I have some experience with CFD, but primarily with very low Reynolds number flows (most work to date is laminar). I am just now starting graduate school, and one problem I am trying to solve is the flowfield about a car. I'm using Fluent 5, and am having trouble with the turbulence energy and dissipation values diverging right away. I'm using the Lam-Bremhorst approach, with an initial turbulence intensity of 8% at the velocity inlet. Freestream velocity is u=25.587 m/s, problem is isothermal, SIMPLEC solver. I have not yet taken a course in turbulence, and would appreciate any guidance one could offer. Feel free to contact me directly by email: kgray@umr.edu

(1). There are three simple solutions: (2). Stop using the code, (3). Ask the vendor to solve the flow over the car, (4). Write your own code. (there is a fourth solution, that is to try other codes. they all claim that their codes can handle arbitrary geometry and from subsonic to supersonic.) (5). If you really like to kill the time, try some simple problems first. (6). I came across a book in the local Barnes & Noble book store last week. The book stated that the richest person of a computer software company said that the main reason to release a new version of a code is definitely not to eliminate the bugs. (the book was on how the users are suffering from the codes with bugs) (7). I also have come to my own conclusion about the CFD codes that the main goal of the CFD code vendor is definitely not to solve the CFD problem. As long as the problem is remain un-solved, there is always market to use the commercial CFD codes. So, based on my theory, your problem is likely remain un-solved.

I hope you have studied the governing equations of k-e model by Lam and Bremhorst. Which means you know that the boundary condition of of epsilon at the wall is non-zero which is physically true but numerically disgusting. If the soultion that you are getting is far away from your initial conditions this boundary condition would keep you frustrated. But if you give appropriate initial conditions or in other words you know the solution of your problem already then what is the use of computation (Ha! Ha! Ha!). What I have doing is that in the beginning use another model with zero epsilon B.C. at the wall like Jones and Launder. If you are not satisfied with its results, use the results as initial conditions for another tough model like Lam and Bremhorst. But do not forget to modify the zero value of epsilon at the wall to a non-zero one.

I do not know if you would be successful but you have to try, eh?

Sana

That is a delightfully cynical response. I feel the overwhelming urge to correct one item however.

>there is a fourth solution, that is to try other codes. >they all claim that their codes can handle arbitrary
>geometry and from subsonic to supersonic

Exa's PowerFlow does not claim to handle supersonic flows.

(1). In the web page, it mentioned airflow over airplane surfaces, wings, aerospace applications. Can one fly an airplane like a car at 60 miles per hour? (2).Even the wing of a commercial aircraft was specifically designed for transonic flows many years ago. So, the code is essentially useless for those design problems?

Thank you, Dr. Sana.

>(1). In the web page, it mentioned airflow over airplane >surfaces, wings, aerospace applications. Can one fly an >airplane like a car at 60 miles per hour?

I don't think so, but even if one could, why not just take the car?

The code can go up to about Mach 0.4, and while this is not suitable for an airplane in the air, it is appropriate for takeoff and landing scenarios, which I suppose are relatively important.

>(2).Even the wing of a commercial aircraft was specifically >designed for transonic flows many years ago. So, the code >is essentially useless for those design problems?

yep. until further notice. transonic flows requires non-trivial extension of the current lattice Boltzmann scheme.

(1). I have to say thank you very much to you, because you are providing more information to our readers.

Hi Keith,

1. As noted by Dr. Sana, it is likely a numerical instability combined with the stiff characteristics of the Lam-Bremhorst model that is going astray. The trick is to get the initial values close enough that it will not blow-up. Since your experience is in the laminar world you have probably gotten used to setting an initial zero velocity field (and you don't need TKE and Length scale values) and setting the code loose.....and usually getting it to converge! Does that sound right?

2. What initial values (u,v,w,k,eps) do you start your flow field off with? If you have 8% TKE intensity at the boundary and 0% inside you have a large discontinuity and can lead to instabilities. Do you actually enter the TKE values or set a percentage? If you set a percentage at the start and (u,v,w)=0, then you have TKE=0 so any calculation dividing by k is going to blow-up!

3. Try this:

i) Start off with a laminar flow solution (it does not necessarily have to converge but squeeze the residuals down an order or two and make sure the overall mass and momentum ballances are OK).

ii) Set the TKE and eps values based on this initial. Epsilon should be such to give a turb. length scale of roughly 0.1 of chanel width or some other transverse geometric dimension. Use that initial for the standard Launder and Spalding k-eps. Again converge a bit.

iii) Use that solution as your initial for the Lam-Bremhorst.

iv) Play around with the above and the relaxation factors/time/grid steps. Watch the residuals and note where and how the blow-ups occur. I had a conversation with a really good, pragmatic cfd guy who came in and solved a problem in minutes that had been driving a guy grazy for months!

It was a cyclone, but typical of large recirculation zone problems, where the turb length scale in the main circulating flow is like 2 orders greater than the inlet pipe. The grid had only a few nodes to make this leap, blew-up in like a couple iters! He ups the turb length scale in the inlet up by a factor...really just playing around at that point but with some physical intuition. It goes 10 iters. Lenth scale up an order...more iters. Meanwhile the guy who was stuck in the mud on this one is complaining.."You can't do that!"..as the turb length scale in the inlet pipe is looking unreasonable. Not long after they get it to converge! The moral of the story is that it is just a model and has inherent assumptions and limitations and taking a very sensative and stiff set of equations like RANS turb model equations and jumping them through a couple of orders of magnitude in a few nodes in space is just looking for trouble. Rather, look at the physics of the problem and how this might interact with the numerical difficulties to achieve the most physically reasonable problem specification as possible then evaluate it and try again...looking at blow-up runs over and over gets pretty frustriating. Whether or not his solution was accurate for the problem concerned..I have no idea..but it would be a good starting point for a new grid or problem specification for round 2!

See some of the archived postings for some more ideas:

1) Re: Differential Stress turbulence model and CFX4.2 (2) - Duane Baker, Thu, 15 Apr 1999, 12:03 a.m.

2) Re: Differential Stress turbulence model and CFX4.2 - Response from CFX Technical Services (1) - Simon Assender, Mon, 19 Apr 1999, 8:04 a.m.

3) Re: Differential Stress turbulence model and CFX4.2 - Converged! (1) - Simon Assender, Thu, 29 Apr 1999, 3:24 p.m.

etc.

Note: The archive has a lot of info and is useful to someone who is just getting started to atleast see some of the ideas....and better than real time...the ones that seemed to work!

Regards,

Duane Baker

Hi John,

I like the sound or 3 with a twist: Learn to use the code as well as the vendor people so that (barring a bug as the source of the problem) the cfd user can solve it properly themselves. This is why service is probably the MOST IMPORTANT factor in the commercial CFD game because without it you do not continue to learn and adapt very well.

Regards,

Duane Baker