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
IAt 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.
No comments:
Post a Comment