[Andrew Norfolk]

Hi Everyone,

I'm trying to develop a correlation between a straight fins thermal performance and a serrated fin of the same length, width and height. Due to the geometry scale of the serrations it is impossible to model an entire heat sink compromised of such fins and you can easily end up requiring ridiculous numbers of elements in order to adequately resolve the flow. The idea of this study is to develop a fudge factor I can apply to a straight fin analysis to get the equivalent serrated fin performance.

I built the two models shown and got the results below (I've attached the pictures in my second post).

Boundary Conditions:

100W energy source at the base of the fin for both cases (same size area 1440 mm^2).
Duct inlet velocity of 5ms^-1 with air at 20°C

Results:

Thermal resistance of straight fin: 0.85 °C/W
Thermal resistance of serrated fin: 0.91 °C/W

These results are odd because the thermal resistance of the serrated fin is actually worse than the straight fin, despite having 27% more contact area with the flow. These fins are used in industry to offer improved performance so this result must be wrong. I think I must be modelling the problem incorrectly but i'm not sure in what way, the set up for both studies is identical apart from the geometry.

I've checked Y+ values as these need to be <1 for accurate CHT problems. I've attach a picture that shows this condition is satisfied for the vast majority of the fin surfaces.

There seems to be an unusually large amount of turbulent kinetic energy for the straight fin in comparison to the serrated one, i'm sure this why the thermal resistance is lower for this case.

Has anybody got any ideas about how I am modelling this incorrectly? I am currently using the SST Turbulence model with default turbulent intensity at the inlet. I've been able to converge the quantities of interest and RMS residuals are all below 10^-5. Could it really be that a serrated fin is not as good as a straight fin? I've heard of riblets used to reduce turbulence and drag but these serrations are far too large to be having this kind of effect.....

[Andrew Norfolk]

Pictures for reference.

[ghorrocks]

I've checked Y+ values as these need to be <1 for accurate CHT problems

Where did you get that from? It is not, in general, correct. Wall functions for larger y+ can work just fine in appropriate conditions.

Which direction does the prevailing breeze flow? Where is the inlet and outlet?

Have you done a mesh sensitivity check?

[Andrew Norfolk]

Thanks for replying Glenn, I knew that if anyone would it would probably be you.

I got the information about Y+ from reading an a few articles about turbulence modelling on this site http://www.computationalfluiddynamic...-requirements/

I'll quote a section from the comments where the author of the article responds to a question:

"The laminar sub-layer actually exists in the range of y-plus < 5. Since you are dealing with an internal flow, which is more forgiving on the boundary layer resolution compared with external flows, we would be inclined to say that your resolution is sufficient for either the SST model or the k-epsilon model with scalable wall functions. Note that we do not have adequate knowledge of your problem to say this definitively. Obviously, if you have a surface where you are also expecting to resolve thermal gradients (i.e. conjugate heat transfer) then we would suggest further refinement to the recommended y-plus of 1 with an appropriate turbulence model for wall-bounded flows, such as the SST model."

I most definitely am trying to resolve thermal gradients, and my flow is external so I decided to go for a Y+ less than 1 and i'm using the SST turbulence model.

I've attached a picture of the flow contours in the stream-wise plane. The fins are both 300mm long in a 100mm x 100mm duct that extends 2000mm beyond the edges of the fin (upwind and downwind). The countours I posted previously are a cross-section of the duct taken half way down the length of the fin (2150mmm from the inlet/outlet).

As for the refinement study, yes the solution is mesh independent. I think the serrated case is not producing enough turbulence or the smooth case too much.......

[evcelica]

Here is my guess: It's all in the mesh.

In the serrated blade mesh, you switched to unstructured tets much earlier than in the straight blade, and perhaps have not properly resolved the boundary layer. I've seen this before where the tets increase numerical dissipation, which reduces gradients. These gradients are what induce turbulence, so with them lowered, turbulence, and the associated turbulent mixing and heat transfer are reduced as well. You show very reduced TKE in the serrated model compared to straight, and I think this should not be the case.

It looks like you could do a structured, swept mesh the whole way through on both models?

[Andrew Norfolk]

Hi Evcelica, thanks for replying.

The problem with using a swept mesh for the serrated fin is that it is not compatible with the inflation feature in the ANSYS meshing tool. Without the inflation tool how can I control my Y+ values? I can't use mapped face meshing (structured meshing) as the serrated fin is a complex spline in the CAD data......

UPDATE: I think your right about the mesh. I looked at contours of the eddy viscosity and it was continuing to increase past the inflation layer in the mesh for the serrated case. In other words I haven't resolved the gradients in the boundary layer fully and numerical diffusion could be damping the turbulence generation. The problem is, the inflation tool (ANSYS Workbench meshing) will not allow me to increase the size of the inflation layer any further.........

[evcelica]

There are other ways to mesh it without the use of inflation. Yes, it will be tougher, but it can be done.
I usually slice up the geometry and then use line sizing with bias factors on the lines making them smaller as they approach the boundary.
For example (straight fin case)

For the serrated case, it might be easier to slice the fin up into identical sections, and only mesh one section. Then use mesh transforming in CFX-Pre to fill in all the sections you left out.

[ghorrocks]

Regarding the y+ required: Why not take a simplified example of your simulation and test some mesh densities? Not only will you find out for yourself what mesh is required but in my experience you usually learn something unexpected about CDF accuracy in the process. I think you will find it a worthwhile exercise.

[Andrew Norfolk]

Originally Posted by evcelica

There are other ways to mesh it without the use of inflation. Yes, it will be tougher, but it can be done.
I usually slice up the geometry and then use line sizing with bias factors on the lines making them smaller as they approach the boundary.
For example (straight fin case)

For the serrated case, it might be easier to slice the fin up into identical sections, and only mesh one section. Then use mesh transforming in CFX-Pre to fill in all the sections you left out.

I understand these meshing techniques. With the straight fin case, because all the faces are quads I can use structured meshing and achieve a mesh like the one you have shown including an expansion layer from the fin surface using line biases.

The problem with the serrated case, even if I only mesh one section and transform it in CFX, is that any line biases I apply perpendicular to the surface along any cuts I make only enforce element sizes/divisions at that edge (as you can't use structured meshing). Once you move away from the edge the elements transition into the default element size set by the sizing function......

[evcelica]

I didn't think it would be too hard to do. This isn't perfect, but this is what I was thinking would be good?

[Andrew Norfolk]

Erik that's a very impressive high quality mesh. Did you do that entirely in workbench? I actually wouldn't be sure how to break the geometry up as you have done in design modeller so i'll have to do some reading, any pointers?

[evcelica]

Thanks Andrew!
Yes, I did it all in workbench.

In design modeler I just draw several separate sketches of where I want all the cuts, then extrude them through one at a time with the "slice material" option. I just make sure all sections end up with 4 sides and are sweep-able.
It's just a couple lines and a couple arcs and trims. I would cut everything longitudinally as well where the fin starts / stops which makes it sweep-able, so each faces is only touching 1 other face.

After you slice it up you must select them all and "create part" so that they share nodes at the interfaces and you don't have to create interfaces within the domain.

[Andrew Norfolk]

I've broken up the geometry like you suggested, however rather than do this in workbench I opted for Autodesk Inventor as I find it much easier to manipulate the curves and apply the necessary constraints. I then imported the multi-body geometry into workbench and separated the bodies into two parts, one body that was the fin, and the all the other bodies that were defined as the fluid part. I then used share topology.

For some reason the share topology icon gave a yellow rather than green tick, does this mean that this feature has failed at some level? I ask because when I tried to generate a mapped face swept mesh on my multi-body part it did not produce a conformal mesh between the different bodies (see picture).

Any suggestions?

[evcelica]

Can you Bring it into Design Modeler first? If so, then Highlight the bodies you want a conformal mesh with, then right click and "create new part". When the bodies are part of the same part, then the mesh will be conformal, as it will share the lines in between them.

I would also suggest to make it easier to mesh, that you delete/supress some of the bodies that are repeating over and over. Only mesh some, then use mesh transformations in CFX-Pre to mirror or copy periodically your mesh to fill in the ones you left out. Make sure to "glue" the mesh in the options when you transform it. You of course can just mesh everything manually if you want, It will just be more effort.