Check my Eagle device/part?

I have made my first Eagle part. Luckily the package was already there however there was no symbol so I had to connect the package to the symbol to create the device. It seems ok but I'm not sure.

Could you have a look?

I don't know how to get the part out of the original Texas library so you will have to scroll down to "OPA 561". I had to zip the library because the forum doesn't let you upload library files and I've also upped the opa datasheet.

Thanks.

Antknee.

**broken link removed**

Hi antknee,

why would you want 12 unused pins on a schematic?

First it will take up more space and second it will ugly with the same pin and pad names with absolutely no function. (pins 1, 10 and 11 through 20 are not connected anywhere)

Here is how I would use the OPA561 (basically) in a schematic with small changes if pins are easier to route without crossing nets.

The DIL-20 package offered by Eagle has longitudinal (Y) solder pads which allow exactly two traces less to route between pad rows. I changed the pad shape to octagon at a diameter of 1.6002mm and a drill size of 0.8192mm.

Here is the device and the zipped Eagle library if you prefer you use that one.

You also forgot to give the symbol a name and a value label. (IC number and value can't be seen on the schematic!)

Regards

Boncuk

Hi Boncuk,

Thank you. That is an improvement and I will use yours. I added the extra unused pins because Eagle wouldn't let me use the symbol without telling it what to do with the extra pins. I'm guessing there is a command to tell Eagle they are unused, if I recall there was an extra connection option saying "EXP", I'd say that was it. Yes I should have given the IC a name

I will remember to be innovative like this because having used part of the sparkfun tutorial to get this far I could see what a large amount of effort making a footprint would be.

Antknee.

Hi antknee,

Eagle lets you design any symbol with any number of pins. Even designing the OPA561 you just use the connected pins as per data sheet.

When going for the device (using a DIL-20 package) just connect the pins off the symbol to the corresponding pads of the package.

The list of pins to be connected is reduced to the number of pins you used for the symbol. If connecting a symbol with less pins than pads are available in the package you must take special care not to accidently connect e.g. pad1 with pin2.

You won't see that error in the schematic, but in the PCB design.

Using a symbol with all 20 pins you must connect each pin with a pad.

Failing to do that you won't be able to load the device into a schematic layout.

You'll receive the error message "device contains unconnected pins" with Eagle refusing to load the device.

Devices with vertically arranged pins (e.g. VSS and GND) always carry the pin number on the left side. You will have observed that in the device the text ">NAME" smears into the pin. Using IC numbers the display is undistorted.

Here's a test circuit showing all connections properly.

Regards

Boncuk

That makes sense, as you explained it I thought 'that will work'. I had no need to have 20 pins, just the ones that were going to be in use.

I am going to start making up a circuit in Eagle using this chip imminently, I have just been looking to source the chip and it seems to be sold out everywhere I usually check - Farnell, Mouser, RS and Digikey. I don't know how long it will take to come back into stock, hopefully soon.

Regards,

Antknee.

antknee said:

... to get this far I could see what a large amount of effort making a footprint would be.

Antknee.

Click to expand...

Are you joking?

The maximum time I spent designing a package was for the SOT227, which took me about one hour.

Other packages are a matter of minutes.

Regards

Boncuk

Thanks for the test circuit.

Perhaps the Sparkfun tutorial is more comprehensive than it needs to be. It certainly looked lengthy