Schematic finally finished - A few questions.....

Community PCB Design
41

konguk, either of these two ways will work in the schematic for connecting a decoupling capacitor:

decouplingcap.jpg1065×438 62.4 KB
http://i18.photobucket.com/albums/b106/ … ingcap.jpg

Note that it does not need to be directly connected to the IC’s supply pins in the schematic.

This is a rough generalization of what it sould look like in the PCB editor:

http://i18.photobucket.com/albums/b106/ … capbrd.jpg

Of course, you may use a different IC and you are not required to use a polarized radial electrolytic capacitor, but you can see the close proximity to the IC and the thick traces.

42

konguk:
Another question that’s not that important but though i’d ask it anyway - the external crystal is being used as opposed to the internal timing function of the atmega8 - why is this needed? Is the external crystal a higher Mhz or more stable signal than the atmega will allow?

I’m only asking as a possible way to eliminate the external crystal from the circuit

Greetings konguk,

For the AVR mega8 the internal RC oscillator is limited to 8MHz.

Depending upon the bin-sort the same uC will operate at a higher

frequency with an external crystal and two capacitors.

If it were me I’d add the three components to the PCB and

if the AVR is operated at or below 8MHz switch to the RC

osc.

This way you can go back to the Xtal if needed. Also, if you

accidently change the fuses for an AVR to external osc mode

and there’s isn’t one it will die.

Comments Welcome!

43

Right, i finally etched a board and soldered all the components to it. But I have a horrible feeling that I have placed all the components back to front :frowning:

I’ll upload some pictures in a bit so that you can see what i mean!

44

Hmmmm, for some reason the board it as created has placed the Atmega back to front although all the other componets are the correct way round…

Heres an image of the routed board

[<LINK_TEXT text=“http://img212.imageshack.us/img212/3051 … eo7.th.jpg”>http://img212.imageshack.us/img212/3051/boardlayouteo7.th.jpg</LINK_TEXT>

Anyone any ideas?](ImageShack - Best place for all of your image hosting and image sharing needs)

45

Difficult to tell, you should have included the silk layer and the schematic.

Leon

46

Here is the schematic and the board with all layers activated

[<LINK_TEXT text=“http://img515.imageshack.us/img515/2554 … uo4.th.jpg”>http://img515.imageshack.us/img515/2554/usbschematicuo4.th.jpg</LINK_TEXT>

[<LINK_TEXT text=“http://img515.imageshack.us/img515/888/ … my8.th.jpg”>http://img515.imageshack.us/img515/888/alllayersmy8.th.jpg</LINK_TEXT>](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)

47

I’d scrap that layout and start again from scratch. The power and ground tracks need to be much wider, and you have the crystal too far from the chip. The crystal capacitors should be returned to the nearest ground pin via a short track.

Here is one of my boards that illustrates what I mean:

http://www.leonheller.com/usb/usb.gif

Leon

48

That is simple enough to hand route and Eagle’s autorouter is making a terrible mess of it. Now I can understand why it is hated so much…

49

konguk:
Here is the schematic and the board with all layers activated.

Greetings konguk,

I’m not sure if you’ve been over these details before but there

are a couple of design errors in your schematic that should be

addressed before attempting a PCB.

(1) LED1 is backwards (and will never light up)

(2) R4 is quite low for an indicator LED. I’d use 1k0

(3) JP2 appears to have the AVR ISP signals. If so, that pin

assignment doesn’t match the AVR ISP 10 pin or 6 pin layout

(4) The uC Reset line (Pin 1) is floating (needs a 10k pull up to 5V)

(5) The AVR ISP also needs access to the reset line to operate.

Next, the layout stinks!

How did the Xtal and capacitors get so far from the uC?

why are the connectors in the board corners?

If all layers are turned on why are there only blue traces?

(Are you trying to do a single-sided PCB)?

I know the EAGLE auto-router haters will have a fit, but

unless the parts are positioned in a sensible way any

auto-router would have trouble with this design.

The design is simple enough to use hand routing and a

bit of common sense in placing the parts for better

connectivity.

If this is a two-layer design then one layer could be used

for either a ground plane or a split power and ground plane

that would improve the noise immunity.

Comments Welcome!

50

As always, i got impatient and etched a board too soon :slight_smile:

I guess i’ll never learn my lesson…

I think I realise what has happened in regards to components being back to front, I have selected a single layer board in the autorouter which has resulted in the blue lines.

Is there an option to tell it that I am not using SMD components? Because when I solder my Atmega to the board everything ends up being in reverse…

If that makes any sense?

51

konguk:
Is there an option to tell it that I am not using SMD components? Because when I solder my Atmega to the board everything ends up being in reverse…

Greetings konguk,

Sorry about the false start (we’ve all been there…).

Can you post (or email to me) your EAGLE *.sch and *.brd files?

To use TH (Through Hole) parts you need to select them

from the parts library. Most common parts come in multiple

shapes, sizes, and technology.

It’s possible that you used the mirror command to

flip parts to the rear of the board and then etched it

as a top sided board.

Remember that in the PC game all parts and boards are

viewed from the above (sky view) and the board is

transparent. When parts are flipped to the back side

(traditionally called the ‘solder side’) the text will be

mirrored. There are no other clues. In EAGLE the

default layer for top is red and for bottom it’s blue.

Comments Welcome!

52

Biglez has revised the schematic for me and come up with a board layout. I have just run the autorouter which seems to have done an ok job apart from one stray airwire.

I am now keen to see if the board works, although this will not be the final design, if I etch this board will it work?

[<LINK_TEXT text=“http://img142.imageshack.us/img142/8742 … kh6.th.jpg”>http://img142.imageshack.us/img142/8742/revisedusbboardjpgkh6.th.jpg</LINK_TEXT>](ImageShack - Best place for all of your image hosting and image sharing needs)

53

Why have you used the autorouter? The Eagle autorouter isn’t very good and autorouters generally don’t do a good job on single-sided boards.

It still has problems. Your power and ground tracks should be a lot wider and why are they wandering about all over the place? If you must use the autorouter, you should route critical tracks like those for power, ground and the oscillator manually. You should mitre all those right angle corners, good autorouters do that automatically.

Leon

54

I have had a go at handrouting, although there are a couple of airwires still present I just wanted to know if I am going in the right direction :slight_smile:

The final revision is going to be constructed with surface mounted components as opposed to through wire so I am going to have to do this all again for the final revision…

I realise my power and ground wires still aren’t thick enough, but am I on the right tracks??

[<LINK_TEXT text=“http://img146.imageshack.us/img146/5971 … jq4.th.jpg”>http://img146.imageshack.us/img146/5971/handroutedjpgjq4.th.jpg</LINK_TEXT>](ImageShack - Best place for all of your image hosting and image sharing needs)

55

From my understanding, you want to keep the trace angles at 45 degrees or less, not 100% sure why this is, but that’s just what I’d heard. Other than that, it looks a lot more concise than the auto routed board, so I’d say you’re definitely on the right track.

56

Regarding right angle trace routing:

First off - if you route at right angles, it doesn’t matter from an electrical perspective at the frequencies that are used on that board. In fact, from what I’ve read, it doesn’t even have a proven deleterious effect at higher frequencies [the studies I read were at ~1-2GHZ]. That being said, I always route my boards with 45 degree miters because I think it looks better, and I can pack stuff tighter.

The reason why people suggest avoiding right angles stem from the following two ideas:

  1. A right bend has a much larger change in width at the corner than a 45 degree bend does. This change would cause an impedance difference in the track causing signal integrity issues at high speeds.

  2. A right angle bend has a sharp point, which tends to concentrate electric fields, potentially acting as a radiator [I can’t quite remember this one, someone please correct me if I’m wrong here].

However, the literature I’ve read regarding experiments done with high speed traces routed at various angles [no bends, S curves, 45, 90, 135] showed no signal integrity issues or increased emissions.

I still like 45’s though ;).

Cheers,

–David Carne

57

busonerd:
2. A right angle bend has a sharp point, which tends to concentrate electric fields, potentially acting as a radiator [I can’t quite remember this one, someone please correct me if I’m wrong here].

Nope, thats right, it’s referred to as “electron wind”. It can even make blinds shutter, charged discs rotate (think, like, a curved throwing star with points at the tips). But seeing as how its all insulated in soldermask, and relatively low power, probably a non issue.

58

The main reason is that it helps with the etching, especially for narrow tracks; right angles will get overetched.

Leon

59

konguk:
I am now keen to see if the board works, although this will not be the final design, if I etch this board will it work?

Greetings konguk,

I routed your current design by hand, using a double sided

PCB and top side ground plane. Notice that the ground plane

is relieved under the oscillator circuit (Xtal and capacitors).

http://www.stonard.com/SFE/NES2USB.jpg

If you are limited to a one sided board this layout can be

revised to remove the ground plane and add one wire link

(zero ohm R7) to complete the circuit.

http://www.stonard.com/SFE/NES2USB_single.jpg

Also, in my schematic the value of R1 should be 1k0 (not 10k).

Comments Welcome!

60

I think you can do it all single sided - Just rotate + move R2 + R3 and you should be able to continuously route that gnd trace without it deviating too far.

Cheers,

–David Carne