1st design

[GARTHWILSON]

BillO wrote:

Do the two enables on the 40x4 LCD need to be controlled separately?

40x4 LCDs are actually two separate 40x2 LCDs in one package. The other lines can be bused; but there's one enable for each of the two LCDs.

[plasmo]

sburrow wrote:

First, is this a 2-layer or a 4-layer board? I see lines running to and from those bypass capacitors, which makes me think it's a 2-layer board. BUT the traces for those (which would be VCC and GND) are really tiny, just as big as a signal trace. I personally don't know if that really changes anything, but I was told and implement myself larger traces for VCC and GND coming from capacitors.

Good catch about the power/ground traces. They absolutely need to be wide traces and forming a grid, especially the ground. The board is unlikely to work in current implementation. If the boards are already in fabrication, you'll need to solder additional ground wires from CPU to RAM, EPROM, and decoding logic. That'll at least get the board to power up and then you can use the board to troubleshoot rest of the circuit. Fortunately, the RAM and EPROM are slow parts. Use the slow old CMOS 65C02 if you have it. WDC's W65C02 is much too fast and noisy for this board design. Good luck,
Bill

[jzaun]

plasmo - it’s not to late. Is it better to just have a solid inner GND and VCC plane, making it 4 layers? It’ll cost more but that’s not an issue. I’d rather do it right, that why I’m here… to learn :)

[plasmo]

Yes, 4-layer pc board is the safest approach. It is also easier to route because power/ground are pre-routed in the inner layers.
Bill

[BigDumbDinosaur]

jzaun wrote:

Is it better to just have a solid inner GND and VCC plane, making it 4 layers?

I highly recommend it! Everything I've built to date has been four-layer and I have not regretted it.

Even with four layers, you must bypass each piece of silicon—I use 0.1µF at 50 volts X7R MLCCs for that purpose. You want them tight up against the VCC end of the chips, with short leads. It's all about minimizing inductance and making it easy for switching noise to get to ground.

We have a topic on building a reliable, high-speed design. It's worth a read before you commit to getting your boards made.

[sburrow]

BigDumbDinosaur wrote:

jzaun wrote:

Is it better to just have a solid inner GND and VCC plane, making it 4 layers?

I highly recommend it! Everything I've built to date has been four-layer and I have not regretted it.

Even with four layers, you must bypass each piece of silicon—I use 0.1µF at 50 volts X7R MLCCs for that purpose. You want them tight up against the VCC end of the chips, with short leads. It's all about minimizing inductance and making it easy for switching noise to get to ground.

We have a topic on building a reliable, high-speed design. It's worth a read before you commit to getting your boards made.

It was BDD who convinced me to use 4-layer boards as well. And I am very thankful that he did! Honestly I probably couldn't design a 2-layer board correctly at this point, because I'm very reliant on the inner VCC and GND planes. Routing is so easy and I have confidence in it's reliability. Because of the enormous cost of larger 4-layer boards, I refuse to go above the 10cm x 10cm mark, ever. If it doesn't fit, then I need a second board or I didn't need that feature to begin with. Just my way of thinking, that's all, I try to be super frugal.

As per that sticky topic on high speed design: I just went through it myself 2 days ago. The whole thing. And there is good information there, but honestly it's so congested and hard to comb through. There are SO MANY links and tutorials and videos and information there, but getting a straight answer through it is a bit hard. On top of that, we all seem to have different opinions on specifics. If we are recommending outside links, I would recommend EVERYTHING from Garth Wilson's 6502 Primer pages. Literally gold.

Chad

[plasmo]

sburrow wrote:

It was BDD who convinced me to use 4-layer boards as well. And I am very thankful that he did! Honestly I probably couldn't design a 2-layer board correctly at this point, because I'm very reliant on the inner VCC and GND planes. Routing is so easy and I have confidence in it's reliability. Because of the enormous cost of larger 4-layer boards, I refuse to go above the 10cm x 10cm mark, ever. If it doesn't fit, then I need a second board or I didn't need that feature to begin with. Just my way of thinking, that's all, I try to be super frugal.

4-layer pc board is like apple pie and motherhood, especially if it is affordable and nowaday it is. I am moving toward 4-layer boards as well, but looking at 57 board designs I did in 2019, 58 designs in 2020, and 25 designs in 2021, I can only find four 4-layer designs, all done in later half of 2021 when 4-layer pcb became affordable. The other 136 2-layer designs worked just fine, except one 68020 motherboard with 16-meg dynamic RAM that generated excessive refresh noise which was promptly fixed with a 4-layer design.
Bill

[Dr Jefyll]

I'm not opposed to four-layer, but there are both pros and cons to be weighed.

Yes, routing is somewhat easier, because about 10 or 15% of your traces go away. Not that big a deal, IMO, although admittedly the traces that go away (ie, Vcc and Ground) are the ones that are more difficult for a novice to do properly -- I mean "properly" if good AC performance is required. But this excludes many novice projects.

sburrow wrote:

Because of the enormous cost of larger 4-layer boards, I refuse to go above the 10cm x 10cm mark, ever. If it doesn't fit, then I need a second board [...]

I'm not opposed to using a second board, either. But once again there are both pros and cons.

I see Bill (plasmo) has posted while I was typing, and I echo his point that a two-layer board is usually entirely viable.

-- Jeff

[sburrow]

Dr Jefyll wrote:

sburrow wrote:

Because of the enormous cost of larger 4-layer boards, I refuse to go above the 10cm x 10cm mark, ever. If it doesn't fit, then I need a second board [...]

I'm not opposed to using a second board, either. But once again there are both pros and cons.

I'm just sharing my personal thoughts on the matter. Indeed there are pros and cons, but at my stage, if it doesn't fit on one board with auto-router, then I'm probably allowing feature creep to set in. Heck my third board coming soon has PS/2 Keyboard, a SNES controller port (which is hunkin' huge), and tons of plug-and-play ports.

And of course this is coming from the guy who refuses to spend $40 on a EPROM programmer, no more than $8 on a board, yet will spend over $100 on chips! Take it with a grain of salt.

plasmo wrote:

I am moving toward 4-layer boards as well, but looking at 57 board designs I did in 2019, 58 designs in 2020, and 25 designs in 2021, I can only find four 4-layer designs, all done in later half of 2021 when 4-layer pcb became affordable. The other 136 2-layer designs worked just fine, except one 68020 motherboard with 16-meg dynamic RAM that generated excessive refresh noise which was promptly fixed with a 4-layer design.

Bill, I didn't know you were so... prolific!

Chad

[plasmo]

sburrow wrote:

Bill, I didn't know you were so... prolific!

It is prototyping with PC board, JLCPCB and Seeed Studio make it possible with fast turn and cheap boards. DHL shipping is the real winner, however.
Bill

[BigDumbDinosaur]

Dr Jefyll wrote:

Yes, routing is somewhat easier...

Have to disagree with you there. Routing is substantially easier, and what is also easier is achieving high component density. That translates to a smaller board for any given design, which translates to a less-expensive board.

As I earlier said, I endorse the use of four-layer construction—the performance benefits are too hard to ignore. From a cost standpoint, yes, there are tradeoffs—you're going to pay more for a four-layer board. However, per-piece costs have drastically reduced in the last several years. Board houses such as JLCPCB are producing four-layer boards right now at price points that got you only a two-layer board five years ago. All of my POC units have been four-layer and I'm paying about half as much right now than I did four years ago for boards of or close to the same size. In fact, with my last two orders for boards from JLCPCB I got five boards per order for about one-fourth the cost that three boards cost me in 2018. Sucha deal!

BTW, I even use four-layer construction with some of my non-computer designs, mainly for the density and routing benefits—none of those designs is noise-sensistive.

[jzaun]

Hi again :)

I've been reeding the "Techniques for reliable high-speed digital circuits" sticky. There is a ton in there and I'm trying to grasp at least some of it. I also learn a lot by doing and getting feedback, so this is my current PCB setup. I split each layer out. Have I made any glaring mistakes?

[GARTHWILSON]

Run the planes between each pair of pads, for much better AC performance, so signals' ground return current doesn't have to veer away from the signal line and go clear around the end of the IC. There's plenty of room to get it between pads.

[jzaun]

GARTHWILSON wrote:

Run the planes between each pair of pads, for much better AC performance, so signals' ground return current doesn't have to veer away from the signal line and go clear around the end of the IC. There's plenty of room to get it between pads.

I'll set the GND plane clearance to 0.254mm so it goes between all the pads.