Minimum solder mask ridge (sliver) for DFN package?

Question

What is better: No solder mask at all under the fine pitch component with thermal pad or shrink the thermal pad to leave room for a solder mask ridge around the thermal pad?

I am making the layout for a surface mount DFN 12+1 pin package (Dual Flat No-lead 3x3mm) from Linear Technology (similar to QFN). The recommended pad layout leaves a clearance of 0.225 mm (8.9mill) between the thermal pad and the periphery pads. With a solder mask expansion of 0.1mm (3.9mill) this leaves a ridge of solder mask (solder mask sliver) of only 0.225mm-2*0.1mm = 0.025mm (1 mill) - clearly not a size which can be produced. In fact the PCB fab house has 0.1mm (3.9 mill) as minimum ridge width. I see two options: 1: Keep the solder mask by: Shrinking the thermal pad's copper land pattern in order to increase the solder mask ridge to >0.1mm (3.9mill). 2: Remove the solder mask entirely (ridge width=0). This is already the case between the periphery pads them selves (pitch 0.5mm (20mill))

I am in doubt as to what is the best option. With option one I have a solder pad which is smaller than the components pad. With option two there is effectively no solder mask at all under the 12+1 pad's of the component and I would fear short circuits.

Any advice would be appreciated.

Answer 1

It is a good idea to have a solder mask ridge between pads, as you say, to reduce the chance of short-circuits. It is not very important that the thermal pad on the PCB is exactly as large as the thermal pad on the component. With a smaller PCB pad you will most likely still get a good electrical connection and good enough heat transfer. (The exception would be when you are trying to use the component near to its maximum temperature and power.)

So, if you are not using the component near its thermal limits, reduce the size of the PCB thermal pad to allow a solder mask ridge around it.

Although not a direct answer to your question, another alternative is to use a smaller solder mask expansion. Perhaps 0.05mm would be enough depending on your manufacturing process.

Answer 2

You didn't specify what tool you're using. The best bet is to find a ready made footprint that was testing in your tool. That's not always possible but it saves a lot of headache.

In this case usually the soldermask would overlap because the pins are so close. However, since solder mask is a negative layer (we don't put soldermask where the layer indicates to positively put soldermask) this would mean no soldermask around those pads. I think this will work just fine. Don't decrease the copper land since that's the manufacturer's recommendation. Solder mask isn't as critical. The comments in the datasheet are "Apply soldermask to areas not soldered". Since this is a bit generic, it seems to agree that it's not critical and should work fine.