Allegro Extra pins and Missing Pins

Hi,

consider this:

http://www.cadence.com/Community/forums/p/10483/11767.aspx#11767

regards

tltoth

Cadence allows a "NC" property to be added.

You can do this on a case-by-case basis or modify your global library.  Examples:

A) NC=2,3,4,5,6,7,10,11,12,13,14,15

B) NC=2 (because I am assuming pin 1, 3 are in use on the sot23)

 Just add this property to the parts and it will compile just fine.  You don't need to graphically edit the parts the way you were doing.

Thanks, but could you please tell me where to set the NC propery. I looked within Allegro 'Display' 'Property' but could not find an NC entry.

I would think creating a new footprint with the NC= for the pins not used would be easiest

I tried adding an NC property within the part properties of Capture, but this has not worked, I still get the same netrev.lst message (I tried it for the Dip16 part)

Addendum: I managed to get the DIP16 to work with an NC parameter added to teh capture side (not sure why it did not work the first time).

 However if I try making a new footprint with a DIP16 layout but only 4 pins defined (1,8,10,16) to match the capture, I still get the error message about the missing pins. Do the PCB Footprint pins have to be in a linear order (ie no skipped numbers)

Do this all the time in Cadence Capture (was Orcad)

For your parts, on the schematic side: 1) select the part; 2) Edit properties; 3) add a comment called NC; make the value whatever the pin number is. (e.g. for the diode you'd add a comment called NC with the pin 1 as the value.

Note: pins should be separated by commas: 1,2,3,4,5

For the 4 pin IC you'd have NC: 2,3,4,5,6,9,10,11,12,13

Works well, and is easy to set up.

Mitch

I'm a little puzzled to know what is precisely the problem. When you say "one component mounts on a Dip16 footprint, but only has 4 pins (pin 1,8,9,16)" do you mean:

(a) the package has all 16 physical pins but only 4 are used (the other 12 not connected)

(b) the package has the same outline as a DIP16 but has only 4 physical pins (those at the corners)?

If it's (a), you should use the usual DIP16 footprint and add the NC property for the unconnected pins in Capture, as has already been explained by Mitch.

If it's (b), you should edit the footprint in PCB Editor to remove the non-existent pins, save it under a new name, and use this new name for the footprint in Capture. Follow the instructions in algrolibdev, which are clear.(It's easy to make a completely new footprint using the New Symbol Wizard provided that you have identified the padstacks first.)

I have no idea whether pin number have to be sequential from 1 (1, 2, 3, etc); every package that I have ever used has been numbered this way and I never worried about it! It seems an obvious convention to follow.The pin numbers used by the symbol in Capture must match those on the package used in PCB Editor.

Good luck, John