CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Which solver (http://www.cfd-online.com/Forums/openfoam-solving/57806-solver.html)

sunnysun March 4, 2009 11:43

Hi everyone, The flow I wan
 
Hi everyone,

The flow I want to simulate is newtonian and has a periodically time varing inlet velocity(between 0.2m/s to 0.8m/s). Should I calculate the reynolds number based on the mean velocity or the minimum/maximum velocity? If I use minimum/maximum velocity, the reynolds number has a range between 700-2800, in this case, which solver would be more appropriate? laminar or turbulent model?

Thanks a lot!

Vivien

sunnysun March 6, 2009 06:56

Hi, Can somebody give me hi
 
Hi,

Can somebody give me hints? Sorry for this basic question...

Thanks!

Vivien

grtabor March 6, 2009 07:48

you've got to decide is the fl
 
you've got to decide is the flow laminar or turbulent? Or transitional? For a pipe, 2300 is the critical Reynolds number, so you've got transitional flow, which is tricky - however you havn't said if this is a pipe flow or not, so its tricky to judge. Sticking my neck out here I would go for a laminar solver and a fine mesh - but if anyone else has a better suggestion I'm quite interested myself.

Gavin

marico March 6, 2009 07:53

Hi, is the simulation compl
 
Hi,

is the simulation complex in terms of geometry, number of cells...?
If not using a turbulent solver doesn't cost anything and should give better results.

Best Regards
Marco

sunnysun March 10, 2009 06:54

Hi,Gavin and Marco, Thanks
 
Hi,Gavin and Marco,

Thanks for the reply, my geometry is a blood vessel section ( a straight vessel section connected with a bifurcation , so 1 inlet and 2 outlets), before the bifurcation is a big aneurysm. The diameter of aneurysm is about 12mm and for other vessel section around 6mm. So maybe I can assume this is pipe flow(correct me if I am wrong)? Geomtry is about 8cm in length and composed of 300,000 elements(generated with Netgen).

Can you please surggest further?

Thanks!

Vivien

gcollecutt March 10, 2009 07:19

Why not use the turbulent solv
 
Why not use the turbulent solver (turbFoam) and look at the results with tubulence on and with turbulence off? There is a turbulence on/off switch in the RASProperties input file.

Gavin / Marco - am I wrong in thinking that the transient laminar flow solution may become unstable in transient / turbulent flow?

Greg.

grtabor March 10, 2009 07:41

Greg; I was about to sugges
 
Greg;

I was about to suggest exactly that.

My issue with running a turbulence model on a laminar case is that I don't know that the k/e and thus the turbulent viscosity are guaranteed to go to zero. In other words I don't know if the effect of the turbulence modeling is going to go away when it is not needed. (If anyone can reassure me on this point I would be overjoyed; I've got a number of projects at the moment operating in just this regime and it would be useful to have an answer one way or the other).

My argument for running laminar is that most of the effects of the turbulence are eddies which could be resolved at this Reynolds number. In essence the laminar solver will do the laminar regime OK (obviously) and operate as a sort of coarse (possibly underresolved) DNS on the turbulent aspects of the flow. It should run though. The only issue which this does not cover is `bursting'; genuine transitional flow exhibits bursts of intermittent turbulence which come from nowhere and disappear as well, which are difficult to model. However in a complex geometry such as this I would think complex flow motions (turbulence if you like) are going to arise naturally from geometric considerations anyway.

Gavin

sunnysun March 10, 2009 08:02

Hi, All, Thanks for the sug
 
Hi, All,

Thanks for the suggestions. At meantime I tried with both turbulence model(turbFoam) and laminar model(icoFoam). I have one question about turbFoam, how can I estimate the internal field k episilon at time instance 0 based on my case?

Thanks!

vivien

marico March 10, 2009 08:11

Hi, for steadystate simulat
 
Hi,

for steadystate simulation the internal (initial field) is only important for the solution: if it will converge and how fast!
A converged steadystate simulation must be independant from the initial field.
Try to use approximate values from the formulas given in OF's users manual (must be the first tutorial, cavity).

Marco

sunnysun March 10, 2009 08:37

Hi, Marco, I am a bit confu
 
Hi, Marco,

I am a bit confused...my simulation is transient instead of steady. I did look at the cavity case, the problem for me is how to estimate the fluctuating component?

Could you please also suggest what kind of case is k-epsilon model most suitable for?

Regards,

vivien

marico March 10, 2009 08:50

Oh sorry, I forgot.... Maybe
 
Oh sorry, I forgot....
Maybe you can run steady state to get initial values you can use for transient run.
Your second question should be answered by some more experts... ;)

Marco

sunnysun March 10, 2009 13:47

Hi, just to complete my ques
 
Hi,
just to complete my question, I run the same case with icoFoam, it diverges(for the same geometry, it converge with constant and lower velocity 0.02m/s at inlet)... would it possible because of I use the icofoam to solve a flow which is turbulent so that get the divergent result?

Thanks!

Vivien

gcollecutt March 10, 2009 16:10

Vivien, I seem to remember
 
Vivien,

I seem to remember that the cavity tutorial showed that the laminar flow solution will become unsteady and ultimately may fail to solve once the velocities increase and turbulence effects (namely turbulent viscosity) become important.

The k-epsilon turbulence model is OK for high Reynolds number flow but may not be accurate in the transitional region, and does a poor job of correctly estimating boundary layer effects and wall drag.

Given that you are starting out with this problem, I would recommend that you use turbFoam with the k-epsilon model. Initialise k to (0.1U)^2 (i.e. 10% turbulence intensity) and epsilon to (Cu^3/4).(k^3/2)/Lm where Lm is the approximately the blood vessel diameter. Also use these values for the inlet patch. I would then run two or three pressure cycles (heat beats) for the fields to settle down. Once see what the k and epsilon values typically settly down to you could use these on the inlet patch.

The adaptive time stepping to control courrant number is the way to go, but set dT to give a small courant number for the very first time step. Often jumping straight in with a 'normal' size timestep can cause problems since the initial field values are miles away from what they should be.

You've made pretty good progress today!

Greg.

gcollecutt March 11, 2009 05:18

Hi Vivien, Try using: wr
 
Hi Vivien,

Try using:

writeControl adjustableRunTime;

writeInterval 0.001;

I guess zeroGradient on inlet patches for k and epsilon may work - I've never tried myself. I only consider myself an intermediate level user, and my background is not really cfd so I don't know all the details on turbulence models' strengths and weaknesses.

Greg.

sunnysun March 12, 2009 04:44

Hi,Greg, Thanks a lot, it w
 
Hi,Greg,

Thanks a lot, it works!

Best wishes,

Vivien


All times are GMT -4. The time now is 12:30.