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

Simple 3D Fluent Analysis

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 21, 2006, 21:29
Default Simple 3D Fluent Analysis
  #1
Chris
Guest
 
Posts: n/a
Hi Everyone,

Perhaps some of you bright individuals out there can give me some pointers. I had done plenty of 2D analysis in Fluent, but as part of a design project we are attempting to do some 3D analysis.

To make matters simple, we are only required to do inviscid 3D. My question is, after above 350-400 iterations, the solution does not converge, but rather hovers around the 10^-4 area, and does not drop below it.

I am using the following settings: Coupled, Implicit, 3D Viscosity I am using as Inviscid. I have the Energy Equation Enabled. My Material is an Ideal Gas, and my boundary conditions are as follows:

I have a cube with a wing inside of it. The wing is attached to one side of the cube. That side of the cube and the wing are considered walls. The top and bottom of the cubes are considered walls as well. The front face, and back face are Velocity Inlet, and pressure outlet respectively. I have been varying my courant number as high as 500, but I find the best results are when I used small courant numbers (<= 5). We are using a convergence criterion of 3e-05.

If anyone has any suggestions or solutions, it would certainly be appreciated!!!

  Reply With Quote

Old   March 21, 2006, 21:58
Default Re: Simple 3D Fluent Analysis
  #2
Ahmed
Guest
 
Posts: n/a
A Taylor series analysis will tell you that errors are function of delta x,..(Remesh and make sure your mesh is orthogonal or near orthogonal, no jumps in the sizes between adjacent cells,i.e. use suitable and reasonable clustering functions) Courant number 500 !!! First, the Courant number (in numerical work), is used to calculate the size of time step , physically, it ranges from 0->1 (The definition and its physical meaning is well explained in many CFD Works), but to accelerate convergence, computational values greater than 1 are used, it is normal to start a computation with values in excess of 1 but when the solution is close to convergence it is reduced to it physical limit
  Reply With Quote

Old   March 22, 2006, 03:03
Default Re: Simple 3D Fluent Analysis
  #3
Razvan
Guest
 
Posts: n/a
I think you are misinterpreting a bit Courant number, Ahmed. Courant number is indeed a local time step (local because it depends on local cell size and velocity), but is wrong to consider that there exists a phisical limit for it!!! There is no such think, man!

The limitations you are talking about are of a different nature: numerical. Explicit formulations have a natural limitation to CFL<1 (and this is true only if there are no programming mistakes that would lower this limit even more), but programming tricks, stabilization numerical schemes can override this natural limit, and you can obtain CFL=3 or even CFL=5 in coupled explicit codes using residual smoothing, for example. But for implicit formulations, these limitations do not apply. Of course, due to nonlinearities, actually there is a stability limitation even to a coupled implicit alghoritm, but it can be very high (CFL=100, or more!!!). There is nothing wrong to use such high CFL numbers, but only if the flow is quasi-steady (this means that the final result does not depend on how large "time steps" you make to get there)!

So, using such large CFL numbers does not influence the quality of the final solution, only the time spent to achieve it (again, this is true only for stady-state flows)!

Now, Chris, there is no problem if residuals do not drop below 3e-05, often in coupled implicit simulations you must use other convergence criterions, and the best are Cd and Cl. If the value of Cd converges, it means that skin friction has converged, which is the hardest to converge in your type of simulation.

A final observation: you said that you are using a velocity_inlet boundary condition. This means that you are asumming incompressible fluid. This of course is not wrong if the velocity is sufficiently low (under M=0.2), but is not recomandable to use a coupled implicit solver. A better choise would be the segregated solver, it will converge significantly faster!

Good luck, Razvan
  Reply With Quote

Old   March 22, 2006, 03:28
Default Re: Simple 3D Fluent Analysis
  #4
Charles
Guest
 
Posts: n/a
Razvan is right. In this kind of problem you really need to monitor convergence on forces, although if you are using inviscid only, there will be no friction. Also, if your Mach number is low, the inviscid result will not be physically realistic anyway.
  Reply With Quote

Old   March 22, 2006, 03:38
Default Re: Simple 3D Fluent Analysis
  #5
Razvan
Guest
 
Posts: n/a
Thank you for your intervention, Charles. I forgot that Chris is not considering a viscous flow. And you are right too, of course, with your last statement.

Razvan
  Reply With Quote

Old   March 22, 2006, 20:26
Default Re: Simple 3D Fluent Analysis
  #6
Ahmed
Guest
 
Posts: n/a
Razvan

Simply accept the following: Get a Book about CFD and read about the Courant number, Solution Stability and The physical meaning of the Courant Number.

Waves are waves, they always behave like waves even if you are not aware or familiar with their presence.

You can also google for some interesting stuff about the Courant Number

As a final resort, use the email button to email me, I might be able to scan useful information for you

Enjoy your readings.

This is an open forum where people exchange opinions and ideas about CFD but using a decent language. It is simple to mock others especially in the anonimity of the internet

Cheers
  Reply With Quote

Old   March 23, 2006, 02:38
Default Re: Simple 3D Fluent Analysis
  #7
Razvan
Guest
 
Posts: n/a
Ahmed,

I am truly sorry that my intervention made you feel like I was mocking you! This was not my intention at all, but as I see that I offended you, I deeply appologise to you.

Nowadays there is more then one way to "define" CFL, but I was reffering only to the very first and generally accepted in day-to-day CFD:

CFL=(delta_t) * velocity / (delta_x)

Now, let me explain myself: all I said earlier about CFL only applies to STEADY simulations (and I clearly mentioned that). In such simulations, CFL losses any "phisical meaning" because truly steady simulations DO NOT depend on the initial conditions, and CFL is restrained to only a simple measure of how fast the calculation "advances" to the ONLY final solution (it's just a "pseudo-time-step").

In unsteady simulations, everything changes, a real "phisical meaning" can be attributed to CFL, and the concept of "waves" is perfectly acceptable now. Even more, if we exceed CFL=1 in such a simulation (we allow "waves" to travel further than local cell size), than inevitably truncation errors emerge and if the numerrical scheme is not self-correcting (to maintain error at an acceptable level), then the error accumulates and the result is total garbage. I am perfectly aware of all this.

BUT I INSIST: ALL I SAID IN MY PREVIOUS INTERVENTION WAS FOR STEADY SIMULATIONS, AND I CLEARLY UNDERLINED THAT.

Again, I appologise to you and I admit that my language was too "offensive", but all this is due to the fact that poor Chris was going to take your words for granted because you did not explained yourself properly.

With all due respect, Razvan
  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
Fluent analysis for SEM race car jhthoh FLUENT 0 February 18, 2011 03:07
exporting results from fluent for fem analysis Kevin FLUENT 1 September 13, 2006 15:14
Uncoupled analysis with FLUENT and ANSYS Mohammed FLUENT 0 September 13, 2006 12:41
Simple fluent questions temp3733@gmail.com FLUENT 0 May 18, 2005 12:50
How does FLUENT fair in absolute heat transfer analysis Steve Aboagye Main CFD Forum 1 August 31, 1998 12:12


All times are GMT -4. The time now is 21:48.