Hello all. In this edition of The Bare (Board) Truth, I will go over 10 things that should be reviewed prior to releasing a PCB design to be fabricated. I want to stress that, depending upon the application, some of these items may not be feasible in a given design, but overall, these 10 steps will save you time and money.

1. Clarify Copper Weight Intentions

Always clarify the copper weight intentions on a drawing or read me file. Note that most fabricators plate up in whole-ounce increments to meet the IPC minimum of 0.8 of a mil in the barrel for continuity. So, a half-ounce starting outer layer would finish at 1.5 ounce or 2.1 mils of inner-layer copper.

Weights should be expressed as a finished copper weight, as typically inner layers do not receive an additional plate up. (Exceptions would be blind or buried layers.) Also, remember that fabricators will typically associate an "etch compensation" based on the known loss from the etcher. A fairly typical rule of thumb is that for every half-ounce of starting copper weight, a half-mil etch comp is performed on the artwork prior to etch.

An example of a potential problem callout: A half-ounce starting outer layer foil with 0.0035" spaces PRIOR to etch compensation. This would result in 3 mil spaces prior to processing and may cause companies to either suggest starting on lighter copper such as quarter-ounce foil (at which point most fabricators do not even impose an etch compensation) or to "no bid" the job.

2. Finished Hole Size versus Annular Rings

To recap from previous columns, remember that a fabricator typically drills 0.004 - 0.005" over the specified FINISHED hole size to plate down to the correct FINISHED size. This means the pads for signal layers should be at least 0.009 - 0.010" over the FHS (0.004 - 0.005" for plate-down and 0.002" per side annular ring prior to plate). For internal plane layers, the clearance or relief size should be approximately 0.015" over FHS (0.004 -0.005" for plate-down and a minimum of 0.005" per side from the edge of the drilled plated hole to adjacent copper pour). Typical tolerances for plated holes are +/-0.003" and for non-plated holes, +/- 0.002".

3. Via-in-Pad Type Structures

If the design includes via-in-pad type structures and one side is cleared of solder mask and the other is "tented" or covered for the same hole, solution entrapment can cause black or oxidized holes. To avoid this, 80% of the barrel size can be cleared on the tented side to allow solution to flow freely through the hole. Or, better yet, for this type of application it is recommended the holes in question be filled, after plating, with either a conductive material or non-conductive epoxy. The surface is then "planarized" or made flat. At this point it does not matter if one side of the via-in-pad is tented and the other cleared.

4. Utilizing 0.003" Traces and Spaces

Only use 0.003"/0.003" where absolutely necessary due to device pitch constraints. Ideally, fanout to a larger width outside the tight pitch areas whenever possible.