[jmhaque]

Hello! I am a new user of Ansys (started last year). I am trying to validate cases of water flow and heat transfer thru a 2D channel with square ribs on one side, with the heated surface being the ribbed surface. My aim is to use a single mesh to test a range of inlet Reynolds numbers varying between 7000 and around 100000. Due to the periodicity of the geometry and the simplicity of rib shape, I had decided to use a structured quad mesh. Pictures of the mesh I had finally used are attached (Figures 1-2). The calculation was performed as a project on Fluent 2023R1, and only the case where Re = 10000 displayed convergence issues (it took more than 3 times the maximum iterations for the other cases for the oscillating residuals to reach the convergence criteria).

However, more importantly, the errors in the obtained values of Nu relative to experimental values, are unacceptable (Figure 3). Moreover, the error will not go down with changes to the turbulence model (realizable k-e from RNG k-e, both with EWT), or with the use of water properties at higher pressure. A plotting of the local Nusselt number and wall y+ at the highest tested Reynolds number shows that Nu spikes very high at the flow separation point (Figure 4). Coincidentally, the wall y+ at this location is over 4.

As a result, I feel I have to redesign the mesh. But there are two issues I need guidance on.

1. My first idea was to halve the cell height of the first layer surrounding the ribs. However, implementing this results in an unacceptable cell aspect ratio in cells close to flow entrance. However, the number of cells in the mesh becomes too high, if I try to address this issue. How do I solve this? Do I need to use a different blocking strategy? My frustrations with this lead me to point 2...

2. I want to try to use an unstructured quad mesh, in which the cells are more refined near the ribs and upper wall and coarser and more ordered in the free stream. Maybe like a hexcore mesh like those developed on ANSA. However, I have not tried this form of meshing before, and have not found a great deal of ICEM CFD tutorials on it. Using the limited set of tutorials, I was able to make this mesh on a first attempt, by doing basic manipulation of the global, part and surface meshing parameters (Figure 5, using an arbitrary channel composed of 2 ribs only).

As can be seen, this is far from an ideal mesh, but I don't really know how to address its issues, and would appreciate guidance on designing the mesh as I envisioned it, all within ICEM, if it is possible. There are a few concepts I have seen, like mesh densities or the usage of blocking and mesh sizing parameters, but I don't understand if they will be useful, and how to implement them well.

Please do let me know if more details are needed. I will submit them as quickly as I can.

(As an aside, which is not relevant, but I hope someone can help me with this: I have measured the wall temperature in two ways, as described in Figure 3. However, can someone please explain why they return significantly different values? The wall point probe is the correct option, and a point in favour of it is the smoothness of the yellow curve in Figure 3, but it returns very low Nu values.)

[siw]

You say this is a (translational) periodic flow (e.g. flow from left to right) so you should not have inflated prism layers on those two edges. Is the top edge a wall? If not likewise you don't need inflated prism layers on it.

You have too large a transition ratio from the last prisms to the adjacent volume elements.

The collapsing prism at the 90deg corners look poorly set-up.

Watch this playlist (https://www.youtube.com/playlist?lis...tuco-qYahdAeG8) about mesh generation topics (not ANSYS specific) from YouTube channel Fluid Mechanics 101, lots of useful information and ideas.

[jmhaque]

Sorry for the long delay in seeing your reply. Thank you very much for your assistance. I believe I have seen some of the channel's videos on meshing before, but I probably really should revisit the concepts to better understand the features in ICEM CFD related to unstructured meshing.

About the mesh: I have a long way to learn, haha. I am semi-competent at fully structured block meshing, but this was my very first attempt at an unstructured mesh. I had excluded the inlet and outlet curves during mesh setup, and yet this was the result, for reasons I am yet to figure out. Unfortunately, I could not find much tutorials on mesh editing in ICEM CFD.

[siw]

I suggest you do not bother with ICEM, it is old and Ansys don't give it any thought nowadays. But if you are single-minded to make blocking topologies then ICEM technology has been added into SpaceClaim Interactive Meshing (SCIM), so that is useful for doing any CAD correction work as well altogether in SpaceClaim (it is oodles of times better than ICEM for geometry stuff). But there is very little training resources for SCIM.

As you are new to CFD then I recommend you just use Ansys Meshing as it is much easier to use. There you can make 2D meshes for Fluent (make sure you set 2D at the beginning and work in the xy-plane) or pseudo-2D meshes for CFX and keep everthing together in Ansys Workbench. If you use Fluent Meshing you cannot make 2D meshes.

This little test in Ansys Student 2024R1 took just a few minutes without any care or consideration of wall height, wake refinement etc. and just using the default options with a User defined global element size and number of inflation layers. The quick geometry made in SpaceClaim without any attention paid to the dimensions.

[jmhaque]

Thank you. I will try Ansys Meshing to create the unstructured mesh.

I had taken a look at it before, for creating the structured mesh that I had made with ICEM instead. In order to replicate that, it looked like I would have to subdivide the periodic geometry into multiple regions in SpaceClaim, and then use edge sizing methods. But that seemed very tedious, and that it would result in many cell zones in Fluent. Is there a way to get the same sense of order in the mesh without having to split the geometry?

[siw]

There is no advantage in splitting up the fluid domain into rectangles, either at the geometry level (in SpaceClaim) or at the blocking level (in ICEM) and then assigning element distibutions on all the edges of the blocks. This video at Fluid Mechanics 101 explains this very well: https://www.youtube.com/watch?v=oa3sxesYsKc, so you should watch this first. This method proporgates high aspect ratio cells were you do not want/need them.

It is better to use an approach like I showed above: better control of the cell sizings, it takes very little time to do it etc.