coincident lines not coincident?

[SEIZMICdesign]

I'm trying to trim this spline at the point it intersects with the vertical line. The spline point is *supposedly* coincident with the end of the vertical line, but as you can see from the screen shot there is a tiny space between the two in *virtual* reality. I've tried redrawing the spline several different time using different techniques to ensure coincidence, but 360 isn't having any of it. Is this a bug or am I missing something? 

[davebYYPCU · Accepted solution]

Are you missing something, I think so,

Are all the sketches 2D, or possible the splnce sketch could be 3D.

I can't see many purple "projected" articles. there is one horizontal curve that is purple.

The vertical line you refer to would need projecting into the same sketch that the spline is in before it can be used.

Quick test, if you turn off visibility for the sketch with the vertical line, then it is obvious why it can't beused for trim if you now can't see it

To join lines at corners in 3D, you need to "Project Intersect" the points you need to use into the current sketch - snap to the red dot this command will supply.

Should get you going again.

Browny

[jeff_strater]

@SEIZMICdesign, if you want to post your design, I'd be happy take a look.  You may just be missing a coincident constraint:

Jeff

[SEIZMICdesign]

Thanks! I'll check into it.

[SEIZMICdesign]

I did it all three ways; i drew the spline by clicking on the endpoint of each vertical line, I drew the spline separate from the vertical lines and then created a coincident relation between each spline point and end point of each vertical line and even tried just dragging each spline point onto the ends of each vertical line. Still can't get them to be truly coincident. I'll try implementing @davebYYPCU 's suggestions and see if I can't get something workable. I can also provide a link to the model.

[SEIZMICdesign]

link:

http://a360.co/2a3U2gR

[SEIZMICdesign]

So in other words, to split/trim a sketch, the sketch I am using to trim has to be in the same sketch as the sketch getting trimmed. Back on track.

[davebYYPCU]

Yes, correct, 

your first post pictures, are exactly what I found when the loft command says "rails don't touch all profiles", knowing I had just drawn them to do so in the same three methods you describe, in the last post.  Zoom right down to the intersection, and it would always be the same as your first pic.

Depends on what plane the Spline is drawn, if it's on the same plane, is a different method, than an intersecting sketch plane, but the cutting-joining tool has to be projected into the spline sketch.

My method, (in your case) is to finish the various section sketches, create the Spline sketch, and while it is empty, start populating the snap points of the Spline, with the projection of the end points, or crossing lines of your sketch plane.  I normally do my rails first, then the profile sketches, but either way is the same result.

Project command works on parallel planes, Project Intersect, for others, 3D sketches its "Include Geometry"

Then I turn all those vertical line sketches off, I'm left with the snap points I want, draw the lines / curves in this current sketch, Loft works straight up, but was the only way to get it to happen.