Spline/Loft Question

I don't do much with splines and lofts, but occasionally, it is the only
way to represent some complex weld geometry. My question is simple:

If I have a 2-D sketch, and I create a closed spline with four spline
points and then constrain each of those spline points to be equidistant
from the origin and aligned vertically or horizontally with the origin,
why is the generated spline not a circle? The curve between control
points is always slightly 'flattened'. Ditto for lofts through 4 profiles.

Of course in a 2D sketch, I could just draw a circle, but when you
extrapolate this problem into 3 dimensions it becomes much more
difficult. Typically, I have a complex sweep or loft which when viewed
from a particular direction should appear circular but never does.

Am I missing something, or is this just something inherent to splines?

Jim S.

 

The math driving a spline is different from that driving a circle. SW
interpolates the curve between definition points of a spline
differently than it would for an arc, which has a mathematic
construction that defines every point on said arc.

Typically, I try to use ellipses (whole or partial) to define lofts or
complex sweeps before resorting to splines. The result is usually more
to my liking and easier for SW to digest. Also, when an ellips reaches
that magic "equal minor/major axis" config, it IS a circle.

 

I played with ellipses for a few minutes after posting. They won't work
for my problem. What I have is four triangular profiles. If I could
connect the vertex of one profile with the corresponding vertex of each
of the other 3 profiles, the resulting shape would be an ovoid. The
shape is symmetric in one direction but not the other.

I will probably have to 'fake' it with several separate arcs and/or
ellipses.

Jim S.

 

Jim,

I don't fully understand how you are creating the spline in 3D, but if
you need it to be a circle from a particular view, then the best way
would be to:
a. Create a circle in the planar view and project it onto the required
surface or use a second sketch to define its 3D shape.
b. Similar, but split the face/surface with the circle.
c. Extrude the circle as a surface and trim it to it the correct
shape.

Alternatively, there is a very close solution.

You are close to the answer by setting the spline equidistant and
horizontal/vertical, but you need to take and set the spline handles to
horizontal and vertical also, then dimension each spline handle and
link them all together. Here is the equation for the spline handle.

Intended diameter x 3.3137085 = spline handle dimension.

Example: You need a 10 inch diameter spline circle. The spline handle
dimensions would be 33.137085

This should give you a spline that matches a circle within 6 decimal
places on a dimension taken at a 45 degree angle.

If you'd like, I can send you the file that shows this.

Dan Sommerfeld
Design Engineer
ITW-Dahti