CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Turbulence model & y+ for Natural convection (http://www.cfd-online.com/Forums/fluent/101404-turbulence-model-y-natural-convection.html)

Bionico May 3, 2012 05:22

Turbulence model & y+ for Natural convection
 
Hi everybody,
I'm simulating a radiator in a room: since a I want to get a very accurate solution about the power generated by the radiator, I'm trying to create a model that let me to predict the laminar-turbulent transition of the boundary layer along the geometry (that is quite complex and close to the real one).
Does anybody have experience with natural convection?
Maybe I must use Low-Re correction or some complex turbulence model like k-kl-omega or Transition SST (not simply two-equations models)... and i think that y+ should be < 1 (now y+ < 4)
Any advice?

sicfred May 3, 2012 07:43

Hello

In my experience in natural convection with transition to turbulent , the best model was the k-e realizable enhanced wall treatment (I compared with experimental resoults).
As advice, you should take into account the the thermal boundary layer in the mesh, and maybe, also include radiations models (if you didnīt include it)

Bionico May 3, 2012 07:51

Hi sicfred, thanks for your answer! :)
I have a doubt: k-epsilon model shouldn't be very useful for boundary layer, so probably it can't predict accurately heat transfer (that depends strongly on the type of boundary layer, laminar or turbulent).
Anyway I'll try it! ;)

foamcfd May 3, 2012 08:51

In terms of turbulence models generally kwsst with a y+=1 mesh are generally more accurate but an RKE model using enhanced wall treatment combined with a y+=1 mesh will not be very different. The important thing is that for accuracy you will need a y+ approaching 1, ideally <5 everywhere. You will inevitably have high aspect ratio cells here but in these cases the fluent can cope since the variation in solution variables is normal to the cell (little variation tangentially). When using these very high aspect ratio cells you may need to run double precision (3ddp) but I would suggest trying single precision first as double will use more memory.

Bionico May 3, 2012 09:04

Thanks foamcfd! :)

What about using II order Upwind instead of I order for the discretization? Does it offer a great advantage?

Here below 3 images of the system I should study:
http://img441.imageshack.us/img441/7708/radiatore3l.jpg
http://img835.imageshack.us/img835/306/radiatore2.jpg
http://img268.imageshack.us/img268/4518/radiatore1b.jpg

foamcfd May 3, 2012 10:49

Discretization method depends on the mesh you have. Complete hex mesh (aligned with flow) results in first order would little differ from second order results. However for pressure discretization I would go with BWF or Presto for natural convection problems. If you want to see the difference, analyze a case with standard method and have a look at near wall velocity vectors.

LuckyTran May 3, 2012 10:52

Quote:

Originally Posted by Bionico (Post 359036)
Hi everybody,
I'm simulating a radiator in a room: since a I want to get a very accurate solution about the power generated by the radiator, I'm trying to create a model that let me to predict the laminar-turbulent transition of the boundary layer along the geometry (that is quite complex and close to the real one).
Does anybody have experience with natural convection?
Maybe I must use Low-Re correction or some complex turbulence model like k-kl-omega or Transition SST (not simply two-equations models)... and i think that y+ should be < 1 (now y+ < 4)
Any advice?

if there is laminar to turbulent transition you'll need to use the transitional SST or equivalent. rke won't work in that case. But are you sure it will transition to a turbulent boundary layer? For natural convection, it would take > 1m. Your radiator would have to be fairly large.

with heat transfer y+ of 4 is probably not good enough. Try to get at least 2 grid points into the linear region (y+ < 5), so shoot for a y+ ~= 2 with a small stretch ratio between cells or go to y+<1 and you can use a bigger stretch ratio.


Quote:

Originally Posted by Bionico (Post 359075)
What about using II order Upwind instead of I order for the discretization?

2nd order schemes are more accurate so always use it if possible. Results from 1st order schemes are in general poor.

Bionico May 3, 2012 11:22

Quote:

if there is laminar to turbulent transition you'll need to use the transitional SST or equivalent. rke won't work in that case. But are you sure it will transition to a turbulent boundary layer? For natural convection, it would take > 1m. Your radiator would have to be fairly large.
the height is about 0.5 m (but there are also radiators 0.7-0.8 high!)
I'm quite sure that it happens: the Rayleigh number is about 10^8 (so in the transition interval). In the lower part the flow is laminar of course, but it increases the velocity and in the upper part of the radiator some tests with smoke underline the turbulences...(ANSYS suggests RNG k-epsilon or k-omega models)
some other data:
T mean rad= 64 °C
T air = 20°C

LuckyTran May 3, 2012 12:25

Quote:

Originally Posted by Bionico (Post 359130)
In the lower part the flow is laminar of course, but it increases the velocity and in the upper part of the radiator some tests with smoke underline the turbulences...(ANSYS suggests RNG k-epsilon or k-omega models)

Most of the flow is laminar, only a small portion of it is in the transition region correct? The RNG models are fully turbulent models with low Reynolds number corrections, they are not trasitional models and are not built for developing boundary layers. You must use one of the transitional models or use a laminar only approach. Application of fully turbulent model to a mostly laminar flow is incorrect and inappropriate.

Bionico May 4, 2012 04:43

I'll try with a laminar model, too! :)

Another question: this is a closed domain so it's possible that the mass (continuity) could be not conserved... right?

LuckyTran May 4, 2012 12:08

Quote:

Originally Posted by Bionico (Post 359246)
I'll try with a laminar model, too! :)

Another question: this is a closed domain so it's possible that the mass (continuity) could be not conserved... right?

For fluid flows, mass continuity must be conserved always (it is built into the assumptions of the fluid model). A closed domain simplifies even further the mass balance as there are no advection terms. Anyway, the mass conservation equation is solved locally on each cell, so individual cells do you even know that the domain is closed or open bounded.

Bionico May 5, 2012 04:57

ok, I said this because I saw the continuity residuals a bit high (it's difficult to push them under 1)

LuckyTran May 5, 2012 14:27

Quote:

Originally Posted by Bionico (Post 359432)
ok, I said this because I saw the continuity residuals a bit high (it's difficult to push them under 1)

That just means your solution is having trouble obeying mass conservation. That has nothing to do with the physical fact that mass is conserved.

aerospaceman May 8, 2012 21:59

Similar question.
 
Hi guys,

I've got a similar question.

I'm running k-omega SST and want to get the best results possible (as this is only a validation case).

I'm confused with the following choices regarding the kw-SST:

1. How is the wall resolved when the "low reynolds number" box is not ticked? Is it wall functions?

2. Similarly, how is the flow resolved when this box is ticked? Does this then imply a very dense mesh (y+<1)?

It seems that a few other people are also having problems with this, so maybe we can clear this up for good.

Thanks.

LuckyTran May 8, 2012 22:54

Quote:

Originally Posted by aerospaceman (Post 360010)
Hi guys,

I've got a similar question.

I'm running k-omega SST and want to get the best results possible (as this is only a validation case).

I'm confused with the following choices regarding the kw-SST:

1. How is the wall resolved when the "low reynolds number" box is not ticked? Is it wall functions?

2. Similarly, how is the flow resolved when this box is ticked? Does this then imply a very dense mesh (y+<1)?

It seems that a few other people are also having problems with this, so maybe we can clear this up for good.

Thanks.

The "low reynolds number" box is an additional damping on the turbulent viscosity to increase the accuracy of the model for low Reynolds number flows, it has nothing to do with wall functions. So the answer to your question is that there is no difference.

As for how the wall modelling is handled:
All of the omega based models use an approach nearly identical to the enhanced wall treatment with the exception of the omega model itself (which is integrated explicitly and does not need to resort to a two-layer approach, the blending of the viscous and log law region are built into the omega equation).

delaneyluke May 9, 2012 07:35

Low Reynolds number correction in turbulence models refers to the accuracy to capture the viscous layer in your BL (viscous layer = low reynolds number)
Without this corretion you will be able to only capture your log-law region at best.

Please correct me if i'm wrong LuckyTran

Regards
Luke

aerospaceman May 9, 2012 09:27

Quote:

Originally Posted by LuckyTran (Post 360021)
The "low reynolds number" box is an additional damping on the turbulent viscosity to increase the accuracy of the model for low Reynolds number flows, it has nothing to do with wall functions. So the answer to your question is that there is no difference.

As for how the wall modelling is handled:
All of the omega based models use an approach nearly identical to the enhanced wall treatment with the exception of the omega model itself (which is integrated explicitly and does not need to resort to a two-layer approach, the blending of the viscous and log law region are built into the omega equation).

Thanks alot for the very helpful reply. So my last question would be:

How can I resolve the boundary layer on the wall? I.e. suppose I actually want to have a very fine mesh at the walls and want to directly (don't mean DNS here) compute the flow, how can I do this?

Thanks a lot once again. You guys been very helpful.

LuckyTran May 9, 2012 11:30

Quote:

Originally Posted by delaneyluke (Post 360085)
Low Reynolds number correction in turbulence models refers to the accuracy to capture the viscous layer in your BL (viscous layer = low reynolds number)
Without this corretion you will be able to only capture your log-law region at best.

You are completely wrong, did you even read my post?

Quote:

Originally Posted by aerospaceman (Post 360109)
Thanks alot for the very helpful reply. So my last question would be:

How can I resolve the boundary layer on the wall? I.e. suppose I actually want to have a very fine mesh at the walls and want to directly (don't mean DNS here) compute the flow, how can I do this?

Thanks a lot once again. You guys been very helpful.

Just make sure you have enough grid points spanning the boundary layer, i.e. really fine mesh near walls. This is taken care of during meshing and is up to you. Depends on what program you use to generate the mesh. A good start is to target a y+ value and if the growth rate or stretch ratio between cells is restricted to a very small ratio, then usually there will be a great number of points in the boundary layer and is not a problem. y+ in the range of 1-2 is very good place to start trying.

enayath May 23, 2014 11:37

Hello Folks,

Sorry I post here as it passed over a year but I have a problem how to check my Y+ value...in other words, how can I make sure hat I have a fine mesh close to the walls...I wanna solve natural convection...

Thank you!


All times are GMT -4. The time now is 14:49.