[imolnar]

Hello all,

I’m a soil science/hydrology guy trying to self-teach myself CFD for the final part of my doctoral thesis and I’ve come across an error I haven’t been able to find a fix for anywhere (I think I’ve read every ICEM and FLUENT help file and just about every post on this forum).

I’ve collected a bunch of x-ray microtomography datasets of contaminated soil and I’m trying to couple the distributions of observed contaminants with CFD-determined flow fields. The datasets are small, but high resolution (0.35x0.35x0.45cm that I’ve cropped to 0.15x0.15x0.35 cm due).

So I’ve managed to mesh them with a decent quality unstructured mesh in ICEM and import them into FLUENT (which took a bit of jiggering, I'm kind of proud of the process). Many of the datasets converge but the last two I need explode/diverge during the pressure-correction step of the first iteration and I can’t figure out why.

The general process is:
1) Import the mesh into fluent. The mesh has about 30,000,000 tetrahedrals to be grid-independent
2) I scale the mesh down to the proper size.
3) Assign pressure-inlet (22 Pa) and pressure-outlet boundaries (0 Pa). The grain surfaces are no-slip walls and the sides of the dataset are set to ‘symmetry’.
4) It’s very laminar flow so I’m just using the laminar flow equation
5) The discretization and under-relaxation factors are left at default (I switch to second-order discretization once the first order converges)

It’s a fairly straight-forward setup. If the mesh was a decent quality everything seemed to work. But this current dataset I’m working on (which actually has the nicest mesh of them all) has a pressure-correction divergence during the first iteration:

x-momentum equation:
tol. 1.3770e-18
0 4.6013e-07
1 2.3124e-08

y-momentum equation:
tol. 1.3977e-18
0 4.6642e-07
1 2.3573e-08

z-momentum equation:
tol. 5.7272e-17
0 3.0011e-06
1 2.2804e-07

pressure correction equation:
tol. 5.0672e-18
0 1.0134e-05
1 1.#QNBe+00

From what I understand, this is due to a division by zero somewhere in the mesh but I can’t find where.

I’ve tried adjusting just about every single parameter in FLUENT, I’ve lowered the urf to 1e-05 with no success, tried every other discretization method. I’ve tried re-meshing multiple times with successively finer grids. But nothing works. I’ve tried every other boundary condition and even tried to converge with a stagnant flow setup (i.e., no mass flow, or velocity or pressure drop across the dataset) but it still explodes during that first multigrid cycle with the pressure-correction.

What I did notice is that if I disable the ‘post-relaxation’ sweep in the advanced solution controls menu the solution will actually make it past the first iteration and start to converge … but I’m not sure why. I want to fix it because its converging sssoooooo sslllooowwwwlllyyy and I need to graduate before it finishes.

Has anyone encountered anything similar before?

[imolnar]

I figured it out late (late) last night and will post it here for future googlers.

I had been keeping the inlet/outlets flush with beginning and end of the soil datasets (i.e., there was no buffer zone between where the inlet/outlets were and the sand). My working theory was that it was related to the pressure gradient at the outlet end somehow, so I moved the outlet a short distance away from the end of the dataset so there was an empty 'buffer zone' between where the soil ended and the outlet was and remeshed the solution. This solved the divergence at the first iteration and it is now converging nicely (knock on wood).


Also, for those interested for future reference (and future googlers looking to do what I did) I meshed the x-ray microtomography dataset for use in fluent with the following steps:
1) I loaded the dataset into imagej (http://imagej.nih.gov/ij/). It's a great image analysis program. Super fast.
2) Convert the gray-scale image to binary where 1's are the grains and 0's are the pore spaces (or vice versa) by using the 'make binary' function in imagej (Process -> Binary -> Make binary). It helps if you've already used an indicator krieging/segmentation routine to identify where the grains and pores are.
3) Loaded the plugin 'create surfaces' from the virtual insect brain project (http://132.187.25.13/ij3d/?category=...reate_Surfaces). This identifies the surfaces of the grains (or pores depending on how you binarized the dataset) and allows you to export it as a .STL. I used the binary .STL option. (Plugins -> Segmentation -> Create Surfaces)
4) You can now load this .STL file directly into icem. Make a box around the imported geometry, separate that box into inlet, outlet and side parts. Mesh with octree. Smooth, check mesh etc... and then you're good to go.

I hope this helps someone someday! Good luck future person.