[Crank-Shaft]

Fellow CFD-enthusiasts,

I have been looking for a way to create grids identical to those in the link below for a NACA4412 -
https://turbmodels.larc.nasa.gov/naca4412sep_grids.html

I am interested in these files -

• (3-D) 2 x 1793 x 513 (2 x 1025 points on airfoil surface) (13.2 MB)
• (3-D) 2 x 897 x 257 (2 x 513 points on airfoil surface) (3.4 MB)

I have a research CFD code and want to modify the boundary conditions given (as they are not implemented) and also increase the number of blocks by equally splitting at selected grid points to export a multiblock CGNS grid with lots of equally balanced/weighted blocks for efficient parallelisation.

Is this possible on ICEM? I have tried using a simple O-grid topology but the bias sizing around the leading and trailing edges don't match the ones on the NASA site. Additionally I am not sure how to smooth out the multiblock structured grids so that near-wall cells are all perpendicular to the aerofoil surface like in this image for example Mesh 1 or Mesh 2
I believe these were created in GridPro and Pointwise respectively.

Any help or suggestions are greatly appreciated.

Best wishes,

[Far]

yes you are correct. first mesh is created in gridpro and second in pointwise/gridgen.

Yes you have option of mesh smoothing in ICEMCFD. But it is tricky to get it done.

[Crank-Shaft]

Originally Posted by Far

yes you are correct. first mesh is created in gridpro and second in pointwise/gridgen.

Yes you have option of mesh smoothing in ICEMCFD. But it is tricky to get it done.

Thanks for your reply Far. I have started working on a mesh and will create three different levels of refinement for this. I have attached the .tin and .blk files and it would be great if you could show us how to convert this to a 3D blocking structure and also apply smoothing to roughly replicate the Pointwise or GridPro results shown in the images.

I tried the 2D-to-3D block transformation and it appears to immediately have a lot of errors in pre-mesh mode and associations are completely wrong.

Your help is greatly appreciated on this and I look forward to learning from your expertise.

[Crank-Shaft]

I've made some progress and restarted from scratch using 3D blocking. I'd like to ask for assistance with my ICEM file. I am not sure whether there are issues with the large domain size and the profile of the aerofoil being 100x smaller, but there are small errors near the edges of the NACA profile and the edges and curves just don't seem to match.

This creates a layer of near-wall cells and the pre-mesh checks have a lot of negative Discriminants. I've tried to redo this several times and re-created the aerofoil curves in different ways but this is persistent. I am wondering if there's a resolution or edge/curve tolerance issue.

If someone could look at the .tin and .blk files attached and share some ideas, that would be greatly appreciated!

Kind regards,

[Far]

I saw your old files. I found very high aspect ratio cells which is making quality worst. Why you are trying with with very very small node distance from wall?

[Crank-Shaft]

Hi Sijal,

I needed to get the y+ value to around 1 and the finest grid resolution will require 2e-6 first-cell height, given the overall chord-based Reynolds number of 1.52e6.

Hope this makes sense. Do you think it would help if I made the entire domain 20 chord-lengths instead of 100c? It might make it easier to work with and also avoid the huge range of length-scales present in the geometry which might cause a mismatch.

Thanks

[Far]

Why you need Y+ = 1? If it is not transition from laminar to turbulent, you can use Y+ = 10 and still get the same results.

[Crank-Shaft]

Originally Posted by Far

Why you need Y+ = 1? If it is not transition from laminar to turbulent, you can use Y+ = 10 and still get the same results.

Hi Sijal,

I was trying to follow the guidelines provided by the reference site.

[Far]

Old times old turbulence wall treatments. New treatment in CFD allows up to Y+ = 10 and still gives the results similar to Y+ = 1.

Moreover try to increase points in stream-wise direction.

[Crank-Shaft]

Originally Posted by Far

Old times old turbulence wall treatments. New treatment in CFD allows up to Y+ = 10 and still gives the results similar to Y+ = 1.

Moreover try to increase points in stream-wise direction.

Firstly, I am using an in-house research code with only a very basic wall-model implemented. Secondly, are you suggesting that if I switch to y+ 10 grid it will resolve the issues?

I will try to redo this maybe by modifying the domain to 20 chord-lengths and also larger near-wall cells.

If you have any suggestions for improving or avoiding the discriminant errors near the surface please let me know.

Thanks!

[Crank-Shaft]

Hi everyone. I decided to redo all the blocking and the association for the domain and the first-cell heights have been increased. Unfortunately, after exporting the structured grid, I noticed that there were negative Jacobians and determinants in the domain.

I ran pre-mesh quality checks for the determinant 2x2x2 and it seems like they are near the inlet. All the edge and even surface associations seem sensible however, there are clearly some of the high-aspect ratio cells which seem to be inverted or penetrating each other.

I have attached the block and geometry file here so your comments and suggestions are most welcome.

[shereez234]

I had a quick look at your files, I noticed multiple curves for inlet and pressure far field. I also noticed multiple fluid surfaces with the name symmetry that is laying over each other. try to use Far Field, Outlet, Fluid Zone(single surface) and then Airfoil other wise projections will be confused by blocked meshing in ICEM

[Crank-Shaft]

Originally Posted by shereez234

I had a quick look at your files, I noticed multiple curves for inlet and pressure far field. I also noticed multiple fluid surfaces with the name symmetry that is laying over each other. try to use Far Field, Outlet, Fluid Zone(single surface) and then Airfoil other wise projections will be confused by blocked meshing in ICEM

Hi Shereez,

Thanks for your reply. I did check the geometric entities contained in each of the farfield, inflow and symmetry parts and can see some room for potential improvements. Firstly, in order to create the smoothest C-grid possible, I tried to avoid any splits along the upper and lower aerofoil surfaces. However, this meant that a single edge (green, diagonal edges in the image) has to be associated with two different curves (for inflow and farfield).

To correct this, I'd have to try and use the vertex at the end of the diagonal line and to split the blue and pink curves, then try to split the block around the aerofoil and ensure that they are either projected on to the inflow, or the farfield, but not both.

Does the above make sense? Do you have any other suggestions?

I really don't know if a proper C-grid is possible with the tools available in ICEM, unless we split into lots of small blocks and that makes it super time-consuming. Also makes it less robust if any modifications are needed for any of the grid distribution along the edges.

Please share your thoughts. Thank you!

[shereez234]

Originally Posted by Crank-Shaft

Hi Shereez,

Thanks for your reply. I did check the geometric entities contained in each of the farfield, inflow and symmetry parts and can see some room for potential improvements. Firstly, in order to create the smoothest C-grid possible, I tried to avoid any splits along the upper and lower aerofoil surfaces. However, this meant that a single edge (green, diagonal edges in the image) has to be associated with two different curves (for inflow and farfield).

To correct this, I'd have to try and use the vertex at the end of the diagonal line and to split the blue and pink curves, then try to split the block around the aerofoil and ensure that they are either projected on to the inflow, or the farfield, but not both.

Does the above make sense? Do you have any other suggestions?

I really don't know if a proper C-grid is possible with the tools available in ICEM, unless we split into lots of small blocks and that makes it super time-consuming. Also makes it less robust if any modifications are needed for any of the grid distribution along the edges.

Please share your thoughts. Thank you!

Hi;

I am sorry but all this time I thought you were doing a 2D mesh which is why i said multiple surfaces.

I realize now you are using symmetry on two sides of the wing.

Why are you blocking this in 3D if there is double symmetry planes? follow these steps if you want.

Make a 2D blocking for the airfoil and convert to unstructured mesh and go the Extrude mesh tab(2nd tab) in Edit mesh features and add 50-100 layers( how many layers you will extrude in Z direction , well this is really upto you).

Good luck
Cheers

[Crank-Shaft]

Hi Shereez,

Thanks for that tip. I've started off a new approach using 2D blocking and the overall topology and associations are much quicker and easier to manage.

Do you know if it is possible to associate the new 3D block faces with the 2nd symmetry plane? Are we able to assign boundary conditions on these new faces too?

Thanks

[Far]

This is how you can make 2d to 3d blocking.

https://www.youtube.com/watch?v=BFn9hL6CrJ8

[Crank-Shaft]

Originally Posted by Far

This is how you can make 2d to 3d blocking.

https://www.youtube.com/watch?v=BFn9hL6CrJ8

Thanks for sharing the video. That was really helpful.

I replicated the node distribution and blocking topology I had earlier but used the 2D to 3D translation. The determinants seem to be fine when I have only a single cell in the Z direction (2Nodes_3DBlocking.png). Unfortunately, when I increased the number of cells in the z-direction to anything greater, there are inverted cells like we had before (20Nodes_3DBlocking.png)!

Any suggestions would be welcome. The associations seem to be correct.

Thanks everyone!

[kad]

Your geometry is still a bit messy as Shereez already stated before. There are double curves and gaps between surfaces in the problematic region. This is causing your problems with multiple layers in z-direction. A single layer can handle these gaps, well, because it is only a single layer. So a not very proper solution would be to create only a single layer and split it afterwards. Improving geometry is one too, of course.

Again refering to Mr. Shereez I think the way to go here is to start with 2d blocking and extrude the unstructured mesh. This makes handling blocking and geometry much easier. I have replied to some threads here involving extrude mesh and explained the method a little bit. Maybe you can search for them.

[Far]

Part I : https://youtu.be/q4kK2w4hMvQ

[Far]

Part II : Extrude 2d to 3d mesh from unstructured mesh

https://youtu.be/jIivveKROH8