Allegro Extra pins and Missing Pins

salasidis said:

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)

Pins do NOT have to be linear order.  They can be random.  There has to be a 1:1 association from the schematic symbol and the footprint.

You might check the OrCAD tutorials for this as well.

Both your statements are what I meant to say.

The part has 4 pins (in the corners, except that pin 10 is used instead of pin 9 in a DIP16 layout).

The schematic of the company lists the [part with 4 pins, but the numbers are 1,8,10,16  (ie not sequentially numbered)

I managed to get the part to load into Allegro with no errors using the NC-2,3,4 etc as suggested by others earlier.

However, if I were to go into DIP16, erase 12 of the pads, but keep the ones remaining with their original part numbers (ie not sequential) it seems to fail whether NC is specified or not.

I woud assume that sequential pin numbring is therefore required, but it makes using the schematic, and correlating it with the actuial datasheet a little more cumbersome.

Just make sure your schematic symbol and PCB Footprint match exactly. If you want 4 pins numbered 1,9,10,16 on the footprint, make sure the schematic symbol matches, i.e has pins 1,9,10 and 16. They do not have to be sequential they just have to match.

Here's a working example.  I took a 4 pin oscillator and mapped it to a standard 16 pin footprint.  Prior to adding the NC property I got the same errors as you.  Look at the oscillator in OrCAD and you will see the NC property that allows me to map it to a 16 pin part.

The "NC" property is added in Capture (schematic), not the layout.

1) Pick the part on the schematic; RMB --> Edit Properties (Properties GUI comes up)

2) Click New Column tab: Add NC as the Name and your pin numbers as the Value

(e.g. New Column --> Name: NC ; Value: 1,2,3,etc. whatever pins are no connect)

Good day.

Mitch