Recently, in my work I have to do a lot of sweeps, like the one bellow:
Now, to close the ends I have to do a revolve:
This doesn´t seem much work, but, to do the revolve it takes about 23 clicks (Revolve, Select Plane for skecth, add references, define axis, project, trim...) for each end. Total of 46 clicks for closing both sides.
I´m trying to figure out a easier way to do this. I tried copy/paste and udf´s , but both fail often.
Jose
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Since this is a channel to be milled, I have to keep the profile (angle and radius):
Nice pic, Huh??
I got to this within a few hundred... maybe a 1,000 clicks 
Only few hundred more clicks might have achieved round'r ends.
I'm proud of it though... fully bound with curvature contraints!
Of course, you could sweep the 1/2 profile around the periphery .
Hah! You know me too well bro! I tried a VSS, figuring it would fail because the section became normal to the spine...and it did. Would be cool if it'd worked...... BUT...the full round is a more powerful tool than people think, it didn't work in this case (for some odd reason, maybe because the end surfs are angled), but if you add a radius to the end lines (ends normal to the sweep), then do a full round, you'd be surprised at how well that works. 
Ahhh, runners. Remember when you got a plastic model to put together, and there was more total material in the runners than the parts?
I may be off topic a little here, but thought this was worth a mention. I create a lot of channels cut into solid blocks, very similar in profile to Jose's. I had the same problem, how to round off the ends, to actually reproduce what a milling cutter would give. My approach is to use the hole feature, specifically 'hole on point placement'. Within the hole feature, you have the option to sketch a hole, sketch 'half' the profile in the same way you would, if doing a revolve end. I have placed datum points at each end of my sweep curve (geometry points added to the curve itself, cuts down on model tree features), select one for hole placement, & voila! you have a rounded end. What brings this into its own, is if you have multiple ends to do, you just copy & paste, selecting a new datum point for another end. Hopefully, the attached model & image explain my approach further.
Regards
John
I was looking for that sketched hole in Creo 2 but didn't see at at a glance. Hope it is still there somewhere.
edit: phew.... yep, still there
That was my initial method as well, Jose, but I ended up with 23 clicks on each half. Since you mentioned 22 clicks per half, I assumed you used the same method. However, that copy/paste thing is nice
Sorry if I wasn´t clear enough. My target is to replicate sweep and revolved ends with minimum number of clicks/references. Ideally, creating a UDF that only asks for a curve and a plane.
I started with the sweep and then creating a revolve at the ends. But to do the revolve, I can use only half of the section, projecting the edges, creating a line in the middle and trimming the curves.
No problem until this point.
Now I try copy/paste to the other end, it asks me all the edges references, and it fails often. I do the revolve manually again, group all features and try to copy/paste using other curve, problems....
I try to copy revolved ends to other sweeps with varied dimensions, problems...
The trick here was to copy the surface, trim it by half, and use all edges for the revolve.
Now I can replicate the sweep with revolved ends just giving a curve, a plane and two endpoints.
I have parts where I have to make twenty or thirty sweeps like these, now I make them much more faster.
Jose
