[keshav_20]

Hello Arun
I am trying to create a cylinder in z-direction at location x = 17.0 and z = 0.2 and radius 0.1. However, the entire fluid domain is removed down below the cylinder. I am attaching the file below.

B 2 1000 1 10
B 10 0.0 40.0 0.0 0.04 0.0 1.0

S 32 17.0 0.2 0.1

// S 61 11.0 17.0 0.0 0.04 0.0 0.3
// S 10 17.0 19.0 0.0 0.04 0.0 0.3
// S 61 19.0 22.0 0.0 0.04 0.3 0.0

// B 101 5
// B 111 10.0
// B 114 17.0

// B 103 5
// B 113 10.0
// B 116 0.3

B 101 5
B 111 10
B 114 17.0

B 103 5
B 113 10.0
B 116 0.2

M 10 4
M 20 2

[kamath]

Hi Keshav,

I am unable to see the problem.
From your attached screenshot, the cylinder is formed, it is in the y-direction and at x=17.0 m.

The grid size probably makes a cut that is not exactly cylindrical, but that is should be fixed with improving the grid?
May be you could start with a regular mesh and then design an appropriate stretched mesh for your case?

[keshav_20]

Hello Dr. Arun
I have tried refining the mesh around the cylinder, still I am receiving this issue. Further, I attempted tutorial on "Flow around a circular pier" with no change in "control.txt" and "ctrl.txt". In this case, I am not seeing the extruded cut for circular pier as can be seen in the image attached.

Thanks and regards
Keshav

[kamath]

Technically, I don't get the cut out in the slice view with your original input either.

Anyway, here are some checks for you

1. Make sure you have the latest version.

2. Replace B 2 with B 1 0.025. Include P 20 1, P 25 1, run for one iteration.
Check output in Paraview. Also check contour solid = 0 on the slice.

This is what I have with the latest version, seems alright?

[keshav_20]

Hello Dr. Arun
I tried the suggestions you suggested. However, I am still getting the correct domain as yours. I have attached the screenshot here.

[kamath]

You seem to be using the FNPF module that uses the Laplace equations with a sigma grid.

6dof floating structures are not supported in this module.

Remove A 10 3 and you will be fine.

[keshav_20]

Although the structure is floating. However, I am considering it as fixed circular. In such case, FNPF module should work, isn't it? In any case, I am still not getting fluid domain with extruded cut of vertical cylinder as I mention in my previous post thread where I am using CFD module only.
I want to use REEF3D:FNPF module to evaluate load on submerged horizontal cylinder as it is computational faster approach. Here, I am approximating the structure to be fixed circular wall only.

[kamath]

You can calculate forces on a structure using the FNPF module only through the ALE approach.
https://doi.org/10.1016/j.marstruc.2022.103190

You cannot include a physical object in the domain to calculate forces.

With regards to the CFD module, we have moved away from a cut-cell approach.
Use the S options for the structure, use P 25 1 and then you can visualise the representation of the structure in the domain using contour = 0 on "solid" in Paraview.

[keshav_20]

Hello Dr. Arun
I have attempted to use CFD module to study flow around the horizontal submerged cylinder treated as wall under current flow. However, REEF3D application stops at reading ctrl as shown in the attached screenshot. I took reference from "tutorial on flow around circular pier". Where am I possibly going wrong? I am attaching the file herewith.

As to the previous discussion, is ALE method integrated into existing REEF code? I am only seeing B85 which uses Morison's equation based on ALE to calculate the load on circular cylinder (I guess). Is this option valid to other shapes as well?

[kamath]

When the execution stops at

"read ctrl"

it means that the program has encountered something in the input file that it is unable to process.

From your attachment, I see you have an older version of the code or text copied from the manual. These have comments which use capital letters.

When REEF3D encounters a capital letter in the input file, it looks for a number to determine the input command option. When there is no valid input read, it just stops there.

The latest download from github has solved files without the comments. (Of course, you can also manually remove the comments, or mainly the capital letters)


Wrt ALE, yes currently only Morison based circular cylinder forces. I am working on making it more general and empirics-free.
The major point though is that FNPF is meant for wave propagation/ event identification and not a replacement for NS

[keshav_20]

Hello REEF3D team,
I am no successfully able to run the program. However, the solution generates the scrap value or residual values. I am simulating the horizontal cylinder in current flow of 0.4m/s using k-omega model. I have referred to tutorial on vortex shedding and flow past the cylinder as benchmarks. I am not able to find where I am going wrong. I am attaching the files herewith.

[kamath]

In your files,
the level set time marching and reinitialisation are set to 0.
Should be F 30 3
F 40 3
for example.

Also you don't have a definition for water depth
F 60 0.2 for example.

Without these values there is no free surface to calculate your free surface flow problem and the values for the free surface and velocities will be junk values.

Hope that helps

[keshav_20]

I am considering the entire rectangular domain as fluid domain which doesn't need to have a free surface. I have attached the image of numerical setup for your reference.
Also, after hit and trial, I found out that if I use W 10, I am getting some results. However, when I tried with W 11, I get residual values. But I want to provide a velocity inlet of 0.4m/s as input. Why is this happening?

//W 11 0.4 0 0
W 10 0.0016

[keshav_20]

Sorry I forgot to attach the files in the previous reply.
Kindly find the attachment here.

Thanking you
Keshav

[keshav_20]

I forgot to attach the files in the previous thread.
Kindly find the attachment here.

Thanking you
Keshav Pathak

[valgrinda]

If you choose B 60 1, then you need to use W 10. This is made with free surface flows in mind and will control the discharge for a dynamic free surface. W 11 works only for B 60 0.

[keshav_20]

Thanks for support Prof. Hans
As per your suggestion, I have used B 61 1 instead of B 60. However, I am getting error "EMERGENCY STOP -- velocities exceeding critical value N 61".

Furthermore, if I increase the grid in vertical direction beyond 50 (B 2 8000 1 50), I get "segmentation fault" error while running DiveMESH module. I have attached the files below.

Thank you
Keshav Pathak

[valgrinda]

After how many iterations do you get the Emergency stop warning?

[keshav_20]

Hello prof. Hans
The "Emergency error" pops up after 12568 iterations.
Further, can you also possible reason behind the segmentation fault error in DiveMESH. I am using the 6 Core processor with 32GB ram.

Thanks
Keshav

[valgrinda]

Hi Keshav,

my recommendations:
- use adaptive timestepping
- use ioflow to control the inflow and start with the potential flow initialization
- then use the discharge instead of the velocity in the inlet
- use implicit diffusion

-> see the attached setup

The problem with DIVEMesh has been fixed in the new release 22.11.