Re: Sweep Path tutorial

Matt,

I beg to differ. Even the Help file in SolidWorks 2006 instructs -

To create a sweep:

1. Sketch a closed, non-intersecting profile on a plane or a face.

1. Create the path for the profile to follow. Use a sketch, existing model edges, or curves. _________________________________

This doesn't address the hierarchy required for the addition of pierce relations, but there are many Sweeps which can be cleanly generated without the need to apply them. I agree, however, that in order to pierce, the profile sketch must come AFTER the path (and optional guide curves).

I'm sure you remember when earlier versions of SolidWorks did NOT allow the profile sketch to exist BEFORE the path in the Feature Manager tree, if the user wanted to select it to create a Sweep with a path further down the tree's column. Our hands were tied, so to speak...

I often complained (via Enhancement Requests) about the earlier limitation in the ordering of the path and profile. This was because it is often difficult or awkward to create the path (and guides) first, since their locations in 3D space may not be easily visualized until AFTER the Sweep's profile has been laid out. I often had to struggle with going back up the tree to move a path and/or guide curve as the cross-section profile (to be used for the sweep) was edited and lost the coincident locations needed to maintain the pierce relationship(s). It's a PITA to have to take X,Y and/or Z measurements from the profile to then go back to the path to relocate its sketch plane or entity endpoint, etc. in order to realign with a revised cross-section.

So, I for one am quite pleased to have the freedom to layout the profile first and then create the entities for driving the sweep. I've always found it counter-intuitive to do it the other way around. (If a Sweep has been created by the selection of a profile which existed in the Feature Manager tree AFTER the path, even SolidWorks itself has always displayed the resulting Swept Feature in the tree by ordering the profile BEFORE the path.)

I do agree that, if pierce relations are needed, the profile MUST reside in the Feature Manager AFTER the path (and guides). Still, as I mentioned, it's often a pain to place the guiding entities BEFORE knowing exactly what the profile will be.

As a result, I usually create the profile FIRST, generate the path and guide(s) SECOND and then make a Derived Sketch copy of the original profile. The Derived copy can have the pierce relations added, as needed, since it resides in the order you suggested and is required for the cross-section. (Obviously, the Derived Sketch is then the one used to create the Sweep. If the cross-section needs to be modified, then the one from which it was derived is edited...)

Sure one is left with an additional sketch in the Feature Manager, but the end result is far more productive.

Per O. Hoel ____________________________________________________

matt wrote:

Per,

Yes, I understand that the rules say you can do it that way, but look at the error the poor fellow was getting. Look at the numbers of his sketches. The ones that worked had the profile last, and the ones that didn't work had it first.

SolidWorks added a backdoor because so many people made the same mistake, and relatively few people understand the pierce constraint. Obviously the backdoor doesn't work as well as it could, so I do things the old way that I can at least rely on. Ease of use vs works predictably? I'll take works predictably.

What is your diagnosis of his problem?

Matt

Matt,

Sorry - I'm at a loss to suggest a diagnosis, s> Per,