Designing a Bass Guitar in SOLIDWORKS
Last month, I took on a SOLIDWORKS challenge: I wanted to create a 3D model of a bass guitar assembly. I have the physical object (a red bass guitar) so I implemented a strategy which uses photos as part of the design process (which I wrote about previously in this article). I also decided to livestream the entire process so that anyone in the SOLIDWORKS community could follow along and design a bass guitar of their own. You can see the video playlist here.
We covered a lot of material in this design challenge and today I’d like to share three of the more interesting areas of this project:
- Adding paint to the body.
- Running the electrical wiring (without using SOLIDWORKS Routing).
- Blending the neck to the headstock.
My hope is that by the end of this article, you’ll have some new tricks to use when facing similar design and modeling challenges in SOLIDWORKS.
Adding Paint to the Body
Guitars are often manufactured by first carving, sanding and painting the wooden body. After this process is complete, additional machining takes place to remove additional material. Pockets are machined into the painted body for things like the pickup cavity, neck pocket and the electronics area. Similarly, holes are often drilled into this body after it’s been painted.
This will leave us with a two-tone result, with one appearance representing the paint and another representing the machined (unpainted) wood. I wanted to capture this effect in my SOLIDWORKS model, and I decided to do it using the surfacing command Offset Surface.
I first created the basic shape of the guitar body using boss-extrude, cut-extrude and a series of lofted cuts to remove material and create the scalloped shape of the body.
I then used the command Insert > Surface > Offset and created an offset surface with a distance of 0.010”. I used the “Select Tangency” command (found in the right click menu) to quickly select all the faces of the body which are tangent to one another.
Once I had this surface offset at 0.010” I was able to use the command Insert > Boss/Base > Thicken and assign a wall thickness of 0.005,” thickened to the inside of the newly created surface.
Pro Tip: I find that having this small gap (0.010”-0.005” = 0.005” gap) helps to avoid some graphical anomalies that occur when you create thin surfaces directly on top of other solid surfaces.
After creating this thickened solid body to represent the paint, I assigned an appearance of candy apple red to the body and was very happy with the results.
The cool thing about this technique is that I can roll these two features (the surface offset and the thicken solid body representing the “paint”) to the bottom of the tree, rollback above these two features and continue designing the remaining features of the wooden guitar body.
I can add pockets and holes and any other features to the body and when I roll forward these pockets and holes will automatically be cut into this offset surface, leaving me with the perfect results.
Running the Electrical Wiring (without using SOLIDWORKS Routing)
The guitar used in this project has a relatively simple wiring harness comprised of a pickup, a potentiometer, a 3-way switch, an output jack and a ground wire running to the bridge. In spots like this, launching and configuring SOLIDWORKS routing is not necessary (plus I know there are a lot of users who don’t have access to SOLIDWORKS routing). So, to create these wires I utilized a “Stub and 3D Sketch” technique.
I started by positioning these components in the correct locations and mating them to the wooden body of the guitar. As we can see in the above image, the appropriate pockets and holes for the electronic components and wiring have been machined into this body.
Next, in each of these electronic components, I created one or more “Stub” sketches. A “stub sketch” is a simple sketch, usually just short line, which is created at the location where the wire connects to this electronic component. In the case of this 3-way switch (shown above) we can see that there are 2 “stub sketches,” one for the red wire connection and one for the black wire connection. After creating these sketches, I used the Sketch Color function in SOLIDWORKS to change the color of each sketch, which helps with identifying the different stubs and what they represent.
Back in the assembly, I was able to show all these “stub sketches.” This sets me up nicely to create my electrical harness using 3D sketches to connect the stubs. I started by creating a 3D sketch and using Convert Entities to convert two of the red stubs from the electronic components. These two converted entities represent the two ends of a single red wire. While still in this 3D sketch, I created a spline between these two short converted entities and assigned a tangency constraint to the spline at each end. Lastly, I create a sweep using the appropriate wire diameter and then color that sweep red.
After running the first wire, I was able to repeat, repeat, repeat.
Blending the Neck to the Headstock
One of the most common questions I get from students is “how do you blend one area to another area?” such as the neck of the guitar into the headstock. This is one of the more challenging parts of this exercise. The approach I took was to create the neck as one body and the headstock as a second body.
This multi body approach set me up nicely for a blend, using a Loft command to bridge the two bodies. Since I wanted the loft to have a smooth transition, I decided to create a larger gap between these two bodies.
To create this wider gap, I made two cuts, one on the neck body and one on the headstock body. I was trying to leave enough room to create a smooth curved blend region, with a smaller radius on the top and a larger radius on the bottom. That is why I created the cuts at an angle.
After creating this gap, I needed to modify the faces of the headstock. I wanted the transition to be coming from the smooth faces on the bottom of the neck and blending into a set of smooth faces on the headstock. Currently, the headstock has sharp corners, so I needed to do some filleting to smooth out these corners.
After smoothing out these edges, I was almost ready to loft. But first, I needed to make sure that each of the profiles had the same number of edges. The flat face of the headstock had a total of six edges, but the flat face of the neck had only two edges.
When lofting, I always try to work with the same number of edges going around each face (or profile). If there are a different number of edges on each face, SOLIDWORKS can run into issues with the loft twisting and/or ending up with an undesired result. So, I created two planes in the neck area and used these two planes to create two Split Lines along the side walls of the neck. That let me break up the elliptical edge of the neck into six edges.
With an equal number of edges on each profile I was ready to begin the Solid Loft command.
To begin the loft command, I selected the end face of the neck as Profile 1 and the end face of the headstock as Profile 2. I always take care to choose each of these profiles in a similar location, to avoid twisting in the loft.
In the above image, we can see that I selected each profile at a similar location—the upper corner of each face. I also like to unselect the option for “Merge Tangent Faces,” which can sometimes help to ensure that the endpoints of each profile are properly connected.
This loft preview looked pretty good—there was no twisting or anything bad about the loft—but it also looked too straight and flat. I wanted a smooth blend from the neck to the headstock, so I edited the options for “Start/End Constraints.”
By choosing the option for “Tangency to Face” for both the start and end faces of our loft, I was instructing SOLIDWORKS to smooth out the transition of the loft, by making the outside faces of the loft tangent to the outside faces of the neck and the headstock. This tangency option worked out great.
Even if you are not a guitar player, this exercise is a useful way to explore a lot of great functionality in SOLIDWORKS, including:
- Using an offset surface to emulate a part which is painted/finished, and which has machining operations performed after the painting operation.
- Creating basic wiring without utilizing the SOLIDWORKS routing add in.
- Making a loft smoother by making sure each profile has the same number of entities and by using the Start/End Constraint option of “Tangent to Faces.”
I hope you found these tips helpful, and I hope you’ll find some areas in your work where you can utilize these techniques to save time and get fantastic results.
About the Author
Toby Schnaars (AKA: TooTallToby) has been a SOLIDWORKS user, instructor and enthusiast for the past 20 years. He has fielded over 10,000 tech support cases and has instructed over 200 SOLIDWORKS training classes. He has earned the ranks of both Certified SOLIDWORKS Expert and Elite Applications Engineer (CSWE + ELITE AE).
Toby regularly posts videos of SOLIDWORKS tips and tricks on his YouTube channel TooTallToby.