How to compute Streamwise Coefficient Multiplier
 

Hi,

I'm using the porous domain and need to specify the permeability and the loss term in transverse direction.

Since, for my case, the fluid in transverse direction is not negaligeable, I need a good estimation of Streamwise Coefficient Multiplier. The CFX tutorial suggests it to be '10 to 100'. But '10 to 100' might be too large for my case. May I ask is there any formula for computing the Streamwise Coefficient Multiplier? How is Streamwise Coefficient Multiplier usually estimated?

Thanks!

It depends on the material. If you had experimental data for permeability when flow is in the transverse direction you could figure out the multiplier.

I don't have the experiment device for this case.

I compute the streamwise permeability by CFD simulation of all the detailed geometry in the porous domain.

Is there a way to measure this factor by CFD?

You can model the material with all its pores and holes and push a fluid hrough and get it. Alternately you might be able to estimate it from assuming it is either laminar flow drag, oriface flow or some other simple flow which has well known resistances.

Shall I set up the boundary condition to let the fluid flow only at the streamwise direction to obtain the pressure drop thus the streamwise permeability firstly? Then set up the boundary condition to let the fluid only flow at transverse direction to extract the transverse permeability? Then I can use the streamwise permeability and the transverse permeability to compute the Streamwise Coefficient Multiplier?

Is this the correct strategy to compute the Streamwise Coefficient Multiplier?

That is correct.

Extending the same point, if I want to simulate the perforated sheet with holes, it is easy to determine it's resistance coefficient (ratio of static pressure and dynamic pressure), either by simulating a small section or using standard resistance handbooks.

Now, if I were to simulate a conical strainer made of perforated sheet, which of the following approaches is appropriate?
1) Using interface with pressure change relation (using Darcy's equation)
2) Using actual thick conical strainer and put the multiplier as, say 1e8 (since there is no flow in transverse direction)?

The use of interface is very tempting but it is used for infinitesimally thin porous regions while the perforated sheet in question has 6 mm holes and is 5 mm thick. Moreover, the incident angle of flow is not always perpendicular at every point on surface, and the fluid emerging out of the strainer follows its earlier path. But the actual simulation of holed perforated sheet shows that the velocity vectors emerging out of the holes are perpendicular!

Thanks
OJ

Can you post an image or drawing of the conical strainers?

I have included a schematic of the arrangement.

As you can see, only a very small portion of fluid at the center of the inlet pipe enters normally into the strainer. Fluid in majority of circumferential region enters at an angle, so does the fluid that goes around the strainer and enters from all other sides.

Now, using the stream-wise coefficients that are generated by simulations or obtained from resistance handbooks may not be suitable here. While transverse flow doesn't exist!

Regards
OJ

I see. I would model the strainer with an interface with a resistance coefficient across it in this case.

Well, that would be the simplest way to do it. But the issue here, as I mentioned before, is that the streamlines emerging out of strainer surface are following the same direction as they had while entering into the strainer surface. Now, the strainer has perforated sheet with 6mm dia holes with 5 mm thickness. When I simulated a small section of perf, I realized that regardless of how fluid enters the perf, the streamlines coming out of holes are perpendicular to the surface.

Autodesk Simulation CFD has a interface model in which they make the streamline coming out of interface perpendicular. When I tried CFX (interface with pressure change), Fluent (Porous jump boundary condition) and Autodesk CFD (interface), I realised that the velocity field downstream of the strainer is different for Autodesk CFD than FLUENT/CFX.

I am torn between the choice of the approachs here. We have experimental data for the strainers but it is mostly pressure, not velocity field, for obvious ease in measuring pressure as compared to velocity.

OJ

I see. Then I would add to the built in pressure drop model for the interface I would apply a user specified momentum source term which makes the non-normal components zero.

Can we specify a user-specified momentum source for interface? How?
I know we can specify them if we model the the volumetric shell of the strainer, and define it as a porous region. But that increases computational time and complexity, which I want to avoid.

OJ

You can define sources on interfaces. Have a look at CFX-Pre on the interface object. If you use a source term linearisation term it should still converge fine.