SparkFun Forums

[RoGuE_StreaK]

Hi all, thanks to the SFE Eagle tutorials I'm designing my first "professional" PCB, going pretty well but I'm running into some issues with a fine-pitch QFN accelerometer (MMA8453Q)
The pads are 0.3mm wide, with 0.5mm spacing between centres; ie. there's only a 0.2mm gap between the pads. Problem is, the soldermask spacing on the pads is such that it overlaps, resulting in no soldermask between the pads. I know what I want to do, but all my searching hasn't found a way of changing this setting, or whether it has to be a "global" setting as opposed to being able to change soldermask tolerances for one particular component?

Can I change a setting so that this Part is fixed retrospecively, or do I have to re-make my library? And if so, are all components going to be affected?

Any help would be greatly appreciated

[macegr]

It is normal for many fine-pitch devices to have no soldermask between the pins. The soldermask process is not usually as accurate as the PCB process, and if the paste is applied correctly the feature size relative to surface tension and volume of solder makes it less likely for a solder bridge to form. You will often just see a "trench" around groups of pads for a fine pitch device. That is essentially what happens when the mask definitions for pads overlap.

[RoGuE_StreaK]

OK, so just ignore those warnings in an informed manner? I'm OK with that, as long as I actually know what the deal is and that it isn't a major issue. Another one of those little tidbits of info to add to the collection.

[MichaelN]

I always like to see some soldermask between pads, since it helps stop solder bridges. Sure, the alignment of the soldermask isn't as good as the PCB process itself, but most companies still get it within 0.002", so that's what I normally use for the soldermask expansion rule on such devices. It's not the end of the world if it encroaches a tiny amount onto the pad area.

[RoGuE_StreaK]

So Michael how do I set the sizing for these pads? And can I set it for just this Part, or does it affect all populated bits?

[MichaelN]

So Michael how do I set the sizing for these pads? And can I set it for just this Part, or does it affect all populated bits?

Sorry, I'm not familiar with Eagle (I use Protel & Altium). Plenty of people around here should know how to do this...

[InactiveUser001]

These days, soldermask should be output at 1:1 to the pads, no oversize.

Let the board manufacturers adjust the soldermask to their processes.

This is specified in IPC-C7351B

[RoGuE_StreaK]

Yeah, but how do I do this in Eagle?

Hmm, just found the following elsewhere, does this sound like a way of doing it for this particular Part?

The mask settings in the design rules are global settings that are valid for all components. You can't define special rules for special components.

BUT you can switch off generating solder stop and cream frame mask automatically for each pad/smd in the library.
CHANGE STOP ON | OFF
CHANGE CREAM ON | OFF
or via the properties dialog.

Now you have to draw the mask manually in the according layers:
tStop bStop tCream bCream

So turn off the auto stopmask when creating the part again, drop in the pads, then on tStop draw rectangles of the appropriate size (same size as pad)?

[holla2040]

I used the sparkfun lib QFN-16_0.5MM.pac for a MMA8452Q and had 2 parts bridge out of 9 assembled. 22% failure. Not good. Looking for recommendations on modifications required to the sparkfun QFN-16_0.5MM.pac. Thanks.

[MichaelN]

I used the sparkfun lib QFN-16_0.5MM.pac for a MMA8452Q and had 2 parts bridge out of 9 assembled. 22% failure. Not good. Looking for recommendations on modifications required to the sparkfun QFN-16_0.5MM.pac. Thanks.

So this footprint didn't have any soldermask between the pads? In this case, I'm not surprised you got bridges, As per previous messages, you want some soldermask between pads. Even a small amount helps to stop bridges.

[holla2040]

Here's what my layout guy says
I would keep the width of the stencil opening the same, but reduce the long dimension - maybe %25?

Here's what the assembly house says
Because the entire part pad is on the underside of the device, once it gets solder, the excess needs a place to go to – in this case it will go sideways to another heat source (the next pad over). Reducing the solder paste in the long direction to inside the silkscreen/outline check layer would provide enough solder to get a good joint without the bridging.

I don't know if the board house adjusted the soldermask as mentioned by mattylad above. My board house and assembly house are different companies.

[holla2040]

From AN4077 - http://cache.freescale.com/files/sensor ... AN4077.pdf
PCB land pad = 0.8mm x 0.3mm
Solder mask opening = PCB land pad edge + 0.113mm larger all around
Stencil opening = PCB land pad -0.015mm smaller all around = 0.77mm x 0.27mm

OK, based on my assembly house instructions, my board layout consultant and AN4077 - MMA845xQ Design Checklist and Board Mounting Guidelines, I've opted for tcream to be as wide as the pin and 25% smaller-ish than the pad. I tried to upload attachment here, but no go, sorry.



I'd recommend that you don't use the SFE lib part, the tcream stencil opening in far too large.

[MichaelN]

From AN4077 - http://cache.freescale.com/files/sensor ... AN4077.pdf
PCB land pad = 0.8mm x 0.3mm
Solder mask opening = PCB land pad edge + 0.113mm larger all around
Stencil opening = PCB land pad -0.015mm smaller all around = 0.77mm x 0.27mm

OK, based on my assembly house instructions, my board layout consultant and AN4077 - MMA845xQ Design Checklist and Board Mounting Guidelines, I've opted for tcream to be as wide as the pin and 25% smaller-ish than the pad. I tried to upload attachment here, but no go, sorry.



I'd recommend that you don't use the SFE lib part, the tcream stencil opening in far too large.

One thing you didn’t mention is the stencil thickness – this, combined with the opening area is VERY important. That app. note states 100 to 125 micron (0.004” to 0.005”) thick, which I would consider the absolute maximum for this type of package, even with the reduced stencil opening size (I’d personally use 0.003” stencils from Ryan O’Hara). More solderpaste greatly increases the chance of bridges, and you hardly need any paste for these types of packages.

I disagree with the soldermask opening Freescale recommend. As per my previous comments, I’d always have some soldermask between pads. Modern PCB manufacturing is accurate enough that this shouldn’t encroach on the pads themselves.

[holla2040]

OK, let me find out more information about soldermask between the pads from my board house.

[holla2040]

OK, the board house says that soldermask between the pads is possible. I'll make the adjustments.

MichaelN, I've got a question though. How much of a border around the pad should I make the solder mask?

Thanks everyone for your comments. If anyone at SFE wants my lib part to replace their problematic one, let me know.