So I was at the Boston Area SolidWorks User group about three months ago, listening to a free technical presentation while eating free food and drinking free cold soda with my co-workers. (Yes, I’m trying to sell you on the idea of going to your local SWUG. It’s fun, you’ll make friends and you’ll learn something about SolidWorks.) The talk was about “4 ways to make a SolidWorks Assembly”, and while the presenter did an okay job laying out the four ways, I feel there are better examples to use, and better distinctions to be made.
For example, if I needed to make a cheap, functional robot out of existing parts to clean up after a global trash apocalypse, I would make something like this:
Yes, that’s a Lego Wall-E, because I’m pretty sure the original Wall-E image is copyright protected, and because it’s cool. Ironically, it also helps make my point. All of the Lego bricks existed in their final shape before the designer put them together, and none were changed by being used in this assembly. This is an example of Bottom-Up Assembly Modeling.
Bottom-Up Assembly Modeling is what we teach in our Essentials classes, the simplest to use, and the first one the presenter talked about. It’s nice to use when you’ve still got your SolidWorks training wheels on.
If, however, you desired the treads on this plucky robot adjust to the size of wheel hubs you design him with, that would be an example of Top-Down Assembly Modeling. This was the second method the presenter mentioned, and we teach it in our Advanced Assembly class because it’s too much for beginners to handle in the same week they’ve first seen SolidWorks. But it’s also so fundamental to machine design that I can’t imagine any real assembly NOT using it.
If you’ve ever drilled a hole in one part using another part’s hole as a location, you’ve used Top-Down design. If you’ve ever said, “this axle should always be 0.010 inch smaller than the hole it goes into”, you’ve used Top-Down design. This is fundamental to what designers do when creating machines, fundamental to using SolidWorks to capture your Design Intent, and a majority of SolidWorks users are afraid of it. But that’s a topic for another post. Enough for another three posts, actually.
So now we’ve designed a plucky little garbage disposal robot from existing pieces (Bottom-Up design), then made him smarter by having some of the pieces relate to each other in hole alignment or size (Top-Down design), but he still looks like a machine, like something cobbled together from separate parts. What if we wanted a robot that looked unified and whole, like it sprung from one overall idea? Something that, as it left our spaceship and scoured the Earth looking for signs of life, would also be smooth and elegant enough to attract the attention of lonely male robots?
Well, in that case I’d probably start with an overall defining shape. Here’s a simple revolve of a spline:
It’s smooth, elegant, but not much of a robot. Robots need moving pieces. So, if I sketch up a short curve, and then use the ‘Split’ command (Insert…Features…Split), my single elegant body is split into two bodies:
The Split command has the option to create separate children part files (which I didn’t choose here), but the main reason I used it was because the split it creates is zero-thickness. Even a thin-feature Cut Extrude would have SOME thickness, and I wanted my robot to fit together seamlessly. In case she’s in a fire, or outer space or something.
If you’re having trouble seeing the two separate bodies, this picture is clearer:
The yellow one will become the head and the purple one, the body. Now I do the same with another sketch and another Split feature to make the arms:
(Don’t mind the reflection of the environment there- it’s just a glitch with my graphics card and not copyright infringement.)
So now we’ve got a part with a smooth overall shape and separate head and arms, but I can’t apply mates to these bodies. I can’t easily move them around, nor make an exploded view in a part file, so what good is it?
If I now use the ‘Save Bodies’ command (Insert… Features… Save Bodies) my problems will be solved, and I’ll be using the Master Model Technique. This was the third way the SWUG presenter discussed, and can really give your assemblies some overall cohesion.
The Save Bodies command makes separate children part files like the Split feature can, but the reason I love using it instead is that it can also automatically put those children files back together in an assembly, in the same position they were found in the master part file! This is the key step to a lot of Master Modeling challenges. After running the Save Bodies command, I can make my robot do this:
Or even this:
…because now she’s in an assembly, where I can apply mates, exploded views, Move with Triad, all the good assembly tools. Better yet, if I go back and decide to change something about that first overall shape, like making it taller, or wider, or changing the Split sketches, the children parts will update and the assembly will update. I can also lock those children so they stop listening to their parent part, once they reach the age that they suddenly know everything. Or I can unlock them, so that they realize that tattoo may have not been a good idea after all. What I’m saying is that information can flow where I want it, when I want it!
I use the Master Model technique of creating an assembly whenever I want my overall assembly to look like it came from one idea, like it was planned ahead of time, or when I just want things to look sleek or cool because every part fits perfectly into the parts around it.
For example, if I had a clean black and white map of New England, I could put that map into a sketch and auto-trace over it to make a detailed extrude in under two minutes:
(What’s that, you say? You didn’t know SolidWorks could trace images in sketches to make 3D maps in just a few minutes? Then you must not have been at my SolidWorks World 2011 talk! Look up the Auto-Trace Add-in in the help menu.)
And then I could use Save Bodies again to make an assembly of states. Then I could realize that a lot of our Connecticut customers work in the aerospace field, our Vermont customers in either granite or alternative energy, our Massachusetts customers in the medical field, and alter the state parts to make something like this:
And THEN I could realize that since I was in an assembly, I could use the Motion Manager to make something like THIS:
So there we have it, the only two reasons in the entire world to use Master Model technique: to make the robot that will save human civilization a lot more attractive, or to make the state of Maine twirl. (Sorry Mainers. If I had more time, I would have made it dance!)