| Designating
polarity: | Trace widths vs. via sizes: |
| Vias:
Annular rings should be maximized wherever feasible. Annular ring of VM = (pad diameter - hole
diameter). Annular rings less than 0.010" may violate IPC's minimum annular ring requirement.
Also, make sure the cross sectional area of the via is equal to or greater than the cross sectional
area of the trace connected to it. See "Trace widths vs. via sizes" section for the formulas
used to calculate cross sectional area. |
| Thru
hole pads: The optimum pad diameter for a thru hole component is twice
its finished hole diameter. |
| Trace
width and conductor spacing: The current minimum trace width is 0.003".
The current minimum conductor spacing is 0.003". Remember, the smaller
the trace and space, the larger the amount of scrap. Anything larger than
0.007" trace and 0.007" space is reasonable enough to keep the
scrap to a minimum. |
| Silk-screens:
The thinnest line width that can currently be silk-screened is 0.008".
Typically a line width of 0.010" is used for component outlines. The
smallest readable text size is 0.050" character height with 0.008"
line width. Any smaller than this and the text will not be readable. If
a component is known to be mounted on the bottom side without a bottom side
silk-screen, a dashed component outline will be displayed on the top silk-screen
to show component orientation. Silk-screens should never be placed on top
of an exposed pad. A minimum of 0.010" spacing is recommended between
silk-screen and pads. |
| Finished
hole sizes: To determine optimum finished hole sizes for leads, add
0.008" diameter to the maximum possible lead diameter. For boards designed
to be assembled by DSI's auto inserter, the optimum finished hole size is
the maximum possible lead diameter plus 0.016". PCB's with the smallest
finished hole size larger than 0.025" in diameter can be drilled three
at a time. All other boards are drilled one at a time. |
| Fiducials:
Any side of a PCB with surface mount components should have a minimum of
three fiducials. The ideal fiducial for DSI's pick and place machines is
a 0.040" diameter pad with a 0.080" diameter or more solder-mask.
Fiducials should be placed as far apart as possible and clear of any traces,
mounting holes or silk-screens. The outer corners of the board are the ideal
placement. |
| Solder-mask:
The typical solder-mask is a 0.005" annular ring around every pad except
fiducials. e.g. If the components pad is 0.060" diameter then its solder-mask
should be 0.070" diameter. For fine pitch components (0.5" mm with 0.009" between pades), use a 0.003" annular ring. |
| Solder-paste:
Typically the dimensions of the solder-paste area should be the same as
the dimensions of the surface mount pad it is applied to. Custom dimensions
may be used in special cases. |
| Board
outline: A 0.010" line width should be used to draw the board outline.
The board outline should always show the ideal board shape, even if it is
not cost effective to route the board exactly as the board outline shows.
For example, zero radius internal corners are difficult to route. Therefore,
all internal corners can be drawn with a zero radius but must have a minimum
radius specified. Any radius 0.0465" or larger (0.093" router
bit) is considered to be cost effective. Using PCAD layout software, the
board outline is typically drawn on the BOARD layer. When creating gerber
files for manufacturing, the board outline should be included on every artwork
to give the artworks common features for alignment. |
| Designating
polarity: |
| Land
patterns for components that electrically can only be connected one way
must have some way of designating polarity. The polarity marking must be
visible even after the component is mounted to aid QC during inspection.
Here is a list of the typical ways to designate polarity on certain components: |
| Thru
hole DIPs: Thru hole DIPs should have a "1" or a dot in silk-screen
next to pin 1. All pads of the DIP should be round except pin 1's pad. Pin
1's pad should be square. |
| Thru
hole connectors: Thru hole connectors should have a "1" in
silk-screen next to pin 1. All pads of the connector should be round except
pin 1's pad. Pin1's pad should be square. Sometimes pin 2 or the last pin
of the connector need to be designated to show how the pins are numbered. |
| Thru
hole polarized capacitors: Thru hole capacitors should have a "+"
in silk-screen next to the positive pins pad. The positive pins pad should
be square while the negative pins pad is round. |
| Thru
hole diodes or LEDs: Thru hole diodes or LEDs should have its cathode
(-) end designated with a bar in silk-screen. Remember the bar should be
visible even after the diode or LED is soldered to the board. The cathode
(-) pins pad should be square while the anode (+) pins pad is round. |
| Thru
hole SIPs: Thru hole SIPs pin 1 is designated with a bar in silk-screen
between pads 1 and 2 or a dot next to pin 1's pad in silk-screen. Pin 1's
pad should be square while the other pad are round. |
| Thru
hole batteries: Thru hole batteries should have its positive pins pad
designated with a "+" in silk-screen. The positive pins pad should
be square while the negative pins pad is round. |
| SMT
DIPs: Surface mount DIPs should have a "1" or a dot in silk-screen
next to pin 1. |
| SMT
connectors: Surface mount connectors should have a "1" in
silk-screen next to pin 1. Sometimes pin 2 or the last pin need to be designated
to show how the pins are numbered. |
| SMT
polarized capacitors: Surface mount polarized capacitors should have
its positive pad designated with a bar or "+" in silk-screen.
Remember the bar designated positive not negative. |
| SMT
diodes or LEDs: Surface mount diodes or LEDs should have its cathode
(-) end designated with a bar in silk-screen. Sometimes for LEDs a "-"
and "+" in silk screen need to be used instead. |
| Transistors
or ICs in a can: Canister type components usually have a tab on the
rim of the can to designate pin 1. This tab should be shown on the silk-screen
to designate mounting orientation. |
| Whenever
possible, number the pins/pads of your connectors and odd components the
same way the manufacturer of that component numbers them. This is very important
especially when designing cables or pining out connectors. This will greatly
reduce error and confusion when assembling cables and trouble-shooting boards. |
| Trace
widths vs. via sizes: |
| The
cross sectional area of a via should be equal to or greater than the cross
sectional area of the trace connected to it. This helps prevent high speed
transmission line glitches, via blow out and reduces overall circuit resistance. |
Formula
to determine the cross sectional area of a trace:
(Trace width) (Copper thickness) = cross sectional area of trace
Typical copper thickness for 1/2 oz. copper = 0.00072"
Typical copper thickness for 1 oz. copper = 0.0014"
Typical copper thickness for 2 oz. copper = 0.0028"
Typical copper thickness for 3 oz. copper = 0.0043"
|
Formula
to determine the cross sectional area of a via plated up 0.001" inside
hole:
(0.001" plating inside holes is the typical minimum plating requirement
for Diversified systems)
(0.7854) (D + 0.002") (D + 0.002") - (0.7854) (D) (D) = cross
sectional area of via
D = diameter of finished via hole expressed in inches
|
