Help designing custom footprint in Orcad Layout 9.2

[Will]

Ok, I'm pretty familiar with Layout so far and most of the parts I've
been using that didn't fit a standard footprint I've managed to kludge
together something that worked but I have a part that just will not
seem to work. The part is a 2SD2457 silicon NPN transistor from
Panasonic (got the datasheet from Digikey) and it has what Panasonic
calls a MiniP3-F1 package. Sort of looks like some of the voltage
regulators I've worked with in the past. Three legs across the bottom
of the chip with the middle leg blossoming out into a big fat pad
underneath the chip and sticking out slightly from the top of the
ceramic. So how the heck do I make the middle pad in Layout? It's
not a rectangle, and I'd rather not use my old trick of making two
pads and linking them together in the schematic. I tried making a
copper pour on the top layer of the board (it's a surface mount part)
and that mostly works, but the soldermask layer doesn't like copper
pours so I can't get it to mask that part off. How do I make
non-recatangular/non-oval/non-circular shaped padstacks that are also
masked in the top solder mask layer? Thanks for any help!!!
-Will

 

[Spehro Pefhany]

Ok, I'm pretty familiar with Layout so far and most of the parts I've
been using that didn't fit a standard footprint I've managed to kludge
together something that worked but I have a part that just will not
seem to work. The part is a 2SD2457 silicon NPN transistor from
Panasonic (got the datasheet from Digikey) and it has what Panasonic
calls a MiniP3-F1 package. Sort of looks like some of the voltage
regulators I've worked with in the past. Three legs across the bottom
of the chip with the middle leg blossoming out into a big fat pad
underneath the chip and sticking out slightly from the top of the
ceramic. So how the heck do I make the middle pad in Layout? It's
not a rectangle, and I'd rather not use my old trick of making two
pads and linking them together in the schematic. I tried making a
copper pour on the top layer of the board (it's a surface mount part)
and that mostly works, but the soldermask layer doesn't like copper
pours so I can't get it to mask that part off. How do I make
non-recatangular/non-oval/non-circular shaped padstacks that are also
masked in the top solder mask layer? Thanks for any help!!!

Look at how the SOT-89 package is handled in the library. I think it's
a set of rounded-corner rectangle "copper area" obstacles on all
relevant layers, attached to an ordinary rectangular SMT padstack.

Best regards,
Spehro Pefhany

 

[Paul S]

Create the weird pin as a simple pad shape that fits within the weird
shape. Then, create a copper area for the weird shape. In the
properties for the copper area, you can specify a pin attachment for
it.

Paul

 

[Spehro Pefhany]

Create the weird pin as a simple pad shape that fits within the weird
shape. Then, create a copper area for the weird shape. In the
properties for the copper area, you can specify a pin attachment for
it.

He also needs to create similar shapes on the top mask and solder
paste layers.

Best regards,
Spehro Pefhany

 

[Boris Mohar]

Ok, I'm pretty familiar with Layout so far and most of the parts I've
been using that didn't fit a standard footprint I've managed to kludge
together something that worked but I have a part that just will not
seem to work. The part is a 2SD2457 silicon NPN transistor from
Panasonic (got the datasheet from Digikey) and it has what Panasonic
calls a MiniP3-F1 package. Sort of looks like some of the voltage
regulators I've worked with in the past. Three legs across the bottom
of the chip with the middle leg blossoming out into a big fat pad
underneath the chip and sticking out slightly from the top of the
ceramic. So how the heck do I make the middle pad in Layout? It's
not a rectangle, and I'd rather not use my old trick of making two
pads and linking them together in the schematic. I tried making a
copper pour on the top layer of the board (it's a surface mount part)
and that mostly works, but the soldermask layer doesn't like copper
pours so I can't get it to mask that part off. How do I make
non-recatangular/non-oval/non-circular shaped padstacks that are also
masked in the top solder mask layer? Thanks for any help!!!
-Will

Make the middle pad out of three overlapping pads. One skinny rectangle,
one square rotated by 45° and one large rectangle. Give them all same pin
number and hope that Layabout does not moan to much.

I do not use Layout so I do not know will it take multiple pins with same
number.



Regards,

Boris Mohar

Got Knock? - see:
Viatrack Printed Circuit Designs http://www3.sympatico.ca/borism/

 

[qrk]

Ok, I'm pretty familiar with Layout so far and most of the parts I've
been using that didn't fit a standard footprint I've managed to kludge
together something that worked but I have a part that just will not
seem to work. The part is a 2SD2457 silicon NPN transistor from
Panasonic (got the datasheet from Digikey) and it has what Panasonic
calls a MiniP3-F1 package. Sort of looks like some of the voltage
regulators I've worked with in the past. Three legs across the bottom
of the chip with the middle leg blossoming out into a big fat pad
underneath the chip and sticking out slightly from the top of the
ceramic. So how the heck do I make the middle pad in Layout? It's
not a rectangle, and I'd rather not use my old trick of making two
pads and linking them together in the schematic. I tried making a
copper pour on the top layer of the board (it's a surface mount part)
and that mostly works, but the soldermask layer doesn't like copper
pours so I can't get it to mask that part off. How do I make
non-recatangular/non-oval/non-circular shaped padstacks that are also
masked in the top solder mask layer? Thanks for any help!!!
-Will

If you need to make an irregular pad (regular = circular or
rectangular) to do the following:

1. Place a pin in the center of your pad-to-be. In your case, I would
make the middle pin just like your outer pins and place it as if the
tab didn't exist.

2. To make up the rest of the pad, you need to use Obstacles. Use Free
Track or Copper Area. These obstacles need to touch your pin to make
electrical connectivity. In your case, copper area is appropriate.

3. Here's the clincher, you must associate the Obstacle(s) with the
pin. Use the Pin Attachment button in the Obstacle properties. This
will keep your DRC from reporting the obstacle touching your pin and
trace on the top layer. In your case, you will have obstacles on the
top, soldermask, and solderpaste layers.

Mark