Current Events > PCB Design Tips
PCB Design Tips
  • Jul 19.2017, 14:49:24
  • 1345
  • 0

Hope the following tips can help you to optimize your PCB design works. More information or any enquiries please contact eric@pcbgogo.com.

1. Holes

1.1 Hole plating

One layer board, all the holes un-plated.

Layer>=2:

Holes without copper annular ring in the file will be unplated.

Holes with copper annular ring in the file will be plated.


Holes without annular ring

Holes withannular ring

1.2 Circles as holes

The circles in the 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 ignored. If they need to be drilled as holes, please kindly specify as such in the file.


Picture Three: Circles as holes

1.3 Overlapped holes

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.


Picture Five: Totally overlapped holes

Picture Six: Partially overlapped holes

1.4 Slot holes

Two holes in the same pad need to be plated. There are two possibilities. The first is that there are two holes in the same copper pad with clearance. These should be drilled separately; in this case, please kindly leave at least 20 mil distance between the two holes (see Picture Seven).

The second possibility is that there is no clearance between the two slot holes (see Picture Eight). The slot holes will be oval shaped once drilled (See Picture Nine).


picture 7

picture 8

picture 9

1.5 Distance of the holes from the edge of the board

Routing outline:

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

The safe distance from the vias to the board edge is 0.2 mm.

V-soring/V-grooving outline:

The safe distance from the holes to the board edge is 0.8 mm.

The safe distance from the vias to the board edge is 0.4 mm.

The holes will be broken following drilling if they are not positioned an appropriate distance from the edge of the board. See Picture 10 for an example.


Picture 10: Hole too close to the edge of the board

1.6 Holes number

The number of holes marked in the Gerber file should be same as that specified in the Excellon Drill Layer file. See Picture 11 for an example of incorrect data.


Picture 11: Hole numbers detailed in Excellon file versus those specified in the Gerber file


2. Copper

2.1 The distance between the copper/trace/pad to the edge of the board

Routing outline: The safe distance between the copper/trace/pad from the edge of the board is 0.2 mm.

V-soring/V-grooving outline: The safe distance between the copper/trace/pad from the edge of the board is 0.4 mm.

See Picture 12 for an example of a situation in which the distance between the copper and board edge is out of the safe range. This design may result in the copper being exposed on the edge of the board.


Picture 12: Copper is too close to the edge of the board

2.2The distance between the copper pads

The distance between the copper pads should be at least 5 mil. See Picture 13 for an example of a design in which the distance between the two copper pads is too small. This might result in a short circuit once finished.


Picture 13: Insufficient distance between the copper pads.

2.3 The distance between copper grids

The distance between the copper grids should be 10*10 mil. See Picture 14 for an example. The distance between the copper grids are smaller than required; as such, the grids could not be made out properly.


Picture 14: Insufficient distance between the copper grids

2.4 he flower copper pad in inner layers

See Picture 15. The best flower pad with clearance A at 12 mil, 10 mil for both B and C.


Picture 15: Details of what this image shows

2.5 Copper annular ring

The copper annular ring is equal to the diameter of the copper pad, minus the diameter of the hole size divided by two.

The copper annular ring should be at least 0.1 mm. The copper annular ring will be broken after completion if the copper annular ring is smaller 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.


Picture 16: Copper annular ring smaller than 0.1 mm.

3. legends

3.1 Legends on the copper layer

The width of the line of legends on the copper layer should be at least 10 mil. The width and height of the legends should be at least 28 mil*40 mil, and the distance between the legends should be at least 6 mil. If the copper legends are smaller than required, the finished legends will be fuzzy (see Picture 17 for an example).


Picture 17: Copper legends smaller than required

3.2 Legends on the solder mask layer

The width of the line of legends on the solder mask layer should be at least 8 mil. The width and height of the legends should be at least 20 mil*30 mil. If the solder mask legends are smaller than required, the finished legends will be fuzzy.

3.3 Legends on the silkscreen layer

The width of the line 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.

3.4 The silkscreen legends cover on copper pads

The silkscreen legends cover on the copper pads will affect the soldering. See Picture 18 for an example. As such, we suggest that the board is designed such that the silkscreen legends are positioned away from the copper pads.


Picture 18: Silkscreen legends in close proximity to the copper pads.

3.5 The silkscreen legends on thick copper

Thick copper refers to anything in excess of 4 oz. If the same silkscreen legend covers both the copper and the base material (see Picture 19 as an example) the silkscreen legends will be broken and will not be clear due to the "step" caused by the thick copper. We recommend that the silkscreen legends are located on either the copper or on the base material but not across both.


Picture 19: Silkscreen legend covers both the copper and the base material

4. Soldermask

4.1 The size of the solder mask resist openings

The solder mask resist openings should typically be 2 mil larger than the copper pads, and the solder mask resist openings should be the same shape as the copper pads. The same copper pads should have the solder mask resist openings on both the top and bottom side. See Picture 20-22 for examples.

Picture 20: Partial copper without solder mask resist opening will be covered with solder mask as the solder mask resist opening is smaller than the copper pads.

Picture 21: The solder mask resist opening is bigger than the copper pads. The copper and trace nearby will be exposed.

Picture 22: The solder mask resist opening is not the same shape as the copper pads; as such, the extra base material will be exposed after the board is finished.


picture 20

picture 21

picture 22

4.2 Shifting of the solder mask

The solder mask resist opening should not be shifted from the copper pads. See Picture 23 for an example.


Picture 23: The solder mask resist opening is shifted from the copper pads. The copper pads will be exposed, and some extra material will also be exposed.

4.3 The solder mask resist opening for IC pads or gold finger pads

The solder mask resist openings are separate 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.


Picture 24: Solder mask resist openings are separate from each other

Picture 25: Solder mask resist openings are connected to each other

5. Panels

5.1 Panel with tab-routing

A minimum of 2 mm spacing is required between the two units in panel with tab-routing, and the width of the tabs should be 1.0 mm.

Picture 26: The width of tab is only 0.5 mm. The tabs will be broken easily during the manufacturing process.

Picture 27: The width of tab is 4.0 mm. This is too large and will make it difficult to snap off the panel.


picture 26

picture 27

5.2 Panel with V-scoring

No spacing is required for panels that employ V-scoring (see Picture 28).

Picture 29: spacing between the two units for V-scoring. The size of units will be larger than you defined after the board is finished.


picture 28

picture 29

5.3 Panel with different size units

V-scoring is not available for panels that incorporate units of different sizes because V-scoring can only go all through the whole board, and this may damage the other unit. Tab routing is recommended for panels that incorporate units of different sizes.


Picture 30: Panels that incorporate units of different sizes
Get the quotation for your PCB now by www.pcbgogo.com/b or contact eric@pcbgogo.com for your projects.
Prev: How to Convert Eagle to Gerber
Next:what is BOM list?
  • Comments(0)
Upload a photo:You can only upload 1 files in total. Each file cannot exceed 2MB.Supports JPG, JPEG, GIF, PNG, BMP
Browse
Submit

PCB Instant Quote