EAGLE - Making the PCB

Errata!!! In the previous post I had the connection VCC & GND going to the WRONG pins on the LM741. Here I have corrected this to pins 7 and 4.

So let's take the simple design of the previous post, complete it and make the PCB.

Here's the completed design:


I have added component values

- Edit > Value, to the resistors R1 & R2

I have named the signals IN, OUT, VCC, VCC2 & GND on the connector and on the circuit, so that Eagle will automatically connect them.

- Edit > Name

Now to create the PCB.

File > Switch to Board, and create it "Yes".

The square representing the board starts off large, reduced it to the size you want using

- Edit > Move, and dragging in the top and right sides to make a board about a inch square

- Tool > Move is used again to place the components on the board. Like this



The components have been moved around and rotated to simplify the layout (a matter of trial and error to get the best layout). The wiring is shown as thin black lines called Airwires.

Run the Auto-Router

- File > Autoroute. This is the result



As you can see there are only red lines. The red ones are on the top of the PCB (blue ones would be on the bottom). You can see all the layers of the PCB design using

- View > Layer Settings, which will open up a window showing all the layers. Various parts of the drawing are located on different layers. Partly defined by the Device characteristics and part by the routing, The most important are the 1Red (Top) and 16Blue (Bottom) layers.

The design as it is Auto-routed is over-complex and can be simplified if only we could get the GND wire from JP1 (centre pin) to the Pin 4 of IC1 without going all round the houses.

A cunning way to do this, and to save removing tons of copper from the PCB, is to create a ground plane. Draw a polygon round the circuit

- Draw > Polygon



Then name it as GND

- Edit > Name, and click on the dotted line

- Edit > Ripup the existing connection from JP1 to IC1 pin 4, as this will now be made with the ground plane (by the way all traces can be ripped up to start again by entering the command "RIPUP;" in the top command line.)



Now re-run the Auto-router and you will get this



As you can see the ground connection is now made with the ground plane which connects to JP1 centre pin and pin 4 of IC1

Layers

Within the Eagle PCB layout items are maintained on "Layers" as follows



You can view layers separately by turing them off/on using View > Layer Settings.

Checks

You can check two aspects of your design

1 Electrical rules in the schematic, Tools > ERC, which will report Errors and Warnings



2 Design rule check on the board, Tools > DRC. This will check that the layout meets the design rules, like the spacing of wires etc.



We have no errors so no report is made.

Design Rules

Suppliers, like Eurocircuits, provide their own Design Rules to ensure that you design will meet their fabrication specs. You can download these from their site and place them in Eagle's /drc folder. Then from the control panel chose Design Rules and load the Eurocircuit one you want to use.

EAGLE - Progressing with a PCB design

After the last post I will now continue with actual PCB design. Starting with drawing the circuit schematic.

A Project

A Project is a folder that will contain all your files - schematic drawings, board layouts etc

- At the Control Panel, right click on Projects and chose "New", name the project.



Then repeat and chose "Edit Description" and give your project a description.



Schematic

With your Project highlighted,

- File > New > Schematic.

- Click on the "Grid" icon top left and switch it On.



Now you can add the Devices to your schematic.

- Edit > Add, will open a window showing all your available Libraries of devices.



Find the one you want and click "OK"



- Add this to your schematic, position it and click. You can repeat the additions if you need more of the same Device, to exit hit ESC.

Add the other components you need, I used the "rcl" library for the resistors (To rotate a component hit CTRL-R)



Now wire up the schematic

- Draw > Net (do not use Draw > Wire as this only draws lines, not connections!). Click on the points you want to wire up.



Wires on your schematic can be given Names, and Eagle will connect all those with the same name, for example "GND" or "VCC", "IN" or "OUT"

- Edit > Name, select the wire and enter a Name.

Text can be added to the schematic to record the wire names

- Edit > Text, enter the name and add to the schematic, ESC to do another name, ESC ESC to exit



You will want to give your components values.

- Edit > Values, click on each component and enter its value (e.g. 4k7)

That's it. Next time I will complete the design and turn this schematic into a board layout.

EAGLE - PCB design software

Eagle is not the easiest software to understand. But I have invested a number of hours to get to grips with it. This is what I have found. (This tutorial was written using the "Lite" version of the software from the Cadsoft web site £60).

This blogpost will cover the starting point for creating Devices to use in your designs if you can't find them in an existing library. A future post will cover drawing a schematic and generating the PCB layout. You could also check out this or this site.



Eagle

Eagle handles these levels, in descending order:

- PCB Design

- Devices or components

- Packages used on PCB layouts

- Symbols use on schematic drawings

- Gates, which are fundamental building blocks of devices (e.g. the individual op-amps in a quad op-amp device)

Libraries and the Device Editor

There are a myriad of libraries of devices from many suppliers, and your software comes with a lot of them, plus many others are made by users for devices they need. There are some web sites, for example this one, to help find if a device exists in a library somewhere.

I would recommend that you chose the libraries you need for your projects, then move all the other unwanted ones to a "oldlibs" folder. This make design a lot easier.

Often you may want to create new devices that you can't find. So here's how to do it using the Device Editor.

Definitions

Device - a combination of a symbol and a package. So that a symbol used on a schematic diagram can be directly translated to a physical device for the PCB layout.

Package - which is the outline and connection types and positions (e.g. SMD or thru hole)

Symbol - the device schematic graphic, and pins to which connections can be made

Gate - parts of a symbol if they are repeated in one device.

When Eagle is started this is the window that appears, called the Control Panel.



There are two important items on the left, Libraries and Projects. under the Library list are all the libraries that you have installed in your /lbr folder, under /Eagle. Under the Projects list are the designs you have made or are working on.





Libraries and new devices

If you can't find the component you need in existing libraries , you will have to design a Device. First create a new library for your components.

- Control Panel, File > New > Library

- Library > Description, enter a description of your library

- File > Save As...

With the Library open you will have this window

I

At the top are three important icons, Device, Package and Symbol.



Making a new device

Start at the level of Gate, creating one of the internal parts of your device.

Symbol

- Chose Symbol icon, then File > New... and name it



In the editor window draw the device and the pins.

- Make an outline of the internal gate, Draw > Wire

- Add pins, Draw > Pins

- Name the pins, View > Info, like the component data sheet

- Set pin direction, Edit > Info > Direction and the pin visibility, Edit > Info Visible (note: chose "pin" to have only the pin name showing on the symbol/schematic)

- Add text, Draw > Text... ">NAME" and ">VALUE", and put these on the 95Names layer, Edit > Info... Layer 95Names

That completes the gate creation. File > Save.

Package

- Chose the package icon, then File > New... to name it



- Set the grid "on" at a suitable resolution for the physical package design, see data sheet

- Draw the pads, Draw > Pads (either SMD and set size) or Pins (thru hole and set shape) and position them correctly

- Draw the outline, Draw > Wire, then Edit > Info to change the lines to the 21Place layer.

Device

Chose the Device icon, then File > New.. and name it



- Add the gate(s) to the left hand pane, Edit > Add

- Rename the gates "A","B", etc Edit > Name

- Set the gate levels to "next", Edit > Info

Add a power supply connection if this is not one of the pins, this will provide a hidden connection to VCC & GND.

- Edit > Add "PWRN", right click PWRN symbol and set Add Level to "request" (Note: it will then not appear on the schematic, but the signals will connect)

- Add the package in the top right pane, New button... chose package

- "Connect" and chose correct pins and pads to be connected

- Set a naming Prefix, e.g "IC", "T", etc (Note: devices on the schematic will be names IC1, IC2 etc)

File > Save All

Additional help

It maybe that someone else has already drawn the package and a similar symbol to the device you are creating. You can use their Package and symbol drawing in your Device like this:

- Control Panel, open libraries. Right click on the library containing the Device with the Package and/or Symbol you want to copy.

- Open the Package or Symbol

- Edit > Group and drag a box round all of the Package or Symbol



This will high-light the selection:



- Edit > Copy

- Now open your Library, chose your Device. Open its Package and or Symbol and Edit > Paste

That's it.

New proposed version of the Radiono TXRX

The Radiono TXRX is a fascinating design, using a bi-directional FET output mixer for RX & TX, driven by a couple of amplifiers one in each direction.

Here's a proposal using MMICs for the two amplifiers. It also has AGC on the audio side to give more "punch".

The input BPF is based on the WA4DSY design aid



and has a response like this: