The reason I want to learn how to use it, is because I am planning on ordering some pcb's with a ATmega328 (with crystal and all the other parts needed to make it run), a 433 Mhz receiver, and then some relays/2N2222's/opto's (depending on what application they are going into).
My problem is now that I find eagly VERY confusing, and is not sure where to start to be able to "see the light".
well it IS a schematic
you might want to check the wires though
far too many joined together!
also the wire to RESET (pin9) seems to go tright through the resistor
you can easily check if it's connected properly
drag the resistor and see if the wires go with it
CTL-Z will "undo"
As a beginner, one should also use File:Export:Netlist when done, it will output a list of what is connected to each signal.
I find it makes the netlist much easier to read if each net has a name - use the "Label" button (looks like ABC over a line) to give each signal a name - double click to drop the generic N$1 name on a signal line, then right click and select Name to give it a meaningful name.
For example, you can see in this schematic that every signal has a name - they will show up as blue lines to be routed when you layout the board; they do not need to actually have lines connecting them on the schematic.
Be sure to use +5V and GND for those names, that will ensure they get routed with thicker lines and not just standard thinner lines.
I like to start a design by trying the autorouter - it will let you see where you component placement was poor - lots of vias, lots of signals going all over te place. Rip up the signals, move things around, try again. You can eventually get down to minimal vias - this design has just 1 where the regulator output capacitor had to connect to the bottom of the board. If that had been a thru-hole component, even that might have been avoided.
One word of caution from my past experience. I once bought a picaxe based bare board of similar design and used right angle male header pins so the board would mount vertically when plugged into a solderless breadboard. The force needed to plug the pins into and removal from the breadboard soon broke many of the header solder joints and lifted the trace pads. I think plated through holes would have given more mechanical strength to the joints, or possible smaller pins instead of the .025 square header pins would be better for breadboard insertion and removal ?
Graynomad:
C3 and C4 are normally 1/10/22uf tant or electro types and therefore larger than you have shown.
I think I got the right ones now...
Graynomad:
There are no decoupling caps, put some as close as possible to the chip's GND and VCC pins.
What would they be? Same as for the 7805?
Graynomad:
What is a 3n3333?
Brain-fart, ment 2N2222
And now... The headacke... Looks like a MESS now... heh, but most of the components should now be on. Still problems with the trace width on power though...
you need to check C1 and C2
one end of each should connect to the crystal (and chip)
the other end should go to ground
one of them seems to wander off to the 2N2222 group
also I would try and get the crystal as close to its pins as possible, you seem to have room to nudge it down a little
mmcp42:
you need to check C1 and C2
one end of each should connect to the crystal (and chip)
the other end should go to ground
one of them seems to wander off to the 2N2222 group
also I would try and get the crystal as close to its pins as possible, you seem to have room to nudge it down a little
They should both be connected almost directly to GND (top left corner).
Tried to move the crystal a bit closer.
I also tried the name thing, but still only getting thin signal traces for the power too.
Netlist
Exported from 8x 3N3333 board.sch at 08-07-2011 19:19:12
EAGLE Version 5.11.0 Copyright (c) 1988-2010 CadSoft
Net Part Pad Pin Sheet
+5V C4 1 1 1
D1 C C 1
IC2 IN IN 1
GND C1 1 1 1
C2 1 1 1
C3 1 1 1
C4 2 2 1
IC1 11 GND 1
IC1 31 AGND 1
IC2 GND GND 1
JP1 1 1 1
JP2 10 10 1
JP2 12 12 1
JP2 14 14 1
JP2 16 16 1
JP2 2 2 1
JP2 4 4 1
JP2 6 6 1
JP2 8 8 1
T1 E E 1
T2 E E 1
T3 E E 1
T4 E E 1
T5 E E 1
T6 E E 1
T7 E E 1
T8 E E 1
N$1 D1 A A 1
JP1 2 2 1
N$2 R2 2 2 1
T1 B B 1
N$3 IC1 9 RESET 1
R1 2 2 1
N$4 C1 2 2 1
IC1 12 XTAL2 1
Q1 2 2 1
N$5 C2 2 2 1
IC1 13 XTAL1 1
Q1 1 1 1
N$6 C3 2 2 1
IC1 10 VCC 1
IC1 30 AVCC 1
IC1 32 AREF 1
IC2 OUT OUT 1
R1 1 1 1
N$7 R3 2 2 1
T2 B B 1
N$8 R4 2 2 1
T3 B B 1
N$9 R5 2 2 1
T4 B B 1
N$10 R6 2 2 1
T5 B B 1
N$11 R7 2 2 1
T6 B B 1
N$12 R8 2 2 1
T7 B B 1
N$13 R9 2 2 1
T8 B B 1
N$14 IC1 16 (INT0)PD2 1
R9 1 1 1
N$15 IC1 17 (INT1)PD3 1
R8 1 1 1
N$16 IC1 18 (OC1B)PD4 1
R7 1 1 1
N$17 IC1 19 (OC1A)PD5 1
R6 1 1 1
N$18 IC1 20 (ICP)PD6 1
R5 1 1 1
N$19 IC1 21 (OC2)PD7 1
R4 1 1 1
N$20 IC1 1 (T0/XCK)PB0 1
R3 1 1 1
N$21 IC1 2 (T1)PB1 1
R2 1 1 1
N$23 JP2 1 1 1
T1 C C 1
N$24 JP2 3 3 1
T2 C C 1
N$25 JP2 5 5 1
T3 C C 1
N$26 JP2 7 7 1
T4 C C 1
N$34 JP2 9 9 1
T5 C C 1
N$35 JP2 11 11 1
T6 C C 1
N$36 JP2 13 13 1
T7 C C 1
N$37 JP2 15 15 1
T8 C C 1
Isn't this how it should be? Or did I misunderstand something?
And if anyone is interested, this is where it is going to be used in
My goal is to make multiple of these devices, and then have different flavors so they can be used in different things.
Like one with the 2N2222's to trigger the buttons in this fan, another with 230V relays to handle lights, and one with opto's to do pretty much the same as the first, but with it isolated more.
This reminds me... I forgot to add pinheader for the RF receiver.
Did you intend to use a big 40 pin device? Or were you shooting for ATMege328 based board like the Uno uses?
H49US is the crystal I think you were after, that's the more normal size.
CrossRoads:
Did you intend to use a big 40 pin device? Or were you shooting for ATMege328 based board like the Uno uses?
H49US is the crystal I think you were after, that's the more normal size.
heh, yeah... I wanted to use the same as the uno and all those boards use... Guess that is named MEGA8-P... Didn't really look that much at it... just saw it had pins and the shape...
If you were after more IO, the bigger part is one way to get there without shift registers/etc. and you get a 2nd hardware serial port also.
ATmega644P (or 324, or 1284, different memory sizes).
Ok, now the tricky bit - draw a polygon (button looks like a piece of paper with top left corner torn off - click a corner follow the perimiter of the board, must finish up where started or will get "illegal poygon" error or similar), name it GND, on both sides of the board. Your thru holes will connect them.
Click the Rubberband button, and let eagle connect everything up to GND. May even be to "ripup" the ground traces.
IC2 is the regulator? Move R1 & D1 left Move IC2 up. Now you can draw a Rectangle under the body (next to the polygon) and extend it down the board, it can act as additional heatsinking for you if you are running from higher voltage, like 12V, vs something lower, like 7.5V, such as
Once you get the hang of it Eagle is really powerfull and friendlier than it seems. PCB design on the other hand is more than connecting wires, you need to pay close attention to the physical layout. Current paths are often overlooked by the beginner, especially gnd and power. As the previous poster suggestion, using polygons is very helpfull for power and ground. Another point is trace widths, the smaller they are the more fragile the pcb is to build.
And now with the polygons and stuff... does this look right?
CrossRoads:
Ok, now the tricky bit - draw a polygon (button looks like a piece of paper with top left corner torn off - click a corner follow the perimiter of the board, must finish up where started or will get "illegal poygon" error or similar), name it GND, on both sides of the board. Your thru holes will connect them.
Click the Rubberband button, and let eagle connect everything up to GND. May even be to "ripup" the ground traces.
Think I got that done... But not sure if the top layer is all one big flat connected one? Or does it only look that way?
I only need the 1x2 pin header I got there right now And I might add a 1x2 next to the voltage regulator too, so it is possible to bypass it. The reason for this is because it is maybe going to be powered by a 230V > 5V usb adabter. And I will then make custom wires anyways and solder it directly on the board to make it as small as possible and not use space on the usb connectors.
And got an protecting diode on for miswireing
CrossRoads:
Which are the pins for the Rx module?
Bottom right corner. JP3
Hmmm... Maybe also add pin headers for FTDI breakout board... hmmmm