Help/advice/guidance translating schematics onto a pcb

[Cqwet Dbdfte]

Not sure how KiCAD does DRC (design rules check) but board houses like JLC has design rule setups for various programs, to make the board both manufacturable and (mostly) error free. (but not optimal).
You may see some faint lines around tracks and vias, do not put anything inside those.

 

[djmiggymigz]

Not sure how KiCAD does DRC (design rules check) but board houses like JLC has design rule setups for various programs, to make the board both manufacturable and (mostly) error free. (but not optimal).
You may see some faint lines around tracks and vias, do not put anything inside those.

Yupp, I found a github files that loaded all the JLC rules in and then double checked/edited the numbers myself in reference to JLC's website! Learned a good bit there too since I had to figure out what "annular width" is among most other parameters!

1) The -- acute angles -- that you see here in this image of your PCB-layout are also known as "acid traps"!!! These are a NO-NO!!!

View attachment 137093

What happens here is.....during the fabrication etching process, the acid that is used to etch the copper off of the laminate is caught inside these -- acute angles -- and ends up ever-so-slightly etching away the copper -- UNDERNEATH -- these angles. Over a period of time, the copper tracks at these points of your PCB may loosen and cause the PCB-track to actually pull-away from the laminate itself. What this means is.....you need to perform all of your track-routing to be be either at a 45-degree or a 90-degree angle.

In addition.....and, I am only assuming that this image may have been taken with the PCB at a slight angle, but.....this image shows that your component copper pad and your N/C Drill hole are -- NOT concentric -- meaning, they're not in perfect alignment with one another. In other words, the "white hole" and the "yellow pad" should be in perfect alignment (or, "concentric") with each other.

2) Your -- track-to-pad -- clearances are "WAY TOO CLOSE" than is necessary:

View attachment 137094 -- View attachment 137095 -- View attachment 137096
>> Don't be afraid to offer at least 15- to 20-mils of clearance between
your tracks and pads, especially on a layout as "loose" as this.

3) R8 is both placed and routed as a -- stub-route -- scenario:
View attachment 137097
View attachment 137098
>> The two upper-most yellow pads shown here are the component pads for R8 and the lower-left corner track that connects to another pad and then angles upwards to the upper-left at a 45-degree angle (also creating the "acute angle") is its same net connecting track. Since R8 is placed in the manner in which it is, technically.....it is -- NOT -- directly within the circuit's operation, but instead is "off-to-the-side", so to speak. While doing this may not much matter with a resistor, it -- DOES -- make quite a difference with capacitors!!! I have worked inside many engineering environments where the Electronics Engineers have literally shown me on their test equipment how the placing and routing of a component using a "stub-route" makes a difference in the circuit operation. And, this minute effect is additive as well. Meaning, the more components that are placed and routed using -- stub-routes -- the less the overall circuit behaves as it was designed to do!!!

However, while in your particular layout circumstance, it probably doesn't matter one hoot.....-- NOT -- placing and routing components in a --stub-route -- situation is a good habit to learn about and get into as you are learning the "PCB Design" ropes and techniques.

/

Yeesh thank you for such a detailed response and critique!! I didn't notice those acute angles at all. I have KiCad set to place tracks at 45/90 degrees but looks like 2 45's meeting caused that issue! Is this something that will still work just is not ideal? I fixed it in the design but I already ordered the pcb's using the design that you were referencing so unless its mission critical to fix that I may jusst try the existing boards out. (The jfets I bought arent cheap tho so I'd rather not risk frying them!)

Also, yeah I took these screenshots in KiCad's 3D model viewer which automatically displays the board from a perspective that shows the depth of the board.

 

[djmiggymigz]

Another question: What's the benefit to adding vias all over the board to make it look "perforated"? I've been seeing a bunch of pcb designs that have this. I think I'm getting close to wrapping up my 312 layout and have a lot of space so might toss a bunch of small vias in where I can.

 

[Cqwet Dbdfte]

Lower impedance reference plane /"ground". Better than "star" ground. All circuits are RF circuits, especially when you don't want it.
I also ground my mounting via's / holes.

Google it.

 

[ruffrecords]

Lower impedance reference plane /"ground". Better than "star" ground. All circuits are RF circuits, especially when you don't want it.
I also ground my mounting via's / holes.

Ground is an unfortunately vague term which should not be used unqualified in an audio discussions. In audio designs there are generally two grounds to consider "0V analogue" and "chassis". 0V analogue is the audio signal reference and is typically the trace that is made into a ground plane of a PCB. Minimizing its impedance is a good thing in general however, in all but the simplest of designs, it is only possible for this ground plane to cover a significant area of one side of the board (because all the other connections are on the other side). Flooding the opposite side and stitching it to the ground plane with vias may provide little additional lowering of impedance. In addition, if there are any high impedance signal traces (as there are in this design) it is important not to add any unnecessary capacitance to ground which is exactly what a ground plane may do.

"chassis" is the metalwork of the enclosure. Its purpose is to route interference away from 0V analogue and straight to safety earth. 0V analogue is also connected, at one point only, to safety earth. You therefore need to take care that mounting holes connected to 0V analogue do not accidentally create an additional connection between 0V and safety ground.

Cheers

Ian

 

[Cqwet Dbdfte]

Ground is an unfortunately vague term which should not be used unqualified in an audio discussions. In audio designs there are generally two grounds to consider "0V analogue" and "chassis". 0V analogue is the audio signal reference and is typically the trace that is made into a ground plane of a PCB. Minimizing its impedance is a good thing in general however, in all but the simplest of designs, it is only possible for this ground plane to cover a significant area of one side of the board (because all the other connections are on the other side). Flooding the opposite side and stitching it to the ground plane with vias may provide little additional lowering of impedance. In addition, if there are any high impedance signal traces (as there are in this design) it is important not to add any unnecessary capacitance to ground which is exactly what a ground plane may do.

"chassis" is the metalwork of the enclosure. Its purpose is to route interference away from 0V analogue and straight to safety earth. 0V analogue is also connected, at one point only, to safety earth. You therefore need to take care that mounting holes connected to 0V analogue do not accidentally create an additional connection between 0V and safety ground.

Cheers

Ian

Right, "ground" can mean a few different things. HV circuits may not be able to handle a high capacitive load, and voltage isolation and creep/tracking distance norms needs to be observed. Extra insulation by cuts/gaps in PCBs is often used to increase creep distance.
Bonding power entry ground directly to chassis is most often done but other solutions exist, like separating the AC safety ground over a pair of high current diodes, or a rectifier bridge, beefy enough to survive a breaker/fuse activation with a "AC hot" to case short.
Much is written on the subject.

 

[djmiggymigz]

Ouu okay I may need to do some re-evaluating of this 312 design then. As you said @ruffrecords , there's only one point in the circuit where my AudioGND is connected to ChassisGND however, KiCad seems to have interpreted that as continuity between all points of audio vs. chassis GND's? For example, my pin 1 on the 500 series card (ChassisGnd) got mapped to the same net as my AudioGND. Meaning its not attached directly to anything other than the AudioGND plane that I have (when in the PCB layout view).

Posting my schematic thus far for reference. (Not done yet, still figuring out how to add a couple things as well as considering several ideas).

So am I interpreting correctly that Chassis and Audio GND's should not be connected throughout the circuit?

 

[MidnightArrakis]

Another question: What's the benefit to adding vias all over the board to make it look "perforated"? I've been seeing a bunch of pcb designs that have this. I think I'm getting close to wrapping up my 312 layout and have a lot of space so might toss a bunch of small vias in where I can.

[What's the benefit to adding vias all over the board to make it look "perforated"?] -- Those types of vias are known as "stitching vias" because they "stitch" the Copper Pours on each side of the PCB together. Think of these vias this way:

Imagine that the "barrel" of the via (the Plated-Thru drill hole) as being a resistor. As you (should) know, resistors in parallel have a lower total resistance. Therefore, the more "stitching vias" (resistors) that you have on your Copper Pours (being all in parallel with one another), the lower the total resistance will be and the closer the two Copper Pour -- GND -- potentials will be the same.

[KiCAD seems to have interpreted that as continuity between all points of audio vs. chassis GND's] -- While I -- think -- I understand what it is that you are attempting to explain here, I don't think you have explained your situation very well. Or, I'm just dense!!! In any case.....

Your included schematic image was too fuzzy for me to read, so I can't specifically assist you. Next time, go ahead and attach your KiCAD schematic file so those of us who also have KiCAD can simply load it in and view it directly (although you may need to add an extra filename extension so the forum system doesn't reject it. Like this: filename_schematic.kicad_sch -- renamed to be -- filename_schematic.kicad_sch.pdf -- Even though the file is actually a schematic file, this forum will recognize it as a PDF file and allow for it to be attached).

Any nodes on a schematic that have the same net-name will be connected electrically together. What is typically done is that different GROUND nets that are eventually tied together are routed separately on the PCB to a single-point location and then they are connected together either using a Zero-Ohm resistor, a jumper-wire or maybe a 3-pin terminal header with a removable jumper plug, so (as an example) when Pins 1 & 2 are jumped together the GROUNDS are connected but when Pins 2 & 3 are jumped together, the GROUNDS are -- NOT -- connected together. Whatever floats your boat!!!

/

 

[djmiggymigz]

OHHHH that makes so much sense thank you!! That's very cool, the more I learn the more enthralled I am with the way certain properties are used to create a huge benefit in and throughout designs! Thanks for such a detailed explanation for that!

Yeah I noticed that after I posted it :/ Here's the KiCad file if you have a second to take a look at it! So what I was referencing is that most of the ground connections are made to pin 5 on the card which is "AudioGND". The only ChassisGND (Pin 1) happening is in the schematic is at the top of the schematic coming from the LED and is happening in parallel with an AudioGND connection (Through R13). Now when I go to PCB mode, Pins 1 & 5 are tied to the same net. Meaning anything connected to AudioGND is also connected to ChassisGND and the only ChassisGND connection that's supposed to be happening is happening through the connection/net to AudioGND.

God that felt like such a mouthful as I was typing it hahah, apologies to the readers.

 

[Cqwet Dbdfte]

OHHHH that makes so much sense thank you!! That's very cool, the more I learn the more enthralled I am with the way certain properties are used to create a huge benefit in and throughout designs! Thanks for such a detailed explanation for that!

Yeah I noticed that after I posted it :/ Here's the KiCad file if you have a second to take a look at it! So what I was referencing is that most of the ground connections are made to pin 5 on the card which is "AudioGND". The only ChassisGND (Pin 1) happening is in the schematic is at the top of the schematic coming from the LED and is happening in parallel with an AudioGND connection (Through R13). Now when I go to PCB mode, Pins 1 & 5 are tied to the same net. Meaning anything connected to AudioGND is also connected to ChassisGND and the only ChassisGND connection that's supposed to be happening is happening through the connection/net to AudioGND.

God that felt like such a mouthful as I was typing it hahah, apologies to the readers.

You can "print" your schematic with a .pdf as the output. The above is just a .xml file rendered as text in a .pdf.

 

[djmiggymigz]

maybe this will work as well!

 

[ruffrecords]

Bonding power entry ground directly to chassis is most often done but other solutions exist, like separating the AC safety ground over a pair of high current diodes, or a rectifier bridge, beefy enough to survive a breaker/fuse activation with a "AC hot" to case short.
Much is written on the subject.

Unfortunately, anything other than a direct bond to chassis will fail both UL and CE safety requirements.

Cheers

IAn

 

[djmiggymigz]

What's most commonly connected to the chassis GND in the case of 500 series pres? +48v when not engaged?

I edited my PCB layout so that ChassisGND is no longer on the same net as AudioGND and routed the LED straight to ChassisGND. Haven't added my mounting holes yet but I think those should be connected to ChassisGND as well right?

 

[ruffrecords]

What's most commonly connected to the chassis GND in the case of 500 series pres? +48v when not engaged?

Nothing at all

The 0V of the 48V is only required on the mic pre if you use 48V to light an LED

I edited my PCB layout so that ChassisGND is no longer on the same net as AudioGND and routed the LED straight to ChassisGND. Haven't added my mounting holes yet but I think those should be connected to ChassisGND as well right?

0V of 48V should not be connected to chassis ground on the mic pre PCB. The 0V of your 48V power supply should be wired directly to the pins 1 of the mic input connectors. There is no reason your mounting holes should be connected to chassis ground. Their purpose is solely mechanical.

Cheers

Ian

 

[djmiggymigz]

Okay interesting very good to know!

I am planning on an LED in circuit with the 48V switch when in the "on" position.

 

[Cqwet Dbdfte]

Unfortunately, anything other than a direct bond to chassis will fail both UL and CE safety requirements.

Cheers

IAn

Yep!

 

[zamproject]

I am planning on an LED in circuit with the 48V switch when in the "on" position.

P48 spec is low current (10mA ?), you better not use a LED on this rail.
Using a dual switch may be preferable, one section for actual P48, one section for the led supplied from signalling or audio rail

 

[vintageampfixer]

Interesting thread and a good steer for me about KiCad. I'd always done PCB layouts on grid paper in the past or perhaps tracing paper over a 0.1" grid with red pencil on one layer for east-west, and blue pencil on a second layer for north-south ...

With "more time on my hands these days", I was looking for something to bring my PCB layouts into at least the 20th Century, if not right into the 21st ... anyway, the upshot was I downloaded CircuitMaker but I can't say I love it, so I'll be happy to look at an alternative!

 

[Disco Volante]

Learning a lot here. Thanks gents!