CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   Doubts about turbulence in a micro channel (http://www.cfd-online.com/Forums/main/109962-doubts-about-turbulence-micro-channel.html)

shardiali December 1, 2012 10:45

Doubts about turbulence in a micro channel
 
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,

FMDenaro December 1, 2012 12:08

Quote:

Originally Posted by shardiali (Post 395161)
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,

I think that your Re number is so small that, even if the flow would be locally turbulent, you can perform a DNS.

shardiali December 3, 2012 04:26

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

flotus1 December 3, 2012 05:02

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.

FMDenaro December 3, 2012 05:07

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

shardiali December 3, 2012 05:24

Quote:

Originally Posted by flotus1 (Post 395394)
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.


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

flotus1 December 3, 2012 07:36

Quote:

Originally Posted by shardiali (Post 395405)
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?
Alireza

Which problems exactly are you facing? Is it that the flow over the rectangular fin is not as you expected? How did you define the Reynolds number (especially the reference length) in this case?

Keep in mind that 2D-turbulence is completely different from 3D-turbulence (no vortex stretching, inverse energy cascade...)

shardiali December 3, 2012 07:57

Quote:

Originally Posted by flotus1 (Post 395438)
Which problems exactly are you facing? Is it that the flow over the rectangular fin is not as you expected? How did you define the Reynolds number (especially the reference length) in this case?

Keep in mind that 2D-turbulence is completely different from 3D-turbulence (no vortex stretching, inverse energy cascade...)

I get no vortex shedding in the case of a rectangular fin. I made a very thin 3D model with symmetric boundary conditions (infinitly long rectangular cylinder which is literaly 2D). I calculated the Reynolds number based on the length (L) of the fin and it gives me 1800. The problem is I got nice results for circular cylinder with Re=600 (for the same flow and critical length=diameter) but I cannot produce the vortex shedding for the rectangular cylinder. I was wondering if it is because of the higher Re number which might make the turbulent flow.
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?

FMDenaro December 3, 2012 08:02

Quote:

Originally Posted by flotus1 (Post 395438)

Keep in mind that 2D-turbulence is completely different from 3D-turbulence (no vortex stretching, inverse energy cascade...)


I agree, DNS means you are solving the 3D problem

shardiali December 3, 2012 08:27

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! :/

FMDenaro December 3, 2012 08:47

yes, provided that dx+, dy+, dz+ are everywhere O(1) and the numerical method is at least second order accurate

flotus1 December 3, 2012 11:56

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.

shardiali December 3, 2012 13:08

Quote:

Originally Posted by flotus1 (Post 395492)
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.

Thank you for the prompt answer. But how do you define very thin? Now i am simulating a fin with 3.5mm (streamwise) by 0.2mm dimensions. I think this might be considered as a plate and maybe in theory no vortex is expexted to appear! :) Any ideas?! :O

flotus1 December 3, 2012 14:02

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.

Engr.RZA December 4, 2012 13:05

Quote:

Originally Posted by shardiali (Post 395385)
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


I suggest you to use the turbulence in flow if there is fin the channel. Without fin u can undoubtedly use the laminar flow.

shardiali December 4, 2012 13:07

Quote:

Originally Posted by flotus1 (Post 395518)
If you expect vortex shedding behind a blunt body, the cross-streamwise extent (in this case 0.2 mm) would be the characteristic length.
.

Can you give me any reference regarding to your statement?
Thank you,

flotus1 December 4, 2012 17:46

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.

shardiali December 5, 2012 05:34

Quote:

Originally Posted by flotus1 (Post 395785)
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.

That is a very good comment! I think I am totally in favor of your idea that characteristic length would be the length which affects the flow more severly although this is not always easy to find (for example an inclined rectangular fin in the flow). In my case I also agree that it is the streamwise length (3.5mm). About the turbulence, I am doing my simulation with laminar model and a fine mesh grid to capture the vortexes. In case of failure I may try turbulence model as well. I am deeply thankful guys. : ) Happy that somebody created this forum
Alireza,


All times are GMT -4. The time now is 18:20.