Started learning Eagle:

[FBX]

I picked up Eagle a few days ago and learned how to do the 3 phases it has (Device, Schematic, and PCB) so I could do up my own SNES digital audio board. The goal was to make a dual output board that supports both optical and coaxial, yet fits in a small enough board to be interchangeable in both regular and mini SNES consoles. This proved to be quite difficult, and in the end, I could only figure out one arrangement that fit both consoles and kept most of the routing to a minimum:



Trust me that I tried several different arrangements, and they would cause issues like running into a heat shield on the mini, or running into a plastic guard on the regular SNES, or causing the routing to be a clusterfuck. It may not be symmetrical or pretty, but she fits.

Anyway, so the idea here is to offer people the option of using the coaxial pads for a no-cut mod solution by using the RF out port (after removing the RF box of course). Technically the board will power and operate both coaxial and optical at the same time, so if people wanted to, they could have both jack types modded onto the system.

I'll be sending it off to OSH Park for prototyping in a couple weeks, but thought I might post the progress here in case anyone spots an improvement or correction I overlooked.

Ciao!

[Woozle]

Is that pad labeled G your ground connection? Seems like it's not connected to anything.

Is C4 a VCC bypass cap? If so it should be connected to the power rail as well as the IC power pins.

I would also recommend editing your SMD cap/resistor packages to include guides on the silkscreen to show component orientation. When your boards get more complex it will help avoid soldering parts on sideways.

Just some quick observations. Looks good overall for just starting eagle.

[FBX]

Is that pad labeled G your ground connection? Seems like it's not connected to anything.

It's a trick to remove thermals, you set the overall top layer polygon to rank 2 with thermals, and then do a smaller polygon at rank 1 without thermals around specific pads where you don't want them. Here's a pic of the copper fill-in: (edit: I didn't mean mask, sorry about that)

Is C4 a VCC bypass cap? If so it should be connected to the power rail as well as the IC power pins.

Edit: Dammit, I just realized you asked about C4, not C1. My bad. Yeah, it's connected to power.

I would also recommend editing your SMD cap/resistor packages to include guides on the silkscreen to show component orientation. When your boards get more complex it will help avoid soldering parts on sideways.

They are there, but I had the silk layers turned off when I took these pics.

Just some quick observations. Looks good overall for just starting eagle.

Thanks! I've been at it for like 3 days now, so I'm getting there. Already had to design a device manually since nobody had a library to share of it. I guess it was for my own good since I needed to learn how to do that too.

[FBX]

My apologies, for some reason I read C1 when you asked about C4, I've edited my reply. ><

[FBX]

Got a brainstorm while on the shitter and went OCD on arrangement for the 2nd attempt. Managed to actually save a few mm of board size:



I ended up swapping the pin assignments for 3 and 4 to make them more direct. I'll be sure to add a wiring chart on the back of the board when I feel it's ready for manufacturing.

Edit: Added in a spot for the 22pF cap that should go on the negative RCA output line. That should be everything needed now.

[xga]

I picked up Eagle a few days ago and learned how to do the 3 phases it has (Device, Schematic, and PCB) so I could do up my own SNES digital audio board.

This looks great, FBX!

I've been thinking about learning Eagle too. Did you come across any good resources whilst learning it or did you just work it out yourself?

[FBX]

I picked up Eagle a few days ago and learned how to do the 3 phases it has (Device, Schematic, and PCB) so I could do up my own SNES digital audio board.

This looks great, FBX!

I've been thinking about learning Eagle too. Did you come across any good resources whilst learning it or did you just work it out yourself?

I watched some very basic tutorials by Jeremy Blum on youtube, then another one by a Russian on how to make device libraries. After that, I started downloading various boards on OSH Park and studying the elements and techniques used. A couple things were complete mysteries on how people pulled it off, and I had to just stare at values and settings until I figured out what they had done.

[citrus3000psi]

Design looks good. I would prefer the GND pad be next the VCC pad though. Makes for a nicer install when running wires.

[FBX]

Design looks good. I would prefer the GND pad be next the VCC pad though. Makes for a nicer install when running wires.

It wasn't going to fit with the cap over there, and I don't have any more room to work with if I want to keep the board 'universal' for both regular size SNES and mini. Also the ground pad is now right over top of where the ground source for the RF box is in the SNES, so it's technically a shorter run than if ground were on the right side.

Still I could do up a version with ground crammed on the right side if you wanted to have a look anyway. I just didn't like how crowded it was getting over there.

[FBX]

Okay so hopefully this is the 4th and final revision of the board layout:



Added a ground pad on both sides for optional wiring depending on your needs. I also squeezed in everything a little more, and it's about as packed as I want to get it at this point. Lastly, I changed the bottom layer to also be ground so I could throw vias underneath the transformer.

Edit: Just now noticed I forgot to ground R2 as per the datasheet for the CS8406 datasheet. >< I've made the correction and updated the image here.

Also there was concern from one person that the lack of thermals on the ground and Vcc pads might make them a chore to solder, but I know from Bort's optical boards that they are not. However, if it does turn out to be difficult on the prototypes, I'll add in thermals on those pads for the 2nd run.

[FBX]

Revision 6:



So the improvement here was I realized I could simply move the TXP 'via' to underneath the CS8406, keeping it safe from solder bridging accidents. This also allowed me to squeeze the right side of the board in to make both sides perfectly symmetrical in length (my OCD got a boner over that).

A suggestion was made that I should consider using a mini-TOSLINK jack that combines coaxial and digital into one socket, where users would have an adapter plug that converts into either RCA coaxial or full-size optical. I thought about it, but I'm not sure I want to do this since people might be turned off on the idea of keeping an adapter handy.

[borti4938]

Good way to start with eagle This was also some of my first designs and today I would do something different.
Some suggestion, what I would further do:

• remove Vcc plane
  It was initially just meant to have some vias to the bottom plane, which you have removed.
• Run the Vin trace all the way up on top layer 1 and then just a short path to the left on bottom layer 16
  You can also shorten the trace a bit by shifting line5 to the left under the CS8406
• change position of right GND pad and C5
• change position of C2 and C3
• stitch vias around the GND pads and not under DA101J
• use a via around groups of GND pads

[FBX]

Good way to start with eagle This was also some of my first designs and today I would do something different.
Some suggestion, what I would further do:

• remove Vcc plane
  It was initially just meant to have some vias to the bottom plane, which you have removed.
• Run the Vin trace all the way up on top layer 1 and then just a short path to the left on bottom layer 16
  You can also shorten the trace a bit by shifting line5 to the left under the CS8406
• change position of right GND pad and C5
• change position of C2 and C3
• stitch vias around the GND pads and not under DA101J
• use a via around groups of GND pads

Thanks for the tips! On the via array under the DA101J, it was something L-Train had done on his board for upsampling SNES audio, and I liked the look of it. May I ask why it matters to have the via so close to the pad instead?

Cheers!

[FBX]

Borti,

What do you think of this layout?



I made all the changes you suggested to some degree. I also increased the annular ring size as I read online that this helps prevent sloppy drill hole alignment from breaking the via.

My only concern now is the C5 cap. Is it okay to send power from pin 1 through 5 to pin 6 like I have here and the C5 cap will still do its job properly for pins 6 and 11? Thanks again for your advice!

Edit: BTW, I also edited the device file for the PLT133/10T and tented the bottom side for all the pads. This will make the board safer for coaxial-only configurations. All the vias are already tented.

[borti4938]

Here are my comments:

(if img-link is broken, look it up here)

Mainly it's:

• separate logic high inputs from +5V supply inputs
• spread some GND vias
• avoid GND in front of pads.

Regarding the last point:
Most Chinese prototype services sometimes produce a shifted solder mask. Together with some hobbyists who strip off wires quite long this may cause a nearly invisible GND short on a signal wire. Thats why I try to avoid such a situation by having no GND plane in front of connection pads.

[FBX]

Okay I'll work on trying those arrangements out. Much appreciated again for your advice!

[FBX]

Okay here we go with revision 9:



Edit: Nevermind, I find a diagram in the datasheet where they show the cap on pin 6. My mistake. Thanks again!

[borti4938]

Great!

Final suggestion: move also the down right pads for V and GND a bit to the right to have a uniform look.

[FBX]

Great!

Final suggestion: move also the down right pads for V and GND a bit to the right to have a uniform look.

Done! (and I made a couple of other minor changes)

[borti4938]

Congrats to your first design

Make sure that the silkscreen font is not too small. Most PCB services requires 6mil; to my experience 5mil also works.
In Eagle you can set it up with the ratio. If your font height is 40mil and ratio is 15% the thickness will be 6mil (6mil = 15% of 40mil). I usually use 40mil font height for pad descriptions and major elements (like ICs) and 32mil for anything else; everything with a ratio of 15%, sometimes 20%. Font type is vector.

[FBX]

Make sure that the silkscreen font is not too small. Most PCB services requires 6mil; to my experience 5mil also works.
In Eagle you can set it up with the ratio. If your font height is 40mil and ratio is 15% the thickness will be 6mil (6mil = 15% of 40mil). I usually use 40mil font height for pad descriptions and major elements (like ICs) and 32mil for anything else; everything with a ratio of 15%, sometimes 20%. Font type is vector.

Ah! That would explain why I got a width error in my logo before. I set up the Design Rules to 6 mils, and my logo was running at a thickness of 5 mils. I didn't realize the font itself was violating width rules. I went back and changed everything to vector with a minimum width of 6 mils. I also made sure all vias are tented above and below the board, and I even edited the PLT133 device file to tent the underside for coaxial-only configurations (it shouldn't be a problem to pierce the masking with a needle to mount the optical jack). Lastly, I put a wiring chart on the back, which is important because I have pads 3 and 4 swapped from your design due to the mounting position of the CS8406. So here's the final image (bottom layer names are hidden):



Thanks so much for all your tips and advice!

Edit: For those wondering about the 2.0 designation, 1.0 was a small prototype board I sent off for fabrication, meant purely for testing the pin configuration I'm using on this board. So this one is technically not my first board in that sense.