Generating & Using 3D splines

[patmat2350]

I've been having trouble with lofted shapes while working on boat hull designs. I think I see the root of my problems, but want to see if I understand correctly.

Problem: Lofting error when picking rails: Rail does not intersect all sections.

Work flow: Create 3d spline from two 2d splines:

1. 2d fixed point spline in XY plane

2. 2d fixed point spline in XZ plane

3. Extrude a surface up from XY spline

4. Create Sketch with 3d option ticked; 

5.  "Project to surface"- 2d spline from XZ onto the extruded surface.

Gripe: In CATIA, I could do this directly from two splines, no extrusion/projection needed!

Zoom in: Now I'm creating a sketch for a loft section. Intersect the 3d spline with sketch plane, get odd results. 

Black dash line is sketch;

Faded blue line is the 3d spline;

Faded dash line appears to be a polyline between 3d spline's control points (???);

Black point was a previously created intersection of spline in sketch plane;

Red point is a freshly created intersection, which seems to lie on the polyline now and not the spline (maybe just display error at this high zoom level?)

Anyway, this process leads to the lofting error, "rail does not intersect sections", when I pick the 3d spline as the rail.

Possible work-around:

1. Create the loft sections using the 3d spline, "close enough" to what I want;

2. Hide the original 3d spline;

3. Create a NEW 3d fixed point spline, picking corners of the loft sections.

4. Use this new 3d spline as a rail.

Am I missing anything here?

[Beyondforce]

Hey @patmat2350 ,

I have created serious videos on Boat hulls:

https://www.youtube.com/watch?v=aAVTM-dXXv4&list=PLjGKAi--ZCobt6eBTiT9ahIawIK4WQjqh

Cheers / Ben
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[jeff_strater]

one comment here:  There is an "Intersection Curve" which can be useful for turning two 2D splines into one 3D spline that I think is what you are after ("Gripe: In CATIA, I could do this directly from two splines, no extrusion/projection needed!").  See the screencast below.

[laughingcreek · Accepted solution]

Jeff-I love using intersecting curves for producing 3d lines.  At least I use to.  After @TrippyLighting  pointed out several times that the edges of surfaces produce better geometry than projected lines, I did several tests and found he is indeed right (not surprised).  Even in the case of using original spline geometry, extruding surfaces and trimming will produce cleaner geometry than using "intersecting curves".

Why is that, and is there any discussion at AD about improving this behavior?

This also applies to projecting lines onto surfaces.  if those lines are going to be used for further surfacing operations, it's better to split the faces.  which kinda makes a mess of things some times.

[davebYYPCU]

Helpful tips I was taught in here, and now live by, 

Connections in Loft - snap to purple geometry.  

Project Intersect, without it Fusion does not connect reliably.  

I have seen videos and Tutorial where this is not done, they get away with it - I can’t.

In the first pic, Split that body, and use the body edge, Fusion can give Tangent and G2 connections to body edges that it won’t do with its sketched counterpart.  

In the second pic connect the black point to the purple point, (Hide the spline) the only way to be sure.

Might help....

[jeff_strater]

@laughingcreek - I'm not really sure, to be honest.  Internally, this command does the same thing:  Each input curve is extruded along the the sketch normal, and the resulting surfaces are intersected to get the curve.  Offhand, my guess is that the conversion to a 3D sketch curve is the source of any bad geometry in this approach.  And, no, we don't have any plan to fix this in the near future.

[laughingcreek]

That's a shame, I was hoping fusion might focus on improving it's surfacing tool set at some point.  It's pretty week in this area.  

here's a pic of curvature from intersecting curves vs using extruded surfaces.