
[Sponsors] 
March 25, 2013, 05:39 
Coupled solver, computational cost

#1 
Senior Member
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 6 
Hi everybody guys,
I'm solving a wind turbine starting with the steady laminar case and using a pressurebased coupled algorithm. I have a few questions about the setup. I've looked at the theory guide but I don't know how the Courant number (the solver one, no the regular one) affects convergence. The only thing theory guide says is 1/CFL=(1alpha)/alpha. I increased CFL from default 200 to 200000 but then I reduced it to 200 as it seemed to increase computational cost. Residuals went up so I had to reduce uderrelaxation factor (URF) to half of its value for momentum and pressure (0.75 to 0.375 each). Now that residuals are starting to go down I would like to increase computational speed as it is way too slow. I know increasing URF will improve that, but what about CFL? For a 1.7 Gb mesh, 8 cores parallel, 12 Gb RAM it's taking 45 min for each step. Also, I will have to do a transient laminar case and steady/transient komega SST, which solver setup should I use? SIMPLEC? PISO? Thanks in advance! 

March 26, 2013, 07:25 

#2 
Senior Member
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 6 
I've increased URF to 0.75 and it obviously takes less to calculate each iteration, but it's still slow (30 min/iteration). Can I increase URF over default values? What about Courant number, how does it affect the simulation?
Also there's reverse flow at pressure outlet, and it's increasing. Any suggestion? Thanks! 

March 26, 2013, 07:31 

#3 
Senior Member
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,134
Rep Power: 19 
30 minutes for one iteration sounds like the simulation is running out of core.
Check the RAM usage while running the case. 

March 26, 2013, 07:38 

#4  
Super Moderator

Quote:
For transient case PISO and coupled are good option as they can accommodate larger time steps... And I would prefer coupled. Still not checked the results, accuracy and speed of these two schemes... 

March 26, 2013, 07:51 

#5 
Senior Member
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 6 

March 26, 2013, 08:05 

#6 
Senior Member
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,134
Rep Power: 19 

March 26, 2013, 08:08 

#7  
Senior Member
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 6 
Quote:
As suggested by Far I'm going to coarsen my mesh a bit more. 8 millions cells seem too much. 

March 26, 2013, 08:14 

#8 
Senior Member
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,134
Rep Power: 19 
Double precision usually is only necessary if there are cells with really high aspect ratio in the boundary layer to achieve Yplus<1.
In most cases, the other errors in the simulation are several magnitudes higher than the roundoff error in single precision. The thing with double precision is that it doubles memory usage. 

March 26, 2013, 08:15 

#9 
Senior Member
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11 
Courant number is proportional to the time step and velocity and inversely proportional to grid size at local cell conditions. The fact that how much sensetive the solution is to Courant number, depends on whether the solution method is explicit or implicit.
With explicit method, there are obvious limitations on timestep, and hence Courant number. For implicit method, typically it should be helpful to increase the Courant number in accelerating convergence. However, you should be careful here since the Courant number should be ramped gradually over say 50100 iterations. This interval should be smaller, and the increase in Courant number should be smaller, at the initial phase of solution, where the transient instabilities have a strong influence on solution. A sudden increase in Courant number may not achieve the steady convergence goal. OJ 

March 26, 2013, 08:20 

#10  
Super Moderator

Quote:
OJ: This cournt number is different. It is for pressure based couple solver only. Recommended value is 200,000 Try SIMPLE , it will cost you less along with single precision. 

March 26, 2013, 08:21 

#11 
Senior Member
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 6 

March 26, 2013, 08:27 

#12 
Super Moderator


March 26, 2013, 10:48 

#13 
Super Moderator

i don't want to sound pessimist:for an 8 million nodes, i'm not surprised. you need to take that case to a cluster. no matter what you change, it will always take too much time...
is it the mesh about the blade ? 

March 26, 2013, 10:52 

#14  
Senior Member
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11 
Quote:
The algebraic approaximation of integral balance for any control volume is given as: Patankar (1980,1981) proposed the underrelaxation factor as This is same as equation 2060 in ANSYS Help documentation of FLUENT. The implementation of CFL in this context is: or, Consequently the governing equation for the control volume becomes: One may wonder why bother using CFL instead of , when the governing equation is same. But a little observation will bring clarity such that the equation advances in time , where . In case of steady state, this formulation can be used in with pseudo transient solver. Thus CFL represents a more intuitive definition of implicit underrelaxation. Essentially, use of CFL helps advance the solution by multiples of timesteps defined by cell Courant number (the original one, not solver). Essentially, for smaller timestep, the coefficient will be large and solution will be slow, universally. The multiple of CFL helps in keeping timesteps different in different regions of the domain, with different values of , instead of employing a singular timescale over whole domain. Thus timestep becomes location specific and is different throughout the domain. This helps in convergence, because in case of single universal timestep, its value may be too small somewhere (in case of higher velocities) so the solution in this region will progress slow in time or too large elsewhere (in regions of small velocities) so the solution in this region may just diverge inducing instability. One of the most important aspect of using this formulation instead of under relaxation factor is that with CFL you have a wider range of advancement factors. Under relaxation factors of 0.9,0.95 and 0.99 imply CFL values of 9, 19, 99 respectively. Thus use of CFL gives a wider (or refined) range of pacechange than URF. Higher values of CFL will advance the solution with larger timesteps, increasing pace of solution. But it is wise to do it gradually than suddenly. OJ 

March 26, 2013, 11:04 

#15  
Senior Member
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 6 
Quote:
I'm working on reducing the mesh density, but what max cell size can I use in the farfield? Thanks! 

March 26, 2013, 11:54 

#16 
Super Moderator

have you tried the block refinement tab, see if you could bring the blocks in far field to 1/2 the others...


March 26, 2013, 11:58 

#17 
Super Moderator

i have the same machine as you , 16gb of ram, i don't go beyond 1 500 000 nodes. i know my machine can't handle them. how much of the extra minutes could you get after inputting the right adequate CFL ??


March 26, 2013, 14:56 

#18  
Senior Member
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 6 
Quote:
Quote:
Quote:
I don't know which is the adequate CFL, I've just started with the 200 default value. I guess the higher the faster so the better for me. Thanks a lot! 

March 27, 2013, 12:37 

#19 
Senior Member
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 6 
I've reduced the mesh from 8 to 2 million elements without changing the y+. Quality>0.2, min angle>18º and volume change <50 (most elements vol change<30)
Then I've run the steady laminar case with single precision, SIMPLE and 2nd order pressure and momentum. inlet velocity is 5m/s, rotational velocity is 1.034 rad/s. It has reached residuals 1e4 for 2700 iteratons, computation time was 1h30 using 8 cores, which seems okay to me. Reverse flow at outlet started in 15,000 cells then it reduced to 0 and started raising up to 6,000 when convergence was reached. The issue is force and moment coefficients for the blade surface are very low: CD=0.04 (xaxis), CL=0.48 (zaxis) and CM=0.0032 (around zaxis) I've checked the flow pattern around the airfoil and it looks good, I think there's some recirculation in the leeward face, which is strange for an angle of attack of 12º (see pictures) What can be wrong? Bad mesh near the airfoil? Bad mesh in the farfield? Wrong solver setup? Is it possible to have stall in the airfoil that early? Another question, could anybody tell me how to meassure lift or drag force over a line (airfoil perimeter) of the blade surface? Any suggestion is welcome! Thank you guys! 

March 27, 2013, 12:51 

#20  
Senior Member
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,134
Rep Power: 19 
Quote:
Have a closer look at the region where backflow occurs and consider moving the outlet further downstream. 

Tags 
cfl, coupled, courant, underrelaxation factor 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Some confusion about coupled solver for incompressible flow  bearcat  Main CFD Forum  0  February 14, 2010 21:40 
coupled solver (again)  lucioantonio  FLUENT  0  April 8, 2009 16:15 
Coupled solver energy equation problem  lucioantonio  FLUENT  0  April 3, 2009 10:21 
coupled solver wont work in star ccm+  richie  CDadapco  5  November 4, 2008 05:51 
Re: Coupled solver + RNG Ke Model  JN  FLUENT  1  April 22, 2001 16:34 