[pj6620]

Hey guys!

I'm making a model in Flow 3D, about the final stages of placing a GBS on the seafloor (1.5m above seabed till 0m above seabed). The total height of my model is 2 m sand + 1,5m water height + GBS. The z=0 line is at the surface of the sand.
I have some problems with my boundary conditions, and with my initial state. t this moment, the initial state does NOT contain water, how can I fix this?

I have a circular mesh, with the following boundary conditions:

- zmin (z=-2m) wall
- zmax (z=4m) pressure (equal to 50m water depth)
- xmin pressure (fluid fraction = 1, fluid elevation = 50, no specified pressure)
- xmax = same as xmin
- ymin = same as xmin
- ymax = same as xmin

My initial conditions are:
- pressure: hydrostatic
- fluid initialization: fluid elevation = 0

Can anyone please help me? I tried the manual, but I find it quite confusing

Thanx!

[sycst911]

Originally Posted by pj6620

Hey guys!

I'm making a model in Flow 3D, about the final stages of placing a GBS on the seafloor (1.5m above seabed till 0m above seabed). The total height of my model is 2 m sand + 1,5m water height + GBS. The z=0 line is at the surface of the sand.
I have some problems with my boundary conditions, and with my initial state. t this moment, the initial state does NOT contain water, how can I fix this?

I have a circular mesh, with the following boundary conditions:

- zmin (z=-2m) wall
- zmax (z=4m) pressure (equal to 50m water depth)
- xmin pressure (fluid fraction = 1, fluid elevation = 50, no specified pressure)
- xmax = same as xmin
- ymin = same as xmin
- ymax = same as xmin

My initial conditions are:
- pressure: hydrostatic
- fluid initialization: fluid elevation = 0

Can anyone please help me? I tried the manual, but I find it quite confusing

Thanx!

Add fluid at initial stage (t=0)

[pj6620]

Thanx for your reply, but how do i do that?

[sycst911]

Please check as per attached.

[sycst911]

Originally Posted by pj6620

Thanx for your reply, but how do i do that?

I supposed you have added the fluid region right? but how can you not seen any water? hmm...

[pj6620]

Thanx for your reply!
When I FAVOR my model, I get fluid now!
But, I still think there is a problem with my Boundary conditions, since my solver gets the following error:

pressure iteration diverging - restarting cycle with smaller time-step size

excessive pressure convergence failures

Or is this due to something different?
(I changed my ymin and ymax to S, since I found in the manual: Axisymmetric calculations without swirl (azimuthal flow) call for symmetry-plane boundary conditions on the Y Min and Y Max boundaries.)

[sycst911]

Originally Posted by pj6620

Thanx for your reply!
When I FAVOR my model, I get fluid now!
But, I still think there is a problem with my Boundary conditions, since my solver gets the following error:

pressure iteration diverging - restarting cycle with smaller time-step size

excessive pressure convergence failures

Or is this due to something different?
(I changed my ymin and ymax to S, since I found in the manual: Axisymmetric calculations without swirl (azimuthal flow) call for symmetry-plane boundary conditions on the Y Min and Y Max boundaries.)

Then, set a smaller time-step. LOL

[JBurnham]

It's good you set the y-min and y-max boundaries to Symmetry (S). If you have swirl, you can use Periodic (Pd) to allow fluid to leave one side and re-enter at the same elevation on the other side.

There are some possible reasons you are getting pressure iteration failures:

1) the mesh aspect ratio is not good. Look at the ratio between cell size in Z and cell size in X: it should be <3:1 (big:small), otherwise the calculations are stretched and hard for the computer. The best ratio is 1:1 (squares).

2) try making X-min symmetry also. The X-min boundary is at the center of the cylindrical mesh, which means it is a discontinuity. Using anything but S at the center of a cylindrical mesh is not good.

3) check that your initial fluid conditions (good job checking them with FAVOR!) match the boundary conditions. That is, if there is a free surface elevation set at the X-max pressure boundary, make sure that the initial fluid is at the same height. If it is higher or lower, then a water wall must collapse at t = 0 and that is hard to solve.

4) check your geometry, if you are using an .stl file. .STL format files must be watertight (one shell), and have no bad or reversed facets. Check this using a free program like netfabb Studio, which can also fix bad files if the problems aren't too bad. If netfabb can't fix them, adjust and re-export the .stl files from CAD.

5) check that there are no "sliver cells". Preprocess the simulation, and go to Analyze > 2-D. Click Contour smoothing and activate "no contour smoothing". Plot the results for only one timestep and look for extreme values. Also look to see if there are cells where the open volume is very small, like a little crack between gray solid. If you find these, they are called sliver cells, and they can cause pressure iteration problems. Either resolve them with cells so that there are at least 3 or 4 cells across the sliver, or adjust the geometry so that they are filled in.

6) if you've tried all of the steps above and still have problems, then try running the case as Cartesian instead. Cylindrical meshes are mathematically more difficult for CFD solutions than Cartesian meshes, because the cell volumes change with distance r from the center. Cartesian meshes are easier because they can be made more uniform.

If you have good results, please let me know: I'd love to see your work as you progress. Cheers, - Jeff

[pj6620]

Thanx for your detailed info Jeff!
Unfortunately, that didn't work either, so I made a Cartesian mesh.

The solver works, but I have another problem now (erosion related), I'll make a new thread for that, since it has nothing to do with this problem.

[Zohaib Nisar]

Hello Mr:

change your boundaries conditions like x min = specfice pressure have fluid fraction is 1 & fluid height = your required height,
X max = outflow, y min, y max, z min = wall & last z max = specified pressure haveing fluid fraction is zero. then run the model.

Originally Posted by pj6620

Hey guys!

I'm making a model in Flow 3D, about the final stages of placing a GBS on the seafloor (1.5m above seabed till 0m above seabed). The total height of my model is 2 m sand + 1,5m water height + GBS. The z=0 line is at the surface of the sand.
I have some problems with my boundary conditions, and with my initial state. t this moment, the initial state does NOT contain water, how can I fix this?

I have a circular mesh, with the following boundary conditions:

- zmin (z=-2m) wall
- zmax (z=4m) pressure (equal to 50m water depth)
- xmin pressure (fluid fraction = 1, fluid elevation = 50, no specified pressure)
- xmax = same as xmin
- ymin = same as xmin
- ymax = same as xmin

My initial conditions are:
- pressure: hydrostatic
- fluid initialization: fluid elevation = 0

Can anyone please help me? I tried the manual, but I find it quite confusing

Thanx!