This huge drawing will probably always be a work in progress. Why? Because until such time as I get hold of exact technical details of every single part, some parts will have to be created using incomplete technical data or if I can find nothing, then as a believable figment of my imagination.
To create a 3D illustration of the complete headlight, I needed to find an example of what the original headlight bulb for the Bentley Blower must have looked like. Nowhere could I find such a picture. Eventually, I found an image via Google of a vintage automotive headlight bulb which, for want of a better example, would have to do. This is an example of the beauty of using AutoCAD and Autodesk Inventor to make such a complex 3D technical illustration. Since each part is constructed in 3D and then assembled into a component which in turn is assembled into a larger component which becomes part of a larger component… and despite the entire car being modelled in such detail, the object can easily be re-drawn and swapped out when a more accurate example is obtained. In the meantime a reasonably believable headlight bulb can serve as a placeholder – the imaginary 3D part is based on an existing object and modified so that it fitted the meagre data that I did have at my disposal.
The Size of a Tiny 3D Part
The biggest problem with such a small part is to get its size more-or less correct. This is actually a symptom of a larger problem – where to get some reference dimensions from which was discussed in this post.
I began by drawing a cross sectional profile of the headlight in AutoCAD using the rough blueprint as discussed in the previous post. The second image that you see in the background is a picture of a vintage headlight:
The blended curves were constructed in AutoCAD on their own layer using many Tangent-Tangent-Radius Circles and trimming. I couldn’t find a decent orthogonal photograph of the headlight , so I had to construct one using these 9 pictures as references. Notice how they all are different – from different year-models and variations, but I could still use them to give me a good idea of what the real shape must look like:
Once the outer shell of the headlight housing looked right, I could then see how large to scale the image of the bulb itself (using the Scale – Reference Command). The AutoCAD profile drawing now looked like this:
Until I get my hands on a more definitive drawing of what the bulb actually looked like, I will use this as a basis.
Into Creative Technical Fantasy Territory – The filament…
Although the basic image that I used doesn’t show it, I decided that the inside of the bulb must have an impressive filament (to go with such an impressive car). I decided that we needed a centre tungsten filament curve with incandescent spirals on either side:
The Positive and Negative terminals at the base of the bulb would need to be connected to the actual incandescent filaments via thin wires that also supported the filaments in their optically optimal positions. As in any light bulb, the wires would be held apart and in position by a glass support holder. The glass was built in Autodesk Inventor using two lofts each loft being controlled by three shared cross sectional sketches and one sketch for the each individual loft. The final individual sketches would simply be circles slightly wider than the wires in diameter but located at different “heights” (different Z co-ordinate values) because they would realistically end at two different elevations. The following images will make this a little clearer.
The second loft used the identical base profile and the other unused cross sections of the second and third sketches. The final sketch was located at a different elevation to it’s corresponding sketch for the first loft:
The combination of the two lofts looked like this:
To finish off the glass holder, I filleted the edges between the two lofts and changed the material properties to Glass:
The Filament Structure for the 3D Model
The two supporting wires and the centre filament were simply created using a 2D Sketch (copied and pasted from the AutoCAD drawing) for the path and a small circle in a second sketch for the sweep profile.
I learnt the hard way to always fully constrain a 2D sketch. However, in a case like this it would take a quite a while to manually insert every parametric dimension. So I simply put in the major dimensions that are important, and simply allow Inventor to automatically dimension the remainder. This can result in an ugly sketch but if I need to change something I can then manually remove as many of the automatically created dimensions as necessary and put in new ones.
The end result looked like this:
The side filament holders were created using a 3D sketch and sweeping two cross-sectional wire profiles:
The Spiral Filaments
The spiral filaments were profile sweeps created in a 3D sketch using a path made up of:
- A short collinear line leading out from the open ends.
- A helical curve
- And a spline curve to join them with tangential constraints
I made the sweep profile diameter just a touch smaller than the supporting wire structure:
The second spiral filament on the opposite side was created simply by making a mirror image.
The Brass Bulb Base
The remainder of the light bulb 3D model is very straightforward. A 2D profile of the base was copied from the AutoCAD drawing and pasted into a new Inventor 2D part sketch. The sketch was then fully constrained. The profile was revolved about the x axis:
The edges of the solid were then filleted. (It’s better to do a fillet on the solid rather than in the sketch):
Using two more sketches, 2 mounting holes and a ceramic base were added:
I then added terminal blobs by extruding an ellipse in a new sketch, filleting it and finally mirroring the terminal blobs. The material was changed to chrome:
The Glass Balloon
I created the glass balloon by copying the balloon profile from the AutoCAD drawing and pasting it into a new part sketch in Inventor. The sketch was revolved into a balloon solid and simply hollowed out using the shell tool. The material was changed to glass.
The Light Bulb Assembly
Now with the three parts completed:
- The Filament structure
- The Base
- And the Glass Balloon
I could at last assemble the parts together. There are many ways to do this and the right way for you might not be the most intuitive way for me. I decided to mate the brass base with the filament holder using the UCS constraint set. I created a UCS on the top flat surface of the brass base with its origin on the centre axis and X direction pointing along it. I created a workplane to parallel to the top flat surface to hold a sketch with a point to indicate the X direction and a sketch on the top flat surface to hold a point to indicate the Y direction:
The UCS for the filament was created in a similar way:
The two parts were then constrained together with the Constraint Set option to produce:
Finally, the glass balloon was attached with a simple Mate and Angle constraint: