Model A: Getting Started

Ok, we’re all back from Thanksgiving. I promised a while ago that I’d go through how I modeled the Model A model I created for the Happy Valley user group. So this is it. I’ll do this in a series of posts that cover the most interesting elements of the work.

Keep in mind that this model was not made for production data, it is primarily just a show model, and so I took some shortcuts with it that I wouldn’t take with a real production model.

Layout Sketches

Many people who ask about models like this start by asking “where do you start?” I can see where it would be difficult to envision where to get started until you’ve been through the process once or twice. Other people who do this kind of work might answer this question differently, but this is where I started:

In the end, the wheels were made as separate parts, so they were not driven by this sketch, but the fenders were. This sketch doesn’t include the cab, or the grille, or the engine, or the windows, or the width of the car, but it offered an overall scale for the model, and a place to start.

It may be dificult to see from the image, but the fender was created as a single spline, and then later split into three sections using the Split Entities tool. Notice that the spline has more points on it than you might consider ideal. This is partially to control wiggle around tight corners, and to try to keep the running board section of the spline as flat as possible. Flatness in splines with more than two points is one o the most difficult things to achieve. Flatness was measured using a curvature comb.

Very often, a complex model will start from more than one sketch. The other starting part for this was a footprint for the top view.

For those who weren’t around for the earlier post, this shape was created with a construction rectangle, then arcs were created at all four sides of the rectangle, and made into construction arcs, and then a Fit Spline was placed over all of the construction arcs, and the fit tolerance allowed for some blending on the corners.

Why didn’t I make the fender sketch offset from the middle plane? Is laziness a sufficient answer? To me, it didn’t matter. Since it didn’t matter and it was extra work, I just drew it in the middle. I didn’t really need a plane on the outside of the car, so I built one fender in middle of the car, and then moved it to one side (Move/Copy Bodies) and mirrored it (Mirror, using the Bodies to Mirror selection box).

Parametric moves like what would be required to move the fender with its plane and all the associated sketches are just very problematic in SolidWorks. To me, it is better to make what you want where it is easy to create it, and then put it where you want it. Moving the finished fender body doesn’t risk anything blowing up. Moving a plane and a set of associated planes and sketches risks blowing up each of the associated sketches. It’s just that simple. Entropy always wins, so start at a low state of entropy, and it does not increase naturally.

Reference Surfaces

When surface functionality was first added to SolidWorks, they were listed in the menus under Reference Geometry, much like planes and axes. Sometimes surfaces really are just reference geometry. One example of this can  be shown in building the cab of the Model A.

From the Fit Spline created in the second image above, I created a surface extruded with draft. The thing was that I wanted to create the cab with a bit of an angle at the bottom, and I wanted to control the angle. I wasn’t able to make this happen through any of the loft options. Sometimes you just have to make your own luck, especially with SolidWorks surfacing.

Here is the cab surface being created from the extruded surface to a sketch point. Yes, things like this happen in real world modeling, this is not just an academic curiosity.

You have several things to look at in this image. The first is that I loft from the edge of a reference surface to a point. The second is that by lofting to a point, I don’t get a pointy loft. The third is the use of the Normal To Profile option with the Point sketch. Forth is the use of the profile weighting. This is a really simple loft, but there is so much going on.

Tangency to a point makes the surface radiate out from the point, which is kind of opposite of what making a loft tangent to an existing surface at an edge does. It is usually used to cap off an open surface, or make a shape like the end of a toothbrush handle, in contrast to the end of a cigarette.

One portion of the truth is that you should try to keep your lofts simple. In the same way that splines with lots of points are difficult to control, lofts with lots of sections are also difficult to control. This loft is the equivalent of a two point spline with tangency and weighting at both ends making a transition around a corner. What splines do in 2 dimensions, lofts do in 3.

Using the weighting enables me to make the top “flattish”, and make the sides follow the drafted reference surface rather than bulging out in a big “pumpkiny” shape. It also makes for a sharper corner. There is a point where pushing the weighting numbers too far can cause an S shape instead of a U shape. The numbers run from 0 to 10, and don’t really mean anything exact. They are just relative weights.

Anyway, after the loft feature, there are a number of things you can do with the reference surface. Some people use Delete Body on it. This doesn’t really delete anything, but only hides it, and makes it unavailable after that point in the tree. Some people will simply hide it. You never know when you might want to reuse it.

I hope this was useful for you.