4
$\begingroup$

I am using an Euler-Euler method to model two phases - both are treated as a continuum using modified Navier-Stokes equations. One phase is air and the other is particles, that are being entrained by the air.

The original geometry is very small, the airpath being 2 x 20 mm.

When the mesh is scaled up 10 times (grid fineness is not changed, the dimensions are, i.e. become 20 x 200 mm), the results match experimental ones pretty well.

Grid independence has already been carried out. Irrespective, the scaling problem is seen in both coarse and fine grids. I am thinking along the lines - discrete phase is more accurately modelled with bigger dimenions.

It is a transient simulation, with atmospheric pressure at inlet and a pressure gradient at outlet. The computational domain resembles a 'T' shape, with powder at the bottom and airflow at the top.

Errors in experimental data are unlikely, as it is an established powder entrainment pattern.

$\endgroup$
6
$\begingroup$

Without knowing anything about your method, this is most common when one of two things are occurring:

  1. There is a boundary layer effect happening in your experiment that cannot be represented in your numerical model. (bigger domain works is a feature!)

  2. There is an inconsistency in how you're representing a boundary condition as compared to your physical system. (bigger domain works implies bug!)

By putting your boundary conditions, which are apparently not quite physically correct, far from the area of interest, boundary layers stop affecting your numerical observations (as much as they do in a smaller domain).

Edit: I don't know much about two-phase NS, but for single-phase NS it seems possible that your BCs are much smoother than is physically realistic. To experimentally ensure a constant pressure and flux on the inflow/outflow would be difficult. Putting the boundaries further away allows flow to establish itself before entering the "region of interest" where your samples are taken. For instance, in pipe-flow, using a constant BC when the "established" flow would be Poiseuille flow would result in more accurate observations far from the BCs. (I'm sure this is much simpler than your case, but hopefully gets you thinking in the right direction!)

$\endgroup$
  • $\begingroup$ Good thinking. I ran some tests. Moving inlet/outlet of the pipe from the powder bed did not change the pattern. However, increasing the diameter of the pipe (this is a 2D simulation) did have a positive result. Would I be correct in thinking this is to do with the wall BC (roughness constant, roughness height)? $\endgroup$ – A.L. Verminburger Jun 26 '13 at 8:54
  • $\begingroup$ That seems plausible to me. What BC are you using there? If you are not resolving a boundary layer near the pipe wall, that would absolutely introduce error in that region. $\endgroup$ – Ethan Coon Jun 26 '13 at 16:47
1
$\begingroup$

I'm not sure what exactly you mean by saying scaling up the grid but keeping the fineness. Surely the solution domain remains constant. You are also leaving out many other potentially important details, such as the numerical method (space and time, steady/unsteady, boundary conditions, etc). I will proceed assuming that you mean coarsening the grid by a factor of 10.

What you see - better agreement between CFD and experimental data with coarse grids - is not unheard of. But it nevertheless is probably spurious in the sense that it does not accurately reflect what is the "true" numerical solution of your model. To obtain this "true" solution, you need to systematically refine your spatial and temporal resolution, i.e. you need to carry out a grid and time-step refinement study. When the numerical results become independent (or close to independent) of the resolution, you have obtained the "true" numerical solution of your model. Any deviations that remain between this solution and the experimental data must be due to the model you are solving. (In your particular case the modeling of the solid phase and the coupling of the phases.) Another source for deviations may be measurement errors in the experiment.

Refinement studies are usually carried out by halving the grid spacing in each coordinate direction for each refinement. This means that you will be carrying out simulations with your original grid of N points (or cells), then with a grid with 4N, 16N, etc. The same is done with the time step. If you solve the unsteady form of the equations, you want to keep the CFL number constant (and small) as you refine the grid. It is not difficult to find papers that use grids that are much too coarse. I remember recent articles on fluidized bed simulations in which it was shown that what was widely thought to be a model deficiency was in fact nothing but a lack of resolution.

Many multiphase flows are inherently unsteady, in which case you need to average your solution in some form. Then you need to be careful about your averaging duration and sampling frequency.

Finally, I base all of the above on the assumption that your code has undergone code verification. This is a prerequisite for any validation (comparison of simulation with experimental data). What I describe above is solution verification. If you are not familiar with these terms, I suggest you look at the book by Oberkampf and Roy.

$\endgroup$
  • $\begingroup$ What is your computational domain? What are the boundary conditions you impose other than the inlet and outlet boundary conditions? Is the original geometry (2x20 mm) identical to the experimental geometry in at least one dimension? (I assume here that you located the inlet and outlet boundaries at an artificial location.) $\endgroup$ – Brian Zatapatique Jun 26 '13 at 7:37

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.