Relationship Counseling – Part 3

The name Relationship Counseling is of course playing off of the marriage counseling bit, and is doubly funny to me, thinking of my self as any sort of relationship counsellor. “What, she won’t let you spool your fishing reel in the living room or clean fish in the sink? Time to move on, buddy!” “No, you can’t come fishing with me, I’m trying to catch fish, not look at the flowers!” Yeah, I can see myself not being too successful in that field.

The other funny part of it for me is thinking about all of the double meaning stuff that we just ignore in the SolidWorks phraseology lexicon. You know, the stuff I wrote about in my “Stuff you can’t say in public” post. I can hardly keep a straight face ever since I wrote that one.

Anyway, relations in SolidWorks are almost as complex as they are in real life. In this post I’m talking mainly about sketch relations, although you can apply the same principles (and the same double entendre jokes) to assembly mates.

When you have to transgress the dogma

Sometimes you just can’t follow the rules. Think of Horizontal Modeling as a set of best practice suggestions. Best practice is typically a set of rules that you follow when you can, but the rules often contradict other requirements that you have to follow, so you have to make choices. Most of what I’m going to talk about in this part is what to do when you can’t make sketch or feature relations to layout sketches, or stable reference geometry. Sometimes you simply have to reference an edge at the intersection of two faces, and there’s no way around it.

The kind you can fix and the kind you can’t

There are two kinds of sketch relations in SolidWorks, the kind you can fix and the kind you can’t. When you are talking about durability through changes, the ability to repair relations is really key. Sketch relations that you can’t fix are:
– Pierce
– On Edge
– Offset
– At Intersection Between Two Faces
– Patterned

… along with maybe a few more. The idea is that if your model depends on relations like these, and you make a change such that the relation fails, you can’t repair it, you have to delete and recreate. When I used to teach SolidWorks to a lot of new users, I was fond of saying “Delete is not an editing option”. Again, a dogma you can sometimes afford and sometimes not.

The way you select something matters

If you select a face and convert entities or select edges individually and convert entities, you get different results. When a face is selected, it is really selecting a parametric outer loop around the face, so if something happens to change the boundary of the face, the loop selection updates. If you select individual edges and something happens to the boundary of the face, your selection loses an edge, and the feature may fail or get a warning. Remember loop selections can be done by selecting faces or by RMB on an edge. Each edge of a solid has 2 possible loops, you can use the little arrow to select which loop is selected.

Other stuff to remember

SolidWorks added the ability to use a sketch endpoint in the Up To Vertex end condition for extrudes a few releases ago (it used to be that you could only use a model vertex). This is very useful if you have created a sketch-based skeleton and are using a sketch to drive the length of a solid feature.

Remember also that starting a couple of releases ago you can specify the Start Condition as well as the End Condition of an extrude, so you can extrude starting 1″ from the sketch plane. This is handy if you want to avoid creating extra planes, but is kind of a hassle for editing because if you double click the feature, that offset value doesn’t display on the screen.

Up To Next and Up To Body are great ways to specify an extrude without using actual numbers, but remember also that this is the kind of relationship that can easily fail, while actual numbers fail less frequently.

One that burnt me just tonight is that when you have a sketch that was created way back in history, and a feature that was created at the end of the tree, editing the sketch is going to be a pain, because SW will roll the whole model back to edit the sketch. AND, and here’s the good part, you can’t reorder consumed features. Yippee!! So that’s delete and recreate time again.

Actually, if all you have is a sketch and that’s as bad as you have it, it’s not so bad. Absorbed curves can’t even be selected from the graphics window for creating sketch relations. Mature software?  Ha! No way. At least not for non-block shapes. Remember the Rings Of Fire! You are ok in the center, but the farther out you go, the more likely you are to find uncharted territory. Unfortunately, robust sketch relations are way farther from the center than they should be.

Here’s what I want you all to do — run down to the SolidWorks Enhancement Request pageand ask for a FeatureManager option that shows straight history, without absorbing sketches under features. And make sure they know to make it fully functional; if they try to put the steering wheel in the trunk again, well, simply tell them you believe that would be a mistake.

And for Part IV…

Part IV will be an example part driven by a Horizontal Modeling scheme using a sketch and reference geometry skeleton.