NX7.5: My First Class-A Surface p.1

This week we embark on what is bound to become a wild and mysterious journey through the magical wilderness of Unigraphics NX 7.5. As with any adventure, it?s best to start at the beginning, and we?ll be doing just that: if you?ve never used NX before, you?ve come to the right place. In this series we?ll be looking at NX from the vantage point of an Industrial Designer, emphasizing the tools and techniques that make NX a world-class tool for consumer products design. (See full article for video transcript.)

Video Transcript:

Lets create a new document by hitting [ctrl]+[n] on the keyboard, just like any other Windows application. This will bring up the ?New File? dialog that impatient click-masters like me are tempted to gloss over. Aspiring NX Junkies take heed: in NX, it is very important to name our model and assign a working directory BEFORE getting into the modeling environment. Once you?ve assigned a name and folder to your model, click ?ok?.

We are now presented with a brand-spankin?-new NX document, bare and naked as a new born babe but for the Datum Coordinate and World Coordinate Systems we see in the center of our 3D viewport. The rest of the interface is not only a little bit old-school, it?s taking up waaaay too much real estate on my diminutive recording screen, and hence totally jacking up my mojo. As it turns out, there?s a gorgeous alternative to this dinosaur interface by the moniker ?full screen mode.? Look over at the top-right of the 3D Viewport, and notice the little YouTube-esque full-screen button, and click.

Now that?s more like it. Somewhere on your screen you probably see something that looks very much like this, the ?Toolbar Manager,? wherein you?ll find tabs with a wide variety of fun and useful tools, gadgets, widgets, and whatnots. Left-clicking a tab reveals the tools underneath, and right-clicking displays a handy drop-down of the same. Notice that after right-clicking I can scrub my mouse over each tab to quickly view its contents at a glance. There are many more pre-made tabs available by right-clicking the empty space in the tab area and checking or un-checking tool groups to your cadjunkie heart?s content. I like to keep the toolbar manager docked at the top-left of my screen. Another interesting hint: notice that if I move my mouse down into the viewport and strike the [alt] key, a heads-up pop-under with the contents of the current tool tab pops up, thus saving us the trouble of moving all the way back up to the top of the screen.

At the top right of the screen I?ve positioned the ?Dialog Rail,? which we?ll discuss in more detail later.
Notice that in Full Screen Mode, we no longer have a menu bar at the top of the screen. Yikes! Don?t panic, my children. Click the NX icon at the top-left of the toolbar manager for access to all of the exact same menubar drop downs you?ll find at the top of the screen in standard mode.

Instead of a menu bar, you?re now given a ?Cue and Status Line,? which will basically help to walk us through various tools within NX by telling us exactly what NX is expecting us to do at any given time.

Now, most beginner tutorials would start out by building a cube or some such mind numbing nonsense. Hogwash! We?re industrial designers, after all. No, our first model will be a beautiful, perfect ?Class-A? quality surface.

The first step toward creating said surface will be to create some 2D curves beginning with the Right view. Right-click in the viewport, mouse over ?Orient View? and drop down to ?Right,? or hit [ctrl]+[alt]+[R]. Locate the ?Curve? tab in your toolbar manager. If it?s not visible, right-click in the blank area on the tab bar and select ?Curve? near the bottom. Under the ?Curve? tools we?ll find an ?arc? tool. It?s also available in the menubar under Insert > Curve > Arc/Circle.

This brings us to our very first NX ?Dialog,? dutifully attached to the ?Dialog Rail? I mentioned earlier. The dialog system is the heart-and-soul of the NX interface, and I like to take a moment of silence in respect for its greatness? Okay that?s enough. At the top of the Arc/Circle dialog box is a drop-down entitled ?type.? Tools in NX often have many sub-tools: rather than having fifteen top-level arc tools like Rhino, NX has opted for a single ?arc/circle? tool with many possible implementation options. Select ?Three Point Arc? from the menu. Notice that the ?Cue and Status Line? at the top of the screen is telling us what NX is expecting us to do next: ?Specify a start point or define the first constraint.? Also notice that in the Arc definition dialog the selection box for ?Start Option? is highlighted. Click in the viewport to define a starting point, and notice that the highlight automatically moves to the ?End Option? field in the dialog. Click in the viewport to define an ending point. Finally, NX asks for the Mid-Point, and we?re done! Almost: I?ve decided the arc is correctly positioned, but it should be a little longer. Notice the sphere and arrow icons at the endpoints of the arc. Dragging them will adjust the start and end points respectively, making it easy to change the cord-length of the arc without changing its curvature. Sweet! Now the arc has been created, but the tool is still active. To truly finish our arc, we have to click ?ok? to the arc dialog.

To return to a nice isometric view of our model thus far, hit the ?home? key on the keyboard. In your NX journey, if you ever find yourself lost in times of trouble, let the ?home? key be your guiding light. To navigate effectively in NX, you?re going to need a three-button mouse. If your mouse has a scroll-wheel, chances are it can act as a middle-mouse button simply by pressing it down. Dragging said middle-mouse button in the viewport allows us to rotate our view dynamically around a center. Use it to rotate the model so that we?re looking down on the XY plane, then hit [F8] on the keyboard to quantize the angle to a perfect top-view, then hit [ctrl]+[F] to fit our arc perfectly in the center of the viewport

This time we?ll use that old Class-A surfacing favorite, Insert > Curve > Studio Spline, or toolbar manager > Curve > Studio Spline. In the Spline Settings tab of the Studio Spline dialog, make sure that the ?Method? is set to ?Poles,? the Degree is set to five, and the checkbox for ?Associative? is active. In the ?Drawing Plane? tab, make sure that the ?View? icon is selected.

Because this is a ?degree-5? curve, we?ll need at least six control vertices to define the curve, defined simply by clicking each successive point in the viewport (1, 2, 3, 4, 5, 6). We can move points by dragging them, add points by clicking anywhere along the curve, or remove points by right-clicking and selecting ?Delete Pole.? Those of you who?ve used curves like this before may like to know that in the ?Analyze Shape? tab, you can click the ?Curve Analysis ? Combs? button to toggle a quick curvature analysis on and off as you draw your curve. You can click or box-select multiple control points to drag them all at once, and you can [shift]+click vertices to remove them from selection. When you?re finished, click ?okay? to the Studio Spline dialog, and our second curve is complete.

Hit [home] on the keyboard to return to the isometric view, and we?re ready to create our very first NX surface. But before we get to the main show, we?ll need a couple of simple ?support surfaces? to help us out. There are three easy ways to activate the ?Extrude? tool in this case, and you may choose whichever seems most intuitive to you: 1) Menubar > Insert > Design Features > Extrude; 2) toolbar manager > ?Feature? tab > Extrude; 3) my personal favorite, hit the [X] key on the keyboard. No matter which method you choose, we?ll be asked to select a curve to extrude, and a direction in which to extrude it. Since our curves are planar, NX infers that we want to extrude ?normal? (aka ?perpendicular?) to the curve plane. If we wanted to change the direction of the extrusion, we could explicitly choose a different direction in the ?Specify Vector? field. For our purposes, the default values will be perfect. In the ?Limits? tab, we are given a ?Start? and ?End? Distance parameter. We can adjust the values by typing a value in the field, or by interactively dragging the sphere and arrow icons on the extrusion itself. Notice that the extrusion can go in either direction, and does not have to start at zero! I?m going to extrude the Studio Spline downward by a few millimeters, with a start distance of zero.

Since I want to make another extrusion with the Arc, instead of clicking ?OK? to exit the tool, I?ll simply click ?Apply? to finish the current extrusion, but immediately fire off a new one as well. Notice that NX is again asking us to select our section curve, so I choose the Arc, adjust the direction and distance, and click ?OK.?

It doesn?t take a nucular skientist in a libary to know that the cadjunkie loves him some conics, and as such it should be obvious that our very first Class-A surface in NX should be a conic section sweep. Menubar > Insert > Mesh Surface > Sections > Section Fillet Rho, or just look in the toolbar manager > Surface > Section Surface, and select Type > Fillet Rho. There are a million ways to define a conic section surface, and this one uses a start guide, end guide, start tangency face, end tangency face, and what?s known in the Class-A surfacing world as a ?spine? curve. We?ll get real cozy with spine curves in NX: understanding spine curves is absolutely essential to creating high-quality surface geometry, and it?s a travesty that packages like SolidWorks completely omit them. But more on that in a future video. Make sure that Section Control > Rho Law Type is set to ?Constant,? and ?Value? is set to ?.6,? then click ?OK?.

Viola! Our very first Class-A surface in NX, and life is good.