CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > ANSYS Meshing & Geometry

[ICEM] Heat transfer in 2D ribbed channel: ideas to address the mesh

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree4Likes
  • 1 Post By siw
  • 1 Post By siw
  • 2 Post By siw

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 24, 2024, 04:40
Default Heat transfer in 2D ribbed channel: ideas to address the mesh
  #1
New Member
 
Join Date: Mar 2023
Posts: 6
Rep Power: 3
jmhaque is on a distinguished road
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.)
Attached Images
File Type: jpg RH_Mesh_004_nearRib1.jpg (196.3 KB, 18 views)
File Type: jpg RH_Mesh_004_nearRib.jpg (191.9 KB, 20 views)
File Type: jpg Results_onlyRNGKE.jpg (117.6 KB, 17 views)
File Type: jpg RH_004_95k_planeTw_manyrib.jpg (118.4 KB, 11 views)
File Type: jpg RH_2rib_unsquadmesh_noblock.jpg (195.7 KB, 19 views)
jmhaque is offline   Reply With Quote

Old   March 26, 2024, 10:41
Default
  #2
siw
Senior Member
 
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 739
Rep Power: 26
siw will become famous soon enough
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 likes this.

Last edited by siw; March 27, 2024 at 02:52.
siw is offline   Reply With Quote

Old   March 28, 2024, 08:08
Default
  #3
New Member
 
Join Date: Mar 2023
Posts: 6
Rep Power: 3
jmhaque is on a distinguished road
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.
jmhaque is offline   Reply With Quote

Old   March 29, 2024, 07:11
Default
  #4
siw
Senior Member
 
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 739
Rep Power: 26
siw will become famous soon enough
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.
Attached Images
File Type: jpg Capture.JPG (152.8 KB, 10 views)
File Type: jpg 2.jpg (138.1 KB, 17 views)
SphericalCube likes this.
siw is offline   Reply With Quote

Old   March 31, 2024, 03:37
Default
  #5
New Member
 
Join Date: Mar 2023
Posts: 6
Rep Power: 3
jmhaque is on a distinguished road
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?
jmhaque is offline   Reply With Quote

Old   March 31, 2024, 11:54
Default
  #6
siw
Senior Member
 
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 739
Rep Power: 26
siw will become famous soon enough
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.
jmhaque and SphericalCube like this.
siw is offline   Reply With Quote

Old   June 15, 2024, 01:05
Default
  #7
New Member
 
Join Date: Mar 2023
Posts: 6
Rep Power: 3
jmhaque is on a distinguished road
Sorry for the late update. I had attempted to make an unstructured mesh for the channel. I used a Multizone method to speed up the meshing process (without Multizone, while keeping my settings, it takes forever to generate the mesh). Inflation layers were setup using the default settings. I had also applied edge sizing constraints to the rib surfaces and rib spacings to try and increase the minimum aspect ratio (which was around 16, for some of the cells next to the rib surfaces). The images show the results.

Are there ways to improve this mesh? The cell size distribution near the rib spacings (beyond the inflation layers) seems like it may need to be improved. I am also unsure of whether the sharp corners of the inflation layers are OK. (I guess I may have to reduce the transition ratio?) Lastly, I would like to set the inflation layer parameters using the first cell height.

Finally, I know this is a case setup question, but it is an issue I'm facing when using the unstructured mesh over the structured ones. The wall of the entrance zone next to the heated ribs is not uniformly adiabatic. Over its length of 27.5 mm, the first 25 mm is adiabatic, but the remaining portion has to have a non-zero constant heat flux. I have tried UDFs, but when I initialize the solution and plot the surface heat flux over the flow direction, it does not indicate the change. I have also tried Fluent expressions, but have not been able to set up the if condition. Can this be solved if I split the wall in Spaceclaim?
Attached Images
File Type: jpg Screenshot 2024-06-13 153059.jpg (119.1 KB, 4 views)
File Type: jpg Screenshot 2024-06-13 153135.jpg (109.4 KB, 3 views)
jmhaque is offline   Reply With Quote

Reply

Tags
2-d, heat transfer, icem cfd, nusselt, rib

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
The Specified y+ Heat Transfer Coefficient Sunfangfang STAR-CCM+ 1 March 8, 2024 05:54
[mesh manipulation] Importing Multiple Meshes thomasnwalshiii OpenFOAM Meshing & Mesh Conversion 18 December 19, 2015 19:57
Difficulty In Setting Boundary Conditions Moinul Haque CFX 4 November 25, 2014 18:30
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 07:20
Question about heat transfer coefficient setting for CFX Anna Tian CFX 1 June 16, 2013 07:28


All times are GMT -4. The time now is 19:28.