Parabolic Sketch for Torispherical Vessel Head

I am modelling a ASME pressure vessel with a Torispherical(parabolic)
head.

What is the best method for constraining the spline points?

WV

 

If you are designing a pressure vessel and need a true parabola, use a
parabola curve and not a curve. In a 2D sketch, use "Insert --> Sketch
entities --> Parabola". Using a spline to trace a parabola will
introduce a measurable amount of error into your CAD geometry. Might
as well start with perfect CAD geometry, as deviations can be copied
with amazing precision with CNC.

 

If you are making a parabolic shape, the best way is to use the parabola
sketch entity, not a spline. A spline will tend to have tangency
problems at the ends and they're always interpolated geometry anyway, so
it won't be exact.

If still you feel the need to use a spline, there are a few ways with
different merits and detractors that you can use:

- if you plan to use a spline as a parabola, you will either need to
overbuild the spline and trim it back or set appropriate end tangency
conditions

- use the auto dimension and just put dims on the spline points relative
to something off the spline, preferably something stable, preferably the
part origin.

- use the Fixed constraint on all spline points

- make the spline proportional and only lock down the ends

- don't worry about it and take your chances with it moving around.
this is actually not as bad as it sounds. splines that are locked to
other things tend to be less predictable than splines that aren't, even
though the common wisdom is to shake your head in horror at blue
sketches.

 

A torispherical head consists of two arcs, one with a large radius and
one near the junction with the cylinder having a small radius. The
closest conic to this shape is an ellipse. You do not need a spline.

 

http://www.edmontonexchanger.com/pvc/head_forming/EdEx_TorisphericalHeadSpecs.pdf