Iam running an arterial tree model using LES. I went through the manual for LES settings and he talks about using Crank-Nicholson scheme and MARS with a blending factor of 1 for the momentum equations.Also he says that averaging should begin after the flow has completely developed

But the solution is very unstable and fails to converge, can someone please suggest how to go about this.

what is your courant number and y+?

I have run a turbulent high reynolds number k omega model on it and the courant number is less than 0.5, i was not sure if checking y+ in LES model is necessary but since my input velocity wave form is pulsatile (it varies from 0 to 1)the y+ranges from about 20 to 50 , but i again my flow is turbulanet at peak velocities so i would assume that my y+ is alright

I would have thought your Y+ is way too big (although I may be wrong), it is usually used with a low reynolds mesh. Also check your integral time and length scales with k-e and make sure they are right.

Inthe manual is he says that your y+ should be between 30 and 100 for high reynolds number models and for low it could be from 0.1 to 100 so i thought at least at my peak velocity i was good enough.

Also i was not sure how to check the integral length and time scale. Thank you for your time

So many questions! First, I take it you want to run DES and not LES? The blending function (which is for DES) changes the discretisation on the momentum equation depending on how it thinks the DES model is behaving: ie MARS where it's behaving like a RANS model and CD where LES. If you actually want to run LES, you should use CD only. Using an upwinded scheme like MARS introduces numerical dissipation which is handy for RANS, but not good for LES because it dissipates out the turbulence you are trying to resolve.

Next, how are you defining convergence? Is it doing lots of PISO correctors on each time step? Are you getting unphysically high velocities, if so where, what are the cells like? Given that you are changing the inflow conditions (and it's a transient calculation), why do you expect it to 'converge'?

Given that you are pulsing the flow, why do you want to get the average values anyway?

If you're actually running LES, a y+ of 20 to 50 is way too large, should be more like 1. With LES you are trying to resolve (and not model) all the turbulent features, which means you need very high resolution next to walls (where you have a lot of very small scale turbulence). Also note, that resolution needs to be in all three directions, ie you need a low u+ and w+ too.

How to fix it? Difficult to say without knowning what's going wrong. Things to think about are: how good is my mesh? Both CrankNicholson and CD are not the most stable schemes in the world, so you need a very good mesh (lots of good hex cells).

If you have a non-optimal mesh, think about switching to STAR-CCM+ or STAR-CD V4, both of which have SIMPLE transient which is more forgiving than PISO, and V4 has a different higher order temporal discretisation scheme which is also more stable than cranknicholson.

The high and low reynolds number models apply to how RANS models behave next to the wall, and not to LES.

Also, it sounds like you are thinking that the high and low reynolds number models is to do with the reynolds number of the actual flow? They don't (although it's a very understandable mistake to make). It is to do with what the RANS model does close to the wall.

PS: low should be 0.1 to 10 (not 100)

Go with Dave's advice, when I was referring to low reynolds mesh I was merely referring to getting the Y+ down...I can't remember the formula for computing the integral scales from a RANS run off the top of my head, I will try and find them tomorrow. Dave might know, it is just a useful way checking that your cells aren't too big to resolve the eddies and that your time step is small enough.

Thank you dave for your response lot of info in it.

Iam actually trying to run an LES simulation (smagorinsky). As i mentioned before iam trying to model an pulsatile simulation of blood flow in an artery, the flow i presume turn turbulent only for a small period of time near the peak velocity (as given in the literature too) so trying to classify it as laminar or turbulent flow would not be nice idea. so I Decided that LES would be good way out, though i have to admit that iam not too familiar with it.

As far as i understand LES i assume it is was inbetween DES and Rans where you try to resolve all the Bigger scales and model the smaller ones.

I have already ran an turbulent k omega high reynolds number model which gave me pretty good results. I have a trim cell mesh which i presume is good enough though iamnot sure if it is good for an les model.

I donot have access to Star-CCM+ or either STAR-CD V4 so i have to stick with what i have.

But coming to usage for MARS i have gone trhough a tutorial for LES which talks about using MARS with a belnding factor of 1 for good accuracy.

Once again thank you for your time i really do appreciate all the help

LES is very rarely a "good way out"!

If you've got good results from k-omega, I'd stop there.

Your description of LES is close, but the thing to remember is that your sub-grid-scale model is not very clever - it's assuming you are going to resolve pretty much anything that you're interested in, so if there's lots going on (like near a wall), a coarse mesh will give you a poor result.

DES is a hybrid LES/RANS model - kind of like cheap LES. It behaves like a RANS model near the wall, so that you don't need lots of cells there, and LES where the flow is detached (hence the name). It's a good model, but if things like a turbulent boundary layer are really important to you, it should be avoided.

If you need to simulate highly transient stuff (like aeroacoustics) and need to know things like the peak velocities/temperatures etc., where mean RANS values aren't good enough, then you should think about LES/DES. It is worth doing some background reading first: there's nothing very complicated, but it is easy to get it wrong.

Which turbulence model to use and when is a bit of a difficult question to answer in a forum like this. If you can get hold of a book like this one: http://www.cfd-online.com/Books/show...php?book_id=37 or Peric's book should be good on turbulence models: http://www.cfd-online.com/Books/show...php?book_id=37

It's starting to sound cliche but thank you once again.

I have done most of my academic reading, classes and work in finite element dealing with galerkin weak statements and Taylor weak statements and was always taught that Upwind is the worst algorithm that you can use in terms of numerical diffusion.

It was when i started my thesis i realized that most of the commercial codes work on FV. I kind of went through patankar's book and i t gave me feel of things but as you know it does not talk to much about turbulent models and stuff. And i have never heard about this DES though i meant DNS in my previous email instead of DES.

Anyways thank you so much for helping me out, i know this is not a right place for personal contact id but if you dont mind i would like to be in touch with you as iam still finding my feet in this industry and it would be nice to discuss things with someone like you who is knowledgeable.

My contact id is :shashankiran@yahoo.co.uk (and please dont hesitate to say no if you find my idea to preposterous) I apologize for any discomfort this may cause you

i mean shashankkiran@yahoo.co.uk

I have tried running it with CD blended with some sprt upwinding scheme and crank nicholsom time marching blended with fully implicit scheme and it seems to be running okay