Learning Forum

[AJMIT]

I am performing steady state CFD analysis on turbine blade for which i imported blade model in design modeler & created hot gas flow path through Export point method in which i have to assign the value of hub/shroud offset (i assigned 4.2 % then ansys shows it's ok otherwise show problem in the model), then i generated hot gas flowpath mesh with turbogrid & mesh solid blade & cooling holes (hole filled by fill option in design modeler & assigned cold fluid part)) with ansys 19.1 meshing & then combined send to cfx (as shown in workbench fig.). Analysis worked well (without error, result matched with experimental values with 10% error).

My problem is that in cfx pre , a short portion of blade model is located outside (see cfx pre fig.) the flowpath generated with turbogrid, i think (assume) it's happened due to hub/shroud offset (see green line in design modeler, in my prespective that the portion of blade between the outer green line transferred to turbogrid)

correct me if am wrong about hub/shroud offset & how can i decrease it

[rfblumen]

Hi AJMIT,nThe Hub/Shroud Offset% in the ExportPoints feature in BladeEditor is to insure the hub and shroud layers (if used) will intersect the blade. The default offset is 0.5%. This offset just means that the hub and shroud layers are moved inward by the percentage of span specified. It will use the blade definition at these new layer locations instead of at the hub and shroud. TurboGrid will extrapolate the blade definition to the hub and shroud from these offset layer locations. Therefore, the specified hub and shroud locations won't change.nThe approach you used (i.e. increasing the offset value when the ExportPoints feature failed) is the correct approach in most cases since extrapolating the blade shape to the hub/shroud from the offset layer locations will only slightly change the blade shape near the hub and shroud. From what you're showing, it looks almost like the hub location isn't matching the blade, which is strange because it shouldn't be affected by the hub/shroud offset.nHere's something you could try to get a better match between the blade solid geometry and the blade surface defined by the flow passage:n-Duplicate the blade body in BladeEditor and use Solid Extension (beta features need to be turned on in DesignModeler) to extend the blade hub and tip in the spanwise direction slightly. Use the blade surface from this extended blade in the ExportPoints feature. You should be able to set the Hub/Shroud Offset% to zero. This should provide a better match between the blade surface defined on the fluid side with the blade surface on the solid side in your CHT analysis.n