Remember - Checking requires putting on your
thinking cap and putting yourself in the shoes of
the manufacturer, assembler, and end user or
customer. The human engineering aspects of design
require that you be able to put the part on the
board with a tool or your fingers and still have
room to do so. You should never have to remove a
part to get at another part. Good design takes
into consideration the sequence of assembly as well as the
tooling requirements. After the board is
assembled, it must be tested. Plan for the type
of tests to be required, leave ample space for
test probes or pogo pins if you have a bed of
nails test fixture. Remember when making changes
to an existing board how the test fixture or
tooling will be affected by the changes to the
board.... component clearances, heights, spacing,
electrical voltage spacing... etc.
Safety requirements... look at Shock
hazard, and Fire Hazards. Is the material flame
retardant? The end result from
manufacturing must conform to your fabrication
specs... did you specify it correctly and
completely? If you cut and paste notes from
another design, did you check to make sure they
are still valid? Do you need test points or a
JTAG test
connector? How will you get heat out? Will the board survive in the hot and
cold environments it will be exposed to? How about
Vibration? Have you specified the correct
materials, how will you de-panel the boards after
they are assembled in panel form? Do you need
test coupons? Etc.. Etc...
INTERPRET DRAWING, DIMENSIONS, AND
TOLERANCES PER ANSI Y14.5M. DIMENSIONS ARE IN
INCHES [MM].
MATERIAL: COPPER CLAD PLASTIC SHEET PER
IPC-4101/26 (TYPE GFN, NEMA FR4) 170 deg C Tg
MIN.
LAMINATE USING B-STAGE PRE-PREG MATERIAL
PER IPC-4101/26, (TYPE PC-GF)
MANUFACTURE IN ACCORDANCE WITH IPC-6012A,
TYPE 3, CLASS 2.
INTERNAL LAYERS SHALL BE 1 OZ (.0014 IN
[0.035mm]) COPPER MIN.
EXTERNAL LAYERS SHALL BE 1 OZ (.0014 IN
[0.035mm]) COPPER MIN.
BOARD THICKNESS TOLERANCE SHALL BE .0625 IN
[1.6mm] +/- .007 IN. [0.18mm].
SEE STACK UP DETAIL FOR LAYER
CONFIGURATION.
ALL LAYERS VIEWED FROM THE PRIMARY
(COMPONENT) SIDE
ALL HOLE DIMENSIONS APPLY AFTER PLATING.
ALL PLATED THRU HOLES SHALL BE IN
ACCORDANCE WITH IPC-6012 AND HAVE A WALL
THICKNESS OF .0008 IN [0.020mm] TO .0012 IN
[0.035mm]
ALL HOLES SURROUNDED BY A LAND SHALL HAVE A
MIN ANNULAR RING OF .001 IN [0.025 mm]
LAYER TO LAYER REGISTRATION SHALL BE WITHIN
.003 IN. [0.08mm].
ALL HOLES SHALL BE LOCATED WITHIN A
DIAMETER OF .006 IN [0.15mm] OF TRUE POSITION
AS SUPPLIED IN CAD DRILL DATA
FINISHED BOARD TO COMPLY WITH IPC-A-600E,
CLASS II.
FINISHED CONDUCTOR WIDTH AND SPACING SHALL
BE WITHIN 10% OF SUPPLIED ORIGINAL CAD DATA.
BOW AND TWIST SHALL NOT EXCEED 0.75% (.0075
IN PER IN) IN ACCORDANCE WITH IPC-A-600F FOR
SURFACE MOUNTED BOARDS WHEN MEASURED USING
IPC-TM-650, METHOD 2.4.22.
FINISHED BOARD SHALL MEET THE REQUIREMENTS
OF UL796 WITH A FLAMMABILITY RATING OF UL 94V-0
OR BETTER. VENDOR'S UL LOGO AND/OR DESIGNATION
AND DATE REQUIRED, TO BE LOCATED ON THE
SECONDARY (SOLDER) SIDE OF THE BOARD.
MAXIMUM RADIUS ON ALL INSIDE SHARP CORNERS
TO BE .063 IN [1.6 MM]
SOLDERMASK USING LPI OVER BARE COPPER PER
IPC-SM-840, TYPE B, CLASS 2, COLOR: TRANSPARENT
GREEN.
ALL EXPOSED CONDUCTIVE SURFACES TO BE ENIG
(ELECTROLESS NICKEL / IMMERSION GOLD) AFTER
SOLDERMASK.
ALL EXPOSED CONDUCTIVE SURFACES TO BE
DIAGONAL HASL (HOT AIR SOLDER LEVELED) AFTER
SOLDERMASK.
APPLY COMPONENT LEGEND(S) USING WHITE
NON-CONDUCTIVE EPOXY BASED INK AS REQUIRED BY
CAD DATA. USE OF WHITE LPI MASK FOR LEGENDS IS
ACCEPTABLE.
ISOLATED OR UNUSED INTERNAL PADS MAY BE
REMOVED AT MANUFACTURER'S DISCRETION.
COPPER THIEVING ON EXTERNAL LAYERS IS
ACCEPTABLE FOR UNIFORM PLATING OUTSIDE THE
BOARD AREA. THIEVING MUST BE OUTSIDE THE BOARD
AREA.
PLUG ALL VIAS WITH SOLDERMASK TO CONFORM
WITH CAD DATA.
BARE BOARD ELECTRICAL TEST IS REQUIRED.
VENDOR TO SUPPLY CERTIFICATION OF BOARD
CONTINUITY BASED ON CAD DATA SUPPLIED.
SEE SHT 2 FOR ASSEMBLY PANEL DETAIL.
Here are a list of check boxes you can go through
to remind you of what to think about... If they
do not apply, simply skip over them.
Mechanical Board Constraints
Board
outline
Mounting
holes
Connector
locations
Hardware
clearances and fasteners
Max
height of components
Board
Material
Mounting Holes
Clearance
for Hardware and components
Lock
washers
Screws
Plastic
Snap Fit hole sizes
Clearances
for Standoffs
Global
Fiducials for surface mount parts?
Sufficient
Land area for Swage
Plated
Non-Plated
Grounding
Material Requirements
Material
appropriate to environment?
Tg
of material appropriate for the maximum
environmental temperature?
Thickness
of material compatible with lead length?
Plating
requirements for surface treatment?
Bow
and Twist requirements?
Prepreg
for multilayer construction?
Dielectric
constant?
Connectors and Brackets
Clearance
for components and hardware
Mating
Dimensions and tolerances
Connector
Orientation
Finger
or tool clearance
Environmental
sealing
EMI
Shielding
Filtering
Holes
sized properly for hand/machine installation
Strain
relief for cables
Clearance
for bend radius of cables
Can
it be assembled? Tool
Interference?
Components
Footprints
match the manufacturers
specifications?
Component
to component clearance?
Fiducials
for fine pitch parts?
Component
to Mounting Hole or board edge?
Component
height clearance?
Pin
one or Polarity clearly marked?
Common
orientation possible?
Common
components or special order?
Ordered
Long lead time items?
All
parts on the BOM?
All
Parts have company
part numbers?
Tooling Clearances
Wave
Solder
Pick
and place
Screening
IR
Reflow Machine
Test
Fixtures
Registration
pins
Holding
Fixtures
Soldering
Iron Clearances
Test
Probe clearances
Trace Geometries
Trace
Widths appropriate to current carrying?
Trace
to Trace spacing less than 7 mils?
Trace
to Pad less than 7 mils?
Trace
sized for Impedance?
Acute
Angles or etch traps that cause undercut?
Break
out from pads sufficient? Fillets needed?
Matching Trace
lengths?
Buses
run together with terminations?
Inner Planes
Clearance
to board edge and cutouts at least 25 mils?
Thermal
pad design? clearances? connects or spokes?
Direct
connections for vias to ground? Inner Pad
removal?
Split
planes? isolation, clearances and return path for
signal traces? Mecca?
Thermal vias?
Capacitance Plane?
Symmetrical Stackup? (avoid warped boards)
Even Copper Distribution?
copper thickness?
Multilayer Board Stackup
Thermal Core?
Symmetrical Stackup? (avoid warped boards)
4 layer
6 layer
8 layer
10 layer
12 layer or greater
Board Outline
Can
the board be trimmed
with a standard .100 or .125 router bit?
Can
the board be panelized?
Radius
appropriate for routing tools?
Can
the board be v-scored?
Are inner layers relieved of copper a minimum of
25 mils around the
perimeter and any cutouts?
Board Information and Text
Board
name and part number with revision in etch or
silkscreen?
Company
name, address, contact name, telephone and fax?
Title
Block and Rev Block filled in.... page numbers,
drawn by, dates, etc.?
Drill
Table filled in with finished hole size, code,
quantity and plated thru or non-plated indicated?
Make a 'read me' text file to be included in the
Gerber package listing all the files it takes to
make the board.
Testability
Test
points located with sufficient clearance to allow
the test probe to contact the board?
JTAG
ports located near power supply connector and
near the Chip under test?
