Symmetrical?

I'm going mad.
I've got an extruded protrusion with a sketch constisting of one
spline. It's a closed spline; the (coincident) end points lie on the
vertical centre line which is coincident with the vertical datum
(although I believe it is no longer considered an end point now that
it's closed). There are 16 points around the spline and they are
spaced symmetrically about the vertical centre line except for 2 which
lie directly on it at the top and bottom. All the little arrows are
there. Yet later on in the model after it has been shelled, some
vertical ribs that are mirrored about the vertical centre do not touch
the inside edge on the mirrored side. I investigated this and found
out the thing isn't symmetrical. It's out by about .002-.003" along
the edge. This measures like this immediately after the protrusion has
been created so it's not something I did to it afterwards. Anyone know
what's going on?

 

: I'm going mad.
: I've got an extruded protrusion with a sketch constisting of one
: spline. It's a closed spline; the (coincident) end points lie on the
: vertical centre line which is coincident with the vertical datum
: (although I believe it is no longer considered an end point now that
: it's closed). There are 16 points around the spline and they are
: spaced symmetrically about the vertical centre line except for 2 which
: lie directly on it at the top and bottom. All the little arrows are
: there. Yet later on in the model after it has been shelled, some
: vertical ribs that are mirrored about the vertical centre do not touch
: the inside edge on the mirrored side. I investigated this and found
: out the thing isn't symmetrical. It's out by about .002-.003" along
: the edge. This measures like this immediately after the protrusion has
: been created so it's not something I did to it afterwards. Anyone know
: what's going on?

Those sketcher splines are tricky little buggers ~ you pull its little finger and
it eyes cross. Something on the left side is a little off and it throws off the
right side too. You'd think, also, that putting more points in would make it more
even, but it just makes the waviness smaller, reduces the deviation from
circularity. You can put 16 or a 100 points around in a circular pattern, connect
them all with a spline, but never get a circle out of it.

One of the things you can do back in sketcher to check what shape you DO have is
to double click the spline to get the spline modification interface. If you're
using 2001 or later rev, there should be an icon that looks a little like a tape
worm. This turns on the curve analysis function. Adjust the scale so that the
normals are big enough to see clearly and adjust the density so that the
connecting curve at the end of the normals is a smooth, stable shape. If anything
is obviously wrong (asymetrical) about the spline, the analysis should show it.

If nothing obvious shows up, start zooming in on points and coincident attachments
to make sure everything is rigged properly. Check dimensions, angles or whatever
is providing the symmetry. If it needs still more help, try putting horizontal
centerlines through the top and bottom points. One of the problems closed splines
can have is one end leading and the other following its curvature and nothing
independent for either end to be tangent to (although, this seems to have been
straightened out in Wildfire's sketched splines). If you can't get either end
constrained tangent, try deleting the spline and putting in the centerlines
through those top and bottom points first, then doing the spline. Also, you may be
able to place a dimensions to the horizontal centerline in place of tangency.
Check again with curve analysis to see if it made any obvious difference.

Personally, though, I prefer creating curves through points where you have some
definite control over start and end point tangency. This curve could also be
'traced' in sketcher or in a half dozen ways for creating surfaces which can later
be turned into solids or 'thickened' instead of shelling a solid.

David Janes

 

Thanks for your detailed response. Mine are interspersed.

Oh, I knew that. I started with the spline having fewer points, and I
added them very reluctantly to get up to 16.

I tried that before (if you mean "display curvature"), and yes, the
display shows the sketch to be asymmetrical.

All points except the ones actually on the centre line have symmetry
constraints.

I tried putting in centrelines. They go through the point, but I can't
add a tangency constraint to the spline. I also can't put a dimension
to the spline (click on spline, point, line) to control its tangency.

I really don't want to delete the spline and start again because
there's too much redefining to do after so I will probably cut it in
half and mirror it. That sounds silly but it will do.

Your latter point about the curve through points is a good one. I
think I will try it with another part that is giving me the same
problems but has fewer features coming after.

You're a very prolific poster!

 

: > <snip>
: > If nothing obvious shows up, start zooming in on points and coincident
attachments
: > to make sure everything is rigged properly. Check dimensions, angles or
whatever
:
: All points except the ones actually on the centre line have symmetry
: constraints.
:
You may have misunderstood what I was driving at. When you've set up your
framework in sketcher (datums, centerlines, points), you've created a lot of
things that the spline can adhere to based on Intent Manager's auto constrain and
snapping to references. So, even while your points are symmetrical, your spline
may not be directly attached to the points. I was suggesting zooming in to check
the attachment of the spline to the individual points. It would take only one that
was misconstrained to throw your spline off the little bit that it was. Unexpected
dimensions are a hint of this.

The procedure I use with splines eliminates this possibility and ensures
symmetrical splines based on symmetrical points. This procedure is like turning
off intent manager but with keeping the normal menus:

* Remove most features, especially the points you wish to anchor to, from the
references. A lot of points as sketcher references really bogs down Pro/e's
variable solver. I've done it, for example, with a lot of center lines for
construction purposes. You need only the normal datums.

* Create the spline away from the points, clicking and creating a control point
for each of the sketcher points and leaving the spline open. Don't let the start
and end points attach to each other or any other reference.

* Use the constraints menu or toolbox to manually constrain spline control points
to sketcher points with coincident constraints.

* Use the coincident constraint to attach start point to end point. The beginning
and end segments should now be curvature continuous. Then constrain this combined
point coincident with the top sketcher point. You need the horizontal centerlines,
really, only when you do half, then mirror the feature or sketched spline. I just
tried this with four symmetrical points and a closed sketcher spline curve. The
spline came out perfectly symmetrical. You couldn't tell where the start/end was.

David Janes

P.S. You can find The Guttenberg Projects collection of Samuel Clemens works on
their website, free for download. It's a 15 meg file when unzipped. That's what I
call prolific. I guess I might be considered prolific, by NG standards, where one
word or two sentence answers are more typical than complete ones, even when the
question deserves more.

 

Thanks again for the advice. I've moved on from that job and did a
work around by cutting the thing in half and mirroring it. It future I
will try it the way you suggested. On this occasion though, I didn't
get around to using datum points to attach the spline points to, I
just had dimensions to the spline points themselves. The only
references I had were the 2 default datums in edge view. I always keep
my refs to the bare minimum necessary; I remove default ones if
they're not needed by my sketch.