[Iggy]

Hello,

I'm new to this forum and this is my first post. I'm having huge problems with my project for masters degree. I want to simulate a horizontal axis hydrokinetic turbine with CFX (steady state). It's a 800 mm turbine with NACA 63-8xx airfoils. The turbine geometry was designed in SolidWorks according to this article:

A.S. Bahaj - Power and thrust measurements of marine current turbines under various hydrodynamic flow conditions in a cavitation tunnel and a towing tank http://www.sciencedirect.com/science...60148106000516

The geometry was cut in several pieces for easier meshing. The meshes for the domain were designed in ICEM CFD and have approx. 3 mil. elements.

I'm simulating 1/3 of the model with periodic boundaries. The other boundary conditions were defined:
- domain front side was defined as inlet with speed of 1,4 m/s
- domain back side was defined as outlet with pressure of 0 Pa
- rotating domain speed was 19,98 rad/s
- hub and turbine blade were defined as no slip walls
- the outer surface of domain was defined as counter rotating wall

GGI interfaces were used between parts in domain. Between rotating and stay domain Stage interface was used. The SST turbulence model was used for simulations.

So my problem here is with the power coefficient. The largest deviation is around 70 %. The thrust coefficient has a deviation below 10 %. What could be the problem? Are there any additional settings in CFX if you want to simulate a hydro turbine?

I may add that my friend is simulating a wind turbine with aprox. same size and does not have any problems (the deviation for both coefficients is smaller than 10 %). And also: Before this project, I was simulating the vertical axis hydro turbine (Gorlov), and the problems were the same as here.

Some pictures of the project are in the attachments.

Every comment would be welcome, because I'm in kind of dead end now.

Mesh1.jpg

Mesh2.jpg

BC.jpg

Cp.jpg

Ct.jpg

[ghorrocks]

Have you gone through the FAQ on accuracy? http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

One problem I can see straight away is that you appear to have non-conformal mesh refinement on mesh2.jpg. CFX does not support this type of meshing. You can do it using a GGI interface but that is a really bad idea this close to the boundary layer. I would remesh with a fully conformal mesh.

Also please post your CCL.

[Iggy]

Thanks fo the reply.

1. Have you gone through the FAQ on accuracy?

The wind turbine project was almost the same size with the same blocking and boundary layer refinement as seen in pictures. The turbullence model was the same (SST). All the settings, except for the inlet velocity, rotational speed and fluid (water) were the same.


2. The non-conformal mesh refinement was not a problem with previous projects. It was used in the same way with the wind turbine simulation and with the airfoil simulations. The results for both simulations were decent with less than 10% error.

In picture mesh2.jpg the GGI interface is already used between the coarse and fine side.

Today I have simulated an unstructed mesh (fully conformal made with ICEM) with no interfaces and the results were even worst.

When applying the refinement near the blade we don't use the function for resolving refinement in ICEM. In CFX you than have two sides (coarse and fine) and between them we use the GGI interface. Do you think the problem is with this function?

Here is may CCL:

https://www.dropbox.com/s/vsqynrfsa9...X_001.txt?dl=0

[ghorrocks]

I take it your comment means you have not gone through the FAQ on accuracy. I recommend you do so.

Looking at your simulation output file - you have only obtained very loose convergence. This is another FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

[Iggy]

1. Tthe FAQ on accuracy

Depending on what you are modelling other sensitivity analyses may be required, covering things such as:

1.1 Domain size (how close can the boundaries be to the region of interest?)

Domain size is the same as in the experiment. Other authors have used the same domain dimensions in their studies.

1.2 Grid density

I think the mesh is fine, the y+ value at BL is below 3. I can't make finer mesh because I'm limited with CPU and RAM.

y+.jpg

1.3 Grid quality

I know the quality is not the best, but is pretty much the same as it was at wind turbine.

1.4 Grid type (e.g., structured versus unstructured)

The mesh is a structured mesh made in ICEM. The unstructed mesh results were even worst.

1.5 Spatial discretization (or advection) scheme: Don't know what that is.

1.6 Temporal discretisation scheme: Don't know what that is.

1.7 Turbulence model

The SST model was used as it given me the best result at previous studies.

1.8 Turbulence numerics: Don't know what that is.

1.9 Turbulence intensity

The medium intensity 5 % was used. The other intensity didn't impact much on the result.

1.10 Boundary condition type

The boundary conditions are mentioned above.

1.11 Any empirical models used, such as heat/mass transfer coefficients, drag laws, free surface model: Can't answer that.

1.12 Two- versus three-dimensional simulations

It's a 3D simulation, beacuse of the geometry.

1.13 Timestep size

It was set to auto timescale if this is what you mean.

2. About convergence.

The simulation was run for about 2 hours as can be seen at CCL file. So this one was short, other ones were run for about 16 hours and the results were the same. Here are some pictures of residuals. The momentum and mass values here didn't get below E-4, but in other simulations did get below E-5. You can see that the thrust and moment does not change a lot.

Moment.jpg

Momentum_mass.jpg

Thrust.jpg

Honestly I don't think the mesh is the problem here. It has to do something with BC or interfaces between parts. I'm not an expert so I don't know what, but it doesn't make any sense since other authors got good results with, if you ask me, worst meshes.

[ghorrocks]

1.2 Grid Density - The most common reason for an inaccurate simulation is inadequate mesh density, so do not underestimate this issue. Unless you have checked your mesh size is adequate you do not know. You need to do a mesh sensitivity study.

1.5 Advection - Options include Upwind, hybrid, hi-res. I would recommend hybrid with a large blend factor or hi-res. But due to your convergence problems you might need to start off with upwinding to get started.

1.6 Temporal - steady state simulation so this is not relevant.

1.8 Turbulence numerics - upwind or hi-res. This will not help until you get better convergence.

1.13 Time step size - As you have not got convergence your time step size was not appropriate. Read the FAQ I posted on post #4.

So I see three problems which require addressing before you can be confident you have an accurate simulation:
1) Inadequate convergence (this is the big one, until this is fixed nothing will work)
2) GGI interface close to boundary layer
3) No mesh sensitivity check

[Iggy]

Hello Glenn,

Thanks for the advices. I will try to refine my mesh near the blade and do the sensitivity study.Also I will try to get rid the GGI interface near the BL.

For the convergence: Yesterday I have set up the simulation through the weekend, we will see the results in Monday and I will post them here.