[PIC] PIC18F4550 - how to add to Eagle PCB designer software?

[K33rg4t3]

Hey
I want to design PCB for my PIC18F4550 board.
But this part is not available in Eagle.
How to add it?
I've found: https://github.com/chiengineer/Eagle-Libraries
But I don't know where to put those files after downloads??
Thanks in adavance

 

[KlausST]

Hi,

* download the library and save it into the libraray folder of EAGLE.
* then start EAGLE
* open/new your desired schematic
* then open the "control panel" window
* goto "libraries"
* behind the library names there is either a grey button or a green button. Be sure that behind your library there is a green button, jus by clicking on it. (Then it is active)
* now go back to the schematic window
* "add" --> select library and part.
* finished

Klaus

 

[Arya Kumar]

i know people say Eagle is best for PCB designing..
But i dont know if they have tried PCB designing in proteus.
the best thing i saw there is no need of downloading schematic of component it is already present there.
Also 3d view can show me how pcb will actually be.
Sorry i am not naswering your question but just give proteus a try.. u will love it

 

[KlausST]

Hi,

I´m using EAGLE for more than 20 years now.
I don´t say it is the best software. But there is really no need to change to another software. Not because of including a new library. It usually takes less than a minute of time.

Klaus

 

[K33rg4t3]

Is proteus easier to use?

I have drawn this so far:


I don't know how to find my push button (the most common push button). Where is it? There are many of the buttons with strange codes....

- - - Updated - - -

also... will Eagle export the mirrored PCB tracks so I can print them for etching?

- - - Updated - - -

I mean this button: https://www.adafruit.com/products/367

 

[KlausST]

Hi,

your drawing is not wrong, but it is more like the pcb layout with the numbering from 1..40 like the package.
Feel free to place the pins in a way that you expect less crossings. Or you can seperate the XTAL and the supply pins.
You can also combine the ports with the pins in ascending port_number.
...just as a hint.

****

The button should be in the EAGLE libraries.
In our company we have our own design rules for the packages, so i often build my own library (here for the push button).

Klaus

 

[K33rg4t3]

I don't want to use pinswap because it confuses me.

This is what I have so far:



I have other questions:
1. How should I put the router on the PCB? I made it manually but its kinda messed up
2. How to connect tracks (in my case VCC rails) when they colide? Is there a way to add a dummy resistor with 0 ohm value as a run-over track?
3. What should I do to finish PCB now??
4. Maybe someone can download my project and do some changes and show me what next??

thanks in advance!

 

[KlausST]

Hi,

Red wires (top) may cross blue wires (bottom).
So you easily can route to wire from one pad to the other on top layer.

Are you sure you want the resistor below the IC?

You shoud add a ceramics capacitor at pins 11, 12.
Additionally a bulk capacitor (electrolytic, tantalum) at Vcc.

Klaus

 

[K33rg4t3]

Hi,

Red wires (top) may cross blue wires (bottom).
So you easily can route to wire from one pad to the other on top layer.

I can't because I will be making PCB myself, how to change red wires to blue or add a jumper?

Are you sure you want the resistor below the IC?

It will be a IC-socket, so I think, yes, is there anything against it?



Anyway... I'm having problems with making Arduino-like pinouts... should I put each goldpin just next to MCU pin? And also, now I don't know how to find goldpins in Eagle...

 

[KlausST]

Hi,

I can't because I will be making PCB myself, how to change red wires to blue or add a jumper?

--> In your picture there are already red and blue wires. This means two layers (top and bottom).

It will be a IC-socket, so I think, yes, is there anything against it?

Usually one avoids this.

I don't know about "arduino like pinout" and "goldpin".

***
If you want all traces on one layer you should change your drawing. "Change layer"

I recommend to use a polygon across almost all of the PCB area, named "GND"... to calculate it use "ratsnest"
Then you don't need to draw any GND trace. Use "ripup" .

As jumper you could add a resistor with the value "0". But I think you don't need a jumper.

Klaus

 

[KlausST]

Hi,

i did something like this.
It is not that sophisticated... more quick and dirty.



Klaus

 

[K33rg4t3]

This is nice, but I have few questions:
1. Did you place all tracks by hand or used autorouter?
2. That polygon big thing was made automatically by Eagle or did you place it by hand?
Also, I need to make a pinouts for each leg, because it is supposed to be Arduino-like board....
Ah and also - some tracks should be bigger, because it makes etching easier for an amateur.

 

[KlausST]

Hi,

1) all by hand. I very seldom use an autorouter, even with complex boards.
2) "Polygon". Place left bottom corner. (select wire bend mode "right angle" with right mouse button). Place right top corner. To quit place left bottom corner again. "Name" "GND". "Ratsnest". finished.

During the layout process I made some screenshots. I hope I have some time to generate a "making of" PDF.
From zero to the result above it was less than an hour. (including schematic, screenshots and some improvements)

Klaus

 

[K33rg4t3]

That's good, can you do it soon and publish the sources of this board in this topic?
I need to add the pins for all the free outputs from the PIC

 

[KlausST]

Hi,

here the fiiles.

The ZIP includes EAGLE BRD and SCH for Version 6.5.

The PDF is a "how to guide" for this PCB.



hope it helps

Klaus

 

[K33rg4t3]

Thx, you could make this topic sticky.

Hey, what is the cause of "POWER pin U$1 VSS connected to GND" ERC Warning?
I think that's normal that I connected the VSS pin to GND, but yet the Eagle complains...

 

[KlausST]

Hi,

Hey, what is the cause of "POWER pin U$1 VSS connected to GND" ERC Warning?

A pin defined as "power" pin doesn´t need to be shown in schematic. But you can "invoke" it.

Power pins of the same names are connected automatically, no need to connect it in schematic.

Nowadays where we often have multiple supply voltages on one PCB it doesn´t make much sense anymore. (At least in my eyes).
I usually define a power pin as "input" so the ERC detects a missing source.

Klaus

 

[K33rg4t3]

I've made a board with your tips, but I used autorouter.
Can you tell is it good and what can I improve?

 

[KlausST]

Hi,

* VCC capacitor at pin 32 is missing
* electrolytic bulk capacitor is missing.
* it seems you choos a type A USB jack --> For a USB device choose type B jack.
* the ground wiring around the PCB couldn´t be worse. (more below)
* GND pins 12 and 31 should have short and low impedance connections to avoid GND currents across the IC.
* VCC pins 11 and 32 should have short and low impedance connections. Either you use very thick shor wiring from pin 32 to pin 11, or you install the capacitor at pin32.
* Don´t use an electrolytic capacitor at pin 18. Use a ceramic one.
* it seems you use an ADC. Place a ceramics capacitor at every ADC input and at VRef with short connection to GND.
* it seems you built a step up converter. This is pulsed current! Keep GND and power paths as short as possible. Here the GND path is extremely long feeding all the switching noise to all other circuitry.
You feed the noise to the IC rather than keeping it away.
* Why so much different resistor packages?
* i still don´t like the idea of resistors under the IC. But as long as you use a IC socket it may be OK.

Please review my short PCB routing guide.


Klaus

 

[K33rg4t3]

Since this is complicated, I will start with this:

Hi,

* the ground wiring around the PCB couldn´t be worse. (more below)
* GND pins 12 and 31 should have short and low impedance connections to avoid GND currents across the IC.
* VCC pins 11 and 32 should have short and low impedance connections. Either you use very thick shor wiring from pin 32 to pin 11, or you install the capacitor at pin32.

I've made a shorter connections - is this what you mean with "impedance" stuff?
Please check only the quoted issues, I didn't try to fix anything else - I will do tomorrow.