PCBs as Front Panels ?

From circuitbending to homebrew stompboxes & synths, keep the DIY spirit alive!

Moderators: Joe., lisa, luketeaford, Kent

Post Reply
ratsnake
Common Wiggler
Posts: 126
Joined: Mon Feb 29, 2016 3:49 pm
Location: Berghain
Contact:

Post by ratsnake » Wed Sep 20, 2017 4:42 am

cool thanks. I found some pages on the interwebs about importing dxfs. gonna have a go soon!

now if only Frequency UK had their panels public.. gonna have to trace photos i guess..fug

User avatar
Morphology
Common Wiggler
Posts: 176
Joined: Wed May 04, 2016 7:31 am
Location: Kent, England

Post by Morphology » Tue Feb 06, 2018 4:09 pm

As a result of this thread, I had these front panels made by PCBWay.

They are 2mm FR-4. The lettering is made using the Top Copper layer, with Immersion Gold plating, and a black solder mask.

Gerbers were made using KiCad, the process being roughly as follows:

1) Use PCBNew to specify the edges and holes, including the rectangular cut-out

2) Draw the whole of the front panel graphic in Inkscape exactly to scale, which means you can use whatever fonts you want, flow text around objects (see the 0-9 scale). The image needs to be White on Black

3) Save this as a high-resolution .BMP file. I used 700dpi, but I think Kicad will let you go up to 1,000 dpi.

4) Use Bitmap2Component to create a .kicad_mod footprint file

5) By default, Kicad will import the graphic onto the Front SilkScreen layer, so edit this file with a text editor, and search and replace all occurrences on F.SilkS with F.Cu save it with a suitable name (Eg front_panel_top_copper.kicad_mod)

6) repeat the search and replace, but this time change all occurrences of F.SilkS to F.Mask save it with a suitable name (eg front_panel_solder_mask.kicad_mod)

7) Place these two 'footprints' on the board in PCBNEW, making sure they are aligned with each other, the holes etc.

8) Plot out the Gerbers. I generated the following:

- Edge Cuts
- Top Copper
- Top Solder Mask
- Non-plated through hole drill file

That's it. I didn't on this occasion, but I understand I could have used svg2mod to directly import the Inkscape .svg file onto the Copper layer rather than go through the BMP and using bitmap2component

A couple of photos:

Image

Image

Pretty satisfied with the way they have turned out.

Morph
There are only 10 different types of people: Those who understand binary, and those who don't

Lars71
Learning to Wiggle
Posts: 18
Joined: Tue Jun 23, 2015 3:59 am
Location: Gothenburg, Sweden

Post by Lars71 » Tue Feb 06, 2018 4:17 pm

Very nice! =)

User avatar
batchas
Super Deluxe Wiggler
Posts: 4549
Joined: Wed Nov 09, 2011 2:51 pm

Post by batchas » Wed Feb 07, 2018 3:21 am

Lars71 wrote:Very nice! =)
Indeed, this gold came out pretty well.

The only issue I met with making pcb panels are the scratches/traces on the surface, no matter which company made them (incl. pcbway) and no matter how I did insist upfront about the fact that they'll be used as panels and not circuit boards.
But the silkscreen itself (I use white on blue) is most of the time near perfect.

The black panel Lars71 posted here looks very good to (no visible traces on this pictures).

Nice job!

schenkzoola
Learning to Wiggle
Posts: 30
Joined: Mon Jan 22, 2018 11:46 pm
Location: Portland Oregon

Post by schenkzoola » Wed Feb 07, 2018 9:32 am

I've been considering using aluminum PCB's as front panels myself. I was curious how the edge cuts turn out. Are they sheared edges or routed?

Has anybody had any success with silkscreen on both sides of a single-sided aluminum PCB? This would allow you to use the copper for circuitry if you so desired.

Thanks!

User avatar
Altitude909
Super Deluxe Wiggler
Posts: 3296
Joined: Wed Aug 24, 2011 5:13 pm
Location: Meesheegan

Post by Altitude909 » Wed Feb 07, 2018 9:41 am

schenkzoola wrote:.. Are they sheared edges or routed?

..
Milled but crappy. The machining on the aluminum panels are pretty rough at best.

User avatar
Morphology
Common Wiggler
Posts: 176
Joined: Wed May 04, 2016 7:31 am
Location: Kent, England

Post by Morphology » Wed Feb 07, 2018 9:48 am

I've had Aluminium PCBs made up as front panels (also by PCBWay).

The edge cuts and cutouts are very clean, possibly waterjet-cut? There is certainly no evidence of shearing or routing.

I used black silk screen on a white solder mask, but was a bit disappointed with the consistency of the white colour - one batch ended up a bit grey.

I haven't tried silk screen on bare Aluminium, though the rear of my panels was plain Aluminium, and looks fairly clean and scratch-free.

I haven't tried copper tracks on an Aluminium PCB, though following my experiments with Immersion Gold plated copper PCBs as front panels (above), I'm considering giving this a go.

These are both Aluminium PCBs, white solder mask, black silk screen.

Image

I haven't tried copper tracks on the back - I guess it'd need to be all SMT devices, with no vias?

Morph
There are only 10 different types of people: Those who understand binary, and those who don't

schenkzoola
Learning to Wiggle
Posts: 30
Joined: Mon Jan 22, 2018 11:46 pm
Location: Portland Oregon

Post by schenkzoola » Wed Feb 07, 2018 9:58 am

Wow, that was a quick response, thanks!

Given the two responses with different results makes me think that different vendors have different edge cutting processes.

My thinking for the copper tracks on the back would of course be for SMD devices. Reverse mount SMD LED's could be interesting. Of course no vias would be possible. It might be possible to do a simple module as just a panel, but the pots and jacks would get weird.

I had an FR4 board made by PCBWay with a white soldermask, and was disappointed with it as well. There were tiny bubbles and voids in the soldermask, sort of like how spray paint ends up with voids if painting a contaminated surface.

Normally waterjet would leave a "sandblasted" look to the edges. You can laser cut thin aluminum as well.

Without using the copper for a circuit, you could get four possible colors.
Gold plated copper, silkscreen, soldermask, and a soldermask releif with no copper under it. (I assume it would be the color of whatever the insulation layer is)

User avatar
elmegil
Super Deluxe Wiggler
Posts: 2910
Joined: Sun Apr 29, 2012 2:57 pm
Location: Chicago

Post by elmegil » Sat Feb 10, 2018 1:25 am

I used AllPCB aluminum process, I put the silkscreen on the back so on the Aluminum side.

As Raph points out, the milling was pretty rough; for what I'm doing that doesn't matter much except for the mounting holes, which look less than professional. I prefer ovals (to be able to snug things up on threaded strips), so I have three holes together, and that's probably part of why it's rough.

Image

User avatar
truman_k
Common Wiggler
Posts: 93
Joined: Sun Jun 26, 2016 10:29 am
Location: Hong Kong

Post by truman_k » Mon Feb 12, 2018 7:44 am

I have tried a couple of times, these are pretty successful, with pcbway.


Image
Last edited by truman_k on Mon Feb 12, 2018 8:30 pm, edited 1 time in total.

schenkzoola
Learning to Wiggle
Posts: 30
Joined: Mon Jan 22, 2018 11:46 pm
Location: Portland Oregon

Post by schenkzoola » Mon Feb 12, 2018 9:13 am

Is that their matte black soldermask?

User avatar
truman_k
Common Wiggler
Posts: 93
Joined: Sun Jun 26, 2016 10:29 am
Location: Hong Kong

Post by truman_k » Mon Feb 12, 2018 8:27 pm

schenkzoola wrote:Is that their matte black soldermask?
yes

User avatar
kleinpa
Learning to Wiggle
Posts: 2
Joined: Mon Aug 15, 2016 12:03 am
Location: Boston, MA
Contact:

Post by kleinpa » Mon Feb 12, 2018 8:31 pm

I've been looking into PCB panels for my own designs for a few months now and haven't found a gerber-generation workflow I like, perhaps someone here has some suggestions.

I'm trying to find some automated process like a Makefile that takes a SVG (or multiple SVGs) containing the board outline and layers then does some "stuff" to them and generates a .zip file ready to send to the manufacturer. I've found tools like cairosvg and pstoedit which are scriptable and can genereate a .dxf or .pdf but I'm stuck figuring out how to transform any of those into a single layer of a gerber file.

I know I'm being picky and I could always just go the bitmap route, but I'd like to explore some other options first.

schenkzoola
Learning to Wiggle
Posts: 30
Joined: Mon Jan 22, 2018 11:46 pm
Location: Portland Oregon

Post by schenkzoola » Mon Feb 12, 2018 8:44 pm

This probably doesn't help much, but KiCad can take .dxf's for the edge cuts, and is scriptable. So at least your edge cuts can be automated. The graphics may require a .bmp I'll have to check.

User avatar
kleinpa
Learning to Wiggle
Posts: 2
Joined: Mon Aug 15, 2016 12:03 am
Location: Boston, MA
Contact:

Post by kleinpa » Mon Feb 12, 2018 10:25 pm

Oh that's cool, apparently KiCad has some python scripting interface that looks low-level but pretty promising. I'll need to take a closer look.

Thanks!

User avatar
Morphology
Common Wiggler
Posts: 176
Joined: Wed May 04, 2016 7:31 am
Location: Kent, England

Post by Morphology » Tue Feb 13, 2018 8:02 am

Also check out SVG2MOD that'll take an SVG and convert it straight into a KiCad footprint, letting you specify the resulting layer as you go.
There are only 10 different types of people: Those who understand binary, and those who don't

trip
Wiggling with Experience
Posts: 269
Joined: Tue Jun 30, 2015 8:15 pm
Location: United Kingdom

Post by trip » Tue Feb 13, 2018 8:31 am

A few tips I've picked up from making my panel graphics in inkscape for eagle using the svg2poly ulp and the instructions here https://learn.sparkfun.com/tutorials/im ... to-polygon if anyone is starting out with it.

Export the whole board layout as a pdf from eagle using circles for the actual size of the jacks with washers on and the pots with knobs on that you want to use (if using vias as drills, the image can sometimes bring some extra gunk into inkscape you have to clean up before you can export as a plain svg.).

Import that pdf in inkscape, lock height and width and resize to 1000mm high - layout your graphics, then delete absolutely everything that came in when you imported the pdf, double check there's no invisible boxes left over around the drill holes, and that there isn't an invisible frame around the whole board. Convert everything to paths and massage nodes according to the sparkfun instructions.

Lock all the components and dimension of your board in eagle and run svg2poly. I've found that a 1000mm high plain svg comes in at the right size (128.5mm in eagle) by using:

run svg2poly -ratio 0.0364

Make sure to change the width of all the polygons as a group, I've found that width 0.005 will show up on all gerber viewers, any smaller and some of them won't show anything at all.

User avatar
truman_k
Common Wiggler
Posts: 93
Joined: Sun Jun 26, 2016 10:29 am
Location: Hong Kong

Post by truman_k » Tue Apr 10, 2018 2:32 am

elmegil wrote:I used AllPCB aluminum process, I put the silkscreen on the back so on the Aluminum side.

As Raph points out, the milling was pretty rough; for what I'm doing that doesn't matter much except for the mounting holes, which look less than professional. I prefer ovals (to be able to snug things up on threaded strips), so I have three holes together, and that's probably part of why it's rough.

Image
the bare aluminum looks cool. if silkscreen on the back, do you have solder mask in front?

User avatar
elmegil
Super Deluxe Wiggler
Posts: 2910
Joined: Sun Apr 29, 2012 2:57 pm
Location: Chicago

Post by elmegil » Tue Apr 10, 2018 7:12 am

I didn't have anything on the back, no copper or anything (had them remove it all, in retrospect that wasn't necessary).

User avatar
State Machine
Learning to Wiggle
Posts: 24
Joined: Mon Aug 10, 2009 6:26 pm

Post by State Machine » Fri Nov 15, 2019 6:22 pm

I know this is an older thread but I am glad I discovered it. I want to do exactly this for some panels using the aluminum material from PCBway. The panels and advice here is excellent. I was not sure if the fabricator can do rectangular holes but to my delight, I saw the panel by Morphology and it looked very good. :yay:

Thanks Guys !
Bill

040B
Learning to Wiggle
Posts: 26
Joined: Sat Oct 19, 2019 1:56 pm
Location: NL

Re: PCBs as Front Panels ?

Post by 040B » Sat Jan 11, 2020 1:44 pm

Some very useful tips and great results in this thread.

:hail:

User avatar
mrand
Common Wiggler
Posts: 123
Joined: Thu May 23, 2013 11:26 pm
Location: Whitehorse, Yukon
Contact:

Re: PCBs as Front Panels ?

Post by mrand » Sat Jan 11, 2020 3:24 pm

FWIW here are a couple photos of a recent JLCPCB panel. I designed a format dedicated to maximizing the low-cost, 10x10cm PCB offerings. It's a very cost effective solution, especially now that the minimum order is down to 5 units. At standard 1.6mm thickness, there is no rigidity problem.

There must be others who have arrived at the same conclusion to use 10x10cm panels?
VCOpanel2_.jpg
VCOpanel1.jpg
You do not have the required permissions to view the files attached to this post.
--ssdp--

User avatar
FetidEye
demonic space drone
Posts: 2040
Joined: Mon Dec 06, 2010 5:00 pm
Location: Red Zone
Contact:

Re: PCBs as Front Panels ?

Post by FetidEye » Sat Jan 11, 2020 4:03 pm

Eagle layout, made at Dirtypcbs (a video matrix mixer)
I draw the picture in Eagle itself.
After a few mishaps with scratches and discolorisations, I now just say that they are panel boards.
No problems since :)
Dirtypcbs also has the option to print the id code on the back, or leave it out totally.
I have not used copper groundplanes. Maybe I'll try this in my next design. More stiff panels are good!


I have yet to find out how to make oval holes and milled cutouts (for sliders and displays for example. If anyone has tips on that, please :)


kleiner.jpg
You do not have the required permissions to view the files attached to this post.

User avatar
Lolo73
Learning to Wiggle
Posts: 37
Joined: Mon Aug 14, 2017 8:42 am
Location: France
Contact:

Re:

Post by Lolo73 » Sun Jan 12, 2020 2:02 pm

elmegil wrote:
Sat Feb 10, 2018 1:25 am
I used AllPCB aluminum process, I put the silkscreen on the back so on the Aluminum side.

As Raph points out, the milling was pretty rough; for what I'm doing that doesn't matter much except for the mounting holes, which look less than professional. I prefer ovals (to be able to snug things up on threaded strips), so I have three holes together, and that's probably part of why it's rough.

Image
I had the same problem with oval holes, but now I use DipTrace and I draw my shapes on the "board cutout" layer. There are no more problems. I use 1.6 aluminium panels, made by PCBWay.
You do not have the required permissions to view the files attached to this post.

User avatar
mrand
Common Wiggler
Posts: 123
Joined: Thu May 23, 2013 11:26 pm
Location: Whitehorse, Yukon
Contact:

Re: Re:

Post by mrand » Sun Jan 12, 2020 3:17 pm

Lolo73 wrote:
Sun Jan 12, 2020 2:02 pm
I use 1.6 aluminium panels, made by PCBWay.
I'm curious, is 1.6mm aluminum panel more rigid than 1.6mm PCB with full "ground plane" on the backside? Wondering if anyone has had a chance to do a fair comparison.
--ssdp--

Post Reply

Return to “Music Tech DIY”