Winning the Battle with Projected Geometery in Inventor Sketches

Issue:

You find that your Inventor sketches often break due to geometry projected from other features. When those features are changed or deleted other sketches become upset and you end up spending a great deal of time fixing sketches. It's all very frustrating and is directly responsible for you having hit your co-worker in the back of the head with a stapler because you became so angry that you had to throw something. 

Solution:

First off, you're on your own with that stapler thing (less coffee might help). But you can keep your sketches lean and clean by adjusting your projected geometry settings. I'll share a couple of tips here that I use every day to work with projected sketch geometry. Including a tip I use for getting projected geometry to come in as construction lines.

Often times you'll get the following message when projected geometry used in a sketch becomes upset:

It may not always be clear what Inventor is trying to tell you with the Design Doctor, but when I see an error like that I know that what Inventor is really saying to me is this:

So the first thing I'll do to help this situation is go to the Tools tab and click the Application Options button. Then on the Sketch tab I'll make sure the Autoproject Edges For Sketch Creation And Edit option is NOT selected. Here is the result of a new sketch created on the top face with this option selected:

Here is the result of a new sketch created on the top face with this option NOT selected (the one green dot is the projected origin, controlled by the Autoproject Part Origin On Sketch Create option.):

So right from the start your sketch is much cleaner when you have this option turned off, and therefore much less likely to get upset by a change to some previous feature.

The next thing I’ll do is create a keyboard shortcut for the Construction Line tool, so that I can quickly toggle it on and off, as I Project geometry into the sketch. This doesn't necessarily help your sketches stay any cleaner, but it's a great tip I picked up somewhere along the way, so I thought I'd throw it in here as well. Go to the Tools tab and click the Customize button:

 On the Keyboard tab, you can select just the Sketch category, and then enter a key to use for the toggle of the Construction command. I use Q, because it's easy to find on the keyboard (note that the Customize dialog box has changed in appearance in later versions of Inventor, so the tabs shown here might not match exactly what you see, depending upon the version you are running) :

So now when I create a sketch, I can click the Project Geometry button, and then press Q on the keyboard so that the Construction Line tool is toggled on:

Then I'll click only the edges I want to reference in my sketch. Recall that projecting a face gives you a projected loop containing all of the edges, and selecting edges gives you just the edges you specify:

Then I'll press the Q key again to toggle the Construction Line tool off, and then sketch my new feature in. This feature will be a keyway centered on the circular cut. 

Notice how I sketch off to the side, without even trying to place it precisely. If you're an Inventor demo jock who places a premium on making things look super slick and automatic, or an Inventor user that obsesses over mouse clicks, you probably think I'm as crazy as the proverbial outhouse rat for even suggesting such a thing! But I do this because I don't want to accidentally place an automatic sketch constraint between my new geometry and the existing projected geometry, and because I want the visual feedback of watching my new rectangle get locked down.  If you're a new Inventor user you might find that sketching off to the side away from projected geometry will help you as well.

Here I'm placing a coincident constraint to precisely position the rectangle:

And then I'll add a couple of dimensions to lock down the size. And because I didn't end up using the 2 projected lines, I'll delete them.

The final part, after using Extrude to cut the keyway:

  

Sketch Constraints and the Eyeballing Game (slightly Inventor related fun)

If you've used Inventor for any length of time you've probably started to develop a "good eye" for sketching geometry at a relative proportion or scale. Sometimes when I apply dimensions to my sketch, I impress myself by just how accurately I've managed to get the sketch by just "eye-balling" it. Other times I'm not even close, though. Often times I purposely sketch things off center or skewed in one way or another, so that it is obvious to me what dimensions or sketch constraints I need to apply.

If you're a new Inventor user you might be employing the "eye-balling" approach inadvertently when you leave your sketches under constrained and/or under dimensioned. Of course this is not a good way to create sketches in Inventor (see: Inventor 101: Simple Fully Constrained Sketches), and you should (almost) always strive for a fully dimensioned and constrained sketch.

With these things in mind, I thought I'd share a link that provides a fun way to practice your "eye-balling" skills, and will likely make you more appreciative of your Inventor sketch constraints and dimensions.

The Eyeballing Game from woodgears.ca, prompts you to adjust a set of geometry for a given condition. For instance here the goal is to drag the lower left corner to make a parallelogram. The blue lines show my attempt, the green shows the correct position:

 

In Inventor I'd simply place parallel constraints to achieve this:

 Here was my attempt at setting a point equidistant to the edges of the triangle:

 

In Inventor I'd create a construction circle and then apply tangent constraints:

Here is my attempt at bisecting an angle:

In Inventor I'd add a symmetric constraint (or add angle dimensions):

Have a go at the The Eyeballing Game and you'll likely come away with an higher appreciation for sketch constraints and dimensions.

http://woodgears.ca/eyeball/index.html

Quick Hole Patterns with the Polygon Sketch Tool

Here's a quick tip for creating a hole pattern using the Polygon sketch tool.


The goal is to add a centered hole pattern with 8 holes:

 

To start I'll create a sketch on the part face to be drilled, then I'll use the Polygon tool found on the Draw panel of the Sketch tab. I'll set the number of sides to 8 and then place the polygon in an approximate location:

 

Next I'll constrain the polygon into place using dimensions and constraints. I'll place a horizontal or vertical constraint on one edge of the polygon to lock in the orientation:

Next I'll select all of the edges. I typically do this by creating a crossing window selection from left to right. Then I'll hold down the CTRL key and deselect the center point of the polygon since no hole is required there:

Then I'll use the Center Point tool found on the Format panel of the Sketch tab to toggle the points from a simple endpoint to center points:

Then I'll finish the sketch and click the Hole tool button. Because I have only one visible, unconsumed sketch present, Inventor automatically chooses the From Sketch placement method. And because my sketch contains 8 center points, the Hole tool automatically selects them:

And here's the result:

One reason not to use this method is that you can't take advantage of the Associative Pattern option in the assembly that allows you to place assembly components by referencing a part level feature pattern. So a little forethought in how the part will be used in the assembly will help. 

With that in mind I find myself using this trick a lot. Many times I'll do this with corner hole rectangular patterns created by offsetting a plate edge:

Inventor 101: Simple Fully Constrained Sketches

Issue:
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?)

Solution:
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.. wait...no. 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