CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   Explicit vs Implicit time-stepping (http://www.cfd-online.com/Forums/main/91864-explicit-vs-implicit-time-stepping.html)

Amdi August 24, 2011 23:01

Explicit vs Implicit time-stepping
 
I wonder which is better, explicit or implicit time-steppings. Maybe, it depends on the purpose: steady problems, unsteady problems, stiff equations, parallel computations? Anyone has ideas or opinions or references? Thanks.

Amdi

cfdnewbie August 25, 2011 06:42

oh, long discussion... explicit vs implicit, which is better?
Totally depends on what you want to compute.... some random thoughts:

implicit:
+ steady state ..
+ if you are not interested in the fastest wave speeds of your prob, or if the dominating physical effect takes place on large timescales
+ incompressible flow
- no pre-conditioner, no gain in speed compared to explicit....pre-conditioning is an art in itself, there are many many combinations of implicit solution methods + pre-cons.... kinda a black art to me.... seems to be a lot of experience and guess work....
- memory requirement can seriously limit your computation
- (my opinion:) less intuitive, harder to program and debug
- harder if not impossible to parallelize well (and get good scaling!)

explicit:
- sucks at steady state
- computation can be bogged down by fastest wave speed
+ very easy to set up
+ often (e.g. turbulence) fastest wave speeds are of importance, so the smallest timescales must be resolved anyway
+ parallelization very easy, almost perfect scaling possible


My conclusion: Totally depends on what you want to do!!

Amdi August 25, 2011 10:34

Dear cfdnewbie

Thanks for your insightful comments!

Just one more question.
Why is it difficult to parallelize implicit schemes and get good scaling?
Each linear solve iteration is like an explicit scheme which scales perfectly, no?

Amdi

cfdnewbie August 25, 2011 10:45

Implicit schemes always require the setup of the system matrix in each step (at least for a non-linear problem), so you have to build and manipulate the matrix in memory....this matrix can become huge, as it scales with DOF ^d, with d = dimension of your problem (2d, 3d)....

so to invert this matrix, you need a) a huge amount of memory b) distribute this matrix somehow over your procs c) communicate a lot between procs (to find the inverse)
This communication is what generally slows down your code, and makes good scaling difficult. I'm no expert on implicit methods, though, maybe there are clever tricks to circumvent this and make the scaling acceptable. I prefer explicit methods, because the problems I am interested in need them anyway..

Amdi August 25, 2011 16:11

It's interesting that it takes a lot more effort to solve a linear system in parallel.
Thanks!
Amdi

cfdnewbie August 25, 2011 16:21

Keep also in mind that implicit schemes have a much higher memory requirement due to the matrix... I know that all people doing implicit stuff always complain that the memory requirement is what kills them when they are trying to get their code to perform on hpc machines...

Again, i am no expert on implicit schemes, i prefer explicit ones, so maybe somebody with more experience can give you an other opinion!

julien.decharentenay August 25, 2011 19:31

Hi Amid/cfdnewbie,

I agree with most comments from cfdnewbie but would like to add a few more.

There are more than one way to do implicit time-stepping:
- iterative solver (conjuguate gradient and the like) can be used to keep memory down and they scale reasonably well in parallel - also quite good for sparse matrix (which most CFD solver require);
- simple/piso like algorithm where the implicit equation are solved in a segregated manner (ie solver u-velocity, v-velocity, w-velocity as distinct equation). This approach again limit memory use as the system is not NxN -where N is the number of cells - in place of (nxN)x(nxN) - where n is the number of equations;
- compressible flows can be treated implicitly - as long as the flow physics you are interested allows for implicit treatment (i.e interaction of a pressure wave with a turbulent field would likely require an explicit algorithm);

cfdnewbie would need to refine his comments on pre-conditioning as it can refer to either pre-conditioning of the equation to reduce the stiffness of the system to solve (physic based such introduction of an artificial compressibility) or pre-conditioning of the system to solve (incomplete LU decomposition as a preconditioned to conjuguate gradient for example).

It is a very wide question and subject. And you need to keep in mind that an appropriate solution for the automotive industry may not be appropriate for the aerospace industry - get the right tool for the job.

Kind regards,
Julien

cfdnewbie August 26, 2011 04:20

Hi Julien,
thank you very much for your insightful comments!

Quote:

Originally Posted by julien.decharentenay (Post 321666)
Hi Amid/cfdnewbie,

I agree with most comments from cfdnewbie but would like to add a few more.

There are more than one way to do implicit time-stepping:
- iterative solver (conjuguate gradient and the like) can be used to keep memory down and they scale reasonably well in parallel - also quite good for sparse matrix (which most CFD solver require);

Could you give a rough idea of the scaling percentage? Strong and weak maybe? Just a rough figure would be nice, I would like to get a feeling for what an implicit solver could do.....
Another question: Is there a clever way to use the sparse matrix to your advantage? I know that people store just the non-zero matrix entries plus their matrix indices, but this mapping is pretty timeconsuming, right?

Quote:

- simple/piso like algorithm where the implicit equation are solved in a segregated manner (ie solver u-velocity, v-velocity, w-velocity as distinct equation). This approach again limit memory use as the system is not NxN -where N is the number of cells - in place of (nxN)x(nxN) - where n is the number of equations;
so you just build the matrix for each variable at a time and solve it? Is that how it is done?

Quote:

- compressible flows can be treated implicitly - as long as the flow physics you are interested allows for implicit treatment (i.e interaction of a pressure wave with a turbulent field would likely require an explicit algorithm);
have you a reference for a turbulent compressible flow treated implicitly? I has seen some weakly compressible implicit stuff, but not yet full compressible implicit solution - at least none which seemed efficient to me...

However, one should forget the mixed approach: treating terms in your equation according to their physics either explicitly or implicitly...RKIMEX and such... that seems to be pretty interesting, but I haven't looked into it yet.

Quote:

cfdnewbie would need to refine his comments on pre-conditioning as it can refer to either pre-conditioning of the equation to reduce the stiffness of the system to solve (physic based such introduction of an artificial compressibility) or pre-conditioning of the system to solve (incomplete LU decomposition as a preconditioned to conjuguate gradient for example).
I was talking about the last one, making your matrix more diagonal, so to speak. Isn't it true that the right (or wrong) combination of solver and preconditioner can make a huge difference in speed? A friend of mine did his PhD on some of this, and always complained that choosing with P to take was a pain in the neck....it seemd pretty arcane to me...

Quote:

It is a very wide question and subject. And you need to keep in mind that an appropriate solution for the automotive industry may not be appropriate for the aerospace industry - get the right tool for the job.
Also true....and maybe I mislead the guy who asked the questions...I was talking from a compressible turbulence researchers perspective, which may be totally different from what sbd would need to get a job done in an automotive setting....

It's not a question which one is better - in general. Each has its uses and disadvantages, but it's good to be aware of them....


Cheers (explicitly ;) )
Cfd newdbie

julien.decharentenay August 26, 2011 07:09

I will do my best to answer your question.

Quote:

Originally Posted by cfdnewbie (Post 321705)
Could you give a rough idea of the scaling percentage? Strong and weak maybe? Just a rough figure would be nice, I would like to get a feeling for what an implicit solver could do.....
Another question: Is there a clever way to use the sparse matrix to your advantage? I know that people store just the non-zero matrix entries plus their matrix indices, but this mapping is pretty timeconsuming, right?

Scaling is case dependent (ie running a 100,000 cells on more than 2-3 processors is not going to scale very well). I would think that the scaling is not as good as an explicit scheme - but it would depend on the coder/system/compiler and the like.

There are clever ways to store a sparse matrix, and even ways not to store the matrix (if you are willing to pay the price of not using a pre-conditioner). An example: if you know that your matrix is tri-diagonal, you can just store 3 arrays (one for the diagonal element and one for the upper and lower diagonal). It would still require a larger memory than explicit.

Quote:

Originally Posted by cfdnewbie (Post 321705)
so you just build the matrix for each variable at a time and solve it? Is that how it is done?

Yes.

Quote:

Originally Posted by cfdnewbie (Post 321705)
have you a reference for a turbulent compressible flow treated implicitly? I has seen some weakly compressible implicit stuff, but not yet full compressible implicit solution - at least none which seemed efficient to me...

However, one should forget the mixed approach: treating terms in your equation according to their physics either explicitly or implicitly...RKIMEX and such... that seems to be pretty interesting, but I haven't looked into it yet.

A very good turbulent compressible flow solver (to the book): nope I have not seen one. But there are quite a few commercial ones - I am under the impression that CFX is a density based solver.

I am afraid that I am more from the industry than the academia - did my phd 10 years ago and moved away from research. I am not too good on papers. But I can still do some mean coding and have a decent memory.

Quote:

Originally Posted by cfdnewbie (Post 321705)
I was talking about the last one, making your matrix more diagonal, so to speak. Isn't it true that the right (or wrong) combination of solver and preconditioner can make a huge difference in speed? A friend of mine did his PhD on some of this, and always complained that choosing with P to take was a pain in the neck....it seemd pretty arcane to me...

I would agree with your comment. My PhD was on low speed turbulent combustion and the assessment of density based versus pressure based solver. For the application, the pressure based solver was a lot faster.

Quote:

Originally Posted by cfdnewbie (Post 321705)
Also true....and maybe I mislead the guy who asked the questions...I was talking from a compressible turbulence researchers perspective, which may be totally different from what sbd would need to get a job done in an automotive setting....

It's not a question which one is better - in general. Each has its uses and disadvantages, but it's good to be aware of them....

Agree with it.

Another note (from the industry). A large amount of time is spent on the understanding the problem, pre, post-processing and reporting. Sometimes it can actually exceeds the solver time -- I am not doing LES...

Good luck with it.

Kind regards,
Julien

RanaP August 26, 2011 09:33

You could also try to use a specialized version of Lapack for inverting your huge array, also you will need to be able to reorder your mesh numbering (for unstructured grids) for limiting the bandwidth of your array. Using a structured grid will give you an already well arranged bandwidth array.

An alternative to a pure implicit solver will be to use the psudo-implicit method of A Jameson, in which you start with an impliciti temporal discretization but, at each time step you will actually use an explicit solver for a slightly modified version of your discretized equation. This is the approach used in a commercial solver like Fluent for example. If you need an exact reference I will find the title of the article in which Jameson presents his method.

cfdnewbie August 26, 2011 13:28

thanks Julien for your insightful comments!

Amdi August 29, 2011 17:57

cfdnewbie, Julien, RanaP,
I thank you all for very insightful comments.

I think I have a better understanding of time-stepping schemes now.

Amdi


All times are GMT -4. The time now is 17:57.