Anyone have any experience using PCB fabrication to make panels for Eurorack modules?
I have a particular DIY module that came with a crappy panel, and thought it might be nice to try designing a new one and have it produced by a fabbing service.
I wonder if there are any pre-made hole/slot parts for Eagle or some other application.
Anyone any tips?
I’m also curious and planned to look into that for a while. Would be great if someone made a tutorial for it .
I only found this one
That is about making 3d cases from pcb’s
I’m going to try doing one in Fritzing, I think.
AndrewF, who is the Perth-based designer of the quirky NonLinearCircuits (NLC) DIY synth modules, swapped to using PCB panels about a year ago. Initially blue (or are they green? I suffer from tritanomaly so I’m never quite sure) PCBs with gold lettering, but more recently white PCBs with gold lettering, which look a lot nicer. Somewhere he posted a discussion of design and fab issues with the panels, but I can’t seem to find it. Maybe just email him to ask about his experience.
However, those are just PCBs as panels, which is I think what you were asking about, although the title to this thread is panels as PCBs. The latter is an even more interesting topic, I think. Some of the MakeNoise modules (Rene etc) spring to mind, and there’s that Chinese module designer who also uses capacitance touch pads on the panel - MengQi, isn’t it? And I noticed this the other day, which appears to have traces and vias on it, suggesting components mounted on the rear of the panel. The name is curious: Charcot was a 19th Century neurologist, who taught Freud, I think, and who lent his name to the not-uncommon Charcot-Marie-Tooth disease. Maybe the name is in reference to Siggy?
It’s fairly easy in Eagle, I did one yesterday!
1/ Draw the outline of the panel around your main PCB. Set the coordinates origin to the bottom left corner of the panel outline.
2/ Set units to mm.
3/ Use the Export / Partlist function to get a text file with the XY coordinates of all parts. You can use grep to remove the lines with R/C components or IC and only get the jacks/LEDs/pots
4/ Create a new blank board and draw the outline. Set the coordinates origin to the bottom left corner. In all the next steps, don’t bother putting things exactly at the right position - put things at approximative locations, and then edit the object properties to fix the coordinates with the exact ones you have in your text file (Note: one of Mutable Instruments’ secret weapons, along with autobom.py is a python script that converts such text files to DXF ASCII for panel CAD).
5/ For the mounting holes coordinates, refer to this. You can use the via tool, this will expose a bit of copper (or gold) around the hole.
6/ For the pots, jacks, LEDs, buttons use the hole tool. The “Drill” property sets the diameter (6.5mm for jacks, 7.5mm for pots, 3.1mm for LEDs…)
7/ For artwork, you have 3 colors in your palette: PCB soldermask color (green, black) is the background color, silkscreen color (white) is what you draw on the tPlace layer, but you can also expose traces (silver for HASL finish, gold for ENIG finish). To draw something in golden/silver, draw it on the Top layer (red color), duplicate it, and set it to the tStop layer (grey hatchings) - in other words, something appears golden or silver on the PCB because there’s a trace there (Top) and because the soldermask is not applied on top of it (tStop).
8/ Use the Print command to print a 1:1 PDF of your board.
9/ Import the PDF in Illustrator or any other vector graphics program. Create all your type/artwork on top of it.
10/ Export the result as a 600 dpi BMP file. Process it in Gimp / Photoshop to get a 1-bit bitmap. I start by going into Greyscale mode, then use Curves to get a high contrast B&W image, then convert to bitmap with 50% thresholding - don’t use dithering - it won’t look good and will make huge Gerber files. Depending on the PCB fab, your resolution on the silkscreen is in the 200-400 dpi range only because it will bleed. The soldermask/traces are a bit more precise, but some PCB houses will run a simplification process on the soldermask (tStop) layers to remove small islands.
11/ Use “run import-bmp” to import your artwork in Eagle. Pick the first color in the first dialog box shown by Eagle (I am not sure if I understand how this step works or if there’s a bug in the Eagle script - I often have to pick the black when I want to import the white! - so if you get your artwork in negative try again with the other color!). In the next dialog box, input the correct DPI value to have the graphics imported to scale (otherwise there’s a lot of trial and error to align it with the board, and you can’t resize it in Eagle once it’s imported). The text will be added to a new layer. Select everything and move it to the tPlace layer.
12/ Bonus trick: if you have elaborate graphics in gold/silver, you can have a uniform polygon (“ground plane”) on Top under the area taken by the graphics, and use only the tStop layer for the graphics - rather than having two copies of the artwork, one on Top and one on tStop. This can help with the Gerber file size.
Wow, an excellent and very valuable set of instructions. Now, if only I had a better-than-freebie version of Eagle… might be time to stump up the cash to buy a copy.
If you use copper only in the middle of the panel (= no vias for mounting holes), the demo version is fine.
Ah, OK, good point (the layout for the demo version is limited to 100mm in any one dimension, and the height of euro panels is a bit more than that). Or I could ask a friend to add via mounting holes after most of the work is done in the free version. That will save several hundred dollars (Eagle isn’t exactly cheap)!
The 100mm x 80mm is the area for traces - you can make your board larger as long as it’s only graphics. That’s what I did for the Shruthi boards.
Thanks very much for the detailed rundown pichenettes. I’ll give that a go!
Adding the graphics runthrough is very much appreciated! This is the one thing I could never fully figure out.
Razmasynth “Unknown Pleasures” is a panel that’s also a PCB. Not a fun build.
Frizting should also work quite well (with many options for mounting holes and other cut outs, the default library also already contains a few touch sensitive elements in case someone wants to make use of such).
It is also possible to import graphics but as yet i have been too stupid to succeed (but i did not try very hard).
I quite like pcb panels, they can look very shiny and elegant (the new Nonlinear Circuits and some others), as well as very agricultural (in particular if you self-etch the fonts). But (at least for Fritzing) the costs for a single panel are not cheaper than a metal frontpanel service (i guess, as usual, costs come down quickly if you order in larger quantities or overseas).
made these for my turing machine
considering that it has been my first experience w/ eagle I can say I’m prertty satisfied.
if anyone is interested I have 2 sets available.
remember that there’s generally a minimum quantity order for pcb prototyping