point will not snap on spline

[milne.brett.a]

I have drawn a spline. I create an offset both sides of 1mm. I want to add a point 1mm in from the end on the spline so I can draw a circle. Then when I try and trim the unwanted parts of the offset I see the circle doesnt intersect both offset lines. When I zoom right in the point is slightly off the spline and I can not get it to snap to it?

[davebYYPCU]

You don’t have enough geometry to do as you wish.  You can’t make anything tangent to a Spline, unless it’s at the spline end point.

draw a line to connect both Offset Splines, at their end points.

Offset by the desired radius.  Trim the offset splines to the diameter line.  

Add two point circle to the end points of the spline / diameter line.

In other words the Splines have to be shortened first.

Might help....

[milne.brett.a]

Thanks Dave 👍. I don't understand "You don’t have enough geometry to do as you wish"

If the spline is there i should be able to sketch a point along it?? Seems pretty straight forward to me. I am a novice however

[laughingcreek]

you can constrain the center of a circle to be coincident with a spline anywhere along it's length.  If that's not working for you, you may need to share an example.

[etfrench]

You can place a point anywhere along the spline as @laughingcreek says. 

You can use the technique which @davebYYPCU described to place a circle 1 mm from the end of the spline in a straight line. 

The only way that I can think of to get a point 1 mm from the end of the spline along the spline is to use a combination of Plane along path and pattern on path.

1. Create spline.
2. Create Plane on Path with the start point set to 0 or 1 depending on which end of spline you want the circle.
3. Create a sketch on the plane.
4. Draw a circle on the sketch.
5. Go the the Surface workspace.
6. Patch the circle.  This gives you an infinitely thin face.
7. Use that face as input to Pattern on Path.
8. Set the Distance to 1mm.
9. Set the Distance Type to Spacing.
10. Create a new sketch on the same plane as the original spline sketch's plane.
11. Project Intersect will give you the precise point 1mm along the spline.
12. Project the spline to the new sketch.
13. Draw your circles.

If your tolerances aren't that tight, then just do it as @davebYYPCU described 😀

[davebYYPCU]

Circles tangent to spline, is not a function available at the moment.

Draw the centre Spline, offset it both ways (22mm) draw the top line connected to the outside splines.

Offset that line 22mm down.  Trim the outside splines to the lower one.  

Connect a 3 point circle to the black dots in the picture. You will notice the centre point is not on the centre spline because they are splines.

Might help.... 

[milne.brett.a]

pic 1. drew a random spline. Drew a centre point circle on the spline path.

pic 2. zoomed in on circle centre and it does not sit on the spline path.

[davebYYPCU]

That is likely graphics resolution.

What is it you are trying to do?

Lines and fit points work as expected, 

Working with Splines and Tangents, is not a Fusion function, yet

work arounds as shown are next best.

[milne.brett.a]

It can't be a graphics problem because if it were the circle would meet both offset paths and you could trim off the excess.

I am creating a profile for an extrusion.

I did as you said and put a line between the 2 offset paths and then filleted each corner which works.

I guess I just want to know why I cant put a point on a spline path. Really appreciate your help! 👍