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

Moment convergence

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 5, 2006, 18:14
Default Moment convergence
  #1
Bunmi
Guest
 
Posts: n/a
how do i know that my moment has converged?

Pls help me in this.I need to monitor moment as my performance indicator

WAITING
  Reply With Quote

Old   January 6, 2006, 01:44
Default Re: Moment convergence
  #2
sharuk
Guest
 
Posts: n/a
solve->monitor->forces

and drop down the list to moment and specify the rotational axis.
  Reply With Quote

Old   January 6, 2006, 03:41
Default Re: Moment convergence
  #3
Bunmi
Guest
 
Posts: n/a
yeah. that is what i did but how do i know when it has converged.Am i going to have a constant moment for a long time or what?
  Reply With Quote

Old   January 6, 2006, 04:47
Default Re: Moment convergence
  #4
sharuk
Guest
 
Posts: n/a
exactly..
  Reply With Quote

Old   January 6, 2006, 07:54
Default Re: Moment convergence
  #5
Bunmi
Guest
 
Posts: n/a
so, if the moment is not constant(i.e it is changing) that means my moment has not converged
  Reply With Quote

Old   January 6, 2006, 09:31
Default Re: Moment convergence
  #6
Jason
Guest
 
Posts: n/a
It either means you haven't reached a converged solution, or that you have an unsteady problem (typically due to vortex production in a region of separated flow... like behind a bluff body or off the separation on a wing).

Good luck, Jason
  Reply With Quote

Old   January 6, 2006, 10:13
Default Re: Moment convergence
  #7
Bunmi
Guest
 
Posts: n/a
ok.i will try to leave d solution awhile and see if it'll d moment will constant
  Reply With Quote

Old   January 6, 2006, 10:16
Default Re: Moment convergence
  #8
Bunmi
Guest
 
Posts: n/a
What could be responsible for this vortex production?

thanks
  Reply With Quote

Old   January 6, 2006, 13:46
Default Re: Moment convergence
  #9
Jason
Guest
 
Posts: n/a
That depends on your model. Separated flow is the most common cause. Separated flows are naturally unsteady. For a bluff body, you'll typically get vortex shedding (like behind a cylinder). For airfoils the separated region will oscillate forward and backwards on the airfoil. The "steady state" solution for these is usually a time averaged value during testing (electronic data is typically recorded over a period of time then averaged, if the data is recorded from mechanical readouts, there is typically some damping in the system to account for small oscillations). Depending on what's causing the unsteady response, you can usually get a solution within a small oscillation (if it's oscillating in the 3rd or 4th significant figure, does that really matter? I'd be willing to bet my hard earned money that your CFD model has more error than 4 sig figs), but this depends on your choice of turbulence models, the extent of the separated region, and your mesh density and quality.

A poor mesh can also cause a "flapping" effect. I've seen it for a poorly meshed airfoil where the grid sensitivity was causing an oscillating pressure coming off the trailing edge of the airfoil that wasn't real. It wasn't separated, but it was a pressure oscillation. We refined the mesh and that problem went away.

If your values aren't converging (or at least oscillating about a small enough range), then you need to look at your solution and try to figure out where the problem is. You can create vertices and monitor the pressure at these vertices to try and locate the problem area if you have to. Try refining your mesh in the problem areas. If you're still having trouble, look into the different turbulence models. You may not have the best model chosen for your problem. If it's a large scale oscillation due to a large separation region (like behind a cylinder) then you may never get a steady state solution, and you might want to run it unsteady and use data sampling to get average and RMS values.

Hope this helps, and good luck, Jason
  Reply With Quote

Old   January 11, 2006, 04:24
Default Re: Moment convergence
  #10
Bunmi
Guest
 
Posts: n/a
Thanks.My model is a mixing tank.I'm carrying out a kind of parametric sensitivity of the turbulence model which is standard k-e model.There has been issues around the use of this model but the computing requirements & robustness still makes it best.But I am trying to optimise the model by changing the constant(C1,C2, Cm) so as to see the effect on the predictions. Using the standard k-e model, the moment converged but changing some of these constants, the moment refuse to converge.I was wondering what could be responsible for this. The surpising thing is that the moment is not converging but the variation of the constants has a great impact on the constant.For instance, some combinations of C1, C2 & Cm gave me good predictions with least error values between the experimental and predicted values. But the moment did not converge. I am really surprised about this.

So u can see the issue now.

Waiting yr response
  Reply With Quote

Old   January 16, 2006, 10:09
Default Re: Moment convergence
  #11
Jason
Guest
 
Posts: n/a
Now you're getting into areas where I'm not too familiar. I pick my turbulence models based on a knowledge database we have where we compare different turbulence models to different situations. I have never gone in to customize a turbulence model. I hope you've researched the turbulence model and what the different coefficients do. Also, you should do some research to see what other people have used for custom coefficients.

I have a feeling that some of the constants effect the stability of the model, which is why you're having trouble getting a converged value.

Also, do you know for sure that your mesh is optimized? Have you run mesh sensitivities with the default coefficients?

Hope this helps, and good luck, Jason
  Reply With Quote

Old   January 18, 2006, 07:29
Default Re: Moment convergence
  #12
kharicha
Guest
 
Posts: n/a
I have played a little with the k-epsilon constants, I could make converging the solution on a very bad grid.... this effect was due the increase of the turbulent viscosity ratio which is known to stabilize the flow(just like normal viscosity).

So it is always possible to modify the constants so that the magnitude and the distribution of the turbulent viscosity damp instabilities.

So I totally agree with Jason, this is dangerous, we should first verify our grid, y+, symmetry of the grid...etc before playing with the parameters.

  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
Convergence Centurion2011 FLUENT 24 May 9, 2015 08:02
Force can not converge colopolo CFX 13 October 4, 2011 22:03
UDF extern variable - mean time moment coefficient enry Fluent UDF and Scheme Programming 0 November 14, 2009 07:56
UDF extern variable - mean time moment coefficient enry Fluent UDF and Scheme Programming 0 November 14, 2009 07:51
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 01:17


All times are GMT -4. The time now is 06:11.