

Hi,


Could you post your current input files, so that we have the exact commands you are using now?


Thanks!

[raul_xusernamex_]

Originally Posted by Ronja

Hi,


Could you post your current input files, so that we have the exact commands you are using now?


Thanks!

Yes, of course, here I sent the files that I used to obtain the simulation that I have so far of the image shown.
I would like to replicate at least one case of scour in pipelines.

Thank you greetings for the help.

[Ronja]

I had a look, here a few comments that hopefully help you to find a good setup:

- be aware of S 19 - total sediment modelling time against hydrodynamic modelling time (check also S 13 .. S 15, it is decoupled by default) and the interval for the sediment calculations (S 41 .. S 48). The (excess) bed shear stress will be evaluated in every iteration of the bed load algorithm.
- check S 16 1 against S 16 3
- domain height can be chosen smaller since your still water level is at 0.40 m, as for now, you have 0.6 m of air phase and a wave height of only 0.1 m
- S 73 gives you the option to use a relaxation zone method for the sediment level to avoid abrupt changes that can lead to problems e.g. at a boundary. (value = level, distance = length of the zone, line angle = if you want to define the zone with an angle otherwise 0, x and y = location) You could use it at the start/end of your NWT.
- The shields parameter influences the critical shear stress directly, however I do not recommend to tune your particle pickup with this parameter, but use a reasonable value. For theory behind it you might also want to check the Shields diagramm depending on the grain Reynolds number and the dimensionless crit. shear stress

[raul_xusernamex_]

Ohhh!! muchas gracias. Ire a configurar mi codigo y probar de la mejor manera.

Saludos

[kamath]

De nada. ¡Tú puedes!

[raul_xusernamex_]

Hello, good afternoon.
Before continuing with Ronja's suggestions in one of the comments above, I wanted to try different values of the element size. For example, I wanted to refine the calculation mesh a bit and I get an error when running REEF3D when calculating with a smaller element size.
Below I show the new input values in my files and the error message that I have problems.

control.txt

C 11 6
C 12 3
C 13 3
C 14 8
C 15 21
C 16 3

B 1 0.005

B 10 -4.4 4.4 0.0 0.005 -0.3 1.0
B 130 1
S 32 0.0 0.1 0.05

M 20 2

M 10 4

ctrl.txt

B 10 1
B 50 0.0001
B 90 1
B 92 4
B 93 0.1 1.43
B 98 3
B 99 4

D 10 4
D 20 2
D 30 1

F 30 3
F 35 4
F 40 3
F 42 1.0
F 60 0.40

I 12 1

N 10 18
N 11 11
N 40 3
N 41 60.0
N 47 0.1

M 10 4

S 10 1
S 11 1
S 12 0
S 13 1.0
S 20 0.00058
S 21 3
S 22 2700
S 24 0.4
S 25 45
S 32 4
S 30 0.11
S 47 0.5
S 48 0.5
S 57 0
S 71 -3.0
S 72 3.0
S 77 -3.0 4.1
S 80 2
S 90 1


P 10 1
P 30 0.1
P 40 1
P 42 1.0

T 10 2

W 22 -9.81

P 52 0.0025
P 53 1
P 55 0.40
P 122 1

P 51 -1.0 0.0025
P 51 0.0 0.0025
P 51 1.0 0.0025
P 51 2.0 0.0025

Then the software stops and does not continue.

[raul_xusernamex_]

Originally Posted by raul_xusernamex_

Hello, good afternoon.
Before continuing with Ronja's suggestions in one of the comments above, I wanted to try different values of the element size. For example, I wanted to refine the calculation mesh a bit and I get an error when running REEF3D when calculating with a smaller element size.
Below I show the new input values in my files and the error message that I have problems.

control.txt

C 11 6
C 12 3
C 13 3
C 14 8
C 15 21
C 16 3

B 1 0.005

B 10 -4.4 4.4 0.0 0.005 -0.3 1.0
B 130 1
S 32 0.0 0.1 0.05

M 20 2

M 10 4

ctrl.txt

B 10 1
B 50 0.0001
B 90 1
B 92 4
B 93 0.1 1.43
B 98 3
B 99 4

D 10 4
D 20 2
D 30 1

F 30 3
F 35 4
F 40 3
F 42 1.0
F 60 0.40

I 12 1

N 10 18
N 11 11
N 40 3
N 41 60.0
N 47 0.1

M 10 4

S 10 1
S 11 1
S 12 0
S 13 1.0
S 20 0.00058
S 21 3
S 22 2700
S 24 0.4
S 25 45
S 32 4
S 30 0.11
S 47 0.5
S 48 0.5
S 57 0
S 71 -3.0
S 72 3.0
S 77 -3.0 4.1
S 80 2
S 90 1


P 10 1
P 30 0.1
P 40 1
P 42 1.0

T 10 2

W 22 -9.81

P 52 0.0025
P 53 1
P 55 0.40
P 122 1

P 51 -1.0 0.0025
P 51 0.0 0.0025
P 51 1.0 0.0025
P 51 2.0 0.0025

Then the software stops and does not continue.

I wanted to know what is due to this type of errors.

[kamath]

There have reports of this problem (program fails to work after grid refinement) on Ubuntu on Windows.
I am guessing you are also using the Ubuntu App on windows?
If so, try the latest release_candidate for DiveMESH and REEF3D.

As a result of this discussion:
REEF3D(22.03 & 22.04) Segmentation fault - problem solving
a bug was detected, which affects windows platforms.

Also, the increase in number of cells results in increased RAM usage. The RAM optimisation carried out recently should also help.

At the end of the day, you will eventually meet a hardware restriction for grid refinement.

So, check with the latest release candidate if the problem persists and let us know.