Footprint size

threadz · 2017-05-16 18:05

Has the Propeller 2's package size been finalized yet? I vaguely recall 0.5mm pin pitch and 20mm X 20mm but I can't seem to find a source on that.
I'd like to make an EAGLE part because I can see me wanting to use this chip frequently.

cgracey · 2017-05-16 20:15

it is going to be in a 14 x 14 mm QFP-100 with exposed bottom pad for ground.

Tubular · 2017-05-16 20:19

0.4mm pin pitch, right?

cgracey · 2017-05-16 20:21

0.5mm pitch.

It was the Prop2-Hot that was planned to go into a 14 x 14 mm TQFP-128, which had 0.4mm pitch.

Tubular, I'm sorry I haven't shipped you those pin I/O boards yet. I keep forgetting when I go down to Parallax.

threadz · 2017-05-16 20:29

Just to be absolutely sure I know what I'm creating, is this it?
Also, how big will the bottom pad be? Should I just assume it covers the rest of the space under the IC?

cgracey · 2017-05-16 20:38

threadz wrote: »

Just to be absolutely sure I know what I'm creating, is this it?

That's it, but there's a big exposed pad on the bottom for all the GND connections.

threadz · 2017-05-16 20:46

thanks Chip! I'm just gonna assume the bottom solder pad takes up 10x10mm and add a restricted block to prevent me from putting vias there. SMD soldering is hard enough when you can see what you are doing, I'm not playing around with blind soldering.

cgracey · 2017-05-16 21:03

threadz wrote: »

thanks Chip! I'm just gonna assume the bottom solder pad takes up 10x10mm and add a restricted block to prevent me from putting vias there. SMD soldering is hard enough when you can see what you are doing, I'm not playing around with blind soldering.

I think the pad is 10.3 x 10.3 mm. Better to starve it a little of paste on the solder stencil. Maybe 50% area through four windows would be adequate.

threadz · 2017-05-16 21:14

So a 10.3 x 10.3mm pad area but only half of it gets solder paste
split into 4 squares or something?
This is the first time I encountered an IC with a bottom pad

tonyp12 · 2017-05-16 21:21

Footprint should already be available in any cad design program, it's the component that will be custom
Yes, don't over paste the centerpad, 50% reduction, windowing is preferable.

threadz · 2017-05-16 21:25

What exactly is windowing in this context? Google doesn't seem to want to be helpful

potatohead · 2017-05-16 21:35

It's smaller bits of paste, the total being 50 percent of pad area.

Think dots. Or blobs. When compressed, it all mushed and spreads out to cover more area without bleeding out past the center pad boundary.

threadz · 2017-05-16 21:49

Oh clever. Thanks!

cgracey · 2017-05-16 21:57

Yeah, too much solder paste will float the chip upwards, causing a mess and open circuits on some pins. Rather than make one large 10 x 10 mm opening on the stencil, make 4 separate 3.5 x 3.5 mm windows to cover the area. Maybe even a 4 x 4 array of windows measuring 1.75 x 1.75 mm each.

threadz · 2017-05-16 22:38

Eagle is kinda a butt about windowing so I'm gonna make the pad not have cream by default and then add 4 squares of cream on top of the pad. the total area of the squares is about half that of the pad.

threadz · 2017-05-16 22:55

Done! With bonus hole in the middle for if you don't have a reflow oven.

threadz · 2017-05-16 23:39

Hey Chip, have the footprints been decided for the 16 and 32 IO Propellers?

Publison · 2017-05-17 00:15

threadz wrote: »

Hey Chip, have the footprints been decided for the 16 and 32 IO Propellers?

Not cast in stone:

http://forums.parallax.com/discussion/164364/prop2-family/p1

evanh · 2017-05-18 10:54

threadz wrote: »

Hey Chip, have the footprints been decided for the 16 and 32 IO Propellers?

I took a few guesses not long ago - http://forums.parallax.com/discussion/comment/1406983/#Comment_1406983

Rayman · 2019-08-09 20:27

I've just started my first P2 board design in Eagle.
First problem: Where's the official footprint specifications for P2?

Doesn't seem to be on propeller.parallax.com...
Not in docs...

From this thread, I think it's a regular LQFP-100 with a 0.4"x0.4" central ground pad.
I just imported a standard one from SnapEda into Eagle.

BTW: threadz: I think your footprint is wrong... Here's what mine looks like (see attached). See how corners are different?

jmg · 2019-08-09 20:52

Rayman wrote: »

From this thread, I think it's a regular LQFP-100 with a 0.4"x0.4" central ground pad.
I just imported a standard one from SnapEda into Eagle.
BTW: threadz: I think your footprint is wrong... Here's what mine looks like (see attached). See how corners are different?

Chip mentioned 10.3mm PAD ?

The finger length can be modified, and fingers that do not intrude too far under the package give more room for inner Vias and Power rings beside the PAD.
The reduced paste detail is a good idea. Even with all the thermal vias, they are quite small, and it's not clear how much solder wicks into those..

Rayman · 2019-08-09 20:54

There was a thread where how many vias to put there was discussed... Have to dig that up...

cgracey · 2019-08-09 20:57

We are using a 9x9 array of vias under the thermal pad. Maybe overkill, but it's the Eval board.

jmg · 2019-08-09 21:05

Rayman wrote: »

There was a thread where how many vias to put there was discussed... Have to dig that up...

P2D2 uses 7x7 array, Drill : 0.2794, tho I found PCBWAY pcb service that has a price corner at 0.3mm holes, whilst JLCPCB supports 0.3mm in 2 layer and 0.2mm in 4 layers, so it may pay to nudge that to 0.3mm ?

Rayman · 2019-08-09 21:58

I wonder if it'd be better to put 4 giant vias under the ground pad and then hand solder them...

cgracey · 2019-08-09 22:59

Rayman wrote: »

I wonder if it'd be better to put 4 giant vias under the ground pad and then hand solder them...

For enabling manual assembly, that would work well.

Rayman · 2019-08-09 23:35

It's just if the idea is to use heat conduction and convection, direct exposure of the thermal pad to air seems like the best..

jmg · 2019-08-09 23:40

Rayman wrote: »

It's just if the idea is to use heat conduction and convection, direct exposure of the thermal pad to air seems like the best..

Best will be to spread the heat in copper first, as copper has far better thermal conduction than air. Then radiate from the whole thing...

Rayman · 2019-08-09 23:56

You're right, radiation is probably the main way it releases heat.
But, with tiny vias it has to go through the vias to get to the ground plane.
With giant vias, it can radiate directly and also have great thermal contact to ground plane.

I have some finite element software that could evaluate this.
Probably easier just to try it though...

cgracey · 2019-08-10 00:16

The ePad package recommendation is to have a via array that goes down to a large thick copper plane.

jmg · 2019-08-10 00:48

Rayman wrote: »

You're right, radiation is probably the main way it releases heat.
But, with tiny vias it has to go through the vias to get to the ground plane.
With giant vias, it can radiate directly and also have great thermal contact to ground plane.

I have some finite element software that could evaluate this.
Probably easier just to try it though...

That also depends on paste wicking and number of planes.
The Eval board has very small vias, and they look closed at bottom, with solder mask, so expect not much wicking, but that is 4L board, so the plane is quite close.

We have used larger vias with paste, on some boards for higher current and thermal vias, and we have also used vias under D2PAK parts, that nicely wick solder paste.
Giant vias may be ok for manual soldering, but maybe a mid-size via, that has solder mask clearance on bottom and is designed to wick, combined with a 100% paste coverage, can give the best volume production thermal outcome ?

Footprint size

Comments