Advice on PCB Design/Manufacture

[GüdPedals]

Hello, all!

I need some advice on small batch pcb design/manufacture. I want to get some pcb's printed for a pedal I've been making, but I don't know the first thing about pcb design. I've been messing around with Eagle, but my problem is potentiometer spacing. For aesthetic reasons, the placement doesn't follow a typical straight line or grid layout. It's easy enough to accomplish with perf/vero board where I can just shift things around if I need to, but arranging a pcb layout is a nightmare with no experience or anything to reference. I don't want to put in an order without knowing for sure it will line up with the enclosure.

I'm getting pretty discouraged from doing it myself. Could I just send an empty enclosure to a pcb design firm and have them do it?

[Marcos - Munky]

For the correct spacing and placement, you can use madbean library for eagle, you can find libraries for the enclosures and pots. Also, you'll need to measure the exact position you want them on the enclosure.

Don't know about pcb design firms, but if you don't want to do the layout by yourself, you probably can find somebody who can do it for you.

[ElectricDruid]

The way I make sure that my enclosure drilling lines up with my PCB is to take a copy of the PCB file and then replace the pots with drill hole symbols that I can print out. I have special "components" set-up that are just a crosshairs symbol on the silkscreen layer for this purpose. Anything else that needs a hole in the enclosure can be treated the same way - LEDs, switches, etc. All the other parts and eventually the PCB itself can all get deleted. The resulting file is a drill template I can print out and stick to my enclosure, and since the holes were lined up on the actual PCB itself, it's bound to line up even if I didn't measure anything or used irregular spacings.

HTH,
Tom

[kraal]

Hi,

I'm using Kicad and here is how I do things:
- create footprints for the parts that I need to be placed correctly (i.e. for potentiometers, I place the origin/center where the center of the shaft is, and show it as a target. This eases placement)
- stick to a set well defined grids (for instance I mainly use 1mm, 0.5mm, 0.25mm, 0.125mm)
- measure the enclosure, draw on paper how I want things to be arranged, place the components in Kicad on the PCB (middle) then move them (to the top, left, right, bottom) based on the measurements I've done.
- make sure that spacing between pots is sufficient (when a knob is placed on the shaft -> more measurement)
- use the drawing layer to sketch the boundaries where the PCB is supposed to go to make sure I've made no mistake.
- verify in 3D that things look like what I'm expecting.
- then when I'm sure that everything's fine I order the PCBs.
- before drilling I apply the measures on the enclosure (manually or using the drawing as a drill template).

It takes time, but it works.

Here are some examples:

PCB with drawing showing placement measures and dimensions:


PCB with drawing showing inclusion of PCB in a 1590B enclosure (and where to drill holes):


PCB with drawing showing inclusion of PCB in a 1590BB enclosure (and where to drill holes):


3D image of a PCB with many potentiometers:


Hope it helps.

[GüdPedals]

All the other parts and eventually the PCB itself can all get deleted. The resulting file is a drill template I can print out and stick to my enclosure, and since the holes were lined up on the actual PCB itself, it's bound to line up even if I didn't measure anything or used irregular spacings.

That's a pretty clever (and simple) way to go about it... I'll definitely give it a go.

Thanks for the input!

[GüdPedals]

It takes time, but it works.

Wow... That's pretty extensive. Makes sense though. I'm still very much learning the software, but I assume EAGLE can do all of that as well.

I appreciate the insight though! Very thorough.

[kraal]

Hi again,

Some more information:

In KiCad, you can create footprints for your enclosures and other "floating" hardware (connected with wires).
You can define borders and add useful dimensions as drawings to these hardware footprints (drawings will not appear on your silkscreen).
The advantage of doing it this ways is that it allows you to always have all the dimensions "at hand", you just place the footprint where it is supposed to be.
You can then assign them a 3D step model and define fabrication attributes (TH, SMD, or virtual).
A single footprint can have multiple 3D models (which allows you to combine them: plug into jack, chip on a socket, etc.)
If you set the fabrication attribute to virtual for your enclosure, you'll be able to show / hide it in KiCad's 3D viewer.

Here is an example of a circuit in a 1590LLB enclosure:


And the same after hiding the virtual model (enclosure):


In this example you can see that the audio jacks do not have the same orientation (one is rotated 180°) to make sure that everything fits.
All in all the challenge is to find the 3D models, draw the footprints.
The only limitation I faced so far is the fact that you cannot easily zoom, remove parts of the model (for instance "open" the lid), you need to do it manually (I do it with scripts which rename/remove the 3D models to show/hide parts)

Cheers,

Michel