Porous Media in Star-CCM+
 

Hi,

I am currently creating an OWC WEC with a Wells turbine in Star-CCM+ - simulating the Wells turbine linear pressure drop with a porous region and just had a couple questions. To create the porous region should I be creating a separate 3D part object and assigning it as a porous region or including it as part of the OWC model?
In the CD-Adapco user manual there is both porous region and porous baffle interface options and I am unsure how to implement them correctly, if I need to implement both and the physics values required.

My project is replicating experimental data where the Wells turbine was simulated using a cloth mesh and having a linear pneumatic damping coefficient of 1145 kg/m^4s. From my research I have gathered I can leave Porosity and Porous Inertial Resistance as 0 and input the Porous Viscous Resistance? The units required for Vr are either kg/m^3-s for porous region or m/s for porous baffle interface. I have pressure drop and velocity data from the experiment and have calculated a value of ~48 m/s for Porous Viscous Resistance using Δp= - ρ( α vn + β) vn. Does this sound correct - I am not seeing the pressure drop across the porous region that I should be? Another method I have found uses q = -(Kp*Acs/mu)*deltap/L and solve for 1/Kp to give viscous resistance of ~5*10^8 however I am unsure of the units for this and where to input.

The attached image shows my OWC with the orange plate at the OWC vent being a fluid region with a porous baffle interface between the upper and lower faces of the plate for context. Any help would be greatly appreciated.

Cheers,
Ben

If you are referring to CD-Adapco anything it is almost certainly out of date. They don't exist as a company anymore. Make sure the help manual you are using matches the software version, otherwise you might find inconsistencies. Regardless, you don't need both a region and a baffle. A porous baffle is a 2D surface with instant dp change whereas a porous region is a 3D volume with gradual dp change. Not sure what a OWC WEC or Wells Turbine is, but if the goal is to impart a pressure drop for flow through the J shaped channel then use a porous region, otherwise, if you can live with an instant change as it enters or leaves, then a porous baffle is a reasonable (but less realistic) choice.

Assuming a porous region is what you want, you will need a distinct porous region and conformal in-place interfaces separating the fluid and porous region(s). Consider a simple case where you have a straight duct with an air filter in the middle. You would end up with 3 volumes for your CAD input. 1) upstream 2) filter 3) downstream and you would assign region 2 to be a porous region rather than a fluid region.

The physics values required are the resistance coefficients and are derived from your pressure drop curve. There is also a the need for tensor notation, but let's not complicate things too much just yet. If you have a normal parabolic pressure drop curve (dp=a*v^2 +b*v), then you simply divide by porous region thickness (dt=dx) so you have dp/dx = Pi*v^2+Pv*v. Your resistances are then Pi = a/L and Pv = b/L for inertial and viscous resistance (refer to help manual for proper definitions).

If you need to derive resistances from discrete test data (so individual dp vs velocity data) then divide dp values by thickness and obtain a 2nd order polynomial fit to get your resistance values. ALWAYS WATCH YOUR UNITS. It is easy to make mistakes.

What you have describe does not sound correct, no. Is there perhaps an equation for pneumatic damping that would be helpful here? I googled it quickly and didn't turn up much. Porous pressure drops are rarely (if ever) linear. The models behind them assume a parabolic curve, not a linear one, so they might not be the right choice for whatever it is that you are modeling.

There are other ways to impart a pressure drop. A porous region is really just a special implementation of a momentum source to correlate a parabolic dp response to linear change in flow. You could presumably do something simple here to get the desired effect, but need the equation that puts the units of your damping coefficient into context. DP is a function of something, this coefficient, probably velocity or flow rate and some other stuff.

If you can provide some insight on the physics of your problem, someone can suggest how to approach a momentum source to model it.

Thanks for your reply Fluid23, that was quite helpful. My apologies, I will provide a detailed insight into my problem below.

I am attempting to model an Oscillating Water Column (OWC) Wave Energy Converter (WEC) that's integrated into a floating breakwater.

Here, I have modelled the outer fluid domain as a Numerical Wave Tank with the model placed inside the tank. The Volume of Fluid model is used with water waves propagating through the tank and entering the OWC chamber, inducing a dynamic air pressure within the chamber which would, typically, turn a bi-direction Wells turbine. To model the linear pressure drop experienced by a Wells turbine they have used a porous cloth mesh placed at the top of the J shaped channel.

My issue at the moment is modelling the porous region (I have the resistance values sorted now). Your response has made it somewhat clearer however the interfaces are causing me issues still. What should I have the inlet of the porous region and the outlet of the porous region interfaced with using my geometry as shown in the attachments?

Ok... your explanation is helpful but I am still struggling a bit with your domain. Is the gray box in image 2 fluid or solid or is that the inside surface of a larger fluid volume? Can you sketch the problem in 2D? It will be easier to grapple with.

A cloth mesh definitely falls under the scope of Darcy-Forchheimer so a porous region or baffle is appropriate. Something that thin may be better with a baffle. With a region (finite thickness) you need to have at least 3 (I like to use 5) cells through the thickness of the region. For something that thin, you end up with a bunch of very, very small cells. I would steer you back toward the baffle if you are modeling anything less than 0.05 inches thick. You should still be able to work out your resistance inputs the same way, if you have issues let me know.

As far as the what goes on the inlet/outlet of the porous region, you should have a fluid region contacting both sides of the ‘cloth’ with a face that has the same shape as the cloth (i.e. conformal). For a baffle you just need to separate fluid regions with conformal face that has the shape of the cloth. Then you change the interface type to porous baffle and assign properties. To (hopefully) make this more obvious, if you have a porous region surrounded by a single fluid volume you would subtract the porous volume from the fluid volume so that the porous region fits inside the hole left by the subtraction.

One issue I think you will run into, and I could (very likely) be wrong because I use the poly-mesh exclusively, is that you cannot have interfaces with a trimmed mesh. It difficult to create a conformal face with curvature using this mesh. Many years ago that this was not supported, but perhaps that has changed.

I've attached a 2D representation of my domain. The outer box representing my Numerical Wave Tank, inside I have the floating breakwater/OWC implemented using an overset mesh. The model is subtracted from the overset mesh around the model and then overset mesh boundary applied to the interface between NWT and overset. All works perfectly up until the porous bit. :confused:

Got it...

Next question, can you clarify what is wrong when you say 'All works perfectly up until the porous bit.'? Are you getting odd results, not able to run the model?

Have you tried it without the porous region?

Yes, it runs fine without the porous mesh. I am having trouble with what to interface the porous faces to - should it be to the overset mesh, faces of the breakwater or the NWT background. I've attempted it with all of the above however sometimes the sim will run for 5 iterations and then give an error, sometimes 'floating point' error. Or will run but produce no pressure drop at all.

There should be totally separate and independent air volume inside the column between the water and porous media. I have never tried a multi phase free surface model like this though, so you may be beyond my help at this point.