[sohoem]

I’m trying to find the permeability through an TPMS structure in ANSYS Fluent. I need the pressure drop and volume flow rate through the void to find the permeability. The problem is that the flow/velocity/pressure does not stabilize. See the pictures on the bottom of the mail. The picture only shows the results for 160 iterations, but I have run the same simulation 1500 iteration with the exact same outcome.

General:
Body is modelled in nTopology in mm (domain 84x84x84 mm) and the mesh is scaled to 84x84x84 micrometers in Fluent. The model is exported as a step file from nTopology. The outlet is shown on the picture below and the inlet is on the opposite side. The fluid considered is water and the flow should be laminar.

Model:
Laminar flow

Boundary conditions:
Inlet: Pressure Inlet with 0.01 Pa pressure.
Outlet: Pressure Outlet with 0 Pa pressure.

I have also tried velocity inlet with 1.2e-6 m/s velocity and pressure outlet with 0 Pa pressure.

All other surfaces has a no slip condition (wall).


2.jpg

Mesh
The mesh is really dense with 14 000 000 elements and 20 000 000 nodes. The geometry has some small surfaces that needs really small elements to be meshed.

4.jpg


Method:
Scheme: SIMPLE
Gradient: Least Squres cell Based
Pressure: Second Order
Momentum: Second order upwind


Residuals and convergence conditions:
Residuals: All set to 1e-7
convergence criteria: volume flow rate, velocity and pressure at inlet and outlet; 1e-7


Initialization:
0.01 Pa, Y velocity: -1.2e-6

Results:

xx.jpg
yy.jpg


Comment to results:
The results are stabilizing with logical correct values for flow, pressure and velocity the first 25 iteration, than it diverges. The contour plots shows really strange distribution of pressure and velocity. When I try to use the coupled algorithm the solver crashes. The mesh is not perfect, but is the quality so low that the solution diverges for that reason?



Note:

The exact same set up has been used on the body below. Modelled in solid works. The domain size is the same, the structure is different but that should yield “similar” results. Pressure inlet (0.01Pa) and pressure outlet (0 Pa). The flow stabilized with convergence criteria set to 1e-7 and all the graphs had a nice curve that converged towards a value. The pressure is distributed as expected.

17.jpg





Thank you!

[LoGaL]

Hi, yes, the mesh quality is pretty bad, especially if those elements with low orthogonal quality (<0.01) are a lot (in an absolute manner, not relative to the total element count). 5-10 cells do not cause so many problems, but if they are more, problems come. If you click on the control button in your mesher (near the plot with the qualities in the bottom of the screen) and set some appropriate min-max orthogonal quality, you may check how many cells are of bad quality. Anything with orthogonal quality below 0.01 is bad.

If coupled solver crashes, not only will also SIMPLE almost certainly crash (because it is less stable), but in my experience you are giving something really bad to the solver, either the mesh or some garbage settings. I've seen coupled solver converge flawlessly in cases with complicated physics (e.g. combustors with liquid droplet particles, radiation and flame chemistry modelling or supersonic flows with real gas equations or conjugated heat transfer problems) and in less than 1000 iterations. Not saying it is necessarily the mesh, but if you want to blame the solver, you must be confident of your mesh first. So work on the mesh, spot the areas where the element quality is bad and fix them.

If you give the solver a good mesh (min orthogonal quality >0.01 and mean value much much above it) and it still crashes, then you can start blaming the solver settings.

If also the solver settings are correct to the best of your knowledge, then perhaps you need to define a proper convergence strategy. But I bet my money on the shitty mesh, just saying