Turbine blade with filleting and tip clearance
I wanna generate structured hexa mesh for a turbine blade with filleting near the hub and very thin tip clearance of 0.2mm. The geometry is imported from a parasolid file, including several surfaces: blade, shroud, hub, inlet, outlet, periodic pressure side and periodic suction side (pic 1). I have blades with two different types of filleting (pic 2 & pic 3). For type 1, it should be emphasized that the filleting is tangent to both blade surface and hub surface. For both types, I want to generate O-grid or C-grid around the solid walls (shroud-green, hub-pink, blade-orange), because I wanna capture the flow phenomena especially vorticity in boundary layer. Additionally, the width of the first grid from wall should be less than 5e-6m in order to keep Y+ on the wall in the order of unity (the axial chord length is 0.04m the the blade hight is 0.06m, so you can have some ideas about the scaling). Of course, the mesh downstream trailing edge should be refined too in order to capture the wakes. And there should be also enough grids in tip clearance so that the tip flow can be simulated.
Please give me some suggestions about strategy for hexa mesh generation. Thanks a lot.
Straight forward for Hexa
ICEM CFD Hexa is perfect for this application. It should also be pretty easy to implement because you don't have a really steep blade angle that requires more exotic blocking.
The question of CGrid or OGrid depends on your trailing edge, which I can't see in this image. Is it rounded or flat? Then OGrid. If it is a sharp trailing edge, then try the CGRID. This is very similar to the 2D examples, except you should start with the hgrid far field and then put the CGrid or OGrid around the blade.
Have you tried the "Stator" tutorial? It is in the 11.0 tutorial set that I have posted links on CFD Online for. That should give you step by step directions, including how to deal with the 3D aspects and periodicity.
If you wanted to give me this model and permissions, I could turn it into a YouTube movie tutorial when I have some time.
Tip Gap considerations.
Oh yea, Tip clearance. Basically, you treat this like a 2D model for the first part until you get your hub blocks all nicely laid out. Then you can usually use "Align" to get the shroud side of the block laid out. (it may help to project the blade tip curves to the shroud for the initial blocking). Then split that initial block at the tip and associate the new edges to the tip. Then put the blocks within the blade into the solid part (or delete them) and leave the fluid blocks around the blade and thru the tip gap. When you setup your distribution thru the gap, it will probably be pretty fine mesh, so don't forget to match edges with the mesh along the blade (as it approaches the tip) so there isn't a sudden change in mesh size.
setting periodicity in the tetin file
I managed finally to have a great mesh of different parts of my turbine, I have the central circle meshed, the airfoil and the gap between the two airfoils... I even meshed the farfield seperately since I need to create a two part mesh, one stationary the other rotating. Do I need to set periodicity for this model? or is it just sufficient to copy the meshes I have into the rest of the circle? and if so, how can I set the periodicity in the tetin file? the axis and angle that is...
On another note, is there a special procedure to "join" the meshes together so that they would work as one part at the end?
The periodicity (set under Mesh (tab) => Global Parameters) is to ensure that your mesh on one side matches the mesh on the other side... Once you see the DEZ (data entry zone), you will understand what you need to fill in. Periodicity is set on the geometry so that the generated mesh comes out periodic, so if you go back to set it, you must regenerate.
Even if you are copying your mesh around to create an annulus instead of a periodic section, it will be easier if you have nodes matching.
Once you copy the periodic mesh into place, you can merge the sections together by using "Edit Mesh (tab) => Merge Nodes (with a tolerance)". I usually set the tolerance very close to zero and use the "single edges only" option. Don't forget to "ignore projections".
However, you could just interactively merge nodes (especially if you don't have a periodic mesh), however, you may also need to use split edge and move nodes... Still, even the manual method without periodicity shouldn't take too long for this example.
|All times are GMT -4. The time now is 05:56.|