Hi,
I’m a beginner in development of PCBs. So would somebody check my PCB for any errors or mistakes :?: I use Eagle.
I will really appreciate it.
I attached my *.sch and *.brd & .epf etc. files (HDD Clock.zip).
I finally want to use BatchPCB to create my circuit board.
Thank you!
EDIT:
I try to make a HDD Led Clock, more info:
For example is it really a problem if there are text layers mix/beyond the edge?
Kind regards,
Melroy van den Berg
Disclaimer: I have not checked the schematic for functionality - it may or may not do what you want 
The board overall looks good for a first timer. Some suggestions (some serious, some more pedantic than others):
Use a ground flood, either on one or both layers. Currently all grounds are 10 mil traces and there is a ton of room to spare. This is as simple as drawing a polygon on a layer, naming it “GND”, and hitting the ratsnest button.
The POWER and IC1 text is off the board. I suggest using the smash tool and moving it back onto the board so you can read it.
Put a date or revision number on it.
90 degree traces are frowned upon. You can use the miter tool to give them 45 degrees.
(Schematic) You have GND going to VDD and +4ish (after the diode drop) going to one VSS pin. Vss (the source) is GND and Vdd (drain) should be +4/5.
Connect all power pins. Also place a capacitor between power and ground (0.1uF ceramic for digital logic is a good starting point)
Thanks for everything…
theatrus:
- Use a ground flood, either on one or both layers. Currently all grounds are 10 mil traces and there is a ton of room to spare. This is as simple as drawing a polygon on a layer, naming it “GND”, and hitting the ratsnest button.
I try to add a polygon with the name GND, however it says that I got already something else with the name “GND”. What should I do? Can I use the whole board for 1 ground?
Fixed that :)
- The POWER and IC1 text is off the board. I suggest using the smash tool and moving it back onto the board so you can read it.
Thanks for the tip, did that too.
- Put a date or revision number on it.
I used autoroute, it there no setting for this for example: "Only 45 degrees"?
- 90 degree traces are frowned upon. You can use the miter tool to give them 45 degrees.
I added the capacitor, hopefully I did it right (check my attachment, please).
- (Schematic) You have GND going to VDD and +4ish (after the diode drop) going to one VSS pin. Vss (the source) is GND and Vdd (drain) should be +4/5.
Connect all power pins. Also place a capacitor between power and ground (0.1uF ceramic for digital logic is a good starting point)
http://translate.google.nl/translate?js … =en&swap=1
Yes, I got also a error message in Eagle about that Vss & Vdd pins, but then this person has also an error in his design right?
Here you can see the schematic from Ian: http://www.ian.org/HD-Clock/HD-Clock-Schematic.png (I try to make my own one)
So what to do? Just switch the Vss & Vdd or was it with deliberately?
He said I can use every OSCILLATOR from 10MHZ, so I think I gonna use this one:
- I would frown upon an offboard oscillator unless it can deliver a fully buffered signal. What are you using?
http://translate.google.nl/translate?hl … %2F1216192
I think it’s also better to add it onboard. Strange is the fact that Ian used 3 pins for the oscillator. But my oscillator has 4 pins 
? I think Ian didn’t draw his VCC input line? I also don’t know if pin 10 (OSC2) & 9 (OSC1) from the PIC should be on the OE and FO or FO and OE?
Thanks already!
EDIT:
File was too big, so I uploaded it here:
http://www.2shared.com/file/6_RzwHNv/HDD_Clock.html
Kind regards,
Melroy van den Berg
Post the image. Many of us don’t use Eagle.
Ow sorry, here are the images:
Schematic:
Board:
EDIT:
Which oscillators should I use I need a 10Mhz, but in the specs they say you got 4 pins in Eagle you see at the schematic 3 pins but strange enough you got on your board 4 pins :?
[](ImageShack - Best place for all of your image hosting and image sharing needs)](ImageShack - Best place for all of your image hosting and image sharing needs)](ImageShack - Best place for all of your image hosting and image sharing needs)
Route the supply tracks and other critical nets first, and don’t bother with the autorouter. It isn’t very good.
Ok, I will switch the Vdd & Vss lines. But also what about the Oscillator in my message above… You can here see an example of the 10MHz OSC:
http://www.ian.org/HD-Clock/HDClock-Int … otated.jpg
Schematic Version 2:
You can see on this schematic:
http://www.ian.org/HD-Clock/HD-Clock-Schematic.png
That that person also do not connect pin 19 (Vss), but only 8…](ImageShack - Best place for all of your image hosting and image sharing needs)
The first oscillator picture appears to be a ceramic resonator - it needs both drive pins and a ground connection as the capacitors are internal.
Your second picture is of a fully buffered oscillator with crystal inside.
I am not a PIC person, but there should be no need to use a dedicated oscillator there - the PIC should be able to directly drive a crystal with the appropriate load capacitors.
Yes, all PICs have a conventional crystal oscillator option. Most of them also have a 1% internal oscillator, which is suitable for many applications.
Yes and yes. The auto router in EAGLE is lousy unless you line everything up for it and make its job really really easy.leon_heller:
Route the supply tracks and other critical nets first, and don’t bother with the autorouter. It isn’t very good.
The N$18 via and the GND via that are connecting both connecting tCopper and bCopper should be farther apart. The two vias are right by pins 13 and 14. This probably wont be an issue but you have plenty of room and might as well spread them out a little. Routing off grid wont crush the design. Oh, and there are a number of right angle traces that could probably be ditched (beware of acid traps).
The 1st picture is from Ian, which made successfully a LED hard drive Clock. I think he used the ceramic resonator not for nothing? :? :?theatrus:
The first oscillator picture appears to be a ceramic resonator - it needs both drive pins and a ground connection as the capacitors are internal.Your second picture is of a fully buffered oscillator with crystal inside.
I am not a PIC person, but there should be no need to use a dedicated oscillator there - the PIC should be able to directly drive a crystal with the appropriate load capacitors.
In his schematic you can indeed see the 2 pins & 1 ground: http://www.ian.org/HD-Clock/HD-Clock-Schematic.png.
But I can try to add this ceramic resonator onboard (so NOT separately), I think he used it for the time (because it will be a clock eventually)…
So what should I do?
Ps.
Don’t forget I’m still a noob 
EDIT:
My new schematic…
My new (2nd try) board design:
My 3D design 8)
New Gerber (View)
Does this one looks better (is the ceramic resonator well placed)? I also don’t know how to make a whole ground (GND) without the error “GND” name is already used…?
Note: I see a small bug in the number “1” (it’s off the board), I will fix that later.](ImageShack - Best place for all of your image hosting and image sharing needs)](ImageShack - Best place for all of your image hosting and image sharing needs)](ImageShack - Best place for all of your image hosting and image sharing needs)](ImageShack - Best place for all of your image hosting and image sharing needs)
Just a few tips:
In the schematic, use separate +5 and ground symbols where needed, rather than showing the wires interconnecting all the pins; it will make the schematic less cluttered. Normally, positive supply voltage symbols (like +5) point up, and negative ones and ground point down. You can use another power symbol, say Vdd, for the net after D1.
You need to connect both Vss pins on the PIC. Tie them together and to ground.
Add a 100nF bypass capacitor between Vdd and Vss next to the PIC
You may need a bulk electrolytic or tantalum where power comes onto the board
Normally, you don’t have any diagonal nets on a schematic
As mentioned, you need fatter traces for power (both sides of D1) and ground
I’d place the resonator on the same side of the PIC as the clock pins
Do you need any mounting holes to mount your board to its enclosure
As for your question about the oscillator, most have 4 pins for mechanical stability. Three, as you guessed, are Vcc, Gnd, and Out. The fourth may be a no-connect, or may be an output enable or disable. Check the data sheet to be sure.
/mike
n1ist:
Just a few tips:1- In the schematic, use separate +5 and ground symbols where needed, rather than showing the wires interconnecting all the pins; it will make the schematic less cluttered. Normally, positive supply voltage symbols (like +5) point up, and negative ones and ground point down. You can use another power symbol, say Vdd, for the net after D1.
2- You need to connect both Vss pins on the PIC. Tie them together and to ground.
3- Add a 100nF bypass capacitor between Vdd and Vss next to the PIC
4- You may need a bulk electrolytic or tantalum where power comes onto the board
5- Normally, you don’t have any diagonal nets on a schematic
6- As mentioned, you need fatter traces for power (both sides of D1) and ground
7- I’d place the resonator on the same side of the PIC as the clock pins
8- Do you need any mounting holes to mount your board to its enclosure
9- As for your question about the oscillator, most have 4 pins for mechanical stability. Three, as you guessed, are Vcc, Gnd, and Out. The fourth may be a no-connect, or may be an output enable or disable. Check the data sheet to be sure.
/mike
New Schematic:
New Board design:
Kind regards,
Melroy van den Berg](ImageShack - Best place for all of your image hosting and image sharing needs)](ImageShack - Best place for all of your image hosting and image sharing needs)
Getting better. Just to clarify a few points:
Use power symbols INSTEAD of wires in your schematic. You can place multiple ground symbols, for example, and the tool will automatically connect them all without cluttering the schematic. So I would place a ground symbol to the left of the PIC, and wire it just to the caps and PIC. I’d place one by each connector that has a ground pin, and connect it to just that pin. I would do the same with your Vdd net. That would make the schematic much more readable.
I just noticed that you have 5 bits going into the ULN2003, but only 3 are connected on the other side.
On the board, power and ground traces should all be wide, and should be short and direct, if possible. For example, look at the connection from D1 through to the PIC; it goes all over the place and is quite thin, in points.
When laying out the board, traces should bend with 45-degree corners, I’d avoid right-angle bends and circular sweeps.
/mike
Where can I find the power symbols, besides that I got already the +5V and Vdd?? I need to wires for my KK Molex connector.n1ist:
Getting better. Just to clarify a few points:
- Use power symbols INSTEAD of wires in your schematic. You can place multiple ground symbols, for example, and the tool will automatically connect them all without cluttering the schematic. So I would place a ground symbol to the left of the PIC, and wire it just to the caps and PIC. I’d place one by each connector that has a ground pin, and connect it to just that pin. I would do the same with your Vdd net. That would make the schematic much more readable.
I tried to add Vss ground symbol, but need the wires become or GND or Vss.
But I got only 1 pin out to that KK Molex connector for GND/Vss so I will be nuts if I try to make 1 GND and 1 Vss or not? Same for Vdd and +5V in this case it’s just the same.
- I just noticed that you have 5 bits going into the ULN2003, but only 3 are connected on the other side.
That is not an issue because it will be connected to the Leds and they have 12V external. And I don’t use not all the inputs so also not all the outputs the extra inputs are just necessary if there is too much power or something like that, they told me. So the schematic should be OK.
I tried to have it has thick as possible and also pass the DRC tests that the same time. So that is why I can't make it thicker or it will be too close to for example PIN 1 from the PICKIT2 connector. But I will try to fix it.
- On the board, power and ground traces should all be wide, and should be short and direct, if possible. For example, look at the connection from D1 through to the PIC; it goes all over the place and is quite thin, in points.
Another person said that I need to use the miter, so it will become more like round corners. Thanks for the tip.
- When laying out the board, traces should bend with 45-degree corners, I’d avoid right-angle bends and circular sweeps.
/mike
New board:
Schematic:
http://img713.imageshack.us/img713/8850 … ematic.png
3D:
http://img43.imageshack.us/img43/7376/hddclock.png
Kind regards,
Melroy](ImageShack - Best place for all of your image hosting and image sharing needs)
You’re already using the power symbols. Schematic nets symbols can be tied together by name only, the wire doesn’t actually need to go from point to point.
Put the power symbol wherever you have a net going to the power pins. For instance, add the Vdd symbol wherever your current Vdd net goes.
