[kweston]

Hi there,

We are a pair of Uni students battling through some extremely basic CFD simulations as part of our undergrad thesis. We have tried so many variations of our models and nothing seems to be working - any help on this matter is greatly appreciated!

Our first task is to undertake a mesh dependency test by looking at the RMS lift and mean drag of 2D uniform flow over a cylinder at Re=100 (extremely basic - we know!).

Our geometry domain is such that the cylinder D = 10mm, and the boundaries from the cylinder are 16D to the inflow, 20D to the outlow, 10D each way to the top and bottom wall (similar to what's used in a lot of research).

We have tried a variety of meshing techniques, but our most recent attempt looks like this:

[IMG][/IMG]

We have looked at three different meshes with the following properties

Coarse:
- Cylinder divisions = 100
- Total nodes = 8364
- Diagonal divisions = 50
- Wake element size (mm) = 4
- Wake bias factor = 5

Medium:
- Cylinder divisions = 152
- Total nodes = 17581
- Diagonal divisions = 76
- Wake element size (mm) = 3
- Wake bias factor = 5

Fine:
- Cylinder divisions = 200
- Total nodes = 31709
- Diagonal divisions = 100
- Wake element size (mm) = 2
- Wake bias factor = 5

Our inlet velocity is 0.01005 m/s and we treat the outlet as an outflow.

To record the lift and drag, we monitor (read, write and plot) Cl and Cd with the following reference values:

L = 0.01m
D = 1.00m
A = 0.01m

To obtain the RMS Lift we take the standard deviation of the lift coefficient while the cylinder is oscillating. Similarly, to obtain the mean drag coefficient we simply take the mean drag over the same period.

The tests have the following parameters

Coarse:
- time step = 0.05s
- number of time steps = 5000
- Max Local Courant number = 2.19

Medium
- time step = 0.0375s
- number of time steps = 6667
- Max Local Courant number = 2.48

Fine
- time step = 0.025s
- number of time steps = 10000
- Max Local Courant Number

Applying all these parameters, we get the following results

RMS Lift Coefficient
- Coarse = 0.237
- Medium = 0.218
- Fine = 0.189

Mean drag
- Coarse = 1.366
- Medium = 1.362
- Fine = 1.347

The change in these is values (especially the lift) is obviously too great to settle with any of these meshes. Can anyone suggest any incredibly obvious things that my partner and I are missing of straight out doing wrong? Any help is greatly appreciated!

[LuckyTran]

The results look very nice except that you are not achieving the desired mesh independence. What does your turbulence model look like and what wall treatment options are your using? Are you using standard wall treatment?

I think you are okay, but is your time-step small enough to resolve the wake frequency?

[kweston]

We are just using a laminar model because we are only testing at Re = 100. Should we be using a different model? Can you elaborate what you mean by wall treatment? Our boundary conditions are a non-slip wall on the cylinder and symmetry boundaries for the top and bottom layer.

Our largest time step is T/100 and then for the medium and fine mesh we halved the time step each time.

[LuckyTran]

Sorry, I got the critical Reynolds number mixed up and thought that Re=100 was turbulent. Then the flow should be laminar and no turbulence model is necessary and hence no talk of wall treatment.

Have you checked convergence at each time-step? How many iterations do you have per time-step? And do you have any monitors to judge whether the solution at each time-step has converged?

Are you using 1st order upwind or 2nd upwind for the discretization of the advective fluxes?

[kweston]

From the residual plot, everything seems to be converging. Is there some way to record monitor the convergence? What can you recommend to monitor the convergence at each time step? All we look at are the residuals!

We have the max number of iterations / time step = 50. The average number of iterations per time step ended up being 7.0, 4.7 and 3.5 for coarse, medium and fine respectively.

[kweston]

We are using second order upwind btw

[LuckyTran]

Originally Posted by kweston

From the residual plot, everything seems to be converging. Is there some way to record monitor the convergence? What can you recommend to monitor the convergence at each time step? All we look at are the residuals!

We have the max number of iterations / time step = 50. The average number of iterations per time step ended up being 7.0, 4.7 and 3.5 for coarse, medium and fine respectively.

What are your convergence criteria, reduction of residuals below 1e-3, 1e-6?

7 may be okay but 4 and 3 are very few iterations. You should definitely monitor the solution values in addition to residuals to verify your solution at each time-step is converged. It's best to monitor a primitive variable like the x-velocity, y-velocity at a point in the flow, preferably in the wake region where the dynamic effects are. But you can also monitor your lift & drag. I generally target a minimum of 8-10 iterations per time-step. Even for simple diffusion problems, convergence can take 6 or iterations because of the influence of AMG solver.

[kweston]

1e-3 is what we are using - should we lower it to 1e-6? Is this how you increase the iterations / time step?

How exactly do we monitor the residuals? At present we are monitoring the solution values of lift and drag and that is all.

Thanks so much for your help with this, we realise how stupid some of these questions must be

[LuckyTran]

Originally Posted by kweston

1e-3 is what we are using - should we lower it to 1e-6? Is this how you increase the iterations / time step?

How exactly do we monitor the residuals? At present we are monitoring the solution values of lift and drag and that is all.

Thanks so much for your help with this, we realise how stupid some of these questions must be

Monitors of lift and drag are better than residual monitors, check these monitors to ensure that your solution is converged. Monitors of a single point velocity is the best way to check. You'll need more than 3 iterations of course to see any asymptotic properties. The easiest thing you can do is increase the number of iterations per time-step to more than 3.

There are a number of ways to increase the number of iterations per time-step. You can increase the reporting interval to say 5 iterations. This way the checks are performed only during the reports ( after 5 iterations, after 10 iterations, etc). This lets you guarantee 5 iterations without having to lower residual requirements. You also of course lower the residual criteria to 1e-4, 1e-5, or 1e-6. You can always turn off the convergence checks and this will force the solver to always use the maximum number of time-steps. Irregardless, you should check your solution values to gain some more confidence on whether each time-step is actually converged. You don't have to manually look at it for every single time-step, that would be cumbersome, but you need to at least do some sanity checks.

Still your problem may not even be related to this issue.

[Ahmed Saeed Mansour]

I have centrifugal pump and I want to make mesh dependence study ...the 2D mesh proved that 1mm cell size is very good in capturing the phenomena and no need to decrease the size anymore...so what should I do to make mesh dependence study if they ask me about it?
I have read some research papers that tell you that they make many sizes around the blades not the volute untill the results do not change and this is what I will do..my opinion is there is no need to test the volute as the results of the 2D is good and we just can make refinements around the blades and check it out...Help please.