HELP with designing a headphones distributor please

[Hubbub]

I should point out you only need 2 wires to each headphone jack, just short tip and ring terminals at the jack.

Before you go too far, something to think about. What if you had a case with a 2-piece top and bottom, picture a clamshell style package. What if these were extrusions that composed 4 sides, and accepted flat panels for the other 2? (Similar configuration molded plastic cases are available, maybe even the preferred choice.) I had always pictured the flat panels as front-back, but you could make them side-side. Now there is a possibility for assembly even with all connectors and controls mounted on the PCB. Yes, the case needs 4 holes for the switches and pots, not too hard to do well if a printed template is attached for drill alignment. Yes, the RJ-45 mounts from the inside rather than outside, but that's doable. Maybe the side panels could be made as PCBs, screen printed even. This concept eliminates a lot of manual wiring of the headphone jacks, no RJ-45 pigtails and doubling the RJ-45 connector count, and it still keeps the connector orientation and minimized depth you have now. Choices, choices....

 

[sonolink]

I should point out you only need 2 wires to each headphone jack, just short tip and ring terminals at the jack.

Right you are! Thanks for pointing that out

Before you go too far, something to think about. What if you had a case with a 2-piece top and bottom, picture a clamshell style package. What if these were extrusions that composed 4 sides, and accepted flat panels for the other 2? (Similar configuration molded plastic cases are available, maybe even the preferred choice.) I had always pictured the flat panels as front-back, but you could make them side-side. Now there is a possibility for assembly even with all connectors and controls mounted on the PCB. Yes, the case needs 4 holes for the switches and pots, not too hard to do well if a printed template is attached for drill alignment. Yes, the RJ-45 mounts from the inside rather than outside, but that's doable. Maybe the side panels could be made as PCBs, screen printed even. This concept eliminates a lot of manual wiring of the headphone jacks, no RJ-45 pigtails and doubling the RJ-45 connector count, and it still keeps the connector orientation and minimized depth you have now. Choices, choices....

Mmmmm I'll give that a spin in my head but I think my buddy has already ordered the Hammond enclosures. So what you mean is to place the flat panels on the sides and the extrusion facing the user, right?

Cheers
Sono

 

[sonolink]

Hi guys,

Last update:


















I got the Hammond enclosures for $7.99 !!
Thanks again for all the support, help and good advice
Cheers
Sono

 

[sonolink]

BTW, I just noticed that the standoffs as it's designed will be screwed to the lid of the box, which is a no go. So I'll leave out the standoffs and use solid core wire to connect the jack connectors to the PCB. That'll give enough structure to the whole thing

Cheers
Sono

 

[Hubbub]

The board is symmetrical, flip it around and mount everything in the 5-sided section. Then you can still call the "lid" the bottom. This also pushes the switches up higher on the finished unit, where they can be more easily accessed. The top ends up having 2 screw heads showing, not too bad to live with.

 

[MidnightArrakis]

> Here are some items I have noticed that you can also ignore:

1) The "Copper Pour" needs to be backed-off from the edge of the PCB by at least 30-to-50 mils. Standard PCB practice. Assuredly, others here will strongly disagree.

2) Perhaps it is due to the low-resolution of your PCB-layout images, but I fail to see any "thermal-reliefs" anywhere that would connect the "Copper Pour" to GROUND, so right now the "Copper Pour" is floating.

3) The routing of this PCB needs to be adjusted in order to allow the "Copper Pour" going between tracks to become thicker.


> As one example, the mitered corner shown in the lower-left corner could easily be increased, which would then allow the "Copper Pour" to flood around the via hole, also shown in the lower-left corner.
> The -- sliver -- of "Copper Pour" shown in the center of the above image and right-of-center in the first image could very well just be etched away during the PCB fabrication process.

4) Even though this is a rather small PCB, I would still implement "stitching-vias" throughout the layout in order to better connect the TOP and BOTTOM "Copper Pours" together. But.....that's just me. You can just ignore my stupid suggestions, OK???

>> After I have completed a PCB-layout and have performed a "Copper Pour" flooding, I will take a look at how the flooding took place and I will then go back and adjust routings and via locations in order to try and maximize how the "Copper Pour" flows around and in-between tracks, pads and vias. While the end result may not look so "orthogonally pretty" as the layout here, that doesn't matter nearly as much to me as having a good and solid "Copper Pour" is, which is greatly helped by "stitching-vias". But, again.....that's just me. The designer of this project seems to also have their own strongly held views with how this project should be designed. So.....what do I know???

/

 

[Hubbub]

In most cases the purpose of a copper pour is a ground plane, and good stitching top to bottom is important. This design is an exception, it really doesn't need anything on the circuit board grounded. All connectors will "ground" to the (consequently) fully shielding case, that is more than adequate for a headphone level system. Given that, the only purpose a copper pour provides is for a reduction in the use of etchant while making the board. So no stitching needed.

But the comment about narrow sections of pour that may become slivers is spot on. Keep the pour fat, never let it drop down below a proper minimum trace width. I'd say 0.25mm is a good minimum. And keeping the pour away from the board edges is important standard practice. It's needed so the solder mask can completely cover the copper around the board perimeter, makes the board easier to router to shape, and safer to handle.

 

[MidnightArrakis]

In most cases the purpose of a copper pour is a ground plane, and good stitching top to bottom is important. This design is an exception, it really doesn't need anything on the circuit board grounded. All connectors will "ground" to the (consequently) fully shielding case, that is more than adequate for a headphone level system. Given that, the only purpose a copper pour provides is for a reduction in the use of etchant while making the board. So no stitching needed.

But the comment about narrow sections of pour that may become slivers is spot on. Keep the pour fat, never let it drop down below a proper minimum trace width. I'd say 0.25mm is a good minimum. And keeping the pour away from the board edges is important standard practice. It's needed so the solder mask can completely cover the copper around the board perimeter, makes the board easier to router to shape, and safer to handle.

[good stitching top to bottom is important] -- Due to my background in PCB-design, "via-stitching" was a mandatory requirement. My PCB-design program even had a special routine for flooding PCB's with hundreds of "via-stitches". (The program I used then called -- via-stitching -- "FREE VIAS").

[really doesn't need anything on the circuit board grounded] -- If the "Copper Pour" isn't grounded, then it becomes an antenna. Or so that's what the skilled "RF" engineers I have worked with all told me.

[All connectors will "ground" to the (consequently) fully shielding case] -- While I am probably missing something here, I haven't seen any easily identifiable Connector/PCB-to-Chassis/Box grounding method and/or scheme here. Please show me.....

[the only purpose a copper pour provides is for a reduction in the use of etchant while making the board] -- You're paying for that copper, whether you use it or have it washed down the drain!!! Therefore, I'm gonna use it.

[0.25mm is a good minimum] -- 0.25mm = ~0.010-inch or 10-mils. The PCB-fabricators I have worked with tell me that, unless your PCB-fabrication notes specify in some manner that a PCB is a "high-density" routed board, that any copper less than 7-to-9 mils in width will probably be etched off. Your mileage may vary. By the same token, but only differently.....PCB-fabricators all have told me that any soldermask less than 10-mils in width probably won't really be there on the PCB as well. Their screens just can't go down that far in physical resolution.

[keeping the pour away from the board edges is important standard practice] -- "THANK YOU!!" for also saying this!!! Since you have said this the OP will probably follow your comment. But, coming from me, the OP would have more than likely ignored my comment.

[It's needed so the.....] -- All of that -- AND!!! --.....at least in the environments that my PCB-designs were used in, keeping the "Copper Pour" away from the PCB edges was to also prevent the possibility of any "Ground Loops" from being formed, should something somehow that was already grounded make contact with the PCB. While something like that certainly won't be happening here in this instance, keeping the "Copper Pour" away from the PCB edge is just a good standard practice to follow regardless.

/

 

[sonolink]

The board is symmetrical, flip it around and mount everything in the 5-sided section. Then you can still call the "lid" the bottom. This also pushes the switches up higher on the finished unit, where they can be more easily accessed. The top ends up having 2 screw heads showing, not too bad to live with.

I had thought of that but my friend wants to keep the top "clean". Anyway, thanks for the suggestion

2) Perhaps it is due to the low-resolution of your PCB-layout images, but I fail to see any "thermal-reliefs" anywhere that would connect the "Copper Pour" to GROUND, so right now the "Copper Pour" is floating.

It's not. Copper Pour is connected to shield connections on switch connectors. These are in turn connected to the aluminum enclosure that connect to the RJ45 D-Type panel mounted connectors.

In most cases the purpose of a copper pour is a ground plane, and good stitching top to bottom is important. This design is an exception, it really doesn't need anything on the circuit board grounded. All connectors will "ground" to the (consequently) fully shielding case, that is more than adequate for a headphone level system. Given that, the only purpose a copper pour provides is for a reduction in the use of etchant while making the board. So no stitching needed.

Glad to hear that. Via stitching is a real pain in Diptrace, although I must say I've never used it in the stuff I build (guitar pedals mainly).

But the comment about narrow sections of pour that may become slivers is spot on. Keep the pour fat, never let it drop down below a proper minimum trace width. I'd say 0.25mm is a good minimum. And keeping the pour away from the board edges is important standard practice. It's needed so the solder mask can completely cover the copper around the board perimeter, makes the board easier to router to shape, and safer to handle.

Ok, I'll take that into account and give it another go

[really doesn't need anything on the circuit board grounded] -- If the "Copper Pour" isn't grounded, then it becomes an antenna. Or so that's what the skilled "RF" engineers I have worked with all told me.

[All connectors will "ground" to the (consequently) fully shielding case] -- While I am probably missing something here, I haven't seen any easily identifiable Connector/PCB-to-Chassis/Box grounding method and/or scheme here. Please show me.....

You missed post #117

The "inside" flat cables aren't shielded, so the shield connection will be achieved connecting the GND plane of the PCB to the switches' shield, to the enclosure, to the externally accessible RJ-45 D-Type connector's shield, to external cable shield, to the PSU GND. The section between the amp output and the transformers will NOT be connected to that.

[0.25mm is a good minimum] -- 0.25mm = ~0.010-inch or 10-mils. The PCB-fabricators I have worked with tell me that, unless your PCB-fabrication notes specify in some manner that a PCB is a "high-density" routed board, that any copper less than 7-to-9 mils in width will probably be etched off. Your mileage may vary. By the same token, but only differently.....PCB-fabricators all have told me that any soldermask less than 10-mils in width probably won't really be there on the PCB as well. Their screens just can't go down that far in physical resolution.

Ok, I'll check it out and give it another twist...

[keeping the pour away from the board edges is important standard practice] -- "THANK YOU!!" for also saying this!!! Since you have said this the OP will probably follow your comment. But, coming from me, the OP would have more than likely ignored my comment.

Don't take it personally. Consider this: if you both say the same thing and you feel I'm ignoring you, you're wrong. I don't ignore anybody in this forum. Maybe it's just that people living in Michigan have a different charm than the ones living in Maryland.....just sayin'.....

Thanks to both for your comments, time and help!
Cheers
Sono

 

[MidnightArrakis]

Maybe it's just that people living in Michigan have a different charm than the ones living in Maryland.....just sayin'.....

Thanks to both for your comments, time and help!
Cheers
Sono

[people living in Michigan have a different charm than the ones living in Maryland] -- So.....you are saying that I don't have any "charm"??? HEY!!!.....but, I was born in Flint, MI and some of my relatives still live there, along with their disastrous and deadly water pipelines. HMMmmmmm.....so my "charm" is no good, huh???

/

 

[ccaudle]

the shield connection will be achieved connecting the GND plane of the PCB to the switches' shield, to the enclosure, to the externally accessible RJ-45 D-Type connector's shield, to external cable shield, to the PSU GND.

Sorry, missed that post until you referenced it again in #129.
What you describe is the classic way to inject large amounts of shield noise into your audio circuitry known as "pin 1 problem."
You seem to be really confused about the purpose and structure of a shield, because you say "the shield connection will be achieved..." and then go on to decribe a list of things which are not shields.
A shield is a metallic structure which surrounds the signal wiring and circuitry and is intended to form a faraday cage to keep RF fields out of the signal path.
The key concept there is "out of the signal path," and by taking the shield (which is composed of conductive chassis and conductive outer layers in cables) and connecting it to circuit conductors, you have created a path to inject noise current, which the shield had previously been keeping out of your audio, directly into your audio.

In the case of high-ish voltage signals and passive transformers to drive the outputs like your "B" box, there is no active circuitry, so most of the problems that this mistake can cause will be avoided, but better to correct your understanding now, because it will cause no end of noise problems in other situations (such as potentially the A box).

Shields should be connected together, so cable shields should connect as directly as possible to the shielding enclosure. Power supplies (including the 0V reference node of the power supply, often referred to as "ground,") are not part of the shield, so the cable shields should make no direct connection there.
To avoid uncontrolled capacitive noise coupling from the enclosure to the circuitry the power supply reference should connect to the shielding enclosure at one point. That holds them at the same potential (at least at low frequencies), but does not allow current to flow since there can be no circuit loop with only one connection point.

 

[MicMaven]

[people living in Michigan have a different charm than the ones living in Maryland] --
So.....you are saying that I don't have any "charm"???

Um. Ahem. Perhaps you misread his comment. He says they have a "different" sort of charm ... not that they have no charm.

As a life-long resident of West Michigan, I appreciate your take on coming from Flint, and I also believe Mr. Sonolink's premise is correct - that different areas of the country have their own, distinct charm - different, but all are charming nonetheless. And if you happen to have lived in multiple areas, you may be multi-charmed, which may produce a completely distinct variant altogether! In any case, I hope you are living a "charmed" life !!

Happy trails to you, Old Man. James -K8JHR

 

[sonolink]

Sorry, missed that post until you referenced it again in #129.
What you describe is the classic way to inject large amounts of shield noise into your audio circuitry known as "pin 1 problem."
You seem to be really confused about the purpose and structure of a shield, because you say "the shield connection will be achieved..." and then go on to decribe a list of things which are not shields.
A shield is a metallic structure which surrounds the signal wiring and circuitry and is intended to form a faraday cage to keep RF fields out of the signal path.
The key concept there is "out of the signal path," and by taking the shield (which is composed of conductive chassis and conductive outer layers in cables) and connecting it to circuit conductors, you have created a path to inject noise current, which the shield had previously been keeping out of your audio, directly into your audio.

In the case of high-ish voltage signals and passive transformers to drive the outputs like your "B" box, there is no active circuitry, so most of the problems that this mistake can cause will be avoided, but better to correct your understanding now, because it will cause no end of noise problems in other situations (such as potentially the A box).

Shields should be connected together, so cable shields should connect as directly as possible to the shielding enclosure. Power supplies (including the 0V reference node of the power supply, often referred to as "ground,") are not part of the shield, so the cable shields should make no direct connection there.
To avoid uncontrolled capacitive noise coupling from the enclosure to the circuitry the power supply reference should connect to the shielding enclosure at one point. That holds them at the same potential (at least at low frequencies), but does not allow current to flow since there can be no circuit loop with only one connection point.

I might be incurring in mistakes but I feel there's a language barrier here or I didn't explain myself clearly. What I meant to say was that enclosures, cable shields and copper pours are connected together, hopefully creating a Faraday cage, and in turn connected through ONE point to GND. This point is located at the PSU 0v terminal.
The copper pour is only connected to the shield terminal of the switches. Nothing else. The switches' shield terminal is connected to the enclosure only, which in turn is connected to the shield of the D-Type RJ45 panel connector, so that when a 6/7/8 cable is inserted between Box A and Box B, its shield is connected too and Box A's enclosure is connected to the shield. Finally, Box A's enclosure is connected to the PSU 0v terminal.
What am I doing wrong?

 

[sonolink]

The transformers arrived. Trying to determine which ones are Primaries and Secondaries I measured Resistance and I get 3R in one coil and 88R in the other. They all measure very similar. I guess 88R is Primary and 3R Secondary, right?


One more question regarding PCBs please: what would be the minimum acceptable trace width in this case? 0.5mm?

Cheers
Sono

 

[MidnightArrakis]

Um. Ahem. Perhaps you misread his comment. He says they have a "different" sort of charm ... not that they have no charm.

As a life-long resident of West Michigan, I appreciate your take on coming from Flint, and I also believe Mr. Sonolink's premise is correct - that different areas of the country have their own, distinct charm - different, but all are charming nonetheless. And if you happen to have lived in multiple areas, you may be multi-charmed, which may produce a completely distinct variant altogether! In any case, I hope you are living a "charmed" life !!

Happy trails to you, Old Man. James -K8JHR

[Happy trails to you, Old Man] -- I am "strongly offended" (HA!!!) to being referred to as "Old Man", because in reality, I am -- OFFICIALLY -- an "Old Fart"!!! That term.....I'm very happy with. THANK YOU!!!

/

 

[ccaudle]

What I meant to say was that enclosures, cable shields and copper pours are connected together

Almost clear. I'll leave this here to explain my thinking, but see below, I misread one connection that made it seem worse than it is.
Enclosures and cable shields are alike in that they are external conductive structures which enclose signal paths.
Copper pours are not external, being on the PCB they are by definition inside the shield enclosure, so by connecting copper pour to the shield at multiple places (multiple switches [EDIT: originally said switches and connectors]) you have now made a shield extension inside the enclosure, and any RF potential difference across the enclosure will cause current to flow in loops across the PCB. That creates a transmit antenna for any interference that had hoped would stay outside to be broadcast around inside your enclosure, or capacitively coupled directly into signal paths.

I had previously misread slightly and thought that the pours were connected to the switch shell terminal and also the shield connection from the D connectors fed through to the PCB mount Ethernet connectors. That would have created a path for currents to flow all the way across the PCB. Since the switches are right next to each other the points are close together with nothing in between, so effectively the two connections points are close to a single point.
So on reading more carefully I think you are right, but I am going to leave the wordier explanation above to explain my original (mistaken) objection.

 

[MicMaven]

[Happy trails to you, Old Man] -- I am "strongly offended" (HA!!!) to being referred to as "Old Man", because in reality, I am -- OFFICIALLY -- an "Old Fart"!!! That term.....I'm very happy with.

Roger ... Um ... my mistake.

{Gratuitous Sidebar - OM and OF are common Morse Code abbreviations used by amateur ratio operators, and they NOT considered mutually exclusive. . . but I will be more rigorous in the future!} ​

SERIOUS NOVICE QUESTION -- Why would the width of the PCB trace matter? I do not wish to derail or distract the thread, but I do not know why that would be a concern. Thanks, in advance. James

 

[MidnightArrakis]

Roger ... Um ... my mistake.

{Gratuitous Sidebar - OM and OF are common Morse Code abbreviations used by amateur ratio operators, and they NOT considered mutually exclusive. . . but I will be more rigorous in the future!} ​

SERIOUS NOVICE QUESTION -- Why would the width of the PCB trace matter? I do not wish to derail or distract the thread, but I do not know why that would be a concern. Thanks, in advance. James

[OM and OF are common Morse Code abbreviations] -- I sincerely apologize!!! I didn't know that you were writing to me in "Morse Code"!!! Otherwise, I wouldn't have mentioned anything.

[I do not know why...the width of the PCB trace...would be a concern] -- In the similar manner to that of using a piece of wire, a wider PCB trace will lower the resistance, inductance and other parameters between any two points within a circuit. Do you want to try and run 15-Amps through a 22-GA wire??? Of course not!!! You would want to use at least a 12-GA wire and using a 10-GA wire would be even better!!!

[sonolink: what would be the minimum acceptable trace width in this case? 0.5mm?] -- 0.5mm is roughly equivalent to around 20-mils, which is what I would consider to be an absolute minimum track width. But, since there really isn't much of anything else going on here, I would feel more comfortable using 30-mil tracks and if there is the room available.....40-mil or 50-mil tracks would be great!!! Others may consider this to be an "overkill", but.....if the room is available for even wider tracks, then go ahead and use them (per constraints as are detailed down below). Remember, any and all copper that you -- DON'T -- use.....is just simply washed down the drain and you have already paid for that copper!!!

1.3 What affects impedance?
In summary, as stated in some of the PCB transmission line models in section 1.1, the impedance
of PCB signal traces is affected by:

• The height of the dielectric layer between the signal trace and the reference planes
• The width and the thickness of the signal trace
• The dielectric constant of a dielectric material
• The spacing between differential pairs traces


PCB Trace Width and Spacing Examples
PCB trace widths and spacings can affect the circuit board in many ways. Here are four areas to consider when deciding what width and spacing values to use:

Electrical Performance and Signal Integrity
Most digital routing on a circuit board will use a default value for its trace widths and spacings, but some nets will require different sizes. Controlled impedance nets, for instance, will need their trace widths calculated based on the configuration of the board layer stackup. Sensitive high-speed traces may require larger spacing values to prevent crosstalk and other signal integrity problems.

Analog routing may also require unique trace widths and spacings depending on the purpose of the circuitry. In some cases, the default trace width may be reduced in tight and constricted areas, but care has to be taken that this isn’t extended across the board. If the trace gets so thin that it gets compromised during PCB fabrication, then the signal integrity of the entire board could be compromised.

Power and Ground Routing
Traces used to route power and ground need to be wider to conduct greater amounts of current. If the traces are too thin, they can get hot and even burn through. Power traces routed on the internal layers of the board also need to be wider for heat dispersal than those routed on the external layers, as exposure to the air will provide more cooling. For those traces that are used in power supply circuitry, it is important to keep them as short and as wide as possible to handle the current, as well as to reduce inductance and noise in the circuit. It is important to increase the spacing for traces that are carrying higher current to prevent the power from arcing between them.

Circuit Board Fabrication
The wider a trace is, the easier it is to fabricate. The fabrication etching process will have a greater effect on traces that are long and isolated, so it is better to make them wider when possible. A 20 mil trace will have a much greater tolerance for losing metal than a 3 mil trace would. Trace widths are also dependent on the weight of the copper being used to build the layer of the board. If that layer of the board requires a greater copper weight due to higher current requirements, the fabricator may not be able to etch thinner trace widths on it as well.

Circuit Board Assembly
Traces that are too wide can affect how easily the components will solder during PCB assembly. The wide traces used for power and ground nets can also act as a heat sink, leading to uneven heating and poor solder joints. Small two-pin parts that are connected to a large area of metal on one pad and a thin trace on the other may be unbalanced enough that the component will be pulled up on end during solder reflow. This effect is known as “tombstoning” and will force manual rework of the board for corrections. An abundance of metal under a BGA can also cause problems during soldering as well, but these errors are more difficult to find due to the size of the BGA on the board.

With all of the potential problems that can happen if the right trace widths and spacings are not maintained, PCB layout engineers need all the help that they can get. Fortunately, there are utilities in the design tools that can help with this.

/73

 

[sonolink]

[I do not know why...the width of the PCB trace...would be a concern] -- In the similar manner to that of using a piece of wire, a wider PCB trace will lower the resistance, inductance and other parameters between any two points within a circuit. Do you want to try and run 15-Amps through a 22-GA wire??? Of course not!!! You would want to use at least a 12-GA wire and using a 10-GA wire would be even better!!!

[sonolink: what would be the minimum acceptable trace width in this case? 0.5mm?] -- 0.5mm is roughly equivalent to around 20-mils, which is what I would consider to be an absolute minimum track width. But, since there really isn't much of anything else going on here, I would feel more comfortable using 30-mil tracks and if there is the room available.....40-mil or 50-mil tracks would be great!!! Others may consider this to be an "overkill", but.....if the room is available for even wider tracks, then go ahead and use them (per constraints as are detailed down below). Remember, any and all copper that you -- DON'T -- use.....is just simply washed down the drain and you have already paid for that copper!!!

The reason why I asked about the traces width is because these PCBs are really running speaker cables, if you know what I mean. In pedals, usually I do 0.3mm traces for signal and 0.5mm for power. Since we're sending a speaker output through the PCBs I thought I should check the width first. I can do the traces even wider but then many traces would be side by side with no copper pour between them. I always tend to keep pour between traces, although in this case it's not really meaningful?

About my previous transformers question: trying to determine which ones are Primaries and Secondaries I measured Resistance and I get 3R in one coil and 88R in the other. They all measure very similar. I guess 88R is Primary and 3R Secondary, right?

Cheers
Sono

 

[Hubbub]

The traces here are handling at most the power needed for 20 headphones, maybe 4 watts or so. Not really like speaker cables, which can run 100+ watts at 4 ohms, i.e. amps. Damping factor presented to the load is also not a concern, that will be mostly determined by volume control setting. So keeping the entire feed loop (including trace resistance) in the low milli-ohms is not a goal here. Add a generous 4 watts for the volume control loss. With an bridge output amplifier running off 18-19 volts you can get maybe 11V RMS. At 8 watts you are below 0.75 amp of current in the A and first B box, less in subsequent B boxes.

I'll add I'm not a PCB or packaging designer, although I've supervised them for developing my designs. And I too am an opinionated "old fart" in too many respects. So in general I would suggest keeping traces as wide as practical between the RJ-45 connectors, use beefy pads for anything that is used for mounting (switches, jacks, pots, transformers), and for interconnections keep to a reasonable minimum, 0.3-0.4mm works. To calculate trace width precisely one needs a slew of factors to be considered, such as expected current, copper thickness, internal vs. external placement, allowable temp rise, etc. (PCB Trace Width Conversion Calculator | DigiKey) and more if running controlled impedance and differential high-speed signals. Been there, done that. I would suggest not getting hung up on that aspect of PCB design for this application.

Provided the lid fits well (???) you will be fully RF shielded, so I have no concern for "RF across the copper pour" (unless it comes in on the speaker lines). Even then, you have no non-linear devices in the circuit, so little chance for rectification (and subsequent audibility) to be a concern. Frankly, I'd have no concern if the entire copper pour was floating. In this design it is mainly to reduce etchant load, it is not needed as a ground plane or a shield. Since I am currently plagued with a recent sheet metal cut on my thumb I can't over-emphasize the value in pulling the pour back from the edge of the board.

As for the transformer, winding resistance can be misleading, but is OK as a beginning indicator. To quickly test a transformer put 1V (or more, for an output transformer) of 1KHz audio across the higher resistance winding, and measure AC the voltage at the lower resistance winding. A budget dual-trace digital scope is handy for doing this as you can see if either waveform differs from a clean sinusoid, and get the RMS readings as well. The ratio of voltages is the turns ratio, and the impedance ratio is the turns ratio squared. Given that the transformer is rated 8 ohms on the output use the impedance ratio to determine the input impedance. And don't be concerned if something falls 10% - 15% different from what you expected, it will still work.

Hope that helps!