CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

stable problem

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   December 9, 1999, 09:10
Default stable problem
  #1
s.t.Wang
Guest
 
Posts: n/a
I calculate a steady flow field around a cascade with my time dependent N-S code in which B-L algebraic model was employed.I found the residual only decreased two orders,and the maximum residual position near trailing edge where a pairs of vortex located. the aerodynamic parameters varied periodically.But most of the researchers point out that residuals can decreased five or more order.I confused!! I hope you answer,thank you.
  Reply With Quote

Old   December 9, 1999, 10:15
Default Re: stable problem
  #2
John C. Chien
Guest
 
Posts: n/a
(1). This is because you are using time dependent formulation. (2). The time dependent formulation does not guarantee to give a steady-state solution. (3). On the other hand, the steady-state formulation will provide a steady-state solution. (4). In your case, if you modify the trailing edge geometry to a sharp one, the oscillation should reduce. But then, you are solving a different problem. It really depends on what you are after in the simulation. (5). In my steady-state calculation, I normally set the normalized residuals to 1.0E-08, and stop the calculation when the residuals drop below 1.0E-06. The right approach should be the monitoring of the flow variable itself VS time or iteration number. So, if your flow variable near the trailing edge is oscillating in time, then the flow is transient flow. (6). The situation is rather complex, because the solution could be real, or artificial due to the mesh, time step, turbulence model, etc. In other words, what you are getting is typical. It takes a great deal of experience to know whether it is useful or not, right or wrong.
  Reply With Quote

Old   December 9, 1999, 10:51
Default Re: stable problem
  #3
Jonas Larsson
Guest
 
Posts: n/a
You've probably got periodic vortex shedding from the trailing edge. One ugly trick to reduce this problem is to mesh the trailing edge with a coarse mesh. This often adds enough numerical dissipation in this region to damp out these oscillations. If you're only intereseted in pressure distributions etc. on the blade then this approach is usally okay. If you are interested in wake profiles and detailed lossed then this is not a good approach.
  Reply With Quote

Old   December 10, 1999, 16:57
Default Re: stable problem
  #4
John C. Chien
Guest
 
Posts: n/a
(1). Your e-mail received. Thank you. (2). You did not mention the Mach number and the blade condiguration, so, it is difficult to know exactly the problem areas. (3). It does make a big difference whether you are using a pressure based method or a density based method. For density based methods, at low mach number, there is always oscillations in the solution. For this type of method, you can try to increase the artificial viscosity parameters to smooth out the oscillations. (4). For the pressure based method, you can use smaller under-relaxation parameters to reduce the oscillation. (5). The mesh used is also important to the convergence of the solution. You can improve the mesh density distribution, the mesh smoothness, and skewness. It is likely that in some areas you don't have enough mesh points. (5). Then, there comes the treatmnet of the boundary conditions. It can also affect the oscillation of the numerical calculations. (6). I think, what you need to do is to isolate the problem first. So, a simple cascade with zero or small flow turning could be used as a test case first. (7). The simplest way to check the convergence of the solution is to print the flow variable up to 4 decimal points vs time step (or iteration number) and observe the change in value until all the decimal points are identical. So, for single precision variable, you should run the calculation until 6 digits are identical between time steps. (8). If you don't know the slow convergence area, then the contour should be used, until two contour plots are identical between two test time steps. (9). So, try a step-by-step aproach to see whether you can learn something in the process.
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Problem with interFoam; Wave/wiggle alpha1 behavior JonW OpenFOAM 3 February 23, 2013 21:41
area does not match neighbour by ... % -- possible face ordering problem St.Pacholak OpenFOAM 9 November 22, 2011 11:02
Problem in implementing cht tilek CFX 3 May 8, 2011 08:39
Adiabatic and Rotating wall (Convection problem) ParodDav CFX 5 April 29, 2007 19:13
Is this problem well posed? Thomas P. Abraham Main CFD Forum 5 September 8, 1999 14:52


All times are GMT -4. The time now is 16:15.