
[Sponsors] 
CFX convergence problem simulating ogivecylinders at varied angle of attack 

LinkBack  Thread Tools  Search this Thread  Display Modes 
April 27, 2011, 22:13 
CFX convergence problem simulating ogivecylinders at varied angle of attack

#1 
New Member
Join Date: Apr 2011
Posts: 3
Rep Power: 11 
Hello all,
I am trying to simulate free shear flow past an ogive cylinder shape (length of 3m, dia 0.25m) in ANSYS CFX and am running into a problem as I change the angle of attack. The ogive cylinder is contained within a cylindrical control volume (length 10m, rad. 3m) with the following domains/boundary conditions:
++  ****** Notice ******   The nondimensional near wall temperature (T+) has been clipped   for calculation of Wall Heat Transfer Coefficient.     Boundary Condition : OCylinder   T+ clip value = 1.0000E10     If this situation persists and you are using the High Speed Model,   consider enabling Mach number based blending between low speed and   high speed wall functions. You can do so by specifying a Mach   number threshold as follows:     EXPERT PARAMETERS:   highspeed wf mach threshold = 0.1 # default=0.0 (off)   END  ++ Things I have tried to solve this problem:
I have reached the limits of my own understanding and am interested to know if anyone else has been able to overcome similar problems or has some ideas as to how I should proceed... 

April 28, 2011, 09:53 

#2 
Senior Member
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 511
Rep Power: 17 
I assume this is a steady state run. Are you hammer starting this solution or using previous solution as a starting point?
Either way, I have found that if I baby step the Timescale Factor (it defaults to 1) up from a very small scale to 1 over some period of iterations, your solution converge easier. This is particularly the case for high mach and angle of attack runs. As an example I use the following expression for timest: step(10.5aitern)*0.001+step(20.5aitern)*step(aitern10.5)*.005+step(30.5aitern)*step(aitern20.5)*.03+step(40.5aitern)*step(aitern30.5)*.08+step(50.5aitern)*step(aitern40.5)*.4+step(aitern50.5)*1 This will step timest up from 0.001 to 1 over 50 iterations (you can adjust as you see fit). Edit: Sorry, just noticed you have adjusted the timescale factor. In the past, I have found that 0.01 might not be low enough to ease into a stable solution. If you interpolate a "close" previous result, you might be able to get away with a larger timescale factor. Try lowering timescale and easing it up. Then use timest in the Timescale Factor under the Solver Control Tab. I hope this helps. Ed 

April 28, 2011, 18:44 

#3 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,644
Rep Power: 130 
Try starting the run using local time scale factor, a value of 5.0 should be OK to start. Once the flow is converging switch back to physical time scale.
Also, rather than using Edmund's CEL function you can do this manually with "Edit run in progress". Depends on whether you want to automate it or keep manual control, up to you. 

April 28, 2011, 20:01 

#4 
New Member
Join Date: Apr 2011
Posts: 3
Rep Power: 11 
Ed:
Your assumption is correct, the simulation is steady state and I am trying to hammer start it. Thanks for the stepping algorithm. I'll give it a shot anyway seeing as it starts off an order of magnitude lower than I've run it previously Glenn: I'll give the local timescale factor a shot as well. At the moment I run several cases via a batch script and use CFX just to create the '.cfx' and '.def' files so an automated CEL function is ideal. Thanks both for your suggestions, I'll let you know how they work out. 

April 30, 2011, 06:48 

#5 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,644
Rep Power: 130 
Oh yes, and another thing  for high mach number flows a good initial guess is very useful. Try doing a model at a lower velocity, subsonic if you have to. No need to converge it fully, just enough to get a reasonable flow field for the initial condition for the full speed run.
Alternately you can ramp the inlet speed up using a function like Edmund recommended for the time step size (or manually do it through the edit run in progress) 

May 10, 2011, 19:16 

#6 
New Member
Join Date: Apr 2011
Posts: 3
Rep Power: 11 
I have had some success with the stepping algorithms and usually employ them for both timest and the inlet velocity.
Thanks a heap for your help. 

February 25, 2015, 21:42 

#7 
New Member
Nizam
Join Date: Feb 2015
Posts: 2
Rep Power: 0 
Hi,
I dont know how to insert these expression in CFX, can u please help me. I know to write expression to evaluate properties in post processing but dont know where to write in solver. thank you 

Tags 
convergence issues, sst, supersonic flow 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
CFX Convergence Problem  Abdul  CFX  12  June 30, 2014 08:55 
a serious problem on a case with attack angle  anne  CFX  0  November 18, 2008 05:28 
Proper output of angle of attack in CFX post  Kevin  CFX  3  October 18, 2006 12:18 
Convergence problem in CFX  Nicola  CFX  4  July 26, 2006 11:44 
CFX 4.4 installation problem  Pandu Sattvika  CFX  1  December 1, 2001 04:07 