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

Channel Flow pisoFoam SA IDDES Re=4560

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 13, 2013, 04:56
Default Channel Flow pisoFoam SA IDDES Re=4560
  #1
New Member
 
Corrado Sotgiu
Join Date: Jan 2013
Posts: 11
Rep Power: 4
ingcorra is on a distinguished road
Im trying to get a fully developed turbulent flow in a channel with a mapped inlet boundary, periodic sides and fixed upper and lower walls. The only way to get some turbulence is to set nuTilda = 0 at inlet, which as far as I know is an ideal condition but then I get zero iterations for nuTilda (so the turbulence model is doing nothing). Any other value different from zero causes the complete dissipation of the turbulence and the flow to be laminar. Is this due to the low Reynolds number? Is it correct to keep nutilda=0 at inlet and have no iterations?

I have the following bundary conditions for nuTilda and nuSgs:

nuTilda

inlet, upper and lower walls: fixedValue 0
outlet: zeroGradient
sides = periodic

nuSgs

sides = periodic
everywhere except at the sides: zeroGradient
ingcorra is offline   Reply With Quote

Old   March 13, 2013, 05:30
Default
  #2
Senior Member
 
Lieven
Join Date: Dec 2011
Location: Mol, Belgium
Posts: 295
Rep Power: 13
Lieven will become famous soon enough
Hi Ingcorra,

If you want to use pisoFoam, you should modify the solver a bit to include a pressure gradient or fixed mass flow rate. Else your flow will simply slow down till there is no flow at all. But you would simply end up with the channelFoam solver. So my advice, start from the latter (is basically an extended version of pisoFoam, but only for LES models).

Cheers,

L
Lieven is offline   Reply With Quote

Old   March 13, 2013, 05:37
Default
  #3
New Member
 
Corrado Sotgiu
Join Date: Jan 2013
Posts: 11
Rep Power: 4
ingcorra is on a distinguished road
Hi Lieven,

thanks for your reply. I forgot to mention that the inlet condition for the U is mapped and has an average value that provides Re=4560, so the flow is not definitely slowing down. Im using it to validate a modified pisoFoam solver (which includes a scalar transport equation) along with the IDDES model with DNS data so I prefer not to use the channelFoam solver.
ingcorra is offline   Reply With Quote

Old   March 13, 2013, 06:37
Default
  #4
Senior Member
 
Lieven
Join Date: Dec 2011
Location: Mol, Belgium
Posts: 295
Rep Power: 13
Lieven will become famous soon enough
Ok, that changes things

Why do you map only the velocity field?
Seems to me that you should do the same with the other fields like nuSgs. You can turn of the averaging for these fields because once the steady condition is reached, the averagingfactor of the U-field should be close to 1.

cheers,

Lieven
Lieven is offline   Reply With Quote

Old   March 13, 2013, 07:19
Default
  #5
New Member
 
Corrado Sotgiu
Join Date: Jan 2013
Posts: 11
Rep Power: 4
ingcorra is on a distinguished road
I mapped nuSgs and nuTilda too (without no average value of course) but I still get zero iterations
ingcorra is offline   Reply With Quote

Old   March 22, 2013, 03:08
Default
  #6
New Member
 
Corrado Sotgiu
Join Date: Jan 2013
Posts: 11
Rep Power: 4
ingcorra is on a distinguished road
I solved by choosing a different initial condition for nuTilda (near to nu). It just converges to a steady value very slow, thanks for the help
ingcorra is offline   Reply With Quote

Old   April 5, 2013, 13:19
Default
  #7
Member
 
Join Date: Jul 2012
Location: Wisconsin,USA
Posts: 34
Rep Power: 5
AA29 is on a distinguished road
Hi ingcorra,

I am facing the same problem. I increased the Re=12000, even then the flow eventually becomes laminar.Did you find a solution to this problem?

Any help will be highly appreciated.
AA29 is offline   Reply With Quote

Old   April 5, 2013, 13:32
Default
  #8
Member
 
Join Date: Jul 2012
Location: Wisconsin,USA
Posts: 34
Rep Power: 5
AA29 is on a distinguished road
And i forgot to mention that i am using channelfoam intead of PISOfoam to simulate a fully developed turbulent flow.
AA29 is offline   Reply With Quote

Old   April 5, 2013, 15:02
Default
  #9
New Member
 
Corrado Sotgiu
Join Date: Jan 2013
Posts: 11
Rep Power: 4
ingcorra is on a distinguished road
You have to provide a correct initial value for nuTilda and nuSgs. There are formulas to calculate it but I guess they're suitable only for external aerodynamics. You could use an initial condition calculated with another turbulence model or just make nuSgs=nuTilda=nu (I assume you already know how to set up the boudary conditions). Let it run until you have an eventually laminar steady flow and check if you have somewhat stable residuals for nuTilda, then add some randomisation to the velocity field and it should develope a nice turbulence
ingcorra is offline   Reply With Quote

Old   March 3, 2014, 21:37
Default
  #10
Senior Member
 
Huang Xianbei
Join Date: Sep 2013
Location: CAU,China
Posts: 266
Rep Power: 4
huangxianbei is on a distinguished road
Quote:
Originally Posted by Lieven View Post
Ok, that changes things

Why do you map only the velocity field?
Seems to me that you should do the same with the other fields like nuSgs. You can turn of the averaging for these fields because once the steady condition is reached, the averagingfactor of the U-field should be close to 1.

cheers,

Lieven
Hi.Lieven
I faced a problem of the convergence when using the icoFoam including pressure gradient. Both the fixed pressure gradient and fixed mass flow rate are performed, however, when I monitor the pressure gradient in the mass flow rate case, the pressure gradient decreases along time steadily, that means delta(grad(p))=const in the same time step change. Also, in the case of fixed pressure gradient, the velocity at the centerline increase steadily as the pressure gradient in mass flow rate case. I don't know why this happens.
huangxianbei is offline   Reply With Quote

Old   March 13, 2014, 10:58
Default
  #11
vut
Member
 
Join Date: Feb 2014
Posts: 56
Rep Power: 3
vut is on a distinguished road
Hi all,

I use OpenFoam for a couple of time (several weeks only). Please be gentle and slow

I am interested in your topic. My task is to simulate a turbulent flow inside an injector.

The solver pisoFoam seems to be suitable for my case study.

Your experiences are greatly appreciated for my following questions:

* Do you have idea about the boundary condition for nuSgs at the symmetry plane.

* How can the lastest solutions of RANS (computed by simpleFoam) be imported as initial conditions for pisoFoam?

All your ideas are wellcome.

Thanks in advance,

VUT
vut 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
Channel flow using InterFOAM DanM OpenFOAM Running, Solving & CFD 37 June 13, 2015 14:50
references for how to maintain a constant flow rate in turbulent channel flow amirrstg Main CFD Forum 0 October 25, 2011 03:17
how to calculate CFL number in 3D convection-diffusion channel flow dryhill Main CFD Forum 0 June 24, 2009 03:33
pressure outlet (open channel flow) Willem Brantegem Main CFD Forum 0 April 3, 2007 09:39
compressible channel flow.. R.D.Prabhu Main CFD Forum 0 July 17, 1998 17:23


All times are GMT -4. The time now is 05:34.