PCB Draft (still new at this)

GroupDIY Audio Forum

Help Support GroupDIY Audio Forum:

This site may earn a commission from merchant affiliate links, including eBay, Amazon, and others.
In your image file - 1.34.06 - the pads that are connected to your COPPER POUR need to have "Thermal Reliefs" on them. This should be a setting somewhere in whatever PCB design program you are using. If those pads - don't - have them, then the COPPER POUR will act as a heatsink when you are trying to solder whatever goes into those pads and the integrity of your solder joint will be at risk.

You can "turn-off" whatever layer the Part Name is on and the reversed magenta text as well. They're not needed. At least in your GERBER files. And, speaking of GERBER files, if your PCB design program has the capability, you - REALLY - want to output what is called an - ODB++ - file instead. The much beloved GERBER files are now archaic and outdated, besides being "non-intelligent" and the ODB++ output file is "computer-friendly" and contains more than enough information to have your PCBs fabricated, electrically tested and even assembled.

In your image file - 1.58.41 - below R11, that track junction is called an "acute angle", which is also known as an "acid trap". What this means is, as your board is going through the etching process of removing the unneeded copper from your board, etching acid will become trapped in that tight angle and will ever so slightly etch - underneath - your route. Then, even though your board will "look fine", over time the copper of that route will loosen itself away from the laminate material and possibly create a problem. But, since these things take time to happen, then maybe you don't care. The types of PCBs that I design, it is required that I - HAVE - to care!!!

I have requested a couple of times that you send me your PCB file so I can take a better and closer look at your layout in my ($3,500) PCB layout program. This would allow me to see how your program is setup and I could then offer you some suggestions on a "Configuration Template" or something along those lines.

While, in general, it is a good thing in the manner in which you are adhering to the X/Y routing scheme on each of the layers, keep in mind that it is certainly permissible to "violate" that scheme, if you can eliminate some vias. I see some instances here and there in your layout where if you placed one route on the "wrong" layer, you could then easily place another route or two on its current "opposite" layer instead and end up eliminating some vias. I am unable to give you any specific areas as I cannot read your PCB text well enough to give you any REF Des's. The GREEN track below C20 is one route I am speaking of.

By the way.....the colors that I had provided you with earlier are - NOT - arbitrary colors. They actually have a history to them and it is a history that I have personally worked in and everybody else in this thread is too young to know about or possibly care. It all goes back to when PCBs were layed-out manually by hand using a variety of adhesive taping methods. Initially, the materials were all black in color. Eventually, colored materials were used and colored filters were used on the cameras that created the films that were used for each different layer of the PCB. When computers came onto the scene and were used to design PCBs, it only made sense for the PCB Designers to transfer their familiar manual color schemes over to their computerized designs. But, that actually couldn't be done until color monitors became available for general use. And.....there is actually a logic behind what the colors are and why. Go back and review the color scheme I gave you and analyze the colors and their layer associations and then figure out "why things are the way they are"!!! Hidden logic.

After you think you have the logic figured out, let me know what your results are, OK??? I would like to know. And, if you cannot figure it out, I'll tell you "why things are the way that they are". But, in any case.....you can use whatever colors in any manner that you want to. I'm - NOT - telling you what to do. I am just letting you know that there is an actual history to "PCB design colors", although I will be criticized by others on this forum for even suggesting to you what colors to use in your CAD program. Such is life, huh???

Anyway.....I have attached some PCB Design and layout information which you will hopefully find to be of some use. In reality, I - could - provide you with enough material that covers the PCB design area that you could spend 10-hours a day for months.....just to learn all of the ins and outs of PCB design.

GOOD LUCK!!!

/
 

Attachments

  • IPC Class 3 Design Guide.pdf
    1.4 MB · Views: 9
  • Fundamentals-of-PCB-Technologies.pdf
    7 MB · Views: 8
  • PCB Design Rules for Analog Circuits.pdf
    133.8 KB · Views: 9
  • Top-10-Circuit-Board-Design-Checks.pdf
    1.9 MB · Views: 9
If the image of your PCB showing the dark-red COPPER POUR is how everything actually is, then you should back off the COPPER POUR 50-mils from the edge of the PCB. The same will go for your SOLDERMASK layers as well. In general, you don't want certain items going all of the way out to the edge of the board, as one type or another of fabrication problem will arise. While I am certain that there will be those on this forum who will heartedly disagree with me, trust me.....you don't want your COPPER POURS or SOLDERMASKS going out to the edge of your PCB.

/
 
Interesting information all around, really appreciate all the members.

I am wondering, would it make sense to use the bottom side of the board as a signal ground plane or copper pour, and fill the top side for the power ground return? Instead of trying to route the power ground pins for all the reservoir caps as a star ground, just do a copper pour and connect that to power ground?

Or is that a bad idea for some reason that I am not seeing?

Thanks!
 
Interesting information all around, really appreciate all the members.

I am wondering, would it make sense to use the bottom side of the board as a signal ground plane or copper pour, and fill the top side for the power ground return? Instead of trying to route the power ground pins for all the reservoir caps as a star ground, just do a copper pour and connect that to power ground?

Or is that a bad idea for some reason that I am not seeing?

Thanks!
It may sound like anathema to many, but star ground is not the best arrangement for low-noise, because it does not minimize the path length. It works in many cases because brute force is used, large gauge wires and connectors. I advocate hierarchical ground whenever is possible, which relies on very short paths from stage to stage. Indeed there are cases where it's not practically achievable because of the size of components and other layout constraints. It becomes clearer when you consider each PCB trace as a resistor.
Read my sig!
 

Latest posts

Back
Top