This is a tutorial about:
- reading manufacturers drawings for a land pattern for an IC having a QFN-16 footprint on a PCB
- making various compromises
A future post may discuss drawing the land pattern using Inkscape, creating an SVG file for Fritzing.
The specific IC is the BQ25504 from Texas Instruments.
The goal is to translate from the chip manufacturer’s drawings and textual recommendations to an SVG drawing for Fritzing.
Many compromises must be made:
- for Fritzing and the Fritzing fab
- for the SVG editor tool, Inkscape
- for lack of standards by manufacturers
The datasheet for the BQ25504 chip shows land pattern data near the end of the document.
Other manufacturers have different drawings.
Compromising between various QFN-16 specifications
Is the QFN-16 PCB land pattern a standard? I assume it is not.
- otherwise why would each manufacturer show their own drawings?
- another TI document describes a package called QFN-16 that has an entirely different, rectangular footprint.
- the pitch between pins can be different on packages called QFN-16
So the Fritzing SVG file will be a compromise in the greatest (or least?) common denominator sense.
The most general description is: the PCB land pattern for a chip that:
- is an SMD device
- is 3mm square
- has pins at 0.5mm pitch
- has four pin/pads on each side
- has pins that are pads underneath on the edge
- has a heat sink pad in the center of the bottom
The result land pattern:
- should work for the BQ25504 chip.
- should work for many other IC’s
- may not work for all IC’s that are purported to have a QFN-16 package.
- may work for other packages that are compatible with the QFN-16 package (a quad SOIC?)
Compromising for Inkscape’s imprecision
The manufacturer’s drawings are “technical drawings”: they have dimensioning artwork. That artwork includes guidelines, arrows, and numeric text for the dimensions. One of the tasks is to translate the printed dimensions to executable dimensions in SVG.
Inkscape is not the best tool for technical drawings. There is a known deficiency: you can’t precisely enter the size of a shape using numbers in a textbox. (You can try, but the number changes after you enter it.)
The comprise we make is to allow shape sizes to differ from specified dimensions by up to 0.05mm.
Compromising on solder mask relief
The manufacturer recommends a solder mask that is 0.07mm wider (all around) than the copper pads. In other words, relieved. The manufacturer refers to industry recommendations. Which say the solder mask should be wider because of the registration tolerance of about 0.07mm for the solder mask, for most PCB fabricators. If the solder mask opening is the same size as the copper pad, a misregistered solder mask that overlaps onto the copper could prevent the pin/pad on the chip from soldering to the pad on the PCB.
Fritzing does not let you specify the solder mask, but generates it automatically. I don’t know whether the automatic process relieves the solder mask. I don’t know whether I should make the PCB pad 0.07mm larger than the manufacturer recommends, so that the solder mask is also larger.
I chose to size the pad as recommended.
Compromising on solder mask between pins
The manufacturer in note C refers to the industry recommendations. Which says that if the solder mask is relieved, the solder mask between pins may approach the minimum width line that will stick to the PCB. They suggest an alternative: a so-called ganged opening, a large cutout in the solder mask around each bank of pins, without solder mask between pins in the gang or bank.
For this chip, the solder mask between pins will be 0.22 mm wide if the solder mask is not relieved, or 0.08mm if relieved.
Again, Fritzing will not let you specify the alternative cutout in the solder mask.
Compromising on rounded land pads
Many SMD land pads are rectangular but the manufacturer recommends a rounded end. This fits the shape of the pin on the chip. It also increases the minimum distance between adjacent pads on the corners of the land pattern. I presume it also helps prevent solder shorts from ends of pads to the central heat sink.
I chose to round the pad ends, on both ends (to simplify the SVG, specifying one stroke with rounded end caps.)
Compromising on pads jutting from beneath the chip footprint
The manufacturer recommends a land pattern where pads jut from beneath the chip by 0.4mm. However, the industry recommendations discuss that a solder fillet to the horizontal portion of each pin is not necessary. And these parts would rarely be soldered with a hand-held soldering iron, instead by reflow technique such as using an oven. So I’m not sure whether the jutting portion is necessary.
On the other hand, some hand soldering techniques require an extra long jutting portion, so you can use a soldering iron to push or drag solder toward the chip, such as for Schmartboards.
The manufacturer’s recommended stencil (for applying solder paste to the land) also has a jutting portion. It is possible that paste from the jutting portion is intended to wick under the chip’s pins during reflow soldering. Proto-Advantage sells an adaptor with a stencil, but they don’t describe the stencil. The land pattern on their adaptor seems to have smaller pads than the chip manufacturer recommends.
Also, the manufacturer shows a rectangular end on the jutting portion. However, it might be easier in SVG to have a rounded end on both ends of the pad.
I chose to keep the recommended length and width of the pad but make both ends rounded.
Compromising on Pin 17, the heat sink land
The manufacturer shows a seventeenth pad in the land pattern. The pad is to be soldered to a thermal pad on the bottom of the chip, to sink heat from the chip to the board. Also the land pattern has four vias (plated holes) in the seventeenth pad to sink heat through the PCB to a copper ground plane on the back.
Also, the manufacturer’s schematic shows pin 17 should be grounded. It probably is grounded to the chip’s ground pin internally to the chip.
I chose to
- create the pad in the land pattern,
- but not to make it a connector
- and not to make vias
( To make it a connector would also require designing 17 pin images for the breadboard and schematic views.)
( To make vias requires knowing how to make holes in PCB’s in Fritzing.)
The BQ25504 is a “power” chip, in the “battery management” class. It is also very small. That explains why it needs a heat pad. Other “logic” chips having the QFN-16 package might be happy without the heat pad.