SMD pads for each pad:
100% roundness for inner corners
0% roundness for outer corners
Overlap the two
SMD pads to create a single shape. Your 48-pin package, therefore, gets 96
Pads need unique names. Name the sharp pad with prefix
_. For example, name the pin 1 rounded pad
1 and name the pin 1 sharp pad
The screenshot shows five pins on a QFN-20 using this two-SMD scheme. The thermal pad is a similar idea, using three SMDs.
This is a kludge, so there are a few disadvantages.
It is extra work to
Route the PCB layout. The second pad creates a meaningless air wire to
Route these with a
5-mil trace to keep them hidden. The trace needs some width to satisfy the minimum trace width in your DRC.
It is extra work to create the
Connect pads to pins as usual when you create the device. But now you also
Append the extra pad for each connection. For example, after you
1 and schematic symbol pin
1, you also
_1 to schematic symbol pin
Unused pins are flagged by the DRC as
To avoid these DRC Overlap errors:
- In the
.sch, add dummy nets to these pins, i.e., nets that connect to nothing else.
- In the
.brd the dummy net is an
airwire between the two pads that form the single QFN signal pad.
- Route this airwire. Use a small width, e.g., 5-mil, to hide the trace under the copper pad artwork.
The schematic shows an annoying
*2 next to each pin number.
*2 shows there are two of each pin. The pin number and
*2 are visible when
Visible is set to
both in the
Symbol definition. There is no way to keep the pin number and hide the
This eliminates the
*2 and the pin number.
The advantage is the automated artwork for the solder paste and solder mask layers.
Solder Paste Details
The solder paste layer is automated if
Cream is turned on for the
SMD (default). The screenshot shows the pads with layer
31 tCream displayed.
The hatched artwork is left as automatic on the signal pads. EAGLE generates correct 1:1 paste-to-copper artwork for small pads.
The OP shows a QFN without a thermal pad. But usually a QFN has a thermal pad. Unless the QFN is small, a solder paste stencil exposing the entire thermal pad results in too much solder paste. Large thermal pads use window-pane paste artwork to reduce the amount of paste. This decreases likelihood of solder voids under the thermal pad. The voids are created by the outgassing flux with no room to escape.
The solid-looking artwork on the thermal pad is drawn manually with the
polygon tool and a small but non-zero wire width.
Solder Mask Details
This information is independent of how you create the
SMD in EAGLE. But the OP shows a QFN footprint, so the mask artwork is the next logical consideration after getting the pad shape into EAGLE.
Automated solder mask artwork is turned on or off for each
SMD just like the
Whether to use the automated artwork depends on:
- the QFN pitch
- the PCB manufacturer's specification for solder mask relief
For example, a
0.5 mm pitch QFN with solder mask relief <=
3-mil uses the automated solder mask artwork, providing individual stop masks on each pad.
But with a
4-mil relief, those individual masks connect. Turn off the automatic solder mask and draw a polygon to gang the solder mask.
Ganged Solder Mask Artwork
Round the inner corner of the polygon (just like the copper pad) to maximize the amount of solder mask between the gangs. If there is still not enough solder mask to stick to the board, reduce the mask relief.
For example, compare a
5 x 5 mm 32-pin QFN and a
4 x 4 mm 20-pin QFN both with
0.5 mm pitch.
4-mil relief on this QFN32 needs reduced relief at the gang ends, otherwise the solder mask might not stick between the gangs:
This QFN20 has more space between the gangs, so the solder mask artwork shows the full 4-mil relief at the ends of each gang: