Powerflow
 

Hy, I recently heard from a friend of a complete new cfd-method. Did you hear of POWERFLOW from Exa inc. ? I looked at their homepage and this seems to be a really new way. They calculate gas-particles ....!!?? What do you think about it ? Sorry, I lost the url but a search engine finds it.

jurek

Re: Powerflow
 

Our company develops and sells a commercial CFD software called PowerFLOW. It is indeed based on a lattice-Boltzmann approach (particle-based method, derivated from kinetic theory). Instead of solving Navier-Stokes equations directly, we simulate the evolution of the particle distribution function. The main interests are: - easy setup and handling of complex geometry (fully automatic cartesian gridding, non body fitted mesh) - unsteady approach - accuracy - parallelization efficiency (up to 64 procs, our code is linear, 98% linear on 128 procs SGI Origin) Lattice methods are seen as promising techniques for CFD (especially for multiphase flows and chemical reactions).

For more informations, please look at our website: www.exa.com or email: info@exa.com

Re: Powerflow
 

My PRIVATE opinion is that this code is full of marketing rubbish:

a) in early days, their sales people have claimed that the code is more fundamental than N-S equations and that no modelling is required. They got slaughtered by the academic community

b) they claimed that no mesh is involved. Rubbish: the mesh is a castelated Cartesian mesh

c) they claim that no turbulence model is involved (but then admit to using wall functions). This is my favourite: I asked questions at the SAE 1999 (after their presentation in an open forum) and found out that the model is the Smagorinsky model (which I also worked out in advance)

e) They claim that the code operates on the "level of molecular interaction", which is another load of rubbish - if you push far enough they'll tell you this is "true but impractical for engineering applications". Ever heard of DNS?

d) in order to obtain the results on efficiency they claimed (at least in the early days), they required SPECIAL processors i.e. you can't just take your workstation and run it!

e) The effective accuracy of the numerics is single precision and it would cost you an absolute fortune to get to double precision.

In summary, what this code does is:

Solve incompressible transient flow in the Large-Eddy-Simulation mode with a zero-equation turbulence model and dubious wall functions. There is a lot of literature on the performance of this mathematical model - if it is appropriate for your purpose, the code might be worth considering. However, it has NO advantages over any other mechanism of solving the same mathematical model and if they tell you differently they are full of it!

Considering the strength of my comments here, maybe I should tell you the following:

- I read the Thesis describing the numerics of Powerflow (which was incidentally extremely difficult go obtain (!?)) - I am an FVM/FEM numerics expert - I know my external aero, LES and turbulence modelling - I've talked to people who use Powerflow and their technical staff on conferences AND seen experimental comparison. - I'll be glad to get into detailed technical discussion about any of the points raised above.

Hrv

Re: Powerflow
 

Dear Dr. Jasak,

Let me give you some partial answers only, since this forum is not supposed to be commercially oriented. Please feel free to contact me directly for a more detailed discussion about lattice-gas methods.

The whole idea of lattice-gas methods is to construct a microscopic description of a fluid that enable to recover the good macroscopic behavior, while being simpler than the true microscopic physics. It can also be seen as a kind of discretized version of the gas kinetic theory. Instead of solving directly the complex and non-linear macroscopic NS equations, lattice-gas methods calculate the temporal evolution of a velocity distribution function (similar to the kinetic theory one). It can mathematically be shown (as it is done in the kinetic theory) that the macroscopic NS equations can be obtained from this distribution function, provided that the microscopic model of the particles interactions is properly chosen.

Originally coming from the NS world, I personaly had some difficulties to clearly understand this concept... Many researchers are developping these lattice-gas methods which are seen as very promising.

Now, some partial answers to your comments (more details on request):

a & c) Yes, we do have models in the code, because the computer limitations does not allow us to use enough resolution to resolve all the length scales: - for walls, we use an extended "law-of-the-wall" type model - for bulk turbulence, the current version has, as you said, an algebraic turbulence model of Smagorinsky type. We are about to release a new version integrating a k-e model. Note that some turbulence people call our software a VLES code (Very Large Eddy Scale), since our turbulence model is used to model the effect of the turbulent structures smaller than our cells.

b) That's a misunderstanding. We should rather say "no complex meshing process"... Our code automatically discretize the space with cubic, space-varying cells, according to the specifications given by the user. This is extremely useful when you're studying complex geometries.

d) The need of a specialized hardware is not true anymore (it concerned the very early version). We do run on Sun, SGI, HP systems and we are going to issue a Compaq version in a couple of months. The NT version will come later this year. As I said, we can demonstrate a very good efficiency of the code on multiprocessors systems (98% linearity on 128 procs on a SGI Origin), due to the simplicity of the basic lattice-gas algorithm.

e) Lattice-gas methods (in general) enable to mimic a fluid. Theoretically, no modelling should be needed if all the length scales are fully resolved. Practically, this is limited by computational performances. However, for low Re flows (we generally say Re<10000), it is possible to run the software in a DNS mode. This has some practical applications in the industry however. If computer performances continue to increase as they are doing right now, we should expend the field of applications of this way of simulating flows. I do not know any other commercial code that has this type of feature right now.

d) You should understand that we do not calculate the "macroscopic" quantities (such as pressure, velocity, density...) directly during the simulation process. We calculate the distributions of particles. These macroscopic quantities are calculated in a post processing step, as moments of the distributions. These distributions are calculated as integers, but due to the fact that we simulate millions of particles per cell, this enable to capture small variations and we do have an accurate solver...

Let me finish with a remark: lattice-gas methods are still under development and are a new way of doing CFD (I don't mean that it is better than solving NS, everybody should judge by himself). These methods have advantages and also drawbacks, but it is also the case with "classical" CFD (else we would have no job any more)...

Regards.

Fred

Re: Powerflow
 

(1). I would say that this is a very good comment from the expert. I would give it a A+. (2). On the other hand, I don't have any problem with the creative sale's approach. (3). So, for the CFD users, I can only say that systematic validation of a code is the only way to a successful solution. ( For example,I had to try several hundred 3-D configurations in the last month to draw the conclusion that this user-friendly code I am using does have a problem in the mesh generation.)

Re: Powerflow
 

>My PRIVATE opinion is that this code is full of marketing >rubbish

actually the code itself is written entirely in C++ and assembly, no rubbish whatsoever, though the marketing literature for may be another matter

>a) in early days, their sales people have claimed that the >code is more fundamental than N-S equations and that no >modelling is required. They got
>slaughtered by the academic community

geez, what do you expect from sales people?? seriously, that was a long time ago and is actually quite embarassing now, and interestingly none of those people work at Exa anymore.

>b) they claimed that no mesh is involved. Rubbish: the mesh >is a castelated Cartesian mesh

i don't know what castelated means, but yes, it is a Cartesian mesh, of cubic cells which the user can vary in size (by factors of 2). complex surfaces are handled via special planar elements which cut through the cubic cells at arbitary position and orientation, thus "stair-stepping" is avoided and the surface resolution corresponds to the local grid resolution.

>c) they claim that no turbulence model is involved (but >then admit to using wall functions). This is my favourite: >I asked questions at the SAE 1999 (after
>their presentation in an open forum) and found out that the >model is the Smagorinsky model (which I also worked out in >advance)

it is true that 5 years ago Exa did not realize that they needed turb modeling. then they figured out that what they were doing actually amounted to a constant eddy viscosity turb model, which corresponded to the Cebicci-Smith model from the 1960's-70's. about 2 years ago a variable eddy-viscosity algebraic model was put in, as you heard at SAE 1999. next release will have a multi-equation turb model, namely, the famous (or infamous?) k-epsilon RNG model. i like to think of it as a maturing process.

>e) They claim that the code operates on the "level of >molecular interaction", which is another load of rubbish - >if you push far enough they'll tell you this
>is "true but impractical for engineering applications". >Ever heard of DNS?

oh. i think those are the same people who are gone now. the correct claim would be that the code operates at the level of the Boltzmann particle distribution function (same as that found in classical kinetic theory).

by the way, the only people who would say that PowerFLOW is impractical for engineering applications must be working for StarCD or Fluent.

>d) in order to obtain the results on efficiency they >claimed (at least in the early days), they required SPECIAL >processors i.e. you can't just take your
>workstation and run it!

ahh the good ol' days. now it runs on SGI, Sun, HP, Compaq Alpha coming soon, and NT soon after.

>e) The effective accuracy of the numerics is single >precision and it would cost you an absolute fortune to get >to double precision.

that was fixed up a few years ago, and now costs you nothing.

>Solve incompressible transient flow in the >Large-Eddy-Simulation mode with a zero-equation turbulence >model and dubious wall functions.

Actually it solves the fully compressible unsteady Navier-Stokes equations. You have a choice between DNS mode for low Re probelms and turb modeling for high Re. If you use enough resolution and an algebraic model you can achieve LES (typically very expensive). When the resolution is coarser, one could think of it as VLES.

By the way the wall functions are no more dubious than others I've seen, IMHO. In fact all turb modeling is rather dubious, but what choice do we have until computers are a lot faster and we can do LES/DNS on routine problems?

>There is a lot of literature on the performance of this >mathematical model - if it is appropriate for your purpose, >the code might be worth considering. However, it has
>NO advantages over any other mechanism of solving the same >mathematical model and if they tell you differently they >are full of it!

That is quite a statement. I humbly submit that you are basing your conclusion on outdated and questionable information. There are significant advantages in ease of use, in fact the gridding process is completely truly automatic. Regarding accuracy, numerical diffusion is essentially non-existent, with a well-defined floor on the lowest viscosity that is achieved. A disadvantage is that for problems with a steady solution the runtime is often longer since the method is inherenty transient and must evolve to steady conditions. Also there is currently a lack of functionality like heat transfer, mass transfer, chemical rxns, and multiphase.

That's the straight dope, take it or leave it. You are entitled to your opinion, but let's at least get the facts straight.

Re: Powerflow
 

Dave,

I like your answer because you sound like the people doing actual work - therefore no overclaims. We still have to remember that whatever method we use in CFD, even with minimal numerical error, the result of CFD still depends on the physical modelling which itself may has great errors in it (turbulence modelling, combustion modelling, multi-phase modelling, just name a few).

Re: Powerflow
 

Hi Guys,

Thank you very much - it is really impressive how much information one can get when talking to experts rather than wasting time with selespeople. I think this is a record - two good technical answers from the people who know what they're talking about in a day, whereas it originally took me more than half a year to get a copy of the Thesis.

Anyway, I hope I didn't insult you too much; at least you got your opportunity to give an informed opinion AND correct any wrong data that I have presented in this Forum. Here's a big thanks to both Fred and Dave - I hope your management appreciates the quality of your effort.

However, let's look at the new data and see what it means:

1) C++: well done guys - you're showing us the good way forward (I am also a C++ programmer trying to spread the Gospel)

2) Sales people: they can go and bullshit their way through the client base at will, I just don't want my life wasted by an accountant with no clue (I'd rather talk to Fred and Dave ;-)

3) Mesh: what you described IS a castelated mesh (with 2-1 embedded refinement). it's completely adequate; the point is that it IS THERE!

4) My data on turbulence modelling comes from MARCH 1999, not 5 years ago. Anyway, this makes PowerFlow more tractable and rather ruins the fun in the Sales Department.

5) Now we've established that we're solving the same mathematical model, I don't need to brood over the numerical mathod, as I can believe it is actually correct. Also, there are problemos out there that really are steady (not many, mind you); for those, the use of an inherently transient code will be impractical!

6) Special computers - Well done on solving the problem. You really needed this one to "grow up".

7) Compressible, incompressible? In my back yard, when you say "compressible", people will soon ask for shocks. I have never seen any shocks done in PowerFlow!

8) Wall functions: are a specification on the MEAN velocity, whereas you've only got the instantenous value. The consequences of mixing the two are well documented and we need not go in any deeper. The fact is: if you want to do wall functions you really need to do RANS!

9) Brilliant - I needed to hear someone opposing me on this! There is an up-side, but there is also a down-side. This is tru for the FVM, FEM and Lattice-Bolzman! I need not argue any longer: both are here for the potential users to see and make their own mind. Thanks for being honest (I expected nothing else!)

> That's the straight dope, take it or leave it!

I take it with pleasure - if you let me get in touch with you once I need to know more I'd be even more grateful. There's nothing to beat a little education.

Hrv

Re: Powerflow
 

Hi Fred,

I just posted a much longer answer below, but I wanted to thank you for the effort. This is a new and different way of doing CFD - it needs development, validation, improvements, just like everything else.

Thanks for the answer - I just got annoyed into starting this because it is almost impossible to get any solid data about the method, modelling and validation from your sales people. I'd be grateful if you could point me to some publicly available documents describing the validation and performance data for the Lattice-Bolzman method on some canonical fluid flow problems, like backward-facing steps or similar. It seems that for Lattice-Bolzman this kind of stuff just isn't there, which in turn means I can't get a decent handle on your results.

Re: Powerflow
 

Dr. Jasak,

Let me add a few things... As you said, lattice-gas methods are new compared to NS, so the work is in progress. We sometimes use the term DFD -Digital Fluid Dynamics- to outline the difference between our method and the solving of NS equations.

We have some technical papers available on our website (www.exa.com). However, you may find them inadequate to answer all your questions since they sometimes are too commercially oriented (well, we have also some physics papers, but I must say that you need a knowledge of lattice-gas and lattice-Boltzmann methods to fully understand them...). I must also admit that I may not be the perfect man to talk to... As an application engineer for Exa, my job is to support our customers in the use of the software and my knowledge is not as deep as Dave's. Moreover, writing papers is a time-consuming job that a small company can not always afford to do the way it should...

Our goal is to develop an industrial tool perfectly integrated into a design process. This is rather ambitious, but we think that lattice-gas methods can remove some practical issues of CFD (mesh generation time, convergence...) for complex problems.

I will be happy to hep you and feel free to contact me by email for more details.

Regards

Re: Powerflow
 

Hy, you seem to be the independent expert for this program. Is it useful for industry (complicated geometry) or an academic tool ? What's the advantage of this method ? jurek

Re: Powerflow
 

(1). I don't keep track of people's name or origin, so, the messages presented here is only related to the previous message posted. (2).I'll have to see the actual code listing to make sure that it is actually written in C++. (3).I think, sale and marketing field is very interesting field. I had said last year here that whether the product is good or bad itself is not important, it is very important to know how to provide the needed service to your customers. A good sales person should be able to sell almost anything to his customers. (4).Regardless of how one look at the mesh, one can always stretch it out into a rectangular mesh. Actually, when using coordinate transformation approach, one is solving the equations in the transformed rectangular mesh. The actually mesh can be 1x1 unit each. You don't worry about the mesh at all. (5). The rate of change of the world is very fast. Whether it is last March or five years ago, for me it is long time ago. Five years ago, I was still using the PC/486/33. Last March, the PC had already gone through two generations of upgrade, even though the monitor and the keyboard were still old ones. Now in December, I have a 17" high resolution 0.25mm monitor and upgraded motherboard, HD, video card/TV, and AMD/k6-2/400 CPU. The used monitor costs only 150 dollars, and the new CPU was around 50 dollars. See, the world is changing at a very fast rate. (6). CFD simulation is human activity. We can simplify the equations or we can make it more complicated. We still learn from books about zero-D properties, steady-state 1-D solutions, steady-state potential flows, steady-state inviscid equations, etc... CFD simulation is flexible. And there is no particular need to find the exact transient real world solutions, if 1-D steady state solution will provide needed answer. (7). The computer hardware is really the driving force behind all these "computational ..." fields. No one is developing a computer just for CFD alone. When they are developing vector computer, CFD is vectorized. Wehn they are developing parallel computer, CFD is parallelized. It looks like that CFD has no backbones at all. (8). From my background, I use Reynolds number, and Mach number. Compressible or not compressible is not official words. By the way, MacCormack's famous 2-step explicit method was invented in his paper on hypersonic impact of particle on solid material.(I hope I remembered it right) Is solid compressible or incompressible material? (9). The wall function concept is something like the classical singular perturbation approach. As long as there is a common valid region of solution, one can always bring two families of solutions together. Anyone can invent his own version of the wall function. (10).Internet CFD is something like electronic flea market, you really can't trust anything. But I think it is one way to stimulate ones thinking. And it will have positive impact on ones health. The brain will produce many chemicals to affect the body, including the effect of high bolld pressure. (11). I think, a person can not be changed after say 18 years old. A country also can not be changed. The only way to change it is to put people in jail (for any reasons). And if you look around the world, that is what many governments are doing to their people. (12). Beauty is in the eyes of the beholder. And the uncertainty principle simply says that the picture will get fuzzier when one try to get closer. So, to enjoy the beauty of Mona Lisa painting, one really have to stand at least 20 feet away. (13). The core of the world is very fuzzy, it must be very difficult for people to live in this ever changing world. (if you decide to change the information in your brain, you may have difficulty to recognize your family members.) So, leave it alone if you can't change it.

Re: Powerflow
 

Wow, this is fun, I had no idea such a forum existed until Fred mentioned it in an email yesterday.

Thank you for the kind reply. Your (9) points above are very good, just a couple more comments:

3) absolutely, and i did not know the word "castelated" but i like it !

5) it can be somewhat impractical in terms of runtime, but sometimes the easier gridding could make it worthwhile anyhow. how this balance plays out seems to depend not just on the problem itself but also on the entire integrated engineering process of the end-users. (if management sees this i'll be headed over to the CFD online jobs area).

7) yeah you're right, PowerFlow cannot yet do flows above Mach ~0.4, so it's usually just a technicality that the recovered hydrodynamic equations are the compressible form rather than the incompressible form.

8) interesting. i'd be grateful for a reference. so actually in PowerFlow the "wall function" is a specification on the local instantaneous surface fluxes, which is consistent with the dynamics of the fluid. some amount of tangential momentum is removed, according to an extended law-of-the-wall model. this model contains some parameters whose values are, not surprisingly, quite empirical. ahhh the joys of turbulence modeling.

you are very welcome to get in touch anytime. also there is some good stuff at www.exa.com, skip the company b.s. and head straight for the validation examples and available published papers.

Re: Powerflow
 

Dave, Hy, et. al, If you take a look at some of the company history, which has accomplished a considerable amount in the short time since it's founding, you will find that there was a transonic version of the code developed with our then partners at General Atomics. This is "fluid-only" 5 speed version and from a business perspective still does not make sense to complete the product and market it to the community that could use it.

Additionally, after having read the latest slew of messages in this forum and mis-information, it's obvious there is no "independent expert" here. We are happy to send "technical info" to anyone who requests it. Try sending a letter to info@exa.com.

Re: Powerflow
 

(1). In a way, I think you are right. There is no "independent expert" on the Internet forum. (2).The forum is open to everyone, just like a flea market, a real time flea market. (3). On the other hand, if one can not satisfy even the non-experts, then it is going to be very hard to survive in the professional meeting places. (3). Progress can be made by hard working people. And I think, the readers posting messages have just one goal, that is to promote CFD and keep the forum alive. It is hard for the readers to address the capability of a code, unless there is a free demo version available for evaluation.

Re: Powerflow
 

You can say what you like - I still claim that I am independent (nobody paid me to learn this stuff and it's no skin off my back whether EXA becomes a #1 CFD code on the planet or goes out of business altogether) and expert (because I really put the effort in to filter the rubbish your seles department is putting about)!

The fact is: you do not WANT anyone to know what you're doing and how you're doing it - that explains the lack of scientific data, bench-mark test cases and any details whatsoever because for your marketing policy this would be disastrous.

Having that in mind (and also the fact that I really enjoy eating EXA sales people for breakfast), I am still open to provide comments to anyone who is prepared to listen.

Re: Powerflow
 

I've followed this thread with great interest. I have to say that I don't fully agree with the critisism that Hrvoje and others have presented. Sales people are always sales people, you can't expect them to have good answers to all your technical questions - I've got equally stupid answers from many sales people from other more established CFD companies.

I've also read Chris Teixeiras thesis and I don't have a problem with the basic foundations of this method - a Lattice-Boltzman method can in the limit reproduce Navier-Stokes. There are some inherently very nice properties of these methods - easy to parallelise, can make efficient use of the fast integer computations in modern CPUs, stability, ... Looking past the marketing hype that Exa and most other codes have - what, more specifically, in Chris' thesis or the papers published by Exa people, is it that you don't agree with?

I have to agree though that their published validations are a bit lacking, since this is a quite new approach I'd really like to see a lot validations etc. And where are the basic papers in JFM, JCP, PoF, ... ? You can't get a new method established in research related fields without any "heavy" papers in the "heavy journals" - conference contributions or applied journals is not enough.

Re: Powerflow
 

(1). Many years ago, a friend of mine told a story about how a degree awarded to a graduate student got suspended when the professor later found a bug in his student's thesis. (2). In recent years, I have been observing real cases that products designed using some CFD codes eventually failed in the test. These are large companies. The consequences of these failure are not going away soon. (3). So, for the benefit of all parties, it would be desirable that standard test cases results be made available to the public. Test cases commonly used are: flow over a cylinder, flow over a backward facing step, flow in a square cavity with a moving wall. In this way, the readers will be able to know the performance of the code.

Re: Powerflow
 

>The fact is: you do not WANT anyone to know what you're >doing and how you're doing it - that explains the lack of >scientific data, bench-mark test cases and any details >whatsoever because for your marketing policy this would be >disastrous.

Wow, I am disappointed that you have reverted to this opinion after I provided you with clear, honest, updated info on all of the problematic issues you mentioned. I have invited you and the rest of the interested community to obtain more of the "straight dope" , as much as you have patience for, because I most certainly do want people to know how things are done in PowerFlow. I guess my two previous messages cannot immediately undo what seems to be a long history of frustration and misinformation.

I am also disappointed that you have not yet been to exa.com and taken a look at the papers there and the references listed within those, which collectively contain abundant scientific data, bench-mark test cases, and a great many relevant details. The lid-driven cavity by Chris Teixeira is an especially good fundamental/DNS study and is available for download. So are the two papers on incorporating turbulence modeling into lattice Boltzmann, containing algorithmic details as well as several benchmark case studies (backstep, u-bend, and some more complex geometries).

If you really are going to be so bold as to claim to be the independent expert, I hope you will be responsible enough to keep on top of the current information such as readily available published literature. [You may find this material is not as easy to "eat for breakfast" as sales talk :) ]

Re: Powerflow
 

Hi Dave,

Thanks, you really made me go to the Exa site and read the papers. Now what I found is really disappointing even for the people as notorious as Exa! I'll use some qoute from the paper: Texeira, C.M.: Incorporating turbulence models into the lattice-Boltzmann method, 1998 , available from the web-site

Lattice gas method, huh? WHAT A LOAD OF RUBBISH!!! And I qoute:

"... Previously it has been suggested that the k-e equations be solved within the LB structure by creating two additional populations, with components in the same directions as the particle distribution so that these new polulations solve the turbulence equations with their "macroscopic" behaviour. Here we take an laternative approach."

Yes, the above description is the consistent way of doing scalar transport in the LB structure, but the cost spirals out of control, so you can't do it like that.

A bit later it says:

... "To solve the turbulence equations" .... "THIS EQUATION IS THEN SOLVED USING AN ADVECTION SCHEME FOR THE SCALAR A WHICH IS EFFECTIVELY A LAX-WENDROFF-LIKE FINITE DISCRETISATION"

You mean, you solve the k-e system with FINITE DIFFERENCES????????? LB-structure????? Efficiensies above other discretisation techniques? exact conservation? Boundedness?

Liar, liar, pants on fire! You have been found out: all PowerFlow and EXA are trying to do is to con the customer base! Go back and hide under your stone and don't come out for a loooooong while, 'cause you'll get slaughtered - the next time I run across an EXA employee in public I'll call him a liar.

Congratulations dr. Texeira - you just discovered finite difference technique AND wasted a huge amount of everybody's LIFE!

Oh, by the way, your near-wall treatment is completely wrong - time to buy a book on turbulence modelling.

Hrv

P.S. And don't waste my life again!

Re: Powerflow
 

You make a very good point about the importance of published validations. Let me mention where things stand now, and ask your opinion on how to improve.

There is a decent body of literature from the last 13 years on the theoretical fundamentals and certain basic validation studies of the lattice gas & lattice Boltzmann methods. The studies include DNS of lid-driven cavity, backward facing step, circular cylinder, decaying turbulent shear layer, decaying isotropic turbulence, and 3D turbulent channel flow. Many of these appear in the journals you mention, as well as Phys. Rev. E, IJMPC, Phys. Rev. Lett., Europhys. Lett., J. Stat. Phys., and others. Naturally there has been considerable evolution of the method during this time. A recent non-Exa-related review is Chen & Doolen, Annu. Rev. Fluid Mech., 30:329-64, 1998. Here one can find reference to all of the above plus a discussion of extensions to DNS of multiphase/multicomponent flow.

However, certain additional developments done by Exa that are essential for a commercial CFD tool are not adequately dealt with in that review. The most important of these are: 1) how to efficiently handle arbitrary surface geometry without stairstepping, 2) the incorporation of turbulence models for high Re flows, and 3) the inclusion of thermal evolution. The first two are published along with a number of high Re validation studies: backstep, u-bend, various commercial HVAC duct geometries, various commercial car geometries, and more; the papers (or in some cases just the references) are available at exa.com (go to Online Access and go to the bottom for Papers). Regarding #3, a publication is in press, and this is not actually in the product yet (next release).

Re: Powerflow
 

Dr. Jasak,

I will overlook the highly offensive and childish nature of your last message in order to address pertinent technical issues that may be of interest to readers of this forum.

1) Exa has recently (last 1-2 years) been working on a method consisting of lattice Boltzmann (LB) with a k-epsilon turbulence model. In other words, the (transient) mass, momentum, and energy (MME) transport equations of the fluid are achieved using LB, while the local dynamic viscosity is adjusted to reflect the presence of an eddy viscosity contribution, as determined by a multi-equation model of the k-epsilon variety. As reported in Chris' paper, transport (in time and space) of the scalar equations for k and epsilon is accomplished via a Lax-Wendroff-like finite-difference scheme on the same grid used for the underlying LB. So far this appears overall to be an improvement over the Smagorinsky-type algebraic turbulence model currently used in PowerFlow.

I feel obliged to mention that in my opinion, this novel and compelling effort, pioneered by Dr. Teixeira, is most undeserving of your ridicule. Furthermore, it cannot possibly consitute the basis for lies or misinformation about the nature of the method, even with regard to long past sales/marketing material, because it does not even exist yet in Exa's released product code. I also note that you failed to mention to the audience the favorable results of the validation studies presented in the papers by Dr. Teixeira and his colleagues.

2) "Efficiensies above other discretisation techniques": I assume this is a reference to considerations of grid construction, which I hear can occupy a significant portion of a CFD user's time and resources for complex geometry cases using traditional CFD methods. The incorporation of k-eps turb modeling has no effect whatsoever on the gridding process in PowerFlow, which will still be totally automatic with no user involvment (the user does get to specify the choice of grid resolution in various spatial regions, as part of case setup).

3) "Exact conservation": I assume you refer to the exact conservation of MME for the underlying LB fluid algorithm. This is in no way altered or compromised by the use of a k-eps turb model.

4) "Boundedness": I assume you refer to algorithm stability. This is a very interesting and deep issue, but I will try to be brief. The underlying LB method found in PowerFlow is highly stable and robust within a range of operating parameters, most notably sim Mach# and lattice viscosity (i.e. in native units). There is some theoretical work that provides some insights into this, and a great deal of empirical evidence. The code does not allow the simulation to run outside of the known stability envelope, and PowerFlow users have never experienced instability, with the exception of cases where the simulation Mach# became too large due to inappropriate boundary conditions.

Exa recognizes that the introduction of separate but coupled dynamical equations, for k and epsilon, introduces an additional potential source of algorithmic instability. However, due to the regular cubic grid, the time-explicit scheme with step size below the CFL limit, and the fact that the hydrodynamic (MME) equations are not being solved as PDE's, it seems reasonable to believe that there will be no significant compromise of stability. While there are no gaurantees, this has turned out to be true on every case that has been tried so far, including but not limited to the ones presented in the literature.

5) Regarding the near-wall treatment in PowerFlow, I am genuinely curious as to the nature of your objection. Can you articulate why you believe it is problematic? However, if you cannot be polite and respectful in your response, please do not bother.

P.S. Regarding matters of personal integrity, you have claimed to be independent and objective. I wonder, is it possible that your comments are motivated by some undisclosed agenda, such as an association with one of Exa's competitors?

Re: Powerflow
 

(1). I didn't know when I started reading the fine print on the canned food, on such information as the salt, sugar, fat, ...etc... (2). Most of the time, after I have read the label, I put it back on the shelf. I told myself, it is not good for my health. (3). I think, as a professional working in the CFD field, I deal mainly with numbers (most of the time in graphic forms). (4). I think, it is also true with other researchers and engineers in the CFD field. (5). The point I am trying to make is, people in this field is constantly checking the accuracy of the solutions. (6). The accuracy of the solutions naturally come from the codes and the methods used. So, the methods or codes become equivalent to the accuracy of the solutions. And people are serious about it. (7). For example, one percent in efficiency or loss can be written as 0.01. On the surface, it is small. But on the other hand, it can also be a very large number. (8). So, if the salt contents on the label is printed "very small", it is difficult to know whether it is 200 mg or 20 mg, because the product is normally measured in 8 ounces and more. 200 mg can be a small number relative to the weight of the product, but it is way too much for some buyers. (9). So, the point the company failed to recognize is that, during the first several months of promotion, it is all right to say that their products are the world best. But after that honey moon period, the company will have to speak in plain language used by the professional CFD researchers and engineers. (10). As I have said before, it is impossible to change a person. But, I also think that , it shouldn't be difficult at all to present the information on the web site, in the forum in a more accurate way, and more user-friendly way consistent with the culture of the CFD circle. (11). Basically, I get the feeling that, the company tried very hard to be outstanding and unique in image, but at the same time trying to come up with new ideas. (By the way, I don't know whether I should give it a C-. A C++ is probably acceptable.) (12). You don't try to say to the potential users or friends that you think you are right and you are the best. The customer is always "?". It is not real to most people, but it is always true.

Re: Powerflow
 

You mentioned the automatic mesh generation.

Exa like any other automatic mesh generator needs a very smooth surface description.

Creating this normally takes most of the time to create a mesh using one of the automatic meshing tools.

There is about no advantage of using Powerflow-Meshing compared to let's say ICEM Tetra.

So cleaning a real car geometry might take a week or more using ANSA or some other tool. This includes manual work for closing gaps ...

It is really funny to see what all the vendors call "fully automatic meshing".

Re: Powerflow
 

(1). You are right! There is no "automatic mesh generation". (2). Before, when I was using a commercial code, the 3-D automatic mesh generation always failed near the end of the process, leaving a few un-meshed. (unable to finish the volume meshing, using the available surface mesh) (3). It was very frustrated to go back to the geometry, and try to either model the geometry or the mesh in a different way. (4). Now I am checking this commercial code with template to get the mesh started. On the surface, it is an advanced concept. But, when I started using it, it divided the flow field automatically into 24 blocks in the template I had selected. (5). Now, to get a smooth grid becomes almost impossible. I had to spend 30 to 50 rounds of configuration changes to get the mesh into the right place with the right stretching. The final resultant mesh is far from smooth. (6). I didn't have this kind of problem when I was writing my own codes. (7). I think, the automatic mesh generation becomes possible only when the person writing the code is familiar with the solution and the geometry of the problem he is trying to solve. (8). If the geometry is not automatic, and the solution is unknown, it is a good idea not to use "automatic mesh generation", because sooner or later people will start using "automatic CAD design". (9). Design is "iterative", so, geometry is "iterative", and the analysis is "iterative. Therefore, the mesh also is "iterative". The mesh has to be changed based on the solution of the problem. (the mesh includes the boundary mesh and the volume mesh)

Re: Powerflow
 

Yes, I understand it can take some effort to provide a smooth, clean surface geometry. It would be nice to have a way to make this less painful.

It also takes some effort to turn the great car design in your head into an accurately fashioned piece of clay or wood. Does this reduce the value of a well-designed wind tunnel that requires no additional fiddling around to get your experiment underway?

Once the appropriate surface description is available, with PowerFlow there are no further "meshing" issues, such as making difficult decisions regarding trade-offs between choice of mesh type, numerical diffusion/error, and chance for convergence. From what I have read on CFD-online, these can also be a cumbersome part of the CFD process.

I would also like to point out that it is not wise to run a simulation with a sloppy geometry. How can you possibly expect to get a good result using a poor representation of the true physical surface? Flow past a smooth cylinder does not have the same behavior as flow past a 20-sided polygon with a few random holes drilled into it. Certainly you would expect to have to take care to provide a good geometry if you were doing a real physical experiment.

Re: Powerflow
 

It seems to me you are saying the following:

1) There is Method A and Method B.

2) I have tried Method A and it does not work.

3) Therefore, even though it is completely different and I have never tried it, Method B must not work either.

Caveat: the fact that you must choose the local resolution means it is still fundamentally an iterative process, because how do you know you made a good choice until you look at the solution? Maybe you cannot even afford a good choice. Nevertheless this is qualitatively different from:

1) a meshing process that "fails" before you have even started the simulation

2) a simulation that never achieves "convergence"

3) a simulation that requires enormous artificial (numerical) dissipation to achieve convergence

Re: Powerflow
 

(1). I am somewhat tired of this strange behavior of CFD forum, CFD codes, etc... (2). So, I will be spending my time more wisely in reading books in the future. (2). As I said before, CFD is not a code. And no one will say that fluid dynamics is a wind tunnel also. That is why companies using a code to do CFD are all having problems. Car companies have wind tunnels, have they solved fluid dynamics problems? Most had problems long before using a code, so, it is not hard to understand why. (3). So, even if one fills the NASA's wind tunnel test sections with cars, I don't think the efficiency will improve when the car comes out of the wind tunnel test section. (4). Over the years, most results from CFD codes were not good enough, and most people would say it was because the turbulence models were not accurate. Such conversation and exercise is ideal for the research institutions. (5). So, you can all talk about the codes, and at the same time, I will be doing more reading, about the 3-D computer graphics and computer games. It is better than talking to a wind tunnel. (if you think a wind tunnel can solve your fluid dynamics problems, then you must be out of your mind. See, CFD is about the mind activities, not about a wind tunnel or a code. )

Re: Powerflow
 

Well stated Dave. In addition, it is important to have a broader vision of the arena in which CFD and CAD/CAE is being applied. If it were just a ping pong match between academics there would be no application to the real world and those of us with the AE and ME degrees in fluids would be driving around broke in our K-cars, gremlins, and pintos or looking for financial aid for our next degree.

So we must look at the entire process from an engineering perspective when developing CFD tools. In terms of CAD, we have progressed from line models, to surface models, to the state of the art solid models. In terms of compute resources we have increasingly faster chip speeds, parallel processors, etc. In terms of CFD, we had panel methods, steady state solutions, and cartesian grids. Now we have body fitted grids, multi-equation turbulence models, and parallel, transient, time-accurate solvers. All three disciplines are being driven by the end-user community with a common goal of predicting reality a-priori through design, engineering and analysis.

So a CFD code that can automatically discretize ANY CAD model and simulation volume that is representing reality accurately is simply one step ahead of where CAD is today in its ability to give the CFD community a discretized surface. In other words, it won't be long before the CAD community will provide us with clean geometry, all the time, so why not have the CFD process in place when it arrives as we do now.

At the same time, I'm sure the CAD community continues to cringe every time we ask for a chunkified (facetized) version of their nice smooth cubic spline surfaces.

Perhaps a goal would be for the CFD codes to interpret the CAD geometry directly from the smooth surfaces of solid. Will we have "arrived" in terms of automatic meshing? Now are we CAD people or CFD people, or both?

Re: Powerflow
 

Dear David,

I shall try to offer a polite answer to the person asking a polite question:

The "law of the wall", which is the basis of the wall function treatment prescribes the level of the MEAN wall shear stress for a turbulent attached boundary layer as a function of the MEAN velocity:

Tau_w^bar = f(log(U^bar))

In Powerflow, just as in LES simulations (see references I have provided by E-mail to one of your co-workers), we could only apply wall functions if we have the U^bar available (this needs time or ensemble averaging during the calculation!). What Powerflow does is:

Tau_w = f(log(U)) instantenous!

As log(U^bar) is NOT the same as (log(U))^bar, this treatment will recover the WRONG mean drag, just like the LES equivalent.

Now, for the dirty bits: (please feel free to stop reading here)

1) What Exa sells is not a Lattice-Boltzmann CFD solver 2) All operations in the solver are NOT integer-based 3) Numerical method used on decoupled equations is antiquated (only used in undergraduate numerics courses!). However I do realize the need to decouple the turbulence from the pressure-velocity solver; for un-initiated, the only real problem is COST OF COMPUTATION, which is curiously absent from any published material. 4) The method requires a turbulence model; I wonder how you'll implement a decent one, which doesn't just vary the effective viscosity(!) 5) The turbulence (k-epsilon) equations are not satisfied to the criterion you claim (i.e. exactly)! 6) Natural bounds on k and epsilon (e.g. k>0) are not present in the numerical solution, thus further reducing the accuracy of the numerics 7) Mach = 0.4 is in reality an incompressible flow. It is a bit rich to advertise a "compressible flow solver" with a limitation of Ma < 0.4!

I also appreciate the "meshing" comments other users have mentioned below - it is nice to hear that Exa is not immune to the "real world" CFD problems.

Finally, I am grateful to you for the statement on finite difference discretisation, as dr. Texeira goes to considerable trouble to exclude this statement from his publication and tries to hide it in academic slang, which I personally consider an insult to my inteligence.

Happy New Year,

Hrvoje Jasak