
[Sponsors] 
Lift is oscillating while using steady state solver. 

LinkBack  Thread Tools  Search this Thread  Display Modes 
March 8, 2015, 07:31 
Lift is oscillating while using steady state solver.

#1 
New Member
Jan Michielsen
Join Date: Mar 2015
Posts: 4
Rep Power: 10 
Hi all,
I'm studying the crosswind stability of the M6train. 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 

March 10, 2015, 09:44 

#2 
Senior Member
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17 
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. 

March 10, 2015, 12:02 

#3 
New Member
Jan Michielsen
Join Date: Mar 2015
Posts: 4
Rep Power: 10 
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 1e3, 1e4 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 

March 10, 2015, 12:23 

#4 
Member
Alex
Join Date: Jan 2014
Posts: 54
Rep Power: 11 
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. 

March 10, 2015, 13:30 

#5 
Senior Member
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17 
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 SpalartAlmaras 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. 

March 10, 2015, 13:46 

#6 
Senior Member
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17 
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, 10e3 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.


March 10, 2015, 14:22 

#7 
New Member
Jan Michielsen
Join Date: Mar 2015
Posts: 4
Rep Power: 10 
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 Komega turbulence model (with wall function) since this is as far as I know a reasonable trade of between computational time and precision. The 1e3 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 

March 10, 2015, 14:28 

#8 
Senior Member
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17 
If you don't have cell quality remediation turned on, do so. You are correct about kw being your best choice. Watch your y+ value though, as this can affect your drag values pretty significantly.


March 10, 2015, 14:30 

#9 
Senior Member
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17 
Scratch that, sorry. I forgot which forum I was posting in. If you are using starccm turn on cell quality remediation. Not sure if that is an option with other software packages or not.


March 17, 2015, 14:18 

#10 
Member
Ethan Doan
Join Date: Oct 2012
Location: Canada
Posts: 90
Rep Power: 12 
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


March 18, 2015, 04:55 

#11 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,597
Rep Power: 70 
I give my ideas...
If the flow problem has an energyequilibrium 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 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Steady State solver for High Mach No flows  mecbe2002  OpenFOAM  10  July 6, 2021 03:56 
[ANSYS Meshing] Help with element size  sandri_92  ANSYS Meshing & Geometry  14  November 14, 2018 07:54 
Is steady state solver grid dependent?  mmkr825  OpenFOAM  4  March 22, 2013 12:46 
Convergence and steady state using simpleFoam  sfigato  OpenFOAM Running, Solving & CFD  0  February 8, 2013 04:14 
Steady State 2 phase problem  fivos  FLUENT  0  April 27, 2009 16:34 