IMPROVING YOUR PRO/E® BATTING AVERAGE

BENNY: Hey, Bruce, got a minute?

BRUCE: Sure, Benny. What’s on your mind?

BENNY: Besides lunch, you mean? Well, I was working on a new design yesterday and started thinking about some of the stuff Pro/E can do to make the job go easier and faster.

BRUCE: Easier and faster sounds pretty good. You sure you weren’t thinking about the Braves losing last night instead of that new design?

BENNY: Sure I’m sure. For example, how about Axis Point in Sketcher? Axis Point lets you create an axis in a protrusion or extruded cut where Pro/E would not normally create one, like if you draw a flange that will have holes or other features at the centers of the corner rounds. Axis Point keeps your model cleaner and prevents making extra features, and that’s good, right?

BRUCE: That’s right, Benny. So…?

BENNY: Just pick Sketch > Axis Point from the menus, and you can place an axis point on the centers of the radii. Those axes will be internal to the sketch, which saves dimensions and meets the design intent. Axis points don’t have to be on something; they can be dimensioned to other geometry in a sketch.

BRUCE: Tell me more.

BENNY: Here’s something in Sketcher that I’ve used a lot: Edit > Replace. It’s handy when you’ve completed most of a 3D model including rounds and chamfers, which, as you know, typically reference edges. For example, let’s say you vertically extrude a sketch of a rectangle and then round the four vertical edges. Later, you decide that one of the four sides of the original sketch should be an arc instead of a line. Sure, you could select Edit Definition for the sketch, delete one line, then sketch an arc, but you could cause the round feature to fail because of missing (that is, old) references. Instead, you should select Edit Definition for the sketch, but first sketch the new arc, then use Edit > Replace, select the arc, and then select the line. Doing this tells Pro/E to replace any references to the original line and its vertices (its end points) with the new arc and its vertices.

BRUCE: How about Edit > Convert To…in Sketcher? Sometimes, you want a perimeter instead of a dimension like a radius. If you pick on the item to be controlled by its perimeter, select Edit > Convert To > Perimeter, then pick on the radius, the radius or other dimension has “var” added to the end of it to indicate that it is a variable item now. Meanwhile, a new dimension is added that ends with “perim.” From there, you can change the radius by specifying the length, or perimeter, of the item.

BENNY: There’s one in Drawing that’s so familiar, it’s easy to overlook. It’s when you do Dimension in Note. Let’s say you have a thin, blow-molded part and you’d like to specify the wall thickness in a note in your block of notes. In this case, the wall thickness is probably specified in a shell feature. To make it work, Edit the feature so the dimension is displayed, then use the Info > Switch Dimensions menus to show the symbolic name of the dimension, for example, “d4.”Now, somewhere in the note on your drawing, just add “&d4.” That way, if you or someone else changes the 3D model file, any dimensions shown in notes on your drawings will automatically show the new values.

THROUGH POINTS ON SURFACE: Use this option before
specifying tangency, to ensure that the curve you have
created will lie in the surface.

AXIS POINT IN SKETCHER: This option lets you create an
axis in a protrusion or extruded cut where Pro/E would not
normally create one.

BRUCE: Faster, easier…and more foolproof. That’s a pretty good combination.

BENNY: And here’s something even more useful: Number of Decimal Points. In Drawing, to change the number of decimal points shown in a note when using a parameter, you can append [.x] after the &symbolname, where “x” is the number of decimal digits you want to show.

BRUCE: That’s pretty cool, but how about Sub/Superscript in Drawing? To put text in a note in superscript, just place @+ in front of it, and to make it subscript, use @-. To return to normal script text, use @#. You can use this feature when referencing the area or volume of a part. It looks a lot better than spelling out the units or using ^.

BENNY: There’s something else I should mention. It’s in Drawing, and it’s called Overwritten Dimensions.

BRUCE: Overwritten, as in you messed up?

BENNY: Nope, not me, never, but you can overwrite a created dimension on a drawing. Just be very careful when you do this. In fact, the only time I do this is in a max or min case. For example, I might want a minimum wall of 0.75”. I don’t want my nominal model to have that thickness because if I tool from the 3D file, 0.75” becomes my nominal, and the tolerances could put it below that. So, instead, I may model it to 1.00”. In the drawing, I create a dimension for that, then edit the dimension text from “@D” to “0.75 MIN WALL@O.” The @D means it’s a dimension. Changing the D to O means you are overwriting that dimension.

BRUCE: Let’s talk about a negative Shell feature in 3D Part Modeling. A common use of the Shell feature is to hollowout a solid shape, and to do that you key in a positive value for the shell thickness. However, what if you’re designing a cover, a boot, or some other part that needs to fit over something? All you have to do is model a solid shape that represents the “air inside,” then use a negative value for the shell thickness.

BENNY: I always think positive, but that makes sense. Here’s one you may like using,

BRUCE: Through Points on Surface. You know how we make a lot of curves in our models to control certain geometry. Now, if I create a curve through points using points on a surface, that curve may not necessarily lie in the surface, as you can see in the figure, even if I specify tangency on the ends.

BRUCE: I’m all ears. I’m running into that on a new part I’m working on.

BENNY: OK. If I select the points, and then, before I specify tangency, I go to the Curve dialog box and pick on the Attributes to redefine, I get a menu called CrvType with Free and Quilt/Surf as options. After I pick Quilt/Surf and Done, Pro/E prompts for a quilt or surface, then it creates the curve so that it is always in the surface. If you are using a Quilt, just use Query Select to make sure you get the quilt and not just an individual surface.

BRUCE: Good stuff, Benny, but I just noticed that we’re out of space. Let’s come back to this in another issue.

BENNY: I’m gone. How about buying me lunch?

If you have questions about Pro/E or any other design engineering topic, please email Benny and Bruce at benny&bruce@rlhudson.com.

Pro/E® and Pro/ENGINEER® are registered trademarks of Parametric Technology Corporation (PTC).

Solutions 3Q08

IMPROVING YOUR PRO/E® BATTING AVERAGE