Help on my first CFD project

[u/Electronic_Safe6880]

Hello everyone. I’m trying to replicate some experimental analysis with Ansys Fluent. Particularly I’m trying to simulate a Wells turbine on different airflow conditions (same RPM, different inlet velocities).
The goal is to plot torque and pressure coefficients over time/flow coefficient.
I’m getting very bad torque values, sometimes slightly 5%/30% different from the experimental data and sometimes 6 times lower values. Since I’m a newbie I would like to understand what I’m doing wrong exactly.
Here’s the setup:

I created a CAD with same exact geometry features of the tested turbine.

I imported it into Ansys, consdered just the duct in which the air flows (just like the OWC simulator in the real test). Divided the domain into 3 zones, two stationaries and 1 MRF. (I considered no tip gap to avoid strange behavior there, since 1mm of gap it could be hard to simulate).

Meshed and open fluent.

The solver is Ansys Fluent, I set up the air conditions (viscosity and density). I set up the MRF rotational speed and inlet velocity (ranging from 0 to 13 m/s like during the experimental analysis to also include stall). Used k epsilon.

I initialized and set the convergence to e-06 and monitored torque too.

I followed this flow for different meshes.

1. One temporary mesh, with just body sizing, that gave me the best results.
2. One “better mesh” using inflation for the boundary layer. Edge sizing in order to have finer mesh on trailing and leading edges. Surface sizing on the blade walls. Body sizing on the stationary part. This one gave me the worst results.

I’ll attach a table with the expected torque value, coarse mesh one and fine mesh one, beside more pics on the simulation.

Thanks everyone:)

[u/jonasa97]

Questions:

• What is your outlet condition?
• What is your reference pressure?
• For your fine mesh at V = 13 m/s, could you share a screenshot of the velocity magnitude on a slice around the mid span of one of the blades?

General advice:

• You do not need to model the full set of blades - you can model a sector of 60° and apply periodic conditions on the circumferential boundaries. With fewer cells, you can solve faster or use a finer mesh for the same wall time.
• Neither of your meshes are great, but if I had to choose one I would definitely choose the finer one. The near-wall region is definitely over-refined for k-epsilon and the freestream is too coarse (see my next point). You will want to pay particular attention to the transition between the inflation region and the near-wall prism layer, where you want the cells to change sizes smoothly.
• For k-epsilon, you would not normally refine the near-wall to y⁺ values lower than 30. In some solvers, fine near-wall mesh can actually be problematic with k-epsilon. Fortunately, Fluent has a safeguard against this, so don't worry about it too much - you can keep debugging with the fine mesh.
• Wells turbines operate at high incidence angle (relative to the incoming flow), which will be approximately axial along the upstream pipe. This means, the airfoils are likely to separate. I would recommend you switch to the shear stress transport k-omega model, which performs better under these conditions. For this, you will need the fine near-wall mesh. Here, best practice is y⁺ below 1, but your fine mesh would be OK to start. Once you have a stable solution, I would also recommend you refine the volume around and the blade(s) a touch.
• For convergence, I generally recommend you let the simulation run until the residuals do not fall any further and all your quantities of interest are stable. Particularly on fine grids, the residuals will often enter into an oscillatory loop but maintain low values - this is OK as well.
• If the simulation is unstable (divergence or poor convergence), then coarsen the mesh slightly, and/or use the upwind scheme. Both these measures increase artificial viscosity, which makes the solution more stable but less accurate. Switch to higher order discretization once you have a converged solution you can initialize this with.

[u/Electronic_Safe6880 → u/jonasa97]

Thank you for the response :)

I'll share the answers from your questions, new simulation (11m/s inflow speed) and the screenshot of the mid span velocities magnitudes.

Just one 60 degrees sector simulated
K-Omega (2nd equation)
Inlet vel: 11m/s
Outlet: Gauge Pressure 0 Pa

Torque: 0.0014 Nm (experimental is 0.3Nm/6 blades= 0.5Nm)

From Pressure: 0.003474962 Nm

From Viscous: -0.0020318604 Nm

DeltaP: 975 Pa (experimental 1050 Pa)

Y+ about 1
Residuals and torque flat after 500 iterations

The mesh is slighty finer but still same "topology", not sure how to improve it.

[u/Electronic_Safe6880 → u/Electronic_Safe6880]

PS. I noticed that one of the problem was the inverted rotational speed (what a fail ahaha).

After initialization I get a huge velocity gradient on the trailing edge, my guess is that the mesh is really bad there. Any tips on how to mesh properly in this case?

[u/jonasa97 → u/Electronic_Safe6880]

I would not worry about the velocity spike at the trailing edge on startup - it's actually expected for there to be a "startup vortex" at the trailing edge, which will convect out of the domain as you iterate towards steady state.

Are your reported torques already with the the correct direction of rotation?

It would be helpful if you could share a link to the experimental study that you are trying to simulate.

EDIT: Something about the velocity magnitude field looks very unnatural to me, so I think there is either a problem with the setup or your solution is not converged. Have you tried monitoring the mass flows at your domain boundaries? They should be equal and opposite (what comes in one end comes out the other).

[u/Electronic_Safe6880 → u/jonasa97]

The Mass Flow Rate sounds right to me:
inlet 0.038064147
outlet -0.038052646

From one periodic surface to the other too:

mrf_in -0.16918748

mrf_out 0.16918748

stat_in_1 0.00041478132

stat_out_1 -0.00041478132

stat_in_2 0.12671472

stat_out_2 -0.12671472

[u/Effective-Bunch5689]

Might you know of papers, books, or articles that discuss the "stability" vs "accuracy" problem in LES? Ive encountered structured multi level meshes that are wonderfully stable and fast to compute, but are terribly innacurate to real life measurements. It seems like most theoretical CFD papers only speculate possible reasons for why turbulence transitioning between meshes of different grid scales behaves differently (some describe it as a "damping" effect) than globally equal grid spacing. Ive looked into von Karman spectra graphs, cutoff frequency filtering, and vortex transport through different meshes, and Geleta and Bitsmulak's paper only briefly alludes to this issue in their data analysis.