Lift is oscillating while using steady state solver.
 

Hi all,

I'm studying the crosswind stability of the M6-train. For flow angles till 30 degrees (compared to train's heading direction) the lift stays more or less steady. For higher angles the lift coefficients starts oscillating (not in a periodic manner) from -3 to 0 (positive lift pushes the train downwards in my case).

Is this due to possible vortex shedding on the train? And if I should run an unsteady case, won't the lift be oscillations over different iterations during one timestep?

The other moments and drag coefficients stay more or less constant.

A figure of the lift coefficient over different itterations is shown in the attachment. (The coefficient was found to be 2.8 in experiments)

Thanks in advance

http://www.mijnalbum.nl/index.php?m=upload&a=20

http://www.mijnalbum.nl/index.php?m=upload&a=20

I cannot access your image, but if your lift is oscillating at high angles of attack it is a good bet that it is due to vortex shedding. It sounds like you are employing an implicit solver that uses a pseudo time step, which is by far the most common approach in my experience.

Yes, you should run this as an unstready case. Make sure you start from your already completed steady state solution and use enough iterations in each time step so that each time step converges. Then you will average your force over long enough that your average doesn't change very much with successive time steps.

Thanks for your reply.

I'm now currently running an unsteady case for a yaw angle of 30 with a timestep of 0.05s. Is it normal that that the solution often converges in timestep after only one iteration (since it's starting value is below the value of the scaled residuals, in my case 1e-3, 1e-4 would take way to long for the solution to converge). The domain contains 3 million cells.

Is there a way to 'force' in into a steady case to speed up the simulation.

The oscillating lift when using the steady case is attached (Hopefully you can see it this time)

Greetings,
Jan

First, if the angle of attack of the train is about 30, it is safe to assume the flow is separated and turbulent. You might want to employ models that are used to predict lift coefficients for stalled airfoils or delta wings at high angles of attack. If you are using a steady model you simply are not capturing the physics.

Note: I know a lot about fluids but not much about CFD. I cant tell you what model to use but can tell you the physics that needs to be captured.

That time step may be too large, I am not sure. Time step is very closely related to courant number so do some research on what a good choice would be based on what you used for your steady state solution. Unfortunately, there isn't much wiggle room on the iterations per time step. Convergence is convergence. You probably won't need more than maybe 5 or 10 though. Starting from your steady solution just means you don't have to wait for it to ramp back up and get basically back to the point you are now. You can cut the initialization time of the steady solution by using grid sequencing expert initilization.

As far as what model to use, HOT_SOUP is correct. You should use the proper turbulence model and numerical approach. For separated flows with lots of turbulent vortex shedding a you really should do an LES analysis with Spalart-Almaras turbulence model or DNS. Unfortunately, if you are concerned about a 3M cell model size these are not on your radar. You would need 10 - 100 times as many cells to pull that off. LES (large eddy simulation) requires you to resolve turbulent eddies that are much smaller than the cell size you likely have with a 3M cell RANS model of a train. DNS (direct numerical simulation) is even worse and requires you to resolve turbulent eddies of all length scales. That is almost certainly beyond the scope of what you are trying to do.

What exactly are you hoping to learn from this data? That has a big impact on how you should approach your model.

Sorry, I misread part of that. Yes, one iteration is unusual. Make sure you select clear solution > history only before you start your transient anaysis. You should see a saw tooth pattern to your residual plots . Also, 10e-3 isn't the absolute value of your residual, it's normalized by defalut. What you are really looking for is 3 orders of magnitude change.

Hi, thanks again for the reply.

I'm using the aerodynamic coefficients to study the crosswind stability of a driving train.

Currently I'm using the K-omega turbulence model (with wall function) since this is as far as I know a reasonable trade of between computational time and precision.

The 1e-3 value for scaled residuals was chosen since the steady state simulation had problems dropping below this value.

I've made another mesh with a higher overal mesh quality and less skewed cells. This simulation looks, so fare, more stable.

Thanks

If you don't have cell quality remediation turned on, do so. You are correct about k-w being your best choice. Watch your y+ value though, as this can affect your drag values pretty significantly.

Scratch that, sorry. I forgot which forum I was posting in. If you are using star-ccm turn on cell quality remediation. Not sure if that is an option with other software packages or not.

hi Jan, i don't think its advisable to capture the lift at high angles of attack with a wall function mesh. you are going to want to have a finer mesh and solve the flow all the way to the wall with a low re model

I give my ideas...


If the flow problem has an energy-equilibrium solution, in general you can try solving for the statistically steady solution (RANS).
However, a high angle of attack produces relevant separation effects, it is well known that RANS approach fails to solve such complex flows as the model coefficients to be fixed strongly depends on large scale effects.
It is advisable to switch to LES/DES approach