Common Errors in PCB Gerber Design and Our Suggestions

No matter how long you have been a PCB designer, creating Gerber files that accurately reflect what you want manufactured is a challenge . However, by learning from others and avoiding the most common errors about PCB design, 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 most common mistakes made with PCB Gerber files and our suggestions.

Missing layers of Gerber Files

Gerbers usually come in a .zip or .rar file,but we often find some layers are missing in it.

Suggestion: Gerber 274X or 274D with all layers including copper layer, solder mask layer,drilling layer, outline layer,silkscreen layer( not necessary),  metric  units or English unit  are both ok.

Missing Aperture List

Your Gerber files specify what to do and where. Your aperture list specifies what tool to use.

Suggestion: 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 do not modify the aperture list your software outputs. An aperture list does not need to be sent with 274X format files, because if 274X gerber, it already shows the tool size.  If you send 274D format, we use your aperture list in combination with your gerber files to create your artwork.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.

Missing circuit board rout outline

A circuit board outline/rout path needs to be included with your files. Gerber files are preferred, but a dimensioned drawing will work provided it is simple to make an outline from, and we can determine how to align it correctly relative to the circuitry. As long as we can identify a line that is the perimeter of your circuit board and it matches your ordered dimensions, we will use it for your board outline.The most common method that customers use for communicating how to cut out their board is to place a 10 mil line on the top copper layer around the perimeter of their circuit, centered on where they want us to cut. We prefer a 10 mil wide line on the mask layer. The edge of the router bit will cut to the center of the given line unless we are told otherwise in the notes. Some customers put the board outline on all layers.

Suggestion:We can make an outline for you, but we will need your confirmation to do so. If your board is a perfect square or rectangle, we can make the outline if we know the exact dimensions and any corner relative to a feature such as the center of a tooling hole. Alternatively, if we know you board is a perfect rectangle and we know the x and y dimensions, we can center this rectangle around you design.

Note: 1. GKO layers will NOT be used as an outline to cut out your board. The GKO layer is meant to be the keep out layer. If no outline, we will ask if you do want us to use the GKO outline as your board outline. 2. With many software packages, the "outline" is seen on all layers (as a global layer), but will commonly not appear in the outputted Gerber files. Gerber file viewers can be used to check if your software is placing the board outline in your files.

Missing excellon drill file or tool list especially no mention PTH or NPTH, or no mention tool size 

Suggestion: 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.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 also ok. 

Insufficient annular ring

An annular ring is needed for some Plated through holes especially when this hole connect to surface copper. The annular ring diameter should be enough bigger than holes. 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 solderability on component holes.

Suggestion: A minimum of .003" annular ring for vias or a minimum of .007" for component holes is required for manufacturing.We All layout packages we will provide as a DFM check. Setting sufficient annular ring in your layout software is the preferred method in order to maintain proper copper spacing. If not, we will set that for you when we make working gerbers.

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. For 1OZ copper weight, a minimum of .004" trace width/spacing is necessary. A premium is charged for trace width/spacing less than .007".

Suggestion : 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.

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. A minimum of .006" inner clearance is required and .008" is preferred for 1oz copper weight.

Suggestion: 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.

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.

Insufficient solder mask open or covered

Suggestion: we will check all these kinds of errors when we make working gerbers and come back to you with our suggestion for your confirmation.

Wrong place of pads, solder mask opening, holes,silkscreen

Place of pads, holes,silkscreen are at wrong places, solder mask opening or covering are wrong.

Suggestion: we will check all these kindsof errors when we make working gerbers and tell you.

Copper exposed may be viewable on circuit board edge or inside cutouts or Non-Plated Holes

Exposed copper may be viewable on the board edge due to copper being to close to the board outline that we will use to cut out the circuit board(s).

Suggestion:

• Single layer pcb(s), Tab-routed arrayed boards and boards with cutouts:

Outer layer copper should be 0.01" away from the center of the board edge to prevent exposed copper. Copper within 0.01" of the center of the rout line may be exposed and viewable from the board edge.

Inner layer copper should be 0.015" mils away from the center of the board edge to prevent exposed copper.

• Scored circuit board(s):
  

For 0.062" thick boards:

Outer layer copper should be 0.015" away from the center of the score line to prevent exposed copper. Copper within 0.015" of the center of the scoring line may be exposed and viewable from the board edge.

Inner layer copper should be 0.02" away from the center of the score line to prevent exposed copper.

For 0.093" thick boards, add 0.005" more of space than described above.

For 0.125" thick boards, add 0.01" more of space than described above.

• Non-plated Drills/holes:  Non-plated holes can have 0.005" spacing from the edge of the drill to the nearest copper.

1) Pull back your copper from the danger zones (as mentioned above) to assure that there will be no exposed copper,

Or 2) Put a note in your order (or write it in an readme.txt file with the gerber .zip) that tells us that exposed copper is intended and/or expected.

Or 3) Put a note in your order telling us that you would like us to pull back any copper that might be in these danger zones so that there will not be any exposed copper viewable when the boards are completed.

Note: If there is copper trace that will be clipped due to being too close to the board edge, Caring Circuits will come back to you with suggestions for your confirmation because of the possibility of severing/lifting the trace.

Discrepancies of unit board or a panel dimension :

If the ordered board dimensions do not match the size of the board seen in the Gerber files or other documentation or emails, the job may go on hold until these mismatches are resolved. If the values are close. PCB orders will be run with the dimensions found in the Gerber files.

Suggestion: Accurately measure the greatest X dimension and Y dimension (extends) of circuit board, or add a note in the readme.txt file that we should run with dimensions found in the Gerber files.

We remind you more

• To make panel drawing economical. Border at two sides 5mm each is enough for manufacturability.
• If you need V-score (V-cut) the panels between small pieces, no need distance between units, otherwise the out size will be bigger.
• Pls mention your specifications, cooper weight, surface treatment, material,solder mask color, silkscreen color, need panel or not.etc. You could write it in .txt ,word,excel or write it in gerber directly.

• If there is mismatches between your purchase order, your email writing and what is found by the CAM Engineer in the Fabrication Drawing, Gerber files, or Readme.txt files , the job may go on hold until these discrepancies are resolved.