PCB GERBER Review Checklist

This is NOT PCB layout review. PCB layout review is done before we send PCB fabrication package to a PCB manufacturer. This review checklist is for us to approve fabrication, because the PCB manufacture will NEVER fabricate a PCB that exactly matches our fabrication package.

A fabrication package may include the following information:

1. GERBER - that describes PCB layer information needed for etching (including soldermask, silkscreen).
2. Drill size and location for plated and non-plated holes.
3. Stack-up information describing thickness of each layer as well as the total thickness of the final PCB.
4. Soldermask
5. Silkscreen

Believe it or not, PCB manufacturers modify all of the above when they fabricate the board. Thus, it is imperative for us the review the “final GERBER” (this is a general term that should include all the above information) BEFORE fabrication to catch possible errors, instead of finding out the errors when we receive the PCB (it is too late).

The review is split up into DFM Review, Stack-up Review and GERBER Review.

PCB manufacturer may not be able to create features we want due to machining limitations. Or they may find certain features may cause reliability issues. They may propose recommended changes which will need our approval. They may also include an option to manufacture “as is” but we bear all the risks. Or they may simply say they are not able to make the board unless we make changes.

We shall review all the items listed in the DFM report and agree to all the resolutions (albeit accepting recommendations, take risk and approve “as is”, etc.)

PCB manufacturers have standard thickness starting material. They take our stack-up proposal as input and matches to their available material and that becomes the final Stack-up which will never be the exact same as what we proposed. Please check the following:

1. Total thickness is meeting our requirement. When there is no specific total thickness requirement, use 62mil as a general thickness number. (You can find on the internet why 62mil thickness is a good general rule of thumb)
2. Check copper thickness that matches what we want for efficiency. (0.5oz, 1oz, etc.)
3. Check layer to layer distance when impedance control is in place.

PCB manufacturer adjusts our proposed GERBER file according to their manufacturing capabilities. Common adjustment examples are:

• Remove via pads from inner layers when there is no connection.
• Enlarge soldermask opening size.
• Adjust trace width considering over etching / under etching possibilities.
• Adjust drill size considering plating thickness.

Please check the following before approving fabrication:

1. Please check the GERBER file in general matches the original PCB layout for gross errors. This is rare but worth glance over.
2. Check the soldermask opening and webbing.
   1. We use NSMD pad design. Soldermask opening should be 1~2 mils larger than the copper pads.
   2. There should be minimum 3 mils of soldermask in between two pads (this is called webbing).
3. Check via pads, tear drops, thermal reliefs and other special features are still in place (sometimes they get removed when manufacturer removes unnecessary via pads).
4. Check minimum trace width and minimum trace to trace distance to make sure they're not outrageous.
5. Check silk screen not overlapping soldermask opening (silk screen may melt during SMT and contaminate the solder joint causing soldering reliability problems)