"on edge" relation - what is it good for?

it bugs me for a long time:
when I create a sketch which is constrained or made from projected edges,
the "on edge" relations are added to that sketch. if I then change the
previous feature and the edges of that feature are changed with it,
solidworks doesn't change the new sketch accordingly?! instead, it gives a
warning on the new sketch highlighting the "on edge" relations as dangling
relations! so for what the hell is this relation good for?

Can somebody please explain me what am I missing?

thanks in advance,
Gil Alsberg

 

I'm sure I'll leave something important out, but the "on edge" relation
is created using the "convert entities" function. You can't create it
directly. If it goes dangling, you can reattach it, as long as it
reattaches to the same type of entity (straight line, arc, etc.)

If you created it by selecting specific edges, you are more likely to go
dangling if editing a previous feature changes the edges. If you select
a *face* to do the "convert entities" bit, it automatically selects the
loop around the outside of the selected face, and changes to the edges
are more likely to work. This is a slick old demo trick, where you draw
a rectangle, extrude it, convert or offset the face, and then go back
and delete the rectangle and draw circle, then rebuild the feature with
the new sketch entities. The convert/offset adapts to the new shape.

The same trick works for selecting inner loops (select face, ctrl select
inner loop edge). Also works for loops selected from the RMB, but it
won't work if you manually select all the edges of the loop.

The relation (on edge or offset) itself is only good for deleting and
reattaching.

Matt

 

Matt,
Thanks for the detailed info. I think it is a reasonable improvement request
from the solidworks guys, to make the "on edge" relation more flexible so it
will update also when it was created by selecting specific edges.

I wonder if you (or anybody else) could help me with the following question
too:

I have a simple part who gives me a headache:

It is designed of two extruded cylinders which between them there is a
vertical loft member. the loft is constrained at both sections of the
extruded cylinders so the tangency relation between them is maintained with
the change of the radius of both cylinders.

Now here is the problematic part:
When I create a horizontal extruded member to that loft with tangency
relations between the silhouette edges of the loft and the arcs on the
extrude sketch, the relation is maintained but in a wrong manner- it seems
that solidworks considers the arc as a whole circle and after the loft
changes, the sketch maintains tangency with the wrong side of the arc,
meaning the missing phantom one!

I would be happy to post by e-mail the compressed part file (as zip file) to
whoever wants to give it a try and explain me what am I doing wrong.

thanks,
Gil

 

....

Silhouette edges in general are fairly unreliable as references.
Intersection curves might be more accurate, but under some
circumstances, these are extremely flaky as well. The best bet is to
make relations to sketches if you can.

I'm having some problem visualizing the "missing phantom one" part of
your description. You could email me at the address shown, but replace
the first "_" with a "j" and the second "_" with an "i", and the domain
should be "net".

Matt

 

What kind of edge are you having trouble with?

Usually plain arcs, lines, and conics converted from actual edges cause
no trouble. I have noted trouble with spline edges and silhouettes.

 

Thanks.
The mail with the file should already be in your inbox.

Gil