|
[Sponsors] |
December 1, 2012, 10:45 |
Doubts about turbulence in a micro channel
|
#1 |
New Member
Alireza Shardi
Join Date: Oct 2012
Posts: 20
Rep Power: 14 |
Dear fellows,
I am trying to simulate the flow in a 3D micro channel with different micro structures. The flow is laminar within the channel since Re number is under 2300, however the question is if the flow is still laminar over the micro fins or not? The shape of fins could be anything like circular or rectangular. I tried to calculate the local Re number on the fns and depending on the size and shape, I got numbers between 600-3000 which could be more also. I am very doubtful about laminar flow simulation. In general do i even have turbulence in my channel and if yes is it considerable considering the small hydraulic diameter of the channel (0.6mm)? I appreciate any help and comments, Thank you guys, Alireza, |
|
December 1, 2012, 12:08 |
|
#2 | |
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,849
Rep Power: 73 |
Quote:
|
||
December 3, 2012, 04:26 |
|
#3 |
New Member
Alireza Shardi
Join Date: Oct 2012
Posts: 20
Rep Power: 14 |
Dear FMDenaro
My question would be dumb, but what you mean is that I may be able to perform my simulation with the laminar model, is it true? Thanks for the answer, Alireza |
|
December 3, 2012, 05:02 |
|
#4 |
Super Moderator
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,427
Rep Power: 49 |
That is the basic idea. If the flow is laminar, you would even introduce an error source by simulating it with a turbulence model.
BTW: If the Re of your channel flow is below 2300, how do you fit obstacles in this channel which give Re=3000? In addition, Re > 2300 indicates a turbulent flow in channels. The critical Reynolds number for blunt obstacles is in general much lower, so your flow might still be turbulent. Nevertheless, the low Reynolds number allows for a DNS even if the flow is turbulent. |
|
December 3, 2012, 05:07 |
|
#5 |
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,849
Rep Power: 73 |
yes, if you set a laminar flow, you set only the molecular viscosity and if your grid is enough fine to catch all the wavelenght, if your flow develop locally turbulence, you will get it
|
|
December 3, 2012, 05:24 |
|
#6 | |
New Member
Alireza Shardi
Join Date: Oct 2012
Posts: 20
Rep Power: 14 |
Quote:
This is good news for me. I ran a 2D simulation for a cylinder in an external flow with laminar model and I got a nice vortex street (for Re=600). However I cannot get a nice result for a rectangular fin in an external flow with Re=1800, I was doubtful if I have to turn on the turbulence model as RE is higher. But from your answer I think the RE number is still low enough to use the laminar model and the problem might be due to some mesh, Bc or ,... .am I making sense?: ) Looking forward to your comments. Regards, Alireza |
||
December 3, 2012, 07:36 |
|
#7 | |
Super Moderator
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,427
Rep Power: 49 |
Quote:
Keep in mind that 2D-turbulence is completely different from 3D-turbulence (no vortex stretching, inverse energy cascade...) |
||
December 3, 2012, 07:57 |
|
#8 | |
New Member
Alireza Shardi
Join Date: Oct 2012
Posts: 20
Rep Power: 14 |
Quote:
In general I am a bit confused about the critical Reynolds number for the external flows. As you guys said with these Re numbers (600-3000) the laminar model would answer me well, but what would be the problem with no vortex generation in the case of rectangular fin? |
||
December 3, 2012, 08:02 |
|
#9 |
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,849
Rep Power: 73 |
||
December 3, 2012, 08:27 |
|
#10 |
New Member
Alireza Shardi
Join Date: Oct 2012
Posts: 20
Rep Power: 14 |
In other words, knowing my problem (Re=1800, flow over a rectangular ocylinder) do you think that refining the mesh or smaller time steps while using the laminar model, helps me to have the vortex shedding? I am still a naive and please ask me if you need more information to help me out on this because I am kinna stuck! :/
|
|
December 3, 2012, 08:47 |
|
#11 |
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,849
Rep Power: 73 |
yes, provided that dx+, dy+, dz+ are everywhere O(1) and the numerical method is at least second order accurate
|
|
December 3, 2012, 11:56 |
|
#12 |
Super Moderator
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,427
Rep Power: 49 |
For the case of the fin, if you define the characteristic length as the extent of the fin in streamwise direction, everything changes.
For a very thin fin, this case corresponds to the flow over a flat plate, which only gets turbulent at very high Reynolds numbers (over 10⁵, i forgot the exact value) Thus I would not expect this flow to become turbulent. Another thing that could cause confusion here is the terminology. A time-dependent flow pattern does not necessarily indicate turbulent flow. For example the Karman vortex street behind a cylinder at low Reynolds numbers is still laminar. |
|
December 3, 2012, 13:08 |
|
#13 | |
New Member
Alireza Shardi
Join Date: Oct 2012
Posts: 20
Rep Power: 14 |
Quote:
|
||
December 3, 2012, 14:02 |
|
#14 |
Super Moderator
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,427
Rep Power: 49 |
If you expect vortex shedding behind a blunt body, the cross-streamwise extent (in this case 0.2 mm) would be the characteristic length.
But an aspect ratio of 17.5 is clearly closer to a flat plate or an airfoil than a blunt obstacle. My experience in this field is practically zero, so I have no idea whether or not to expect vortex shedding. But there should be enough people in this forum that are to able answer the question. |
|
December 4, 2012, 13:05 |
|
#15 | |
New Member
RZA
Join Date: Nov 2012
Posts: 25
Rep Power: 13 |
Quote:
I suggest you to use the turbulence in flow if there is fin the channel. Without fin u can undoubtedly use the laminar flow. |
||
December 4, 2012, 13:07 |
|
#16 |
New Member
Alireza Shardi
Join Date: Oct 2012
Posts: 20
Rep Power: 14 |
||
December 4, 2012, 17:46 |
|
#17 |
Super Moderator
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,427
Rep Power: 49 |
No, I cant. But just to make this clear: Using the cross-streamwise extent as a characteristic length makes no sense if the flow is mainly affected by the streamwise extent of the obstacle, which is clearly the case at an aspect ratio of 17.5.
I think the best way to find out if your specific flow is turbulent is by actually running a DNS. |
|
December 5, 2012, 05:34 |
|
#18 | |
New Member
Alireza Shardi
Join Date: Oct 2012
Posts: 20
Rep Power: 14 |
Quote:
Alireza, |
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Turbulence length scale and integral length scale | rizhang | CFX | 2 | April 22, 2016 08:22 |
Using pimpleFoam to model pulsatile flow in a micro channel | isaacp | OpenFOAM Running, Solving & CFD | 0 | January 30, 2012 01:03 |
DNS of turbulence in a channel flow | YANGLIANG | OpenFOAM | 0 | March 4, 2010 09:40 |
question about turbulence model selection and sensitivity | karananand | Main CFD Forum | 1 | February 26, 2010 05:41 |
turbulence modeling questions | llowen | Main CFD Forum | 3 | September 11, 1998 05:24 |