[MangoNrFive]

Hello

I'm simulating a leaf seal by modeling the leaf pack as porous medium with directional loss model in CFX. At the downstream interface from porous domain (left) to fluid domain (right) the velocity changes from high to low to high etc. normal to the fluid flow (see figure). The wiggles can be seen in the pressure field as well. They start with slight variations in velocity and keep growing until solver failure due to floating point exception.

I tried some things to maybe get a solution as a good initial condition and then start from there, but failed as well
- upwind-advection scheme
- high-speed numerics (this activates High Resolution Rhie Chow Option as default as well, which could be useful)
- various timesteps
- double precision

I have some ideas as to what could be a problem with this simulation
- I define the loss coefficient Kloss for the directional loss model as a function of Reynoldsnumber (by a pipe friction factor). Can this additional coupling between velocity (Reynoldsnumber) and pressure (momentum source) cause numerical instability?
- Are the aspect ratios at the Interface a problem? They are lower than 20. The mesh is otherwise perfectly fine with close to rectangular cells.

[evcelica]

The additional coupling between velocity and pressure could be causing some of this. Should be easy just to change to constant and see if it still occurs.
What is your function? Does it use velocity or velocity w?

It looks like you start using very small mesh size in line with the flow at the interface for some reason. This may also be causing some problems, as there looks to be a pretty aggressive mesh BIAS as well as aspect ratio. I don't see a reason for this at a fluid-porous interface like this?

[MangoNrFive]

The function is :

Kloss := lambda/(2*gapSize)

with

lambda := if(Re > 2320, 0.348/Re^0.25, 96/Re)

The Reynoldsnumber calculated as

Density*absVelocity*2*gapSize/Dynamic Viscosity

gapsize stands for the width of the gap between 2 leafs of the leafseal. The hydraulic diameter is 2 times gapsize. The formulas can be reached by applying pipe-flow Theorie, I'm pretty sure that the physics itself are correct, just not stable it seems.
So it uses the absolute velocity in the end. The jump between turbulent and laminar flow doesn't seem to be a problem. I tried it with lambda = 96/Re (laminar) for all Reynoldsnumbers already.

I'll define Kloss as a constant close to the value reached at the problematic region and see if the problem persists then.

I did the mesh refinement because i expected high gradients at the interface as a result of the jump in porosity and change in flow direction as well. The fluid in the porous domain is confined to a angled plane by a low permeability normal to the plane. Would you advice to not refine the mesh at all at the interface or just not as much?

[evcelica]

Yeah, so when your velocity goes to zero, like at a wall, your Kloss goes to infinite.
You may want to put a numerical limiter on the minimum Reynolds number. It won't make much difference at very low velocities anyways, but it does to the numerics as you divide by zero.

I would also smooth the transition from laminar to turbulent. I'd probably just use a 1D user function, where I could also set the max Kloss at low Reynolds numbers.