There’s nothing meaningful I could do to compare the entire Solid Edge and SolidWorks programs in a single blog post. That’s why when I have taken the topic up on the Dezignstuff blog, I would bite off “small” areas like surfacing, sheet metal, or the overall interface. In this case I’m going to look at sketching, arguably the single most important function of any CAD program.
You might think Solid Edge and SolidWorks sketchers are pretty similar because they both use the (Siemens) Dcubed constraint solver. In the end, that similarity probably means that they share the strengths and weaknesses of Dcubed, but the comparison can’t be limited to that. The differences between them are much more structural. When you consider that Synchronous Technology has a big impact on sketching, the conceptual differences become even larger.
The one thing I will say right off the bat is that I like the SolidWorks way of adding items to toolbars better than Solid Edge’s. I like to select an icon from a list, then drag and drop it where I want it. The SE method requires you to find the command from a set of cascading drop-downs, then find the area of the ribbon where you want to put it, and then use the Add>> <<Remove buttons in the middle. I remember this from a ’90s version of Netscape.
Also, where SW (in the Tools>Customize interface) gives you a block of icons, SE gives you a linear list (cascading drop-downs). The rectangular block is less organized, but more space efficient. This probably belongs more in the interface discussion than the sketching function.
What is SE missing? Well, 3D sketch is missing. There is the Frames functionality, and it can draw lines in 3D space, but Frames in SE are done in an assembly (weldment equivalent in SW). I would like to see the 3D sketch capability added to parts. It took SW a long time to get 3D sketches to the point where they were only difficult to use (as opposed to impossible or frustrating). It’s my understanding that SW uses a different solver for 3D sketches vs 2D sketches, and the constraints in 3D sketches in SW are what makes it so unbearable. I’m not saying that SE 3D sketch equivalent is any better, being a noob and having no experience with it.
SW early on had this concept that you should be able to sketch with either the click-click or click-drag. And that worked well. You had a choice depending on your preferences or what software you had used before. Then they started adding things like the Enable Onscreen Numerical Input On Creation, which only worked for click-click mode. So. Solid Edge sketching works click-click. No games. It just works the way its supposed to, and you can count on it.
SW had a cool idea of having dimensions added immediately as soon as an item was sketched. At first I thought I would love this, but in the end, it turned out to be one of those things that you might want to use selectively, but not all the time.
In Solid Edge sketches, you can add numbers as you sketch, and it seems to flow well.
SW has Modify Sketch, as well as Move, Copy, Stretch tools. Again, duplicated tools instead of one thing that just works. SE has the Move, Copy, Stretch, Mirror, Rotate, Scale. Just one copy of each, as far as I can tell.
The reason I bring all of this up is that SolidWorks sketch workflow, like much of the rest of the workflow in the program, is all over the map. There are duplicated functions. No wonder they had to gut the software and start all over again. The Solid Edge guys seem to have done better homework, and much better housekeeping. The two software packages are the same age, yet SE just seems cleaner, much less sloppy.
SE doesn’t have Face Curves, but it does have Intersection Curve. It also doesn’t have the weird schizophrenia about sketches and curves that SW has. In SW, curves are kind of bastards. They follow different rules, and are generally harder to deal with than sketches. Also in SW, some sketch types are called curves, which I’m sure would be confusing to my counterpart, an SE veteran learning SW. Projected Curve is a curve, but Intersection Curve is a 3D spline. In SE, so far as I can tell, curves and sketches are treated about the same. In fact, what is called a Spline in SW is called a Curve in SE.
SE doesn’t have a parabola or a conic (but it does have conic fillet/blend option). Of course SW doesn’t have conics either, but the parabola has improved at some point over the last several years in such a way that it’s actually usable. SolidWorks just got the CtrlA for Select All in a sketch in 2012. I notice this is also in ST4, but I don’t know when it arrived.
But then SolidWorks doesn’t have Freesketch. Freesketch is a very cool tool, and I can see that it’s the kind of thing that some people will love and others hate. You can just drag your cursor to sketch a shape and SE interprets that as lines and arcs. It’s the quickest way I know to get a bunch of lines on the screen without clicking. I’m sure it’s a mainstay with the demo jock community, but I can see some practical use for it, especially for concept creation. I’ll bet with a Wacom tablet it’s really nice.
Freesketch, by the way is tough to find with the Command Finder. It’s in there, but you have to click the “Show matches outside environment” link. You can find Freesketch in the Help, but it doesn’t tell you where to find it. I just stumbled across it yesterday, and for some reason, today I can’t find it again. I’m sure it was on the Line dropdown. I eventually found it on the Line drop down in the Ordered mode after starting a sketch. Not sure if that’s obscure or if that’s just me. Why isn’t this available elsewhere? I couldn’t find it in Customize Ribbon either.
I got called out for saying SolidWorks Help sucked without giving examples. So here are some examples. SolidWorks Help has no Index, so if you know what you are looking for, you can’t just go to it. Solid Edge Help has an Index. In the SolidWorks Help, I can’t use the Back button programmed on my mouse, you have to use the special Back button on the SW Help interface. On Solid Edge I can use my mouse. Solid Edge has all the help in one location, on your computer. You don’t have to fool with multiple locations to get the same information like in SolidWorks. Also SolidWorks Help is cluttered with all sorts of stuff that’s not related to CAD, stuff I’ll never use, and when you do searches, you get stuff from all those categories that just dilute the quality of the search. If you need more reasons, refer to old posts on the Dezignstuff blog.
SolidWorks has Derived Sketch. Solid Edge has Tear Off Sketch, which I think is just a copy, not a linked copy.
And then you get to the really odd stuff in SolidWorks. The stuff that people tend to not use. There’s Rapid Sketch, which I’ve always thought was a bit of a disaster in SW, but it’s roughly the way things work in SE.
There’s Instant 3D in SW, which should have been more popular, but wasn’t. This is essentially a weak response to direct edit as a whole. It gives you that direct edit feel for some types of features. If you use it. And I rarely see people use it. It used to be turned on by default, I’m not sure how they do it these days, not doing many totally fresh installs. It’s usually one of the first things I turn off when sitting down on a new computer. I’ve seen a lot of users have it turned on, but never use it. Instant3D is actually a cool idea. But it’s a bandaid compared to Synchronous Technology.
Here are some more sketching topics I’m working on:
Best Practice in SolidWorks is something that serves the needs of the CAD, not of the design. Solid Edge ST4 has less need for imposing best practice type rules
Create a plane and move it freeform using steering wheel
Reorient the axis of a sketch when creating it by using the B and N keys (on a face with non-perpendicular edges).
Solid Edge users are less obsessed with referencing the origin. They also appear to not care much about “fully defined” sketches.
Right clicking/ESC gets you out of just about anything.
Reattach dimension by clicking on dim line then alt-dragging leader to another edge.