6502.org Forum  Projects  Code  Documents  Tools  Forum
It is currently Thu Nov 14, 2024 4:30 pm

All times are UTC




Post new topic Reply to topic  [ 49 posts ]  Go to page Previous  1, 2, 3, 4  Next
Author Message
PostPosted: Tue Nov 07, 2017 9:47 pm 
Offline

Joined: Mon Oct 23, 2017 9:16 pm
Posts: 22
Well, several late evenings and one bored-of-hearing-about-it girlfriend later...

Here is the schematic for "release candidate 1", and an SVG of what I might sent to the board house. Unfortunately SVG is the best output I can find from Kicad's PCD editor. edit: Scratch that, the forum doesn't allow SVG attachments. I've printed the SVG as a PDF. (cf. https://xkcd.com/763/)

I've incorporated the flip-flop on the clock, jumper headers for modifying the memory map, an NMI button (debounced the same way as the reset signal, because I can't get a nice double pole switch for the SR flip-flop debouncer) and possibly some other bits...

I have one final question about AC construction - On the large DIP packages, it's very difficult to get the decoupling cap close to both power pins, they're just too far apart, and signals need to be routed between. I've mostly gone for putting the cap near the ground pin and then bridging it directly to the internal Vcc plane. Would placing one cap on each of the Vcc and ground pins be better? Or should I really be going back and finding a way to put a single cap equidistant and directly between the package's power pins?

I've excited, and apprehensive... the PCB will cost slightly over $100 in full 4 layer. The extra space left around the EEPROM is so that a ZIF socket will fit...


Attachments:
65m2-brd.pdf [79.69 KiB]
Downloaded 108 times
rc1.pdf [223.3 KiB]
Downloaded 76 times
Top
 Profile  
Reply with quote  
PostPosted: Tue Nov 07, 2017 10:21 pm 
Offline
User avatar

Joined: Fri Aug 30, 2002 1:09 am
Posts: 8540
Location: Southern California
If you have both a power plane and a ground plane (and they're true planes, not copper pours which don't qualify as a plane), I don't think it would matter which of the two ways you do it. Myself, I would put the capacitor next to the power pin, with the shortest possible connection from the pin to the capacitor, and from the capacitor to the ground plane. Dr. Howard Johnson had a good article on that, but now you can't see it anymore without paying, so my link is basically dead. [Edit: I'm not sure which article I was thinking of when I wrote this, but I found his articles available, free, in the archives, at https://web.archive.org/web/20120302190 ... eyword.htm .]

_________________
http://WilsonMinesCo.com/ lots of 6502 resources
The "second front page" is http://wilsonminesco.com/links.html .
What's an additional VIA among friends, anyhow?


Top
 Profile  
Reply with quote  
PostPosted: Wed Nov 08, 2017 12:12 pm 
Offline

Joined: Mon Oct 23, 2017 9:16 pm
Posts: 22
Thanks, I'll do that. By placing the caps on the underside of the board, I should be able to put them really close to the ground supply pins. I am going for a proper 4 layer board with true Vcc and ground planes on the internal layers. It's twice as expensive, but everything I've read here suggests I should just do it. It also simplifies routing a lot, and I'm a bit of a board layout novice, so that's a big plus.


Top
 Profile  
Reply with quote  
PostPosted: Wed Nov 08, 2017 5:47 pm 
Offline
User avatar

Joined: Fri Aug 30, 2002 1:09 am
Posts: 8540
Location: Southern California
Assuming you'll be assembling by hand, you can also put vias in the pads themselves, further saving board space and facilitating routing and reducing inductance. You can't do that for production unless these vias are plugged and plated over, because when they screen the solder paste on, anywhere there's a hole, the solder paste will squish out the other side and make a big mess. An exception might be in that now we have a supplier that doesn't make a silkscreen for solder paste, but they actually spray it on kind of like an inkjet printer works, so the tool-up cost is reduced since it's all controlled in software only.

_________________
http://WilsonMinesCo.com/ lots of 6502 resources
The "second front page" is http://wilsonminesco.com/links.html .
What's an additional VIA among friends, anyhow?


Top
 Profile  
Reply with quote  
PostPosted: Wed Nov 08, 2017 7:07 pm 
Offline
User avatar

Joined: Thu May 28, 2009 9:46 pm
Posts: 8484
Location: Midwestern USA
mdpye wrote:
I have one final question about AC construction...

On my POC units, the bypass capacitor is placed as closely as possible to Vcc on the device being bypassed. The Vcc pin on the device is connected to the corresponding pin on the capacitor and the capacitor is what makes the connection to the internal power plane. This arrangement is based upon Dr. Howard Johnson's and others' recommendations and is one I have used for years. The other side of the capacitor is connected to the ground plane, as is the ground pin of the device.

The attached illustration of POC V2.1's four-layer PCB shows this layout arrangement—look at C8 and U8 (center) for an example.

Attachment:
File comment: POC V2.1 PCB
poc_v2_pcb.gif
poc_v2_pcb.gif [ 102.73 KiB | Viewed 1257 times ]

_________________
x86?  We ain't got no x86.  We don't NEED no stinking x86!


Top
 Profile  
Reply with quote  
PostPosted: Thu Nov 09, 2017 5:49 pm 
Offline

Joined: Mon Oct 23, 2017 9:16 pm
Posts: 22
Thanks. I notice you're using some pretty fat power traces in various places. I don't think they're going to be delivering loads of current, does a fatter trace help reduce noise on the power lines? I imagine the opposite would be true for a signal line, although that's an intuition, and my intuition about power is the opposite (like, the object is to stay stable, not switch quickly!)


Top
 Profile  
Reply with quote  
PostPosted: Thu Nov 09, 2017 5:54 pm 
Offline

Joined: Mon Oct 23, 2017 9:16 pm
Posts: 22
Quote:
Assuming you'll be assembling by hand, you can also put vias in the pads themselves, further saving board space and facilitating routing and reducing inductance.


Ah, that's good to hear. I had placed a lot of vias inside pads for the reasons you mentioned, but a quick Google convinced me to change them after reading about "solder slurping" problems. I was sceptical based on my experience hand soldering, but I can see how forced application of paste would be a problem. That didn't occur to me, but now I understand I'm more comfortable breaking with "accepted best practice"

I'll probably move some of them back to the pads where it neatens things or shortens power delivery lines :)


Top
 Profile  
Reply with quote  
PostPosted: Thu Nov 09, 2017 6:37 pm 
Offline
User avatar

Joined: Tue Oct 25, 2016 8:56 pm
Posts: 362
mdpye wrote:
Thanks. I notice you're using some pretty fat power traces in various places. I don't think they're going to be delivering loads of current, does a fatter trace help reduce noise on the power lines? I imagine the opposite would be true for a signal line, although that's an intuition, and my intuition about power is the opposite (like, the object is to stay stable, not switch quickly!)



Fatter traces = less resistance and impedance, neither of which are things you want on a power line.

_________________
Want to design a PCB for your project? I strongly recommend KiCad. Its free, its multiplatform, and its easy to learn!
Also, I maintain KiCad libraries of Retro Computing and Arduino components you might find useful.


Top
 Profile  
Reply with quote  
PostPosted: Thu Nov 09, 2017 8:10 pm 
Offline
User avatar

Joined: Fri Aug 30, 2002 1:09 am
Posts: 8540
Location: Southern California
I wouldn't worry too much about that. A .008" trace of 1oz copper is good for a half amp of current at 20°C rise, and has less than a fifth of an ohm's resistance at three inches' length, meaning a half an amp on that teeny trace would drop about one-tenth of a volt across three inches. 5mA, or 1% of half an amp, would cause about 1mV of drop across three inches. The ratio of width to separation from the ground plane does affect characteristic impedance for fast AC signals; but when there's a bypass capacitor from the power trace to ground right at the IC anyway, neither of these things matter.

_________________
http://WilsonMinesCo.com/ lots of 6502 resources
The "second front page" is http://wilsonminesco.com/links.html .
What's an additional VIA among friends, anyhow?


Top
 Profile  
Reply with quote  
PostPosted: Thu Nov 09, 2017 9:06 pm 
Offline
User avatar

Joined: Tue Oct 25, 2016 8:56 pm
Posts: 362
I agree that it is not of great importance in this case, but that is why one typically has fatter traces for power nets - or if you've got a lot of current. Even if its not necessary, if you have the room it can only help.

_________________
Want to design a PCB for your project? I strongly recommend KiCad. Its free, its multiplatform, and its easy to learn!
Also, I maintain KiCad libraries of Retro Computing and Arduino components you might find useful.


Top
 Profile  
Reply with quote  
PostPosted: Fri Nov 10, 2017 5:42 pm 
Offline
User avatar

Joined: Fri Dec 11, 2009 3:50 pm
Posts: 3367
Location: Ontario, Canada
Alarm Siren wrote:
I agree that it is not of great importance in this case, but that is why one typically has fatter traces for power nets - or if you've got a lot of current. Even if its not necessary, if you have the room it can only help.
Hmm. Not wishing to appear contrary, but this isn't always true, at least not with regard to the VCC trace. Let's assume the GND trace *is* nice and fat, or is an actual ground plane. Also assume that near each chip is a bypass cap attaching the chip's VCC pin to the fat trace or ground plane. This satisfies the need for a good AC connection between the various chips (Garth mentioned this, too). IOW, the VCC trace can be skinny because it only needs to carry a little bit of DC. There's no significant advantage if it's fat.

But a fat VCC trace can actually be a disadvantage in certain troubleshooting situations, such as when a chip or a bypass cap has shorted. You're better off to have skinny VCC traces because their resistance is high enough that there'll be a measurable voltage drop across the trace that feeds the shorted component. (Have been there and done this IRL -- a tidy solution to an otherwise nasty situation.)

_________________
In 1988 my 65C02 got six new registers and 44 new full-speed instructions!
https://laughtonelectronics.com/Arcana/ ... mmary.html


Top
 Profile  
Reply with quote  
PostPosted: Fri Nov 10, 2017 5:49 pm 
Offline
User avatar

Joined: Thu Dec 11, 2008 1:28 pm
Posts: 10977
Location: England
Hmm, that's an odd kind of advantage! Seeing Garth's calculation of a tenth of a volt drop, I think I'd rather have the fat trace...


Top
 Profile  
Reply with quote  
PostPosted: Fri Nov 10, 2017 6:09 pm 
Offline
User avatar

Joined: Thu May 28, 2009 9:46 pm
Posts: 8484
Location: Midwestern USA
Dr Jefyll wrote:
But a fat VCC trace can actually be a disadvantage in certain troubleshooting situations, such as when a chip or a bypass cap has shorted.

Fortunately, I've not had anything like that occur in one of my contraptions—yet! :shock: I'm depending on the PC power supply I use to run my POC units to kick itself off-line if something does short. If it doesn't...well, I guess I'll have a little mess on my hands. :evil:

_________________
x86?  We ain't got no x86.  We don't NEED no stinking x86!


Top
 Profile  
Reply with quote  
PostPosted: Fri Nov 10, 2017 6:19 pm 
Offline
User avatar

Joined: Fri Aug 30, 2002 1:09 am
Posts: 8540
Location: Southern California
BigEd wrote:
Hmm, that's an odd kind of advantage! Seeing Garth's calculation of a tenth of a volt drop, I think I'd rather have the fat trace...

The tenth of a volt drop was for 500mA through 3" of .008" on 1oz copper. For 5mA it's on 1mV. for 500µA (getting closer to what one CMOS IC might take), it's only 100µV. IOW, a .008" trace is plenty wide.

_________________
http://WilsonMinesCo.com/ lots of 6502 resources
The "second front page" is http://wilsonminesco.com/links.html .
What's an additional VIA among friends, anyhow?


Top
 Profile  
Reply with quote  
PostPosted: Fri Nov 10, 2017 6:26 pm 
Offline
User avatar

Joined: Fri Dec 11, 2009 3:50 pm
Posts: 3367
Location: Ontario, Canada
BigEd wrote:
Hmm, that's an odd kind of advantage! Seeing Garth's calculation of a tenth of a volt drop, I think I'd rather have the fat trace...
You need to keep the numbers in perspective. Notice that a drop of one-tenth volt hardly puts a dent in the 5% tolerance of many digital IC's; moreover the half-amp figure Garth chose is far more than most IC's require.

FWIW, the troubleshooting case I cited involved heavy current and rather fat traces. But it's all a matter of proportion. The traces were not unnecessarily widened; if they had been then I'd have been sunk. :(
Attachment:
IMG_4449.JPG
IMG_4449.JPG [ 284.75 KiB | Viewed 1158 times ]
Attachment:
b-w photo.png
b-w photo.png [ 358.74 KiB | Viewed 1157 times ]

_________________
In 1988 my 65C02 got six new registers and 44 new full-speed instructions!
https://laughtonelectronics.com/Arcana/ ... mmary.html


Last edited by Dr Jefyll on Fri Nov 10, 2017 6:50 pm, edited 1 time in total.

Top
 Profile  
Reply with quote  
Display posts from previous:  Sort by  
Post new topic Reply to topic  [ 49 posts ]  Go to page Previous  1, 2, 3, 4  Next

All times are UTC


Who is online

Users browsing this forum: pdragon and 7 guests


You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot post attachments in this forum

Search for:
Jump to: