Setting up a porous medium
 

I'm working on a design for one of my projects in university. Its a duct for a tidal turbine.

To simulate the turbines presence in the duct, I wanted to use a porous medium in the center to replicate the rotor. But I am having a hard time setting that center area as just the porous medium. I embedded a cylinder in my CAD drawing so now there are two bodies. But I do not know how to define the interaction between them in the simulation.

Could somebody send me in the right direction of where to start looking? Thanks

Use a momentum source term to do this. They are move general and you can apply a resistance to the flow in any form you like that way.

And the source term can be applied as either a volume or a surface the flow passes through (eg an interface).

ok, my prof recommended a porous medium over a momentum source... but you are right it should work fine.

Any suggestions on setting up the cylinder in the center? I cannot get them to interact well with eachother. It wants me to define the cylinder's surface as a wall or outlet etc. Should I stick with opening?

If you like you can use the porous flow equations in your region. But because your region is a turbine and not a porous region then I cannot imagine why you would want to. A general momentum source can be written which has the performance curve of the turbine you are using - you cannot do this with porous regions and it is far more accurate.

Assuming you are applying this as a 3D region, then select both the fluid volume and the turbine volume as the domain. Then you make the turbine region a sub-domain and apply the source term (or porous region if I am not convincing enough). No need for inlets or outlets. Also make sure the mesh is continguous between both regions.

Hmm, for some reason, it will not allow me to define the turbine region as a subdomain. Is that because it is a boundary region? Should I leave the CAD model as 2 bodies, with the second being the rotor and overlapping the fluid region around the shroud?

A subdomain is a 3D region. A boundary is a 2D surface on the outside of a 3D region.

Yes, but it will not allow me to select it as a subdomain because I subtracted the cylinder from the rest of the model.

When I didn't combine them it seemed to get confused on the interaction between the bodies

You need to decide what approach you are going to use. If you remove the region then you use a inlet/outlet pair to produce the flow. While this is simple it does make it hard to link to a fan characteristic curve. You can leave the region in and apply the fan as a momentum source. This is a little trickier as you have to do some extra meshing operations and define the momentum source term but is a better approach for most applications.

Hmm, I'm trying it with two bodies and using a momentum source. But, I've never sucessfully done a simulation with two bodies and am getting this error:

Probably a basic mistake

I can't figure out how to tie the two regions together in CFX-Pre.

When I set a domain interface, it one let me select the end of the main body. Only the cylinder itself. Do I need to separate them and make a void in my CAD software? Because I think they are overlapping in the CAD software.

You need to define an interface to connect them with your current mesh. It can be a bit tricky selecting the correct surfaces but if you hide and unhide the bodies you can do it.

But a better approach is to remesh and make the common surface have a matching mesh. Then you will have no need for an interface.

Finally got that to work.

I had to separate my model again, making a void for the cylinder, then placing one as a second body inside of it.

Placed connections in CFX-Pre for their contact, and then the domain interfaces.

The subdomain is set as a -10 kg/m^2 in the Z component (against flow).

I'm having problems with divergence of the solution now, at about 25-40 iterations my KTurbKE starts to oscillate.

Any hints on how to keep that under control? What should I look into modifying?

Good progress.

You will probably need a source term linearisation coefficient. Read the documentation about source terms for this, but if you have defined a constant source then I think that goes to zero anyway so will not help.

Be careful with constant source terms - that means you are always adding momentum there, regardless of the flow conditions. It is better to define a fan curve.

It is also better to not require the domain interfaces. Try to mesh it with contiguous meshes so you do not need the interface. If you do not know how to do this then do some meshing tutorials.

But for your current convergence issues I would not worry about the turbulence equations too much yet. Get the pressure & momentum equations converging before you worry about the turbulence eqns.

I just used a constant because I wanted to get a solution to work, I will add a fan curve as I make more progress.

The turbulence equation stated oscillating and I was assuming that it threw off the rest of the solution as it had started then the pressure and momentum were soon to follow.

I'm using Ansys meshing and the tutorials suck for it. Its very difficult to have defined control over what is going on. But I'll see what I can dig up.

Let me give you a tip on the meshing - you need to define the two bodies as a single part and the interface surfaces will get a contiguous mesh. Look up multi-body parts in the tutorials or doco.

Your convergence problem probably just needs the normal approach - smaller timesteps, better initial conditions, better quality mesh.

Thanks, got it to converge now, with setting the timestep (forgot I reset all the data on Workbench) and high res turbulence.

Now to figure out that pump curve.

I can't find any tutorials that use a momentum source. Any names of them come to the top of your head?