• WANTED: Happy members who like to discuss audio and other topics related to our interest. Desire to learn and share knowledge of science required. There are many reviews of audio hardware and expert members to help answer your questions. Click here to have your audio equipment measured for free!

Relays that are "audiophile" grade

JayGilb

Major Contributor
Joined
Jul 22, 2021
Messages
1,371
Likes
2,308
Location
West-Central Wisconsin
I would just make both pours the GND net. There's no reason to make a power plane for the +12V since its just powering 3 relays. There could also be a potential problem if the +12V power supply is noisy, it could induce noise into the audio traces if it surrounds all of those traces. Remember if there are landlocked areas which won't pour, use vias from the top to the bottom layer so this doesn't happen.

Good advice on not creating a V+ power plane.
 
OP
S

starfly

Senior Member
Forum Donor
Joined
Jun 6, 2019
Messages
353
Likes
288
Okay, I think this is the final PCB design, with M3 mounting holes in the corner, connected to top and bottom pours, so that grounding also goes to the metal enclosure this board will sit in.

About the routing of the +12V trigger signal, that itself is not connected to ground on the board, it will just flow back to my AVR in this case. That should be fine, right?

1633453035778.png
1633453087090.png
1633453156340.png
 

MakeMineVinyl

Major Contributor
Joined
Jun 5, 2020
Messages
3,558
Likes
5,871
Location
Santa Fe, NM
Okay, I think this is the final PCB design, with M3 mounting holes in the corner, connected to top and bottom pours, so that grounding also goes to the metal enclosure this board will sit in.

About the routing of the +12V trigger signal, that itself is not connected to ground on the board, it will just flow back to my AVR in this case. That should be fine, right?

View attachment 157356 View attachment 157357 View attachment 157358
The traces in the lower left corner of the board (Net-J2-Pad2 and Net-J3-Pad 1) should ideally be at 90 degree angles to the pads. This is because a trace exiting another trace at 45 degrees creates an area at the junction which can potentially cause etching problems due to the narrow angle - it also looks messier the way you have it. Also, you have several instances where traces come too close to pads on another net. You should keep unrelated traces and pads a safe distance away - I use the distance of the width of a trace as a guide, not including the pour keep out area when possible.

These are small issues, and your board will undoubtedly work as-is, but these suggestions should help you in producing professional level boards. :)
 
OP
S

starfly

Senior Member
Forum Donor
Joined
Jun 6, 2019
Messages
353
Likes
288
The traces in the lower left corner of the board (Net-J2-Pad2 and Net-J3-Pad 1) should ideally be at 90 degree angles to the pads. This is because a trace exiting another trace at 45 degrees creates an area at the junction which can potentially cause etching problems due to the narrow angle - it also looks messier the way you have it. Also, you have several instances where traces come too close to pads on another net. You should keep unrelated traces and pads a safe distance away - I use the distance of the width of a trace as a guide, not including the pour keep out area when possible.

These are small issues, and your board will undoubtedly work as-is, but these suggestions should help you in producing professional level boards. :)

Ah, I somehow thought 90° angles were to be avoided in traces. I made a few minor changes:

1633457449090.png
 

MakeMineVinyl

Major Contributor
Joined
Jun 5, 2020
Messages
3,558
Likes
5,871
Location
Santa Fe, NM
Ah, I somehow thought 90° angles were to be avoided in traces. I made a few minor changes:

View attachment 157371
You want to always leave a trace at 90 degrees, then go 45 degrees as needed. Around K3, pin 3 and pin 4, that trace is a bit close still. Also on pins 5, 6, and 8, have the trace a bit longer at 90 degrees as it exits the pads because if they're too close, the same etching problem can happen between the trace and the pad. I try to have traces which go to square pads do so at 90 degrees, but I've seen it done either way. K1 pin 6 has a trace too close. Make the trace from pin 6 exit at 90 degrees so you can keep away from pin 5 (like you did on pin 2).

Lots of detail to mess with in laying out PCBs!
 
OP
S

starfly

Senior Member
Forum Donor
Joined
Jun 6, 2019
Messages
353
Likes
288
You want to always leave a trace at 90 degrees, then go 45 degrees as needed. Around K3, pin 3 and pin 4, that trace is a bit close still. Also on pins 5, 6, and 8, have the trace a bit longer at 90 degrees as it exits the pads because if they're too close, the same etching problem can happen between the trace and the pad. I try to have traces which go to square pads do so at 90 degrees, but I've seen it done either way. K1 pin 6 has a trace too close. Make the trace from pin 6 exit at 90 degrees so you can keep away from pin 5 (like you did on pin 2).

Lots of detail to mess with in laying out PCBs!

Ok, a few more changes:

1633462406268.png


1633462440098.png


1633462496692.png
 

MakeMineVinyl

Major Contributor
Joined
Jun 5, 2020
Messages
3,558
Likes
5,871
Location
Santa Fe, NM

MakeMineVinyl

Major Contributor
Joined
Jun 5, 2020
Messages
3,558
Likes
5,871
Location
Santa Fe, NM
Are the mounting pads actually connected to the pours by copper? I didn't see a connection there if that is what you wanted. Other than that, I think that's it! :D
One last thing, make sure that your holes are specified as plated through. I missed this on one of my boards and all the vias and pads didn't connect the layers. Oops...
 
OP
S

starfly

Senior Member
Forum Donor
Joined
Jun 6, 2019
Messages
353
Likes
288
Are the mounting pads actually connected to the pours by copper? I didn't see a connection there if that is what you wanted. Other than that, I think that's it! :D
I believe they are. When I click on the pads, I get:
1633463136460.png


And then when I select "All copper layers", and then go to Properties, I can select GNDS net. I'm assuming that means it'll connect to GNDS on both the top and bottom layer. But to be sure, I guess I could also select the F.Cu and B.Cu (Front/Back Copper) and connect it to GNDS there too, just to be sure. But that's probably redundant.

Edit: So actually, when I connect it to the GNDS net, I get lines pointing to J4 pins 2 and 4, implying it needs to be connected. Let me figure out how to do that.
 

MakeMineVinyl

Major Contributor
Joined
Jun 5, 2020
Messages
3,558
Likes
5,871
Location
Santa Fe, NM
I believe they are. When I click on the pads, I get:
View attachment 157388

And then when I select "All copper layers", and then go to Properties, I can select GNDS net. I'm assuming that means it'll connect to GNDS on both the top and bottom layer. But to be sure, I guess I could also select the F.Cu and B.Cu (Front/Back Copper) and connect it to GNDS there too, just to be sure. But that's probably redundant.
I don't know how its handled in your layout program, but when in doubt manually assign what you want connected together by editing the net names to be exactly the same for those points.

Here is the pad dialog in Altium:


Untitled-2.jpg


Under 'Properties' the pad focus is specified as Multi-layer, and the Plated box is checked. The assigned net is also shown and can be edited if needed.
 
OP
S

starfly

Senior Member
Forum Donor
Joined
Jun 6, 2019
Messages
353
Likes
288
I don't know how its handled in your layout program, but when in doubt manually assign what you want connected together by editing the net names to be exactly the same for those points.

Here is the pad dialog in Altium:


View attachment 157389

Under 'Properties' the pad focus is specified as Multi-layer, and the Plated box is checked. The assigned net is also shown and can be edited if needed.

This is the dialog in KiCad. You will see that Net name is set to "GNDS" and copper is set to "All copper layers". But when I do that it gives me an error when I run the Design Rules Check that the pads aren't connected.

1633464210184.png
 

MakeMineVinyl

Major Contributor
Joined
Jun 5, 2020
Messages
3,558
Likes
5,871
Location
Santa Fe, NM
This is the dialog in KiCad. You will see that Net name is set to "GNDS" and copper is set to "All copper layers". But when I do that it gives me an error when I run the Design Rules Check that the pads aren't connected.

View attachment 157390
You may have to change the design rules to force it to do what you want. That's very often the case I run into.
 
OP
S

starfly

Senior Member
Forum Donor
Joined
Jun 6, 2019
Messages
353
Likes
288
You may have to change the design rules to force it to do what you want. That's very often the case I run into.
Ok, it was something very simple. The mounting holes needed to be fully within the copper pour layers. Some parts were sticking out, so that's why it didn't work. And I also had to connect F.Cu and B.Cu to the GNDS net, not just All copper layers. But now it works as intended.

The final design here. I've ordered all the parts and a breadboard is on the way too. Will test the design first on that, and if it works as intended, I'll get the PCB manufactured. Thanks soooo much for all your help!!!

1633467881060.png
 
OP
S

starfly

Senior Member
Forum Donor
Joined
Jun 6, 2019
Messages
353
Likes
288
The PCB arrived! I'll solder on all the components one of these days, and I still need to order the enclosure for mounting everything. Once I have all that I'll try to take some measurements using my Motu M4.

20211020_112041.jpg
 

MakeMineVinyl

Major Contributor
Joined
Jun 5, 2020
Messages
3,558
Likes
5,871
Location
Santa Fe, NM
Looks good!
 
OP
S

starfly

Senior Member
Forum Donor
Joined
Jun 6, 2019
Messages
353
Likes
288
I can confirm the board works as intended. Put 12V on the trigger input and tested continuity with my multimeter and it works as designed.

Final test will be in fully assembled enclosure with XLR sockets and proper grounding to the chassis, to see how it does with ground loops.
 
OP
S

starfly

Senior Member
Forum Donor
Joined
Jun 6, 2019
Messages
353
Likes
288
I created a new thread here showing the final build:

 
Top Bottom