[keryfluid]

hello everyone,
Recently I've been working on ribbed channel flow,and heat transfer is of great importance in this problem. I found that heat transfer coefficient distribution calculated by the k-e model (with enhanced wall treatment) are not quite satisfying compared to the experimental results. I wonder if there's some logic to guide me to choose a proper turbulence model, or I can only try them one by one?
Your remark are highly appreciated!

[cfd_newbie]

Originally Posted by keryfluid

hello everyone,
Recently I've been working on ribbed channel flow,and heat transfer is of great importance in this problem. I found that heat transfer coefficient distribution calculated by the k-e model (with enhanced wall treatment) are not quite satisfying compared to the experimental results. I wonder if there's some logic to guide me to choose a proper turbulence model, or I can only try them one by one?
Your remark are highly appreciated!

hi,
Ribbed channel flow is a very new area to me can you give more details like the Reynolds number involved, details of operating conditions geometry etc. ?
Raashid

[keryfluid]

Originally Posted by cfd_newbie

hi,
Ribbed channel flow is a very new area to me can you give more details like the Reynolds number involved, details of operating conditions geometry etc. ?
Raashid

It's a serpentine channel used for internal cooling of gas turbine blade. Reynolds number depend on the hydraulic diameter is around 50,000, rib height is approximately 0.1 Dh, rib pitch is 10 Dh. The channel is square with an aspect ratio from 1/4~4 and it may have a 90-degree or 180-degree turning section. Rotational effects is not considered yet.

[cfd_newbie]

Originally Posted by keryfluid

It's a serpentine channel used for internal cooling of gas turbine blade. Reynolds number depend on the hydraulic diameter is around 50,000, rib height is approximately 0.1 Dh, rib pitch is 10 Dh. The channel is square with an aspect ratio from 1/4~4 and it may have a 90-degree or 180-degree turning section. Rotational effects is not considered yet.

Did you try the SST turbulence model, this is generally the safest bet and nice starting point. What Y+ are you using right now ? What is the mach number involved ?
Raashid

[keryfluid]

Originally Posted by cfd_newbie

Did you try the SST turbulence model, this is generally the safest bet and nice starting point. What Y+ are you using right now ? What is the mach number involved ?
Raashid

Mach number is near 0.03 so I think it's a incompressible problem. Y+ at most part of the wall is around 3, except for some point on top of the rib ,where yplus can be 10.

[cfd_newbie]

Originally Posted by keryfluid

Mach number is near 0.03 so I think it's a incompressible problem. Y+ at most part of the wall is around 3, except for some point on top of the rib ,where yplus can be 10.

I think since it's an internal flow than you can increase your mesh count (I hope you have sufficient hardware resources) so that nowhere the Y+ is more than 2. Once you have new finer mesh you can "solve to wall" instead of going for wall functions.

[azt]

hi

you probably need to go to a low re turbulence model with Y+ around 1, k-w-sst is a good model.

Experience would suggest that the metal temperature is probably being predicted too high. I found this when I did cht analysis on turbine blades. Changing to a low Re model will reduce the metal temperature by around 10 K.

Only problem is you'll need a lot of cells 20 -25 prism layers in the boundary layer

allan

[cfd_newbie]

Originally Posted by azt

hi

you probably need to go to a low re turbulence model with Y+ around 1, k-w-sst is a good model.

Experience would suggest that the metal temperature is probably being predicted too high. I found this when I did cht analysis on turbine blades. Changing to a low Re model will reduce the metal temperature by around 10 K.

allan

In addition to what Allan has said, if there is a significant laminar to turbulence transition than you should use LMT transition prediction turbulence prediction model.