PCB Design Guideline 1:DFM---Design for manufacturability Tips

1. The outline of the board edge should be shown clearly in PCB file,usually in mechanical layer or keepout layer.

1-1.The safe distance of the PTH hole edge to the board edge is 0.4 mm.

1-2.The safe distance of the via edge to the board edge is 0.2 mm.

1-3.The holes will be broken following drilling if they are not positioned an appropriate distance from the edge of the board. See picture for an example.

2. NC drill file (Excellon file)should be provided correctly.

2-1.For one layer board,all hols will be un-plated.For 2 layer or more,holes without copper annular ring in the file will be un-plated,holes with copper annular ring in the file will be plated.

2-2.Circles in mechanical layer or outline layer without copper, which also have no corresponding holes in the Excellon file (see Picture Three for an example),will normally be regarded as non-plated holes.

2-3.There are two possible types of overlapped holes: totally overlapped holes and partially overlapped holes.

A)Totally overlapped holes: the small hole is totally inside the bigger hole (see Picture Five). Please kindly remove the small hole as it will not be required when the big hole has been drilled.

B)Partially overlapped holes: the small hole is crossed with the big hole. These holes will be drilled according to the file design.

2-4. The number of holes marked in Gerber file should be same as that specified in the Excellon Drill Layer file. See the picture below for an example of incorrect data.

3. The distance between the copper to the board edge should be more attention.

3-1. The distance between the copper to the board edge should be more than 0.2mm,or the copper will be exposed on the edge of the board,just as picture 12 shown.We usually shave the copper if permitted.

3-2. The distance between the copperp pads should be at least 5 mil. Or shortage will be appeared after finished the board.

3-3. The annular ring is the PTH hole for soldering, equal to the diameter of the copper pad, minus the diameter of the hole size divided by two.The copper annular ring value should be at least 0.1 mm. It will be broken after completion if the the value less than 0.1 mm. See Picture 16 for an example. The annular ring on the left and right of these holes would be broken after completion.

4. Legends on the silkscreen layer is usually used for component position indication and polarity marking.

4-1.The line width of legends on the silkscreen layer should be at least 8 mil, the width and height of the legends should be at least 20 mil*30 mil, and the distance between the legends should be at least 4 mil. If the silkscreen legends are smaller than required, the finished legends will be fuzzy.

4-2.The silkscreen legends on the copper pads will affect the soldering process seriously.We recommend designers to move the silk-screen legends which cover the pads.Or the silk-screen legends on pads will be shaved if permitted.

4-3. Silkscreen legends on both thick copper and the base material (see Picture 19 as an example) the silkscreen legends will be broken and will not be printed clearly.

5. Solder mask resist openings are on PAD(SMD pad,PTH pad,via pad exposed copper) for soldering parts.

5-1. Solder mask resist openings typically 2 mil larger than the copper pads.Picture shown below are all error designs for Solder mask resist openings.

5-2.The solder mask resist opening for IC pads or gold finger pads.

The solder mask resist openings are separated from each other for the IC pads (see Picture 24). There will be a solder mask resist oil bridge between the IC pads after the boards are finished.

The solder mask resist openings are connected to each other for the IC pads (see Picture 25). There will be no solder mask resist oil bridge between the IC pads after the boards are finished. We recommend you to add solder mask resist oil bridge for fine pitch parts to avoid soldering bridge during refow process.