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?
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, 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.
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".
Are you deleting the sketch entities in the prior feature?.
Think of the parent child scheme. Sketch line = feature wall = feature edge. If you delete a sketch line and recreate it you also have created a new face and a new edge with new internal ID's and then any sketches that are referenced to the edge, or face will go dangling.
PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here.
All logos and trade names are the property of their respective owners.