## Simulation CFD

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic to the Top
- Bookmark
- Subscribe
- Printer Friendly Page

# Airflow analyses around wheel - can't get convergence!

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

Hi,

I'm trying to simulate the airflow around a rotating wheel; in particular my objective is to obtaine the wall forces (on wheel) in flow-direction, to finally calculate the cd coefficient.

__The problem is that i can't bring my simulation to convergence__, and after 800-1000 iterations, results are still disturbed.

I've noticed that setting ADV on 5 apparently solves convergence problems (i can get some results), but the strange thing is that ADV 1 works well with a similar simulation made with the same items and conditions on my colleague pc, and she reach convergence after less than 300it; this is her screenshot:

So i'm looking for some help to understand:

-if I have an option which makes my result going wrong (or what may be the problem)

-if ADV5 would be better than ADV1 in any case, or not: with ADV5 i can get some results of wall-forces, but they are different (about 15%) from the results obtained by my colleague using ADV1.. so, which of them are more realistics in a simulation with this conditions?

I've attached both the .ipt and .cfz files;

Thanks very much for your help!

PS1. Some info: the flow speed is 16,67m/s, the ground is sliding with the same velocity in the same direction, and the wheel is rotating with a speed of 65,66rad/s

PS2. The mesh used for the simulation attached is not so fine, but i've also tried with a well-defined mesh, which took a night to process results, and the problem is the same.

Solved! Go to Solution.

# Re: Airflow analyses around wheel - can't get convergence!

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

Have you tried modifying the model so you don't have a tangent condition between the circular tire and the wall? This can lead to meshing and/or numerical instability problems, according to my training on CFdesign a few years ago. Not sure of your setup but I have done this by making sure the center of the tire is less than one radius from the floor (i.e. a contact patch with some area and not a line).

# Re: Airflow analyses around wheel - can't get convergence!

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

Yes, I've tried to start a simulation after modifying the model to avoid the tangent condition using your solution, but the problem still remains.. 800 iterations and no convergence..

Other possible causes?

thanks for your support!

Lorenzo

# Re: Airflow analyses around wheel - can't get convergence!

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

Hi

ADV1 is a first order accurate while ADV5 is second order accurate scheme. Essentially, ADV5 is more accurate than ADV1 because it induces lesser diffusion (because of smaller truncation error). But at the same time, this makes ADV5 more vulnerable to instability, while making ADV1 more stable because of increased diffusion that pacifies turbulent and transient instabilities. That is the reason why you get quick convergence with ADV1, but with a solution that is less accurate, owing to diffusive effects. That also explains difference of 15% between the two schemes.

I would recommend following to have stable convergence.

1) Make sure you have Intelligent control enabled in the Solve dialogue box

2) Reduce the underrelaxation factors for pressure, velocity turbulence etc to 0.35 from 0.5.

3) Get the solution using ADV1 and k-epsilon for 500 iterations

4) Switch to ADV5, and RNG turbulence model and continue till 1000 iterations

5) Try reducing under relaxation factors even further if you see no stability by 900 iterations with ADV5

6) Since information of mesh is not provided, make sure you have arrived at appropriate mesh using mesh independence tests. If mesh is too large, the elements are too small and capture the turbulence effects of smaller length scales, further inducing instability.

Having said all, there is no written rule that every solution MUST converge within 1000 iterations. If it doesnt converge within 1000 iterations, run it till 2000 iterations! There is no need for panic unless you see divergence. Instability is a part and parcel of CFD.

OJ

# Re: Airflow analyses around wheel - can't get convergence!

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

Lorenzo,

The other aspect is that there are some simulations that are inherentl unsteady.

Flow around a cylinder will induce vortex shedding. This unsteady phenomenom can be captured with a SteadyState solution however it will get smeared and averaged out as well as potentially introduce enough of an oscillation that the AutoConvergence Assessment will have difficulty in assessing a steady solution.

As OJ mentioned ADV5 will be more accurate and less diffusive than ADV1, while 1 can be more stable (due to its diffusive nature).

Following some of the other points as well, be sure that your mesh is sufficient, not just to capture the geometric shapes but the oscillations within the flw field (such as the recirculation within the wake).

If the oscillations happen to be large enough, you can manually assess convergence once assuming that the oscillations are constant.

# Re: Airflow analyses around wheel - can't get convergence!

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

I finally managed to solve the problem, but I forgot to thank you!

Thanks again for support,

Lorenzo