PCB Fabrication Design Guidelines

Data Package

A complete data package is required for accurate PCB fabrication. The package must include:

• All Gerber files in RS274-X format
• NC drill files in Excellon-1 or 2 format with an embedded tool list
• Fabrication drawing (Readme.doc)
• For flexible PCBs: a layer stack-up diagram showing flexible materials, stiffeners, and cover lay layers

File format and naming:

• Use Gerber RS274-X format. Avoid the outdated RS-274-D format
• Do not include original CAD files, Graphicode GWK files, PDF, Word, or Excel files, parts lists, or assembly information
• Use clear, concise file names that indicate the layer function. Add a readme file if layer function is not evident from the file name
• Avoid overly long file names

Data preparation:

• Verify all Gerber and Excellon files with a Gerber viewer before submission
• Provide all fabrication instructions within the Gerber and Excellon files
• All data must be provided at 1:1 scale (full scale)
• Gerber and Excellon files must not contain zero-size apertures (0.00 mm / 0 mils) or zero-sized tools
• Use the same offset for all Gerber layers and Excellon drill data — zero offset is preferred
• Use consistent units (mm or inches) across all output files, matching your CAD software settings
• Structure data from the top of the PCB to the bottom
• Do not mirror or transform any data layer
• Text on the top side of the board should be readable. Text on the bottom side should be mirrored (non-readable)

Drill Layer

The drill layer must include the following specifications:

• Hole sizes and tolerances
• Hole locations and coordinates in US standard units (inches or mils)
• Plating requirements for all drilled holes, including PTH and NPTH information
• Detailed specifications for countersunk holes, including diameter, depth, and side
• For flexible PCBs: drill tolerances and hole placement relative to bend areas to avoid tearing or stress concentrations

Drill guidelines:

• Ensure drill holes do not overlap — overlapping holes can cause broken drill bits and voids in plated hole barrels
• Do not use overlapping drill holes to define slots
• Drill increments are typically 0.05 mm (2 mils) — combine drill sizes within 0.05 mm (2 mils) of each other where possible
• Provide separate drill files for PTH and NPTH holes where possible. If not possible, clearly specify different tools for PTH and NPTH holes
• Avoid overlapping NPTH holes on the board contour. Treat them as part of the outline and draw the outline accordingly
• Clearly indicate any PTH holes located on the board edge in the mechanical layer

Copper Layers

Copper layer specifications must include:

• Copper weight for each layer in ounces or micrometers
• Trace width and spacing following design rules for signal integrity
• Impedance control requirements including trace dimensions and dielectric properties
• Copper layer thickness to ensure proper current carrying capacity
• For flexible PCBs: copper type (rolled annealed copper is recommended) and any special routing considerations for dynamic bending applications

Copper layer guidelines:

• Use flashes for pads instead of drawn pads (pads filled with small draws)
• Avoid drawn planes — use contours or polygons to define copper areas or planes as standard in RS-274X output
• Include the board outline in all copper layers to ensure proper layer alignment
• Include the board outline in a separate Gerber mechanical layer
• Remove copper pads from NPTH holes if unused or unconnected
• Maintain copper pattern clearance from the board edge per fabrication requirements
• Clearly indicate in the mechanical layer if a copper area extends to the board edge or if edge plating is required
• Use top-viewed right-reading text to label every Gerber layer
• Avoid peelables and same net spacing errors
• Use full copper instead of hatch patterns in copper planes
• Always provide the correct layer sequence for multilayer boards — indicate layer sequence by placing a logical number in each copper layer (e.g., 1 for top, 2 for inner 1, 3 for inner 2)
• Maintain a minimum spacing of 0.20 mm (8 mils) between isolated pads to prevent shorts from copper slivers
• Avoid thermal isolation — clearly define all thermal relief pads to meet annular ring, track width, and gap requirements
• Recommended thermal relief gap: 0.25 mm (10 mils); thermal segment width: 0.20 mm (8 mils)
• Use balanced board construction to prevent bow and twist — copper layers should be symmetrical around the center of the stack-up
• Place plane layers symmetrically in the stack-up to minimize warpage risk
• Add venting or copper patterns in inner layers to equalize pressure distribution

Solder Mask and Legend

Solder mask guidelines:

• Minimum solder mask growth/mask opening around the pad: 0.10 mm (4 mils) to accommodate mis-registration
• Minimum solder mask dam: 0.10 mm (4 mils) — dams below this size are difficult to process and may lift from the PCB surface
• Non-green masks require wider mask openings and larger mask dams than green masks
• For flexible PCBs: specify any areas where mask should be omitted or modified to accommodate bending

Legend guidelines:

• Minimum font height: 1 mm (40 mils) — fonts below this size may be unreadable after printing
• Break or clip any legend print that overlaps the solder mask layer to prevent legend ink from covering pads
• Minimum line width for fonts: 0.10 mm (4 mils) — remove any lines thinner than 0.10 mm (4 mils)
• If no solder mask layer is present, clip the legend against the corresponding copper layer. If no copper layer is present, clip against the drill layer
• Maintain a minimum distance of 0.20 mm (8 mils) between legend elements and the copper image
• For flexible PCBs: specify any areas where legend should be omitted or modified to accommodate bending

Mechanical Layer

The mechanical layer must include:

• Exact board outlines with dimensions in mm or inches
• Exact positions and sizes for all internal milling, slots, and cutouts with dimensions
• Use the center of the contour lines as the board's actual outline regardless of line thickness

Additional requirements:

• A reference hole showing X and Y distances of the drill hole center from the PCB outline (required for NPTH holes without copper pads)
• Positional indication of all drills using symbols in a drill map, with different symbols for different drill sizes
• PTH/NPTH indication for all holes and slots
• A clear layer sequence or buildup drawing showing all copper layers, solder mask, legend layers, and any additional layers in the correct sequence from top to bottom with corresponding data file names
• If PCBs are to be delivered as an array for assembly, include the mechanical drawing for the array

For flexible PCBs, the mechanical layer must also include:

• Bend lines with precise locations and bend radii
• Areas requiring stiffeners with material and thickness specifications
• Finished thickness requirements for flexible and rigidized areas
• Dimensional tolerances in both flexed and unflexed states

Selective Plating and Carbon Printing

• Clearly indicate the side(s) of the PCB for selective plating or carbon printing (one side or both sides)
• Indicate position through proper file naming and a clear buildup or layer sequence description in the mechanical layer
• Include the board outline in all plating and carbon layer output files

Carbon printing design rules:

For flexible PCBs: specify plating requirements for flexible areas, noting any limitations on plating thickness or processes that may affect flexibility.

Peel-off Mask

• Peel-off mask is typically applied to the bottom side of the PCB only
• If peel-off is required on the top side or both sides, clearly indicate this through file naming and a description in the mechanical layer
• Include the board outline in all peel-off layer output files
• Avoid many small, randomly placed peel-off areas — where practical, connect separate areas into one larger area for easier removal after soldering

Peel-off mask design rules:

For flexible PCBs: consider whether peel-off mask is appropriate and how it interacts with bending areas.

Via Fill

• Completely closed via holes can only be guaranteed through via fill
• Maximum via hole end size that can be completely closed: 0.25 mm (10 mils)
• Via fill covers the via pad and hole with a second layer of solder mask
• Provide via fill data as a Gerber file containing only the via pads to be filled, including the board outline
• Via fill is typically applied to one side of the PCB only
• Clearly indicate the side (top or bottom) for via fill application through proper file naming and a description in the mechanical layer

Fabrication Drawing (Readme.doc)

Include a fabrication drawing (Readme.doc) file with the following:

• List of all file names and descriptions
• Gerber format details (for Gerber-D files)
• PTH/NPTH hole details
• Any other special requirements

Address the following questions within the fabrication drawing:

• Should non-functional pads in inner layers be removed?
• Should copper thieving be added for better plating?
• Are there any logo placement restrictions?
• Should teardrops be added at trace and pad intersections?
• Is a void rim acceptable if a non-plated through-hole passes through a copper land?
• If spacing is inadequate for a solder mask dam for a fine-pitch SMT package, is a gang opening acceptable?
• If hole size tolerances are missing, is +/- 0.075 mm (3 mils) acceptable?
• If PCB thickness tolerances are missing, is +/- 10% acceptable?
• If PCB size tolerance is missing, is +/- 0.25 mm (10 mils) acceptable?

Countersunk holes: Countersinking creates a conical indentation on the hole surface to allow a screw or bolt to sit flush with the PCB surface. If a countersunk drill is required, provide the drill diameter, countersunk angle, depth, and side in the mechanical drawing. Include an image showing the required values.

For flexible PCBs, the fabrication drawing must also include:

• Material specifications for the flexible base material (e.g., polyimide), cover lay requirements, and stiffener details
• Bend radius requirements and bending limitations
• Stiffener details including material, thickness, and placement
• Any impedance control requirements specific to flexible materials