CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Which solver

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   March 4, 2009, 11:43
Default Hi everyone, The flow I wan
  #1
Member
 
Vivien
Join Date: Mar 2009
Posts: 52
Rep Power: 8
sunnysun is on a distinguished road
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 is offline   Reply With Quote

Old   March 6, 2009, 06:56
Default Hi, Can somebody give me hi
  #2
Member
 
Vivien
Join Date: Mar 2009
Posts: 52
Rep Power: 8
sunnysun is on a distinguished road
Hi,

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

Thanks!

Vivien
sunnysun is offline   Reply With Quote

Old   March 6, 2009, 07:48
Default you've got to decide is the fl
  #3
Senior Member
 
Gavin Tabor
Join Date: Mar 2009
Posts: 181
Rep Power: 8
grtabor is on a distinguished road
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
grtabor is offline   Reply With Quote

Old   March 6, 2009, 07:53
Default Hi, is the simulation compl
  #4
Member
 
Marco Müller
Join Date: Mar 2009
Location: Germany
Posts: 94
Rep Power: 8
marico is on a distinguished road
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
marico is offline   Reply With Quote

Old   March 10, 2009, 06:54
Default Hi,Gavin and Marco, Thanks
  #5
Member
 
Vivien
Join Date: Mar 2009
Posts: 52
Rep Power: 8
sunnysun is on a distinguished road
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
sunnysun is offline   Reply With Quote

Old   March 10, 2009, 07:19
Default Why not use the turbulent solv
  #6
New Member
 
Greg Collecutt
Join Date: Mar 2009
Location: Brisbane, Queensland, Australia
Posts: 21
Rep Power: 8
gcollecutt is on a distinguished road
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.
gcollecutt is offline   Reply With Quote

Old   March 10, 2009, 07:41
Default Greg; I was about to sugges
  #7
Senior Member
 
Gavin Tabor
Join Date: Mar 2009
Posts: 181
Rep Power: 8
grtabor is on a distinguished road
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
grtabor is offline   Reply With Quote

Old   March 10, 2009, 08:02
Default Hi, All, Thanks for the sug
  #8
Member
 
Vivien
Join Date: Mar 2009
Posts: 52
Rep Power: 8
sunnysun is on a distinguished road
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
sunnysun is offline   Reply With Quote

Old   March 10, 2009, 08:11
Default Hi, for steadystate simulat
  #9
Member
 
Marco Müller
Join Date: Mar 2009
Location: Germany
Posts: 94
Rep Power: 8
marico is on a distinguished road
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
marico is offline   Reply With Quote

Old   March 10, 2009, 08:37
Default Hi, Marco, I am a bit confu
  #10
Member
 
Vivien
Join Date: Mar 2009
Posts: 52
Rep Power: 8
sunnysun is on a distinguished road
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
sunnysun is offline   Reply With Quote

Old   March 10, 2009, 08:50
Default Oh sorry, I forgot.... Maybe
  #11
Member
 
Marco Müller
Join Date: Mar 2009
Location: Germany
Posts: 94
Rep Power: 8
marico is on a distinguished road
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
marico is offline   Reply With Quote

Old   March 10, 2009, 13:47
Default Hi, just to complete my ques
  #12
Member
 
Vivien
Join Date: Mar 2009
Posts: 52
Rep Power: 8
sunnysun is on a distinguished road
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
sunnysun is offline   Reply With Quote

Old   March 10, 2009, 16:10
Default Vivien, I seem to remember
  #13
New Member
 
Greg Collecutt
Join Date: Mar 2009
Location: Brisbane, Queensland, Australia
Posts: 21
Rep Power: 8
gcollecutt is on a distinguished road
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 is offline   Reply With Quote

Old   March 11, 2009, 05:18
Default Hi Vivien, Try using: wr
  #14
New Member
 
Greg Collecutt
Join Date: Mar 2009
Location: Brisbane, Queensland, Australia
Posts: 21
Rep Power: 8
gcollecutt is on a distinguished road
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.
gcollecutt is offline   Reply With Quote

Old   March 12, 2009, 04:44
Default Hi,Greg, Thanks a lot, it w
  #15
Member
 
Vivien
Join Date: Mar 2009
Posts: 52
Rep Power: 8
sunnysun is on a distinguished road
Hi,Greg,

Thanks a lot, it works!

Best wishes,

Vivien
sunnysun is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
segregated solver vrs coupled solver sm FLUENT 0 November 6, 2007 02:24
How to do it if i change the seregated finitevolume solver to segregated finiteelement solver dandes OpenFOAM Pre-Processing 0 March 22, 2006 22:06
AGM-SOLVER MANOJ FLUENT 5 August 1, 2005 04:49
solver fuf FLUENT 0 June 19, 2003 13:54
coupled solver / uncoupled solver Jaan Unger Main CFD Forum 0 September 3, 2002 08:30


All times are GMT -4. The time now is 14:20.