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BENNY & BRUCE
Sketching Made Easy
(or, How to Shorten Design Time Without Sacrificing Accuracy)
by BENNY FOREMAN & BRUCE SUMPTER
Benny: Let’s talk about Sketcher Mode. When I taught classes, I always felt it was the most important topic, because you spend probably thirty to forty percent of your time in there, and it has a lot of power that people may not be leveraging to the fullest.
Sketcher
basics: And shoot us an e-mail if
you
have suggestions that
we might share
about how
to get the most out of Pro/E.
You can reach
us at
benny&bruce@rlhudson.com. Pro/E is a fantastic
program, so
get in there and create great things
with it!
Bruce: Yes, I’m hoping to learn something today! One of the things I’d recommend is that everyone try to keep their sketches as simple as possible. You don’t want to sketch in features that you can build in later, such as rounds or chamfers. Anything that could go away, you don’t want to sketch in because the design may later dictate that you don’t have that chamfer, and it’s a lot easier to just delete that chamfer feature than to go back and edit the sketch.
Benny: And don’t dimension to things that are likely to change.
Bruce: As much as possible, I try to dimension to datum features, datum planes, datum axes. Hopefully those won’t go away. The main thing is, keep it simple.
Benny: Simple is good, but don’t sacrifice design intent. Dimension features to what they are related to. Just remember, surfaces and datums are more stable than edges.
Bruce: One of my rules of thumb is, if I have more than ten dimensions in my sketch, then it may be too complicated, and I might look for ways to break that up into two different revolves or two different extrusions.
Benny: And try not to have redundant dimensions.
Bruce: One of the things I like to do is try as much as possible to use dimensions you would show in the final drawing. That way, you’re not recreating anything later. If I have a dimension from, say, one edge to another edge that I know I need to show in the drawing, I go ahead and specifically call out that dimension in the sketch.
Benny:And placement of the dimensions in the sketch matters, too.
Bruce: Absolutely. Wherever you place a dimension in your sketch, that’s where it will show up when you get to your drawing and show dimensions. If I know I want to show certain dimensions on one side of the part, I create them on that side of the part.
Benny: One place where I worked, we were doing nothing but downhole tools. We set up a revolved cut, and we wanted to show the dimensions on one side of the drawing, but they wouldn’t show up there because they were created on the other side. So, we made it a practice to create all of our external features above the centerline, and all of our internal features below the centerline, so on the drawing the dimensions showed up where we wanted, and that kept things nice and orderly.
Bruce: A lot of people know that they can create relations within the part itself and within assembles, but in Sketcher Mode, you can also create relations between dimensions. If one dimension always needs to be, for example, twice as big as another dimension, you can set that up in the sketch.
Benny: And that keeps your model even cleaner if you build the relations in Sketcher. That way, you don’t end up like my family tree, with lots of tangled branches.
Bruce: Okay…
Benny: Also, I suggest getting used to the constraints sub-menu, which lets you define things like perpendicularity, parallelism, symmetry, and equality. Use those as much as possible. Build in those relationships instead of adding extra dimensions. If you’re sketching rounds, and they’re all the same, instead of having each one dimensioned separately, take advantage of constraints for equality and make them all the same. If you have to make a change later, you only have to change one instead of having to change all six or eight or whatever.
Bruce: That makes me think of using construction features when sketching. Construction features are things like an axis point, or a centerline; helpful tools that make the design work easier. In many sketches, I have a centerline, and that’s one of the things I have a mapkey for. I touch the “C” on my keyboard and I immediately create a centerline, which, again, is used a lot for symmetry. You need a centerline for revolved sketches.
Benny: We should probably talk about defining and using mapkeys in more detail in another column. That’s a great topic. But your point is right on; construction features are there to help you get the dimensions you want. I use construction circles a lot where, for example, I have a series of protrusions sticking into a part and they all need to line up on a diameter. And I use construction points to show me theoretical sharps, then use them as a guide to help me dimension what I want for the drawing.
Bruce: Normally when I create a construction feature, I just sketch a normal line or circle, then right click on it and use the pop-up menu to turn it into a construction feature.
Benny: Or you can select the centerline option from the fly-out menu for lines, then just sketch the centerline directly. Either way works. But the great thing about a construction feature, such as a construction circle, is that it doesn’t actually create any real geometry; it’s there solely as a reference tool to help you properly dimension what you want.
Bruce: We’re almost out of space. To sum up: Keep your sketches as simple as possible. Think about where you want dimensions to show up on your final drawing, and place them there in the sketch. Build relationships between dimensions where helpful. And take advantage of constraints and construction features to make your dimensioning easier.
Benny: And shoot us an e-mail if you have suggestions that we might share about how to get the most out of Pro/E. You can reach us at benny&bruce@rlhudson.com. Pro/E is a fantastic program, so get in there and create great things with it!
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