CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > General Forums > Main CFD Forum

Laminar model solves seemingly turbulent flow

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

Like Tree1Likes
  • 1 Post By FMDenaro

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 10, 2018, 05:41
Default Laminar model solves seemingly turbulent flow
  #1
New Member
 
Novák Martin
Join Date: Jan 2018
Posts: 2
Rep Power: 0
nmartin9319 is on a distinguished road
Hi!

I have to calculate the flow field in a stirred vessel (15 mm radius, 15 mm height) where the blades (10 mm radius) at the top of the geometry rotating with 3000 RPM.

It's a transient simulation, and until now I've tried to solve it with SST, since the Reynolds number is around 150000. The convergence is good, but if I want to keep the abs RMS at 1e-5 in every variable, then I have to run it with small stepsize (~1e-6 s) for about 5 seconds. Unfortunately I don't have that much time.

First it seemed like an idiotic idea, but I've tried to solve it without any turbulence modelling, and it worked. With 1e-3 s stepsize, the abs RMS in the velocities decresed to 1e-6 and to 1e-4 in the continuity in 10-20 iterations. The results also seem valid.

My question is that why the laminar model working in an obviously turbulent case. My mesh consists ~500k elements, so I doubt that I'm in the DNS regime. Should I believe my results? (I'd love to, but not sure)

Thanks in advance
nmartin9319 is offline   Reply With Quote

Old   August 10, 2018, 05:45
Default
  #2
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 5,424
Rep Power: 58
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Quote:
Originally Posted by nmartin9319 View Post
Hi!

I have to calculate the flow field in a stirred vessel (15 mm radius, 15 mm height) where the blades (10 mm radius) at the top of the geometry rotating with 3000 RPM.

It's a transient simulation, and until now I've tried to solve it with SST, since the Reynolds number is around 150000. The convergence is good, but if I want to keep the abs RMS at 1e-5 in every variable, then I have to run it with small stepsize (~1e-6 s) for about 5 seconds. Unfortunately I don't have that much time.

First it seemed like an idiotic idea, but I've tried to solve it without any turbulence modelling, and it worked. With 1e-3 s stepsize, the abs RMS in the velocities decresed to 1e-6 and to 1e-4 in the continuity in 10-20 iterations. The results also seem valid.

My question is that why the laminar model working in an obviously turbulent case. My mesh consists ~500k elements, so I doubt that I'm in the DNS regime. Should I believe my results? (I'd love to, but not sure)

Thanks in advance



You are solving a coarse DNS, also denoted as LES no-model. But that can have some physical meaning only if you run a 3D case and the grid is quite refined close to the wall. Depending on the action of the local truncation error, if it dissipates by means of the numerical viscosity, this approach is also denoted as Implicit LES (ILES).
nmartin9319 likes this.
FMDenaro is offline   Reply With Quote

Old   August 10, 2018, 06:00
Default
  #3
New Member
 
Novák Martin
Join Date: Jan 2018
Posts: 2
Rep Power: 0
nmartin9319 is on a distinguished road
Quote:
Originally Posted by FMDenaro View Post
You are solving a coarse DNS, also denoted as LES no-model. But that can have some physical meaning only if you run a 3D case and the grid is quite refined close to the wall. Depending on the action of the local truncation error, if it dissipates by means of the numerical viscosity, this approach is also denoted as Implicit LES (ILES).

Thank you for your quick answer! Yes, it's a 3D model. I've attachetd two images of my boundary mesh. So there might be a chance, that my results are not completely wrong?
Mesh1

Mesh2
nmartin9319 is offline   Reply With Quote

Old   August 10, 2018, 06:21
Default
  #4
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 5,424
Rep Power: 58
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Quote:
Originally Posted by nmartin9319 View Post
Thank you for your quick answer! Yes, it's a 3D model. I've attachetd two images of my boundary mesh. So there might be a chance, that my results are not completely wrong?
Mesh1

Mesh2



The mesh appears not enough smooth in the refinement..however you should also compute the y+ you get close to the wall. But I suspect that with only 500K grid points you cannot have any physical results in terms of viscous action over the vessel. What about your scheme?
FMDenaro is offline   Reply With Quote

Old   August 10, 2018, 12:33
Default
  #5
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,033
Rep Power: 48
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Of course laminar model will work, the computer just solves whatever equation you tell it to. Not using a turbulence model basically just means you no longer have an eddy viscosity.


You'd have to check your grid resolution to see if you are like a DNS or not. But given that you are able to take much bigger timesteps with the laminar model, I'd say probably not. Otherwise, you'd be having the opposite result.
LuckyTran is offline   Reply With Quote

Reply

Tags
fluent, laminar, rotating, sst, turbulent

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Laminar transient or Turbulent steady state? zippostyle Main CFD Forum 21 February 13, 2019 15:13
theoretically turbulent but chosen as Laminar Flow oozcan FLUENT 2 August 18, 2017 08:14
Ratio of eddy viscosity to molecular viscosity : Laminar or turbulent flow? JuPa CFX 7 September 9, 2013 08:45
Can I use turbulent model to solve a laminar flow? nikhil FLUENT 5 February 1, 2011 11:42
Is this understanding of turbulence models correct? 3kha Main CFD Forum 3 January 31, 2011 22:31


All times are GMT -4. The time now is 02:11.