CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] heat exchanger, too much fins (

diamondx September 20, 2012 10:53

heat exchanger, too much fins
good morning,
I got this heat exchanger to mesh, exept it has too much fines, around hundreds, gap between them is 0.1 mm. as shown in the picture below

Can't go structured on this one, the picture is just simplified model. unstructured mesh is difficult to generate specially with densities around the fins, giving me too much elements. just loading the geometry is a pain for my machine... i can't remove the fins to simplify the geometry. what's the best way to deal with it. generating shell mesh then delaunay ?? i'm running out of option...

Thanks a lot.

cfd seeker September 20, 2012 12:34


generating shell mesh then delaunay ?? i'm running out of option...
2nd option is to directly compute using octree and then convert it to this means delaunay will only octree surface mesh to compute volume mesh

yonchong September 20, 2012 15:11

Sector model?

diamondx September 20, 2012 16:28

sorry i don't get your question yonchong

yonchong September 20, 2012 16:35

I wasn't a question. It was a suggestion.

You seems to have a repreating geometry. It is a heat exchanger so I am guessing that you are trying to calculate Heat Transfer Coefficient and Fluid Temperature map.

Would it be possible to do a sector model with one gap and half fins on either side?

diamondx September 20, 2012 17:02

nice but not doable, my geometry is more complicated than that !! i got three more lines of tube , in totaly it's 72 tubes. i really need to keep it like that ! im struggling, now i'm trying a surface mesh in eache fins then a delaunay flood to the volume...

BrolY September 24, 2012 05:19

This is what we discuss on your thread about unstructured mesh.

The easiest way is to generate octree volume mesh, then delete volume mesh, and finally create delaunay volume mesh (don't forget to smooth your mesh at each step).
Or, if the quality of your geometry is good, you could create a 2D mesh (patch dependent method) and then create the delaunay volume mesh.

To specifiy a small size mesh around the fines, just specify a small mesh size on the curves of the fines.

Don't forget to specify the fines as internal walls ;)

PSYMN September 24, 2012 08:38

If Octree has a weakness, its that you need to mesh very fine to prevent jumping in these small gaps (assuming it is two much work to setup thin cuts).

So if you want coarser mesh than that, and if the geometry is good quality, I would suggest surface meshing with patch conforming. You can go larger.

But if you want prism to grow between the fins, it will need to leave one layer of tetra elements between the prisms... It sounds like this may be tough to do in your case...

In the end, your best bet may be using hexa blocking. If you can't handle the whole thing, how about a sub model and merge it with the rest (or join with non conformal). This is a pretty standard plan for underhood models where the majority of the geometry is too complicated to hex mesh in a reasonable time, but high quality layers are needed on the radiator and oil cooler.

diamondx September 24, 2012 10:18

thanks a lot for your replies,
In fact, unstructured mesh generated around 12 millions elements, without having an accuracy on geometry.


your best bet may be using hexa blocking
That is what i was trying to do recently, i ended up with some troubles:

in the picture above, you only see two fins, in the real geometry i have 170, also instead of the one tube, i have i have three lines of 22 tubes. it means it's a lot of work. before trying to to 170 split, i'm looking for a more efficient and easy way to do that. my first approach was initializing a block between two fins, like in the picture above. then i did associations, after that i duplicated the blocks (copy using vector), result was very good, but associations were not, i removed all the association, and i tried "auto". not working too. Another problem, the fins are considered as wall, so i have to do "face to surface association", i couldn't find another automatic way to do it...

A little break outside of lab made me think about another approach:

I initialized ONE 2D block in one fin, did all the necessary stuff, i converted it to unstructured, then i used the extrude mesh in "edit mesh" tab. extrusion was done nicely, from first fins to last fin . But then again the mesh was ignoring the fins between the first fin and the last one. can i leave it like that and try a repair mesh, using "make mesh conformal with geometry."

There is a third approach, I'm very sorry i made very long :

in order to for my fins in the middle to not be ignored. i can i initialize ONE 2D block in one fin, transform the mesh (duplicate) in 170 others fins. then instead of extruding the first fins like i did before, i extrude all of them , with a distance of 0.1 mm so the extruded of element will lie on the next fins (side part), will this work ?

I'm sorry i made this long, due to the number of duplicated geometry, i can't get my mind of this (transform option), since i think it's the most suitable in this case, and THANK YOU VERY MUCH

diamondx September 24, 2012 10:47

It's me again,

i just tried the last approach, it worked, but not sure what to do next, here is what i did:

i copied the mesh in the first fin to all the other fins, notices that by copying, i had to use the "make mesh conformal with geometry."

For this case i selected all the element in the first and the second fins, then i extruded them to their next respectable fins. for the volume and top and side, i selected inherited, not sure if that was a right move. in my case i have an AIR part, may be i had to select AIR in volume part ?

in this last picture you can see the result, one thing i dont understand, i used extrude i was expecting volume element, why i have shell element too , in purple ??do i have to delete them, i admit that there is no box surrounding my fins, should i make one (surfaces)?

PSYMN September 24, 2012 10:59

A slide modification on your method to work with unstructured mesh instead of blocking...

Mesh one sector. Instead of extruding it, actually mesh the sector. you can use periodicity if you want to, but it may not be necessary for a simple submodel... Convert to uns mesh. Remove the shells from one side, then copy it to get the others... The copy of the first side shells will give you all your fins... User "merge nodes" with a tolerance to fuse everything together.

Whether you extrude or mesh one sector and copy, you will get/need side elements. Creating a box around your fins in an "interface" part is a good idea. The side elements on the hexa side can then be merged with the tetras around the box using this as an interface. Alternatively, you could go with non conformal meshes, but will still need an internal wall to define the interface for the solver.

diamondx September 24, 2012 19:21

I'm back again, this time with good news. I solved my problem :)
Simon thank you very much.
some small modification i did tough:


Remove the shells from one side, then copy it to get the others... The copy of the first side shells will give you all your fins
this method really works but you will end up with the last fin without element on it. if you want element on it, you will have to do (number of copy +1) but in this case you will end up with extra volume element that you need to delete.

Here is what i did, hope it can help somebody else in the future:

I created interface as you can see in the picture below

then i copied the mesh using transform mesh in the edit mesh option, you can see that the last surface is blue, while it has to be green. what we need to do now is make force those elements to belong to that last surface, whish is green normally, i did that by associating the mesh with the geometry.

forcing the merge to adapt to the surface he is on:

i create the tetra elements outside,here is a screenshot of the elements before merging

a screenshot of the merged element, here i indicated the following surfaces: interface,surface in orange and surface in:

a scan plane of the mesh with the volumes:

i exported everything in fluent and it looked as it should. Thank you Simon for you support.

All times are GMT -4. The time now is 03:10.