[Crank-Shaft]

Hello fellow CFD-Onliners,

I have been studying vane-type vortex generators on an exposed ramp surface to understand the fundamental flow features downstream. This includes physical variables such as the kinetic energy, vortex core motion, boundary layers and eventually the frequency response of the shed vortices.

My computational study includes stream-wise variation in addition to angle-of-attack. I managed to block and mesh all of the flow domains with the 0 angle-of-attack using Workbench DM and Meshing. However, I am switching to ICEM now since the rest of the domains are much more elaborate and difficult to block.

I have tried to learn ICEM using the customer portal tutorials and also Far's turbo engineer channel on youtube and they have helped me a great deal however, I am still unable to prevent some of the cells from protruding out of my geometry. I have attached the files for my blocking exercise just to learn about the process. Although this is not the exact domain, I believe blocking the rest of the geometry is simple, once the VG and the surrounding region is completed.

Can someone please provide some further guidance and highlight what I am doing wrong? It is absolutely critical to my research.

[Far]

Does this one fulfils your requirements?

Change extension to .rar

[Crank-Shaft]

Originally Posted by Far

Does this one fulfils your requirements?

Change extension to .rar

Thanks so much for the prompt reply Far. You're an absolute legend in my books!

The blocks above the VG definitely looks similar to my previous work in Workbench mesher. I had a lot of problems trying to block the sides of the VG since I didn't know how to avoid the wedges which appeared at the apex where it meets the ramp surface. This is where your blocking strategy shows significant improvement and this should work well with my attempts at generating a full hexahedral mesh. The two rectangular blocks at the rear of the VG should also be compatible with my ramp as I need them to follow downstream in the direction of flow.

For my own understanding and curiosity what process did you follow to create this? Did you create surface blocks and then extend to 3D?

I tried to start with a full 3D block over the entire domain and then use splits followed by associate edges and vertices. This left me with the highly skewed blocks and cells extending into the empty space where the VG resides. This was obviously a poor choice.

I look forward to your comments.

[Far]

The process is very simple and I recall that blocking is also shown in one of the YouTube tutorials. I have been asked to include voice to make them more useful which I am currently trying to do. Any how steps are:

1. Initialize with 3D block and use "auto-associate" command to associate outer edges and vertices to corresponding curves and point respectively.

2. Splits to capture the vortex generator. You will get rectangle shaped block for VGJ and merge vertices on one end to get the shape of geometry.

3. Associate vertices and edges to points and curves of VGJ.

4. Change material of VGJ to solid and uncheck it from part list.

5. Go to Blocking > Edit block > Set Type > Y-Block (from drop-down box) and select two wedge shaped blocks (parallel to solid block) and apply.

6. For rapid mesh size specification go to mesh > Part mesh setup and max size to 2 for all parts.

7. Go to Blocking > Edge mesh parameters > update all

8. Display pre-mesh. To fine-tune mesh sizing go to edge mesh parameters and set edge parameters. Set spacing 1 and 2 for the first cell height. Set Ratio 1 and 2 for the growth. Now to decide which parameter (1 or 2) set, look at the arrow direction on each edge. Starting of the arrow is spacing 1 and ratio 1 and end of arrow is spacing 2 and ratio 2.

[Crank-Shaft]

I have some new updates to share with you all.

I basically followed what Far suggested with the association of the edges, the merging of the vertices and the Y-grid. This produced some great results with orthogonal quality and hexahedral cells. This was with the simplified, pilot fluid domain I was using to learn ICEM.

Now I have tried this technique on the whole fluid domain of interest for my study. This includes inlet, outlet, ramp and a vane vortex-generator at an angle-of-attack of . I have included my initial blocking attempt and the IGES geometry file as an attachment. Key areas that require improvement are -

• The thin longitudinal blocks at the tail of the Vortex Generator should continue until the outlet.

• The second layer adjacent to the near-wall blocks should continue along the domain.

• The thin vertical blocks above the VG do not retain their original width. The lines also lose their vertical relationship when the lower vertices are associated with the VG vertices. Is there a way to translate the entire edge and maintain the original width of block while also associating with the VG ?

Thanks in advance for any ideas and assistance. I have attached an image from 'Validation of Vortex Generator Models in Edge, William Tougeron (2011)' as a desired output however, mine should include the Y-grid strategy.

[Far]

I am thinking to add one artificial block of same shape as VGJ and apply two Y-blocks. Advantage is Nice o-grid around VGJ. Let me try...

[Far]

I tried to reproduce the meshing topology in the first image. Hope you will like it. I will also need your help in applying flow control in low pressure turbine research.

[Crank-Shaft]

That is fantastic work Far! I will try to emulate this blocking strategy myself perhaps later on this week.

I was using index control and eliminating all the other blocks fore and aft of the main ramp when splitting the blocks for the VG Y-grid. I suppose if I tried the same thing while leaving them on, it will create that 'tail' region that I wanted. Is that how you did the above mesh?

I am yet to find a technique in ICEM which allows me to move an edge parallel to another. This is really the only way to achieve longitudinal blocks fore, aft and above the VG with the same width as itself. Please share if you have any ideas.

I would be happy to help you out but I am afraid my knowledge is very limited. I would be happy to share some of the findings from my thesis about the fundamentals of vortex generators.

[Far]

[QUOTE=Crank-Shaft;414853]

I was using index control and eliminating all the other blocks fore and aft of the main ramp when splitting the blocks for the VG Y-grid. I suppose if I tried the same thing while leaving them on, it will create that 'tail' region that I wanted. Is that how you did the above mesh?

Can you show some pics pls...

I am yet to find a technique in ICEM which allows me to move an edge parallel to another. This is really the only way to achieve longitudinal blocks fore, aft and above the VG with the same width as itself. Please share if you have any ideas.

I have used edge length option and set length to 28. At VG width of each block is 27.3 or so.

I would be happy to help you out but I am afraid my knowledge is very limited. I would be happy to share some of the findings from my thesis about the fundamentals of vortex generators

We have applied dimple and bump to low pressure turbine to make flow turbulent before laminar separation point. Hence higher energy and no separation. That work was published in ASME conference. Moreover that work was 2d. Now I am trying to apply different devices to it like active and passive including passive and active VGJs. Can you suggest me from where I start and should I go to 3d or prove effectiveness on 2d blade and then move to 3d (here I will extrude blade by 0.3 chords in Spanwise direction and which is enough according to litrature)

[Crank-Shaft]

Based on my limited knowledge it may be best for you to start with the 2D geometry since it would make it easier to define all the boundary conditions, understand the basic flow features and also determine interpolation, coupling and solver schemes. This is similar to my own approach but it was slightly easier to transition from the 2D to 3D domain since the geometry just required a simple extrusion.

Are you able to share any images of your geometry with us?

[Crank-Shaft]

Hello everyone,

I have been trying to conduct some grid independence studies and sensitivity studies with the ICEM meshes created with the Y-grid technique. Far, I currently prefer that first method we discussed without the two Y-grids superimposed. I believe it will be better for biased edge sizing once near-wall refinement is neccessary.

The major hurdle with the grid independence study when we follow Roache's GCI or Generalised Richardson Extrapolation is that the blocking strategy, biased sizing and the overall approach must remain the same. This is only really possible if the blocking if maintained and a new geometry can be implemented.

I understand that in Fluent we are able to keep the same case settings and simply insert a new mesh and geometry, while maintaining all the boundary conditions and schemes. Is there a way in ICEM to maintain all the settings and blocking strategy, but insert a new geometry which the VG at 80mm off-leading edge rather than 60mm?

Are we able to maintain the same blocking within a .blk and then simply impose these on a new geometry file which contain the same bodies, but slightly translated relative to one another?

Please share your knowledge and experiences. Thank you Far and everyone to contributed so far.