[chaz]

Hello,
I am trying to match theory for taylor-couette flow. It is a cylindrical body with the inner wall rotating and the outer wall fixed. No inlets, no outlets. I need assistance with convergence at high speeds.

At low rotational speeds (<10 rad/s) the problem converges fine, and the result matches theory for the moment exerted on the inner wall within ~7%.

At high speeds, I can not get the problem to converge, at all. Things I have tried:
-tet mesh with varied mesh densities (netgen in salome)
-tet mesh with boundary layers, varied mesh density (netgen in salome)
-hex meshes via cfMesh, varied mesh densities
-a single mesh with a single inner cellzone, using MRF for that cellzone (no AMI, continuous mesh made with partitions in salome)
-a mesh with inner rotating region and outer fixed region, with MRF applied to the inner region, with communication across the interface with AMI
-all of the above using simplefoam
-I have tried using 5.0-dev and v1712
-I have tried a transient simulation using pimpleFoam
-I have tried various settings in vfSchemes and vfSolutions, including as guided by http://www.wolfdynamics.com/wiki/OFtipsandtricks.pdf


For my most recent efforts, I have been using hex meshes via cfMesh, with two inner and outer meshes linked using AMI, solving in simplefoam. Solves fine at low speed. I have noticed that as the problem diverges the spike in velocity begins at the pressure reference point, and spreads across the domain.

Can anyone advise me on how to get convergence on this problem? Is the fact that the divergence begins at the pressure reference a clue on how to fix it?

[Taataa]

Assuming you've already checked the quality of the mesh and boundary conditions are correct, I have a couple of suggestions:
1- If you're using tet meshes it's better to use leastSquares for gradSchemes;
2- Try using PCG solver for pressure and PBiCGStab for the rest and tighten all the tolerances specially that of pressure a couple of orders of magnitude (e.g. 10^-12)
3- Set all the divSchemes to upwind (except for that of nuEff which should be linear)

If you're able to get it to converge then start to loosen the tolerances step by step and use higher order divSchemes preferably llimitedLinear.

[chaz]

Thank you for the thoughts. One thing I did not mention is that the model is laminar, not adding turbulence until I can get stability with a laminar solution.

I am using cfMesh's Cartesian mesh, with:
Mesh non-orthogonality Max: 43.0882 average: 5.17368
Pretty good, I think.

Boundary conditions: top and bottom U is slip, P is zero gradient
outer U is 0, inner U is rotatingWall. Both walls are P = zero gradient.

With all walls being zero gradient for pressure, the reference pressure should certainly be referenced.

After making the changed you suggested, The solution is slower to diverge. Rather than at about 30 iterations, it slowly diverges at about 120 iterations. The same issue is apparent, the pressure rises tremendously in the volume, with a huge gradient near the reference point. As a result, in U the velocity spikes from the pressure reference point out.

This is a simple model of simple theory, but it looks like the boundary conditions for P will not let it be solved. new vf files attached.
Any ideas?

[Taataa]

With 43 you don't have to use limiters for gradSchemes, you can set it to linear. Also, use corrected for laplacianSchemes and snGradSchemes. The geometry is not complicated and by using the limiters you're smearing the solution unnecessarily. Another thing would be to set the relTol to 0 for both.

If it didn't help maybe the mesh is not fine enough. Have you conducted a mesh convergence study?

[chaz]

Originally Posted by Taataa

With 43 you don't have to use limiters for gradSchemes, you can set it to linear. Also, use corrected for laplacianSchemes and snGradSchemes. The geometry is not complicated and by using the limiters you're smearing the solution unnecessarily. Another thing would be to set the relTol to 0 for both.

If it didn't help maybe the mesh is not fine enough. Have you conducted a mesh convergence study?

Per your earlier question, I took a look at the choice of boundary conditions. I also made the solver changes you suggested. Rather than having a wall with zero gradient on the top and bottom, I looked at patches on the top and bottom with p=0. Similar problems.

Up to about 20 rad/s, the results match theory. Up to 80 rad/s, the system will reach a point where the residuals are constant, but not dropping or rising. Result does not match theory. Above 80 rad/s, the problem diverges. Mesh made by cfMesh, merged, with AMI between the inner rotating region and the outer stationary region, similar to mixer2D example. Run in v1712.

Full problem and images of the mesh attached. Currently about 175K cells. Previously I did not see improved convergence with up to 1M cells.

I'm very surprised that such a simple problem is so difficult to get to solve. Any advice?
Full problem: https://www.dropbox.com/s/cvimmshjsl...teV10.zip?dl=0

[Taataa]

Taylor-Couette is not a simple problem due to complex structure of the produced turbulence. People usually do DNS as the geometry is simple.

As you increase the Re number, deviation from experiment is expected because you consider the flow laminar.

My suggestion is to turn on turbulence and conduct a mesh convergence study to make sure the mesh is fine enough.

[chaz]

Originally Posted by Taataa

Taylor-Couette is not a simple problem due to complex structure of the produced turbulence. People usually do DNS as the geometry is simple.

As you increase the Re number, deviation from experiment is expected because you consider the flow laminar.

My suggestion is to turn on turbulence and conduct a mesh convergence study to make sure the mesh is fine enough.

Hi,
Yes, Taylor-Couette flow in the real world is not simple, but the first step of modeling it that I am doing should be (relative to matching experiments with foam with turbulence). I am not trying to match experimental results (that is much later). I am simply trying to get a laminar simulation in foam to match the analytic solution for the laminar R-S equations. Phenomenon such as Taylor vortices are initiated due to instabilities (turbulence), and should not be an issue in this study matching laminar theory to laminar numerical solution. Foam and the analytic solution for theory are solving the same equations for laminar flow, so they should be identical up to very high speeds. Laminar couette flow has a linear flow profile, laminar taylor couette flow solutions have a slightly curved solution, depending on the geometry. My foam solution matches well for low speeds, and not for high speeds, the result should just be scaled up, same profile, same solution.

The reson I am first solving laminar solutions with simpleFoam is two-fold: 1, verification of the foam setup and underlying solver, and 2, can provide an initial condition for turbulent solutions. From my experience with cfd, and what I've read over the years is that laminar solutions provide good initial conditions to turbulent, more realistic solutions. If I can't get a laminar solution to converge up to ~300 rad/s, it would be unwise to jump in and expect a turbulent solution to converge. (I started there, more problems than this current laminar study).

For example, a straight tube with an inlet and outlet on the ends, solved with an analytic solution and a laminar solver should give the same results for low flow rate, and high flow rate. Sure, it may not match an experiment at high speeds where turbulence is induced, but they are both a solution to the same governing equations. It's just math, one solved analytically, the other numerically, regardless of inlet velocity, the solution is just scaled.

I'd love to know why doubling rotational speed causes the laminar solution in foam to diverge from theory (with poor divergence), and doubling the speed again causes the problem to diverge.

thanks for your help!

[Taataa]

I see. Have you tried this case?

[akidess]

I don't have the time to look at your case, but I have solved TC flow at higher rpms.

[chaz]

Thank you for the link, Taher.The method used in that study is much better. At low RPMs, the problem converges nicely. This uses a single mesh with the inner and outer walls having the u bc of rotatingWallVelocity. No MRF at all, no use of two domains with AMI. This is simpler than the other approaches I was using, which were based on examples such as the 2d rotor and the propeller using simple foam or pimpleDymFoam.

At low speed (0-2 rad/s, Taylor # up to 3000) the results match theory well, and converge. They deviate from theory a bit above 2 rad/s, but still converge, with clear taylor vortices forming. This is believable, given the taylor number and the fact that the problem converged.

At high RPM (100 rad/s), the probem does not converge. There are clear vortices, but the residuals kind of oscillate. Image attached. Perhaps at these speeds there is inherent oscillatory behavior, making it not converge?

[chaz]

Hello Anton,
Any observations on how, or if I should be able to get convergence with simpleFoam? latest case attached. Please see my other comment. Inherent oscillatory behavior making convergence at high speed not possible? Mesh or other issues? I used 90K cells, then up to 500K cells, with the same result at 100 rad/s.

Link: https://www.dropbox.com/s/oovivc77oggjz4o/v11.zip?dl=0

[akidess]

How to give enough info to get help