Message 1 of 11
It appears that the tool is very picky about the way you pick the edges and the setting that are in set for the offsets. When you pick the edges first then apply the offsets it usually fails. When you apply the offsets first the pick the edges it usually works! ANy reason for this?
Message 2 of 11
Message 3 of 11
You edited your post just as my reply went in. However, my reply is still the answer to your question. If your profile is perfectly contiguous, then you can happily make your pick anywhere along it, the command will be able to auto-chain pick the other edges. If you have too much discontinuity, then the command will have a problem because the sweep it produces will have self-intersections. The answer then would be to use the extruded boss/cut command instead, or if the discontinuity was not intentional, correct it first.
Message 4 of 11
Don't want to get into a sketcher and VX constraints discussion again but....
Taking that file as the example, I created the sketch by drawing the spline and centre line, mirroring, adding the end arcs centred on the origin, then using the fillet tool on the corners. I then applied VX auto constraints to fully define the profile (didn't have to do that I suppose but its habit).
Surely by default if I choose a corner fillet, the fillet is tangent to both entities without having to force an additonal tangent constraint on it?
When I chose the lip tool (edge first selection) I shift clicked the edge and the preview showed the lip, but the command failed. Why would that be?
If I can shift select the edge the edge is picked up by the app as being tangent continuous, yet possibly this appears to not be the case.
Finally (something that is more bothersome to be honest), the tool appears to forget what the purpose of a moulded lip is for. If I apply the lip to the outside edge of that part, the lip you get gives you an undercut.
Would it not be more effective to make the lip cut so that it has a pull direction (+/- Z say) rather than simply cutting away a form that has Offset 1 at top and bottom? Could the command not be changed to be Offset 1 (at selected edge), pull direction, draft angle, Offset 2.
In an ideal world the lip tool would take the form of a more useful variant for plastic part design as follows:
Create the part (top and bottom as one).
Have VX define the split line (be good to have this capability in the standard Designer software BTW).
(Optionally choose a DESIRED split plane)
Choose Lip/Split tool
Select part to split
Select parting plane/split line (either VX generated or desired)
Enter minimum draft angle
Enter lip profile offsets
Enter clearance values
Have the tool split the part, apply any required draft to faces, add the lip to to the top and bottom parts including any clearances.
OK not thats not going to be easy :-)
But this is nothing more that what you can already achieve in VX (apart from perhaps the forcing draft angle bit).
Personally, if we are going to have new tools, I'd rather see development going into this direction, as these would be real genuine WOW! features as well as huge timesavers.
Sorry got a bit OT there!
Message 5 of 11
Concerning the original Sketch continuity, blindly applying automatic constraints can lead to the wrong description of the shape. The best thing to do is to manually constrain the key elements of the profile so that they satisfy your exact requirements rather than the computer's "best guess". You do not even have to dimension or constrain most sketches unless you need to parametrically edit their shape later, so when the shape is correct "for now", do not apply auto constraints, you can change the parametrics later if the need arises.
If you study the Lip preview carefully, you will see that it is not perfect and hence the failure.
Concerning the enhancements as you describe, well, that is design automation and it is something you can setup for yourself using the macro language. As features go, I do not think the Lip tool, good though it is, is particularly important to most VX Users. In fact, I expect that many long-standing customers may not have noticed that it exists, because the extruded boss/cut method works well and that is what they would have learnt to use in training. Add this to the myriad of lip shapes you find out there in the real world, and we can see that the most common solution will be a sweep of special cross-section profile.
Message 6 of 11
Message 7 of 11
I can also draft it back around the lip base so that it's not an undercut.
The difference of Lip to similar construction techiques (e.g. sweep) is that lip
uses a true offset of the surfaces in question. Lip is, in a very real sense, a
combination of shell and fillet. And, in fact, it is implemented that way.
The "divide style" lip command would be very valuable, there is no question
about that. The "knife-and-fork" means to do that would be to copy the part,
trim it in half, lip that, draft, take the lip faces, use them to do a divide operation
on the original part.
Some extension may be needed, but only in theory.
I'm sure there is plenty more to say about this, but only after some discussion
Message 8 of 11
What did interest me was why you bothered to change it the constraints at all Chris. Then of course why those particular ones. Were the original constraints wrong?
Message 9 of 11
The constraints were wrong in that they were holding a gap between the entities. The gap value is essentially "zero", but in computation speak that is not the same as "no gap". This minuscule difference can upset the success of a chain select, so if you get unexpected x/y constrains, trim the entities to each other. Sometimes, the CPU's number crunching power can tip the balance. I remember a model, also one of Kevin's, that failed (boolean/fillet, something like that) on his Intel based PC. It also failed on my Intel based PC but my AMD machine solved correctly.
Message 10 of 11
Message 11 of 11