Thursday, March 3, 2011

Inventor 101: Simple Fully Constrained Sketches

You've been using Inventor for a while now, but you find it frustrating and find yourself spending almost as much time fixing your sketches as you do creating them. You've been told that you should always fully constrain and dimension your sketches, but when you try it becomes overwhelming, as Inventor seems to want waaaaaay too many dimensions! So you just create your sketches as you see fit, but then sure enough, if you try to change one minor thing, the whole sketch falls apart. Inventor sucks! (right?)

Consider these "from the trenches" best practices:

  • Be nice to your sketches: stop trying to cram everything into one sketch, they don't like it and will become rebellious. Instead of making one sketch responsible for 12 features, start with a simple base sketch, create a base feature from it and then build on it. Your sketches will thank you for it.
  • Think inside the box: I create every sketch I can starting with a rectangle. Even when I'm creating complex curvy stuff, I still start with a rectangle. Typically this is just a construction bounding box, but it helps me add structure to the sketch.
  • Be lazy: (when's the last time somebody told you that was a best practice?) Only create as much line work in a sketch as you can constrain and dimension easily. If getting your sketch fully constrained turns into work, your sketch is too busy. 
 Let's see these concepts in action:

Here is a base flange. This should be easy enough to create, right?

First let's look at how many users would approach this.
  • Create a rectangle (good job).
  • Base this rectangle so that it is centered on the part origins (good job).
  • Add every other feature this part has to the sketch (good job... what.. Bad, this is bad.

Why is this bad? 
Because even with the jumble of dimensions already present, Inventor requires 121 more dimensions to be fully constrained (this might actually be sketch constraints and dimensions combined).

A sure fire way to add too much complexity to your sketches is to add fillets or chamfers at the sketch level. I know, I know: "you luvs you some fillets and chamfers", but there be will time for those later, as placed features, not as sketch based features. The same thing goes for patterns and mirrors: don't do them in the sketch, create these as features.

Q: Why does Inventor have these things in the sketch tools if you shouldn't use them?
A: Okay good point. There are times when you must place fillets, chamfers, patterns, etc. in a sketch, due to specific work flows or tools to be used later in the design. But as a rule avoid these things in sketches most of the time. 

Okay, so here we go. This is the battle tested, from the trenches, best practices, approach:
  • create a base rectangle
  • constrain it around the origin (in this case using a diagonal construction line)
  • fully dimension the sketch
That's it! Sketch complete. (good job)

Next: Make it 3D already!

Okay, now let's create another simple sketch, based on the first feature (the edges of the first feature have been projected into the sketch).

I know you're tempted to add 99 more lines and 283 more dimensions, but let's move on. Come on now, step awaaaaay from the sketch... slowly, no sudden moves... that's it... 

Now cut the base feature with this second sketch.

Okay, now we're going to create another sketch and ... yep you guessed it, create a rectangle dimensioned and constrained to the projected edges of the existing features. (I've added a center point to the midpoint of one edge of the rectangle in order to have something to grab for the center dimension.)
 Make it 3D!

Next...yep, a rectangle. Dimensioned and constrained to the midpoint of the existing edge (the edge has been projected into the sketch).

Extrude cut. 
And were moving right along.

Now let's get "crazy" and add a Full Round fillet feature.

Next, use the feature Mirror tool to "copy" the protrusion and the fillet.

That was fun, huh? 
Alright, you can do it again:

Okay, I know you've been itching to round those corners since step one, so go on,  have fun adding some fillets:

Well, there you go, simple sketches rule the day!
And you might have noticed, the number of dimensional inputs was less than 20 compared to over 121! 

You might also have noticed we never used the line tool! Believe it or not, that's far more common than you might imagine.

Although this approach might seem dumbed down or too "mickey mouse" for you, in reality you'll find that most experienced "expert" users of Inventor (and other 3D modelers) will employ a similar approach. Keep in mind you will have plenty of opportunity to challenge yourself with complex parts that demand more complex sketches as you create designs. But if you use this approach for most of your work, you'll find yourself spending more time and energy focused on designing and less on drafting.

Want to practice these concepts?
You can find 24 sheets of detailed part drawings for practice in a PDF at this link:

Part Modeling Practice Drawings for Inventor