[Search] [Contact Us]
Progettazione Elettronica Controlli di Macchine Automatiche  
Firmware uC
Masters PCB
Circuiti Ibridi
Software Custom

Eagle CAD
B2Spice A/D
Electra Autorouter
Eagle Power Tools
SuSE Linux

Embedded Linux Board
Moduli I/O USB
Moduli I/O Ethernet
Moduli A/D Ethernet

LPC900 Programmer
PRM-W1 Boards

Cerca nel sito



 Brd FAQ 

EAGLE: Library FAQ
How to clone a part? (from R.W. Davis)
    Open the library where the new part is to be added.
    Under Drawing, Select SYMBOL to get a blank part.
    On the Control Panel, expand the list of libraries.
    On the Control Panel, select the library containing the SYMBOL to be copied, and expand the library to show the parts.
    Drag and drop the SYMBOL (highlighted name from library list -- NOT the picture) from the control panel onto the target library. This automatically copies any packages associated with the old part.
    Under the list of packages to the right, right click on and delete any packages that are not associated with the NEW part.
    If the package for the new part is on the package list, go to STEP 12.
    Click the NEW button below the package list. IF the right package is listed, click on it and go to STEP 12.
    In the open Library window, click Package in the Library pull down menu. Using the same method used for the part, find a package in a library and Drag and drop the PACKAGE. (Can be a different library than the Symbol came from.)
    On the Symbol editor (right side), right click on any packages that don't apply and delete them.
    On the package list, again, click NEW and then select the correct package from the list.
    If an exclamation mark in a yellow circle shows up next to a package, click the package, and then click on CONNECT. Link the correct pad names and net names to map the schematic to the part.
    In the library menu, select RENAME and enter the new part name.
    Save the library.

How do I make a part with multiple symbols? I want to break it up into logical functions (such as the power pins, config pins, generic I/O, specific I/O, etc).
Do same as for any device, define package, and symbol(s), finally create the DEVICE.
Draw the complete package as one part, all 240 pads.
Draw as many schematic symbols as you would like, for example a box with just the power pins, or perhaps, even just the power pins themselves. Ditto for the I/O pins, maybe you'd like to group them, or maybe you'd like just a box or "flag" shape with one input or one output pin, NOTE: for the single I/O pin approach, you only need one symbol each for an input pin or an output pin.
When you create the device, use the ADD symbol icon (looks and acts almost like the add symbol icon in the schematic editor. Although it makes a mess in the device window, I eventually move/place all my symbols directly over the insert point (the little + in the window) this makes it easier to grab the gate when editing the schematic as you know the "handle"/insrt point for the gate is somewhere near its middle. Add as many symbols as you like/need to cover all 240 pins/pads.
Finally use the connect function of the device creation window to connect the pins of the symbols to the respective pads. You will then probably want to "name" each of your gates (I usually have to experiment a bit to get this part to my liking). Use the appropriate ADDLEVEL and SWAPLEVEL for each gate. For example, the I/O pins you probably want all the input pins at 1 swaplevel, say 10 for example, and all the output pins at another say 11 for example. This will allow you to swap input pins or output pins but not allow you to swap an input with an output. I'd probably use addlevel "next" for the I/O pins and "must" or "can" for the power pins.

How do you make package Variants?
The correct way, as you have tried, is to add a variant to the device. To do this open up the library for editing and select your device, IRF9630. First rename the current package variant from the default setting by right clicking and selecting rename. Then click on the "new" button below the window showing the current packages. Select the desired package from the list and give it an appropriate variant name as above. Now connect the device up, click connect and either make the connections between the symbol and package manually or by copying over from the original part by selecting the device from the list that can be accessed just above the cancel button. Check that the connections are correct. You should then have the device variant available, after updating the library in your project of course (in the control panel right click on the library and select update.)

I am mounting the power switch on my pcb board. The terminal is in rectangular shape but the pad in eagle is round. Is there a way to create a custom pad shape?
Not without a fair bit of trouble. You will have to find a board company that will cut the hole out for you. Most people accept the round hole, unless it's obviously a bad solution.

How do you copy devices from one library to another?
See "How to clone a part" above for a method that works with more recent versions of Eagle. For older versions:
Open Destination Lib, FILE/EXPORT/SCRIPT
Open source and destination script files using text editor.
Copy .pac, .sym, and .dev from source into destination (placing the .pac, .sym. and .pac into correct sections of destination file).
Save destination script file.
Open Eagle, from Control Panel select FILE/NEW/LIBRARY
Run destination script using FILE/SCRIPT
Save destination library with same name as original destination, overwriting it. Using this method, you don't have to recreate the device

 Brd FAQ 

Site made with Sworg - Simple Web Organizer
©Copyright 1998-Today PRECMA S.r.l.
All Rights Reserved - Copyright Notice