Free surface Problem

[martinjacoby]

Hi. 

I cannot run a simulation with free surface, the results that I obteinded are incorrect or illogical so i suppose that there is something i am not configuring correctly

Here are my steps..for example in a dam model

1. Load model from Fusion
2. Launch CFD Simulation from Fusion
3. Apply material to all (water)
4. Apply HOF to one of the volumes
5. Solve (enable Free surface, vector (0,0,-1) gravity Z =9810mm/s2
6. Define interval an time steps

Its ok my workflow? or I am doing something wrong?

Thanks

[waited]

Hi Martin,

A couple more questions,

1. what is your time step size?

2. how many elements are in your model?

If you can attach your cfz file, I can be more specific.

Dave

[Jon.Wilde]

It also sounds like you are doubling up on gravity - setting the 0,0,-1 in the free surface window is sufficient.

[waited]

Good catch Jon.

When you set the earth gravity direction vector to 0,0,-1, it is more than a direction, if also infers magnitude.  So, 0,0,-1 will assign 980 mm/s^s as the magnitude as well.

The Acceleration components are normally used for non-gravitational accelerations ( like sloshing tanks, earthquakes, etc. ).  So if you only have gravity, then use only the upper input and leave the Acceleration components zero.

Dave

[martinjacoby]

What a good Support team! Thanks! 

Altought I still can not reach good results in free surface simulation, Here is  an example, a simple run of water, the quality of the free surface is very poor and sounds not to accurate, its seems like if there is something I am missing...

Martin

[waited]

thanks Martin for the file download.  I run this a bit and see how we can improve it.  Dave

[waited · Accepted solution]

Martin,

Made a few changes ( cfz file attached ),

For a simple run of water, like a river, it is best to specify the inlet flow rate ( 500 m^3/s ) and set pressure = 0 on the outlet plane.  SimCFD will automatically add in the static pressure head based on water level on this exit plane.

The free surface option requires a good quality mesh and the mesh needs to be fine enough to capture the water surface shape.  For the simple run of water, I set a manual mesh, size = 1 meter for both volumes.

In the attached pressure image you can see the hydrostatic pressure head.  Also note that the water level drops slightly from inlet to outlet as expected.

Dave

[martinjacoby]

Dave! 

Thanks for the work you have done! I Improved a lot my free surface simualtions with adjusting the mesh size! 

Last question! In order to evaluate fluid in a forced movement situation I designed a simple circulating water tank with a free surface at the top of it, where the phenomenon of free surface plays a important role. Its ok how did I set the boundaries and mesh size? A proppeler its supposed to be the one that gives fluid momentum. How will you do to represent turbulence made by a proppeler?

Thanks in advance! 

Martin

[martinjacoby]

Anyone??

[Jon.Wilde]

Hi Martin,

I can jump in here.

Firstly, could this not be run in 2D? It would be so much faster and probably more accurate due to the mesh requirements of a fres surface model.

What is the actual goal? There is only one inlet and one outlet right?

Some points:

• Suppress the solids from the mesh
• Refine the fluid, probably using a uniform mesh (or manual, it's the same and a manual mesh is quicker to assign) as your wave front will pass through the entire model (I think - or is it full already?) - have at least 5 elements across the thickness of the channel (this is a real minimum). In 2D you could go mesh crazy and run it faster too
• Could you use an internal fan to cause rotation in the flow, or try the external fan boundary condition. It might need to be circular though. Start simple - try just the flow rate first

I hope this helps.

Kind regards,

Jon

[martinjacoby]

Thanks Jon!

Are you saying that free surface simulation could be run in a 2D geometry?

The actual goal is to simulate the flow path in a circulating open water tank, and also study the free surface  phenomenon

There is only a inlet and outlet 

What do you mean by suppresing the solids from the mesh?

Its better to insert a rotating solid propeller or to assign external fan boundary condition?

[Jon.Wilde · Accepted solution]

Hi Martin,

No problem.

Yes, discounting any fluid rotation at the inlet, a 2D model would be great.

I was not sure if this was empty initially as you have HOF set, which means it is 100% full of water. Which leaves me unsure why you need to run a free surface analysis 🙂

Suppress the solids from the mesh - within meshing select the solids and press 'suppress'. This means they will not be meshed, which saves on memory.

Honestly I am not sure on the fan, either could be OK. I suggest you try both and see which best represents what you need. I would not recommend using an actual rotating part though, that would be hugely memory intensive. Either an 'internal fan' as a solid part (applied to a cylinder within a shroud) or just apply the boundary condition.

Kind regards,

Jon

[martinjacoby]

Jon,

Thanks for your advices. Here I attached the actual file of the channel, with all your advices taken into account.

The goal of this simulation is to study the flow in an circulating water channel, used in marine engineering to test prototypes of ships. Thats why I was interested in rotating regions to study the turbulence phenomenon that they produce.

Are the settings I applied ok? Any suggestion?

Thanks 

PD: I am a marine engineering student, I had downloaded the Student Version from this site.

[martinjacoby]

Sorry, the volume in which the propeller are, is with HOF because its full. The volume above it is to enable waves in the surface of the volume with HOF, as its a open channel.

[martinjacoby]

Did you recieved the file? Thanks

[Jon.Wilde]

Hi,

Yes, but I have been out for a bit.

If you plan to use actual propellors you ought to read this guide as the setup will be pretty complex. Are you sure you need to model them?

Barring your propellors (they need rotating regions added - just use the tube diameter) the setup looks OK). You are also likely to need more mesh, especially where you have a free surface.

I suggest you first run this in 2D to get an understanding of the mesh you will need and then run 3D without the rotating regions. Then add in the propellors - they are going to need a lot of mesh. A model like this is likely to need quite a large amount of RAM to be accurate. Just a single propellor simulation would need a good 10-20GB. Could you not just use a fan boundary condition at the inlet to get some swirl and have a P=0 at the outlet with a gap inbetween?

Kind regards,

Jon

[martinjacoby]

Jon!

I was wondering cause wasn’t sure if the attachment was send. As always your support is outstanding!

If I use a fan boundary condition, its seems that there is a big impulse of momentum, and the free surface made a huge wave, explained by a suddenly addition of mass to the system. How would you do to avoid that effect? Giving boundary condition a transcendent value? I did it and the effect was the same.

How this analysis could be run in 2D? It’s possible to load a planar geometric? I mean in terms of transversal turbulence caused by rotator blade.

[Jon.Wilde]

Hi!

Yep, I am still here 🙂

(only just notied I didn't send this reply, apologies).

A 2D model would just be stepping back a bit to be sure you understand the meshing levels required for a free surface model. It would only have a simple vel inlet and P=0 outlet, no rotation.