|
Creating Gerber files that accurately
reflect what you want manufactured is a challenge no matter how long you have
been a pcb designer. However, by learning from others and avoiding the most
common mistakes, you can speed up the turnaround time, reduce the chance of
orders placed on hold, and complete your projects faster. The following list
reviews the top seven most common mistakes made with Gerber files and how you
can avoid them.
1. Missing Aperture List
Your Gerber files specify what to do and where. Your aperture list specifies
what tool to use. A single comprehensive aperture list for all layers should be
sent with your Gerber files, rather than a separate aperture list for each
layer. Please note: An aperture list does not need to be sent with 274X format
files. If you send 274D format, we use your aperture list in combination with
your Gerber files to create your artwork.
Requirements: One comprehensive aperture list for all layers, English Units.
Please do not modify the aperture list your software outputs. An aperture list
does not need to be sent with 274X format files.
Resolution: All layout packages which output 274D also output an aperture list.
Common extensions include .rep, .apt, and .apr. If you have difficulty
outputting an aperture list, please send 274X format.
2. Missing Excellon Drill File
Excellon drill files are used to determine what size holes to drill and where.
Plated and non-plated holes need to be included in one drill file, with plated
and non-plated holes having different tool numbers.
Requirements: Excellon Format, ASCII Odd/ None, 2.4 Trailing Zero Suppression,
English Units, No Step and Repeats.
Resolution: Nearly all layout packages will output an excellon drill file. If you
cannot generate one, we can in most cases create one from your fabrication
drawing for an engineering fee.
3. Missing Tool List
A tool list is used in combination with your excellon drill file to create your
drill. Your drill file specifies where to place the holes. Your tool list
specifies what tool to use. A tool list should be embedded in your excellon
drill file or sent as a separate text file. Using a tool list provided on a
fabrication drawing is not preferable, as it eliminates many of the automatic
verifications and makes data entry errors far more likely.
Requirements: Tool list embedded in excellon drill file or sent as a separate
text file.
Resolution: If your layout software will output an excellon drill file, it will
also output a tool list. Common extensions include .tol and .rep.
4. Missing Gerber Files
Believe it or not, many times people submit orders and forget to attach their
gerber files.
Requirements: Gerber 274X or 274D, English units are preferable.
Resolution: ODB++ files are acceptable; It is possible to convert many other
file formats to gerber.
5. Insufficient Annular Ring
An annular ring is the donut (“annulus”) created when your drill pierces a
copper layer. It is defined as the radius of this donut. For example, a .030”
pad with an .020” hole would have a .005” annular ring. This is required to
allow for complete plating on vias, as well as solder ability on component
holes. Many times people do not allow for the proper annular ring requirements.
Requirements: A minimum of .005” annular ring for vias or a minimum of .007”
for component holes is required for manufacturing.
Resolution: All layout packages provide this as a DFM check. Setting sufficient
annular ring in your layout software is the preferred method in order to
maintain proper copper spacing.
6. Insufficient Copper Trace Width/Spacing
Copper spacing is the minimum air gap between any two adjacent copper features.
Trace width is the minimum width of a copper feature, usually traces.
Requirements: A minimum of .005” trace width/spacing is necessary. A premium is
charged for trace width/spacing less than .008”.
Resolution: All layout packages provide this as a DFM check. Setting sufficient
trace width/ spacing in your layout software is the preferred method. Trace
width and spacing push and pull against one another, so changing a problem area
may require rerouting traces, adding vias, or moving components.
7. Insufficient Inner Clearances
Inner clearance is the minimum distance from the edge of a hole to any
adjacent, unconnected, inner layer copper. Sufficient inner clearances help
ensure that your drill does not cause shorts to your inner copper layers. This
is important for both plated and non-plated holes, as non-plated holes may
either cut into an adjacent trace or cause shorts during assembly.
Requirements: A minimum of .012” inner clearance is required and .015” is
preferred.
Resolution: Most inner clearance issues can be resolved if negative image
inners are provided, but it is preferred to not modify these. Setting these
clearances in your layout software is the preferred method, as this will
maintain intended connectivity. While most layout packages provide this as a
DFM check, not all do. Those that do not can usually be manipulated to check
for this violation by setting spacing and annular ring higher.
General guidelines: Spacing + Annular ring = Inner clearance. Another trick
that can help resolve problem areas is to move the affected traces to outer
copper layers, where this is not an issue.
|