Problem using intersect sketch points to attach surfaces - no actual intersection but only rough approximation

[chrisQX8DX]

so i have a surface which i want to connect to another surface with a loft using rail curves. i am creating sections of the initial surface so i have starting points that i can attach to. the problem i am having is that the starting points i create with Sketch>Project/Include>Intersect are not actually located on the surface i used for the intersect. so later on when i try to use the original surfaces edges as a rail i get an error because the edge does not intersect with the points.

here are some screenshots and a simplified debug file is attached where you can see/check that the points are not on the surface.

sketch on plane used to intersect and generate starting pointsresulting intersect point is not actually located on the surface

i don't quite understand this and don't see the point of the intersect command if it doesn't actually intersect the surface with the sketch plane precisely but only aproximates which makes it useless for whyt i want to do. Is there a setting somewhere that can be adjusted to get precise sketchpèlane/surface intersections. How else would i go about doing this so i can use/position point at exact intersections of surfaces adn sketch planes so a loft further down the line doesn't throw errors ?

Here is the link to the file download: https://a360.co/4awni8r

I just saw that one of my threads has been pinned ( https://forums.autodesk.com/t5/fusion-design-validate-document/include-3d-geometry-why-do-edges-some... ) and this issue is actually totally related to it since i am again modeling the transition from neck to backplate of the headstock, just trying it differently this time. the last couple of times i just did it in rhino where i don't have these problems, if i include an edge or an isocurve from an object or surface it is located exactly on the object/surface. i just thought i'd give it another try in Fusion but it seems impossible.

The last time (the other thread) it was a problem with project/include and i had some wonky surfaces, but as you can see in the example file here it's just a straight loft from two circular arcs with perfect curvature, so i really don't get why this is not generating precise intersection points.

[laughingcreek]

in this particular case I think you're just seeing a graphics issue.  you can't "check" things like this by zooming way in.  what's represented on the screen is an approximation of the underlying data, and when you zoom way in you sometimes get graphic errors like this.  if you use the measure tool, fusion indicates that the point is on the edge-

[chrisQX8DX]

ah yes it might be that with this simplified example it's acurate, however when measuring in the original model which i can't share the intersection points are way off. i finally managed to get my patch to work by using only one curve and the rest only surface edges. however i'm still baffled by the inacuracy of the intersect when using it withobjects and surfaces.

[davebYYPCU]

Disclaimer or not, without the actual file or data doing the same thing, 

we can only tell you - what you expect to happen is the only way to do it.

If the rail gives a ‘not connected ‘ error, then it has not been connected. You get the red blob showing where the problem is.

If you are lofting 2 arcs (in this example,) you are working harder than need be, Extrude is simpler.

if you avoid lofting with sketch profiles, use body edges / faces as profiles, you gain the Tangency / Curvature options, that may eliminate the Rails.

Might help….

[chrisQX8DX]

i'll try to extract the parts that are causing problems from the file i was working on since it still seems weird that when you intersect a surface with a sketch plane the resulting points are not actually connected to the intersected surface.

but in the end it turns out i was overcomplicating things trying to create a surface with several lofts whereas i only needed one curve to be able to create a surface with the patch surface command by using the edges of the other surfaces and the one curve. typical case of analysis paralysis 🙂

thx in any case for your replies and happy easter weekend !

[davebYYPCU]

Some terminology that we understand.

Surface Body.  Construction or Origin Plane, and a sketch placed onto it.  Sketch 1 and Extrusion.

Create the Sketch 2 -Project > Intersect the body, gives you the sectional sketch articles representing the body at the sketch location.  Keep the link, will be purple, no link will be undefined - (blue in my scheme) Hide the body 1 and Sketch 1

Snap to the end point and add the rail. (Snapped Point is black)

Create Sketch 3 on the end of the Rail.  Project > Intersect the End Point of the Rail - Purple point.

Hide Sketch 2 to see it, draw a profile snapping to the purple point in Sketch 3

Show Body 1 and Sketch 2 & 3.

Loft the edge of body 1 to Sketch 3, use Rail from sketch 2, and Select Tangent / Align Edges.

Follow this process, Loft works with first attempt.  Miss a step, and it won't always work.

Might help....