Splitting a loft

tcarrigan

I have a simple wing like geometry that was created by performing a solid loft operation between two identical profiles, each consisting of four curves. As you can see, even though the profile consists of two curves (red and green) that represent the rounded leading edge, when performing the loft only a single surface is created for the leading edge. For my case, when performing a solid loft, I need the leading edge to be split along the dashed yellow line. I had wrongly assumed that there would be an edge running along the loft between the sets of vertices in each profile, but that is clearly not the case. 

Rather than creating individual surface lofts for each profile curve, which is the only way I currently see this working, is there a way to get what I need? If not, I'll log a feature request to get this added. 

Just a little background info for those interested. Being able to easily split along a leading edge like this that was created via the loft command, or similarly through the fillet operation, is essential for high-fidelity CFD (computational fluid dynamics) grid generation. The ability to use stretched elements can significantly reduce the overall cell count and computation time for a CFD simulation. However, leading edge curves are required to specify the correct boundary conditions for the grid generation algorithms that enable this type of meshing. 

leon_poot

You can split a face of a part with "Split", selecting the face and a plane / surface to split it by.

Jason_S

@tcarrigan

You can split any face with a plane or a surface using Split face.



With this example I split the face of the leading edges with a plane, but in this document I did it with a surface as well for more complex geometry. Hope this helps.

Jason

Jason_S

P.S. Take a look at these custom features for airfoil creation

https://cad.onshape.com/documents/972dc31f395640d97dd6edca/w/8125816b48d1d07ebf0af701/e/31fa0727e4e6c9eb38ab1bb4

https://cad.onshape.com/documents/4bf18c75321ea2c8c2ea770d/v/a158158337c7f50415c36414/e/66a45520ab078f494b4346d1

Good luck!

tcarrigan

Thank you both very much. Jason, I checked out the more complex example you posted. If you don't mind, could you illustrate that process as well? And just for my information, is there a specific reason that edges are not created between profile vertices during a solid loft?

tcarrigan

tcarrigan said:

Thank you both very much. Jason, I checked out the more complex example you posted. If you don't mind, could you illustrate that process as well? And just for my information, is there a specific reason that edges are not created between profile vertices during a solid loft?

This is actually the case I'm working on, https://cad.onshape.com/documents/58e7bedd5802200f741d5663/w/d0823a2c715d49d35e3151f2/e/1fd8be5a46ebe043cdd84a82

I'm trying to split each wing element along the leading edge. This is probably more complex which is why I was looking for just a bit more guidance. 

leon_poot

Nice little spoiler you got there, @tcarrigan.
I think that in order to split the leading face you'd have to 

• loft new individual surfaces of top or bottom curve, 
• sweep the leading edges of these in some non-tangential direction, 
• then split the faces of the solid with the swept surfaces... 

Seems like you can't just loft the camber lines since the starting/ending angles differ even with the same end conditions, and you'd have to sweep because you can't extrude an edge apparently.
...which all in all is more work (on top of the solid lofting) than creating individual surface lofts for each profile curve anyways.

Wild guess: could it be that the edge is there, but Onshape just doesn't want to show it? Nothing shows up when you import it into whatever CFD software you're using?

Ben_Misegades

One way I was thinking about splitting your leading edges is by simply projecting a line or curve from the front (in your case right) plane onto the elements. However, since the elements are not straight, this is a bit tricky to do without having any kind of guide curve from the lofts to work with.

I then tried to re-loft one of the elements as two separate halves, which seems to work, though this doesn't help you much either since OS currently lacks the ability to create "solids" out of surface bodies and vice-versa.

tcarrigan

Leon, 

Yeah, it's a non-trivial process indeed...which it probably shouldn't be. I imported the geometry into my grid generation software and no, the edge is not there. The surfaces are rendered and accessible just as they are in Onshape. 

What would be fantastic is if there were an option, just a checkbox, to create an edge between profile vertices when performing a solid loft. 

tcarrigan

@ben_misegades435 I though of something similar, even just tried to create a series of surface lofts. But yes, I found that even after creating the surface lofts and capping the ends, I was unable to convert the closed collection of surfaces into a solid. Sounds like another feature request.

Ben_Misegades

@tcarrigan yes, it's absolutely a feature request, in my opinion. I'm pretty sure that I've already posted in the forums somewhere about that exact topic at some point. I'm not hugely worried about writing a new IR for it, though, as I'm assuming that it's just another one of those "coming soon" items.

Jason_S

@ben_misegades435 It is indeed one of those items

michał_1

Very awkward workflow. This looks like a task for surface modeling, rather. I doubt FS will help. I don't know how end result supposed to look like, but try to create each wing as a separate part studio. If something needs to be built in context use assembly and in-context editing.