Eagle advice please

Thread Starter

stirling

Joined Mar 11, 2010
52
Hi

I'm trying to create an Eagle part in my own lib of an MM232R USB/UART where pins 1 AND 16 are both SHIELD but can't figure out how to do this.

If you were to look at the Atmega MEGA8P (Atmel.lbr) for example, in the .sch, pins 8 and 22 are both named GND and then when you switch to .brd, there's an air wire all nice and in place between these two pins. That's what I'd like to do with the SHIELDS in my effort.

I looked at the symbol of the MEGA8P (DIL28-3) in the Atmel.lib and see that the term GND@1 is used for pin 8 but when I tried similar - no joy. I also can't see anything in the package or device editors that show how this is done.

Anyone know how to do this?

Many thanks.
 

SgtWookie

Joined Jul 17, 2007
22,220
Well, you start off with in the Symbol dialog, one pin named as the signal you wish, GND for example.
The next pin you name as GND@1, next as GND@2, etc.

Then in the Device "Connect" dialog, you connect those pins named GND, GND@1, etc. to the package pins that they belong to.

For example, in the MEGA8 Device "Connect" dialog, G$1.GND@1 is connected to pad 3, GND@2 to pad 5, and GND to pad 21. Eagle only displays GND for those NAMED nodes.

In the Help file, under Editor commands -> PIN, you'll find:
Pins with the same Name

If it is required to define several pins in a component with the same name, the following procedure can be used:
For example, suppose that three pins are required for GND. The pins are allocated the names GND@1, GND@2 and GND@3 during the symbol definition. Then only the characters before the "@" sign appear in the schematic.
It is not possible to add or delete pins in symbols which are already used by a device because this would change the pin/pad allocation defined with the CONNECT command.
 

Thread Starter

stirling

Joined Mar 11, 2010
52
Thankyou for your reply. That's what I'd tried but alas it doesn't appear to solve the issue. This scheme certainly allows you to have several (2 in my case) pins apparantly NAMED the same on the schematic but that's about all so far. There appears to be still no actual logical (internal) connection between the two pins as per the example I gave of the MEGA8-P device.

For example in the MEGA8-P, because pins 8 and 22 are tied with an air wire "inside" the package, when you route (hand or auto), a trace that is connected to (say) pin 8 in the schematic can legitimately be ACTUALLY connected to pin 22 on the board. This isn't (so far) the case with my attempt.

It's strange though because having examined the MEGA8-P device it seems that the naming scheme you suggest (the method I've tried) is ALL that's evident. I can see nothing else in there that causes the physical connection and the air wire to be displayed.

Thanks
 

Thread Starter

stirling

Joined Mar 11, 2010
52
Cracked it. It seems it's the pin DIRECTION attribute that I was missing. It appears that if you name two or more pins the same as we've discussed AND you set the DIRECTION to Pwr, then they're "internally" wired and you get the automatic air wire on the .brd view.

From the help file...
Direction

The logical direction of signal flow. It is essential for the Electrical Rule Check (ERC) and for the automatic wiring of the power supply pins.
Thanks Sgt for pointing me at the right place in the help file. You know how it is - when you're learning a new app - sometimes it's difficult to know what to even look for in the mans.

Thanks
 

Thread Starter

stirling

Joined Mar 11, 2010
52
Thankyou - I've been watching vids and reading whatever I can find until I'm about cross-eyed - but I'll certainly take a look. Board is done and winging it's way to the fab house as I type.
 
Top