PCB Design Guideline and Manufacturing Input RequirementBetter the designing and better the PCB manufacturing!
It is observed that PCB designers are concentrating their attention on electronic parameters. Keeping eye on a large number of components available in the market, selecting the correct component and updating the component library they forgot to pay attention on production capacity of their supplier.
From our experience we can list out some basic guidelines here.
- Your data package should contain, PCB layout files means all copper layers, soldermask and legend layers, board outline or mechanical layer, SMD pasta layers, carbon layers, peel-off layer, etc should be in gerber RS274-X format and drill file should be in Excellon-1 or 2 format with embedded tool list.
- If possible avoid data in Gerber RS274-D format as it is already obsolete format. If you send data in gerber RS274-D format then make sure aperture file is there and with the apertures used in the design.
- Do not send PCB Design data.
- Please do not provide any additional files such as original CAD data, Graphicode GWK files, PDF files, Word files (doc), Excel files (xls), part lists, placement and assembly information, etc.
- Where possible check your generated output data (Gerbers & Excellon) with a Gerber viewer before you send it on to production. Make sure that all instructions or other necessary input needed for making the boards are included in the Gerber and Excellon files.
- Use clear and easy to understand file naming and try to avoid long filenames. Make sure that we can easy determine the layer function from the filename or add readme file for file identification. Avoid too long file naming.
- Do not scale your data. All data provided must be scale 1/1 (100%).
- Make sure that your Gerber files do not contain apertures with a zero-size (size =
0.00mm) and that your Excellon data does not have zero-sized tools (size=0.00mm).
- Use the same units (mm or inch) in your Gerber & Excellon output files as in your CAD PCB design software. This will eliminate conversion or rounding errors.
- Use the same resolution (grid) for your Gerber & Excellon data to allow a perfect match.
- Make sure that your data is supplied as seen from top to bottom through the PCB. Do not mirror (or reflect) any data layer – image or drill. Viewing a PCB from top to bottom through the board is the universal practice in the PCB industry. This means that when viewing your Gerber data, text on the top side of your board (copper, soldermask, legend) should be readable and text on the bottom side (copper, soldermask, legend) should be non-readable (= mirrored).
- Do not overlap drill holes. These can cause broken drill bits and the small pieces of material left behind may cause voids in the plated hole barrels.
- Do not use overlapping drill holes to define slots.
- All PCB drills are manufactured in step of 0.05 mm so wherever possible combine the drill size that are within 0.05mm with each other.
- For PTH holes on the board edge, clearly mention for it in the mechanical layer.
- If possible, do not overlap NPTH holes on the board contour / outline, consider it as a part of outline and draw the correct outline.
- When generating output, use “flashes” for pads and avoid “drawn pads” (i.e. pads filled with small draws)
- Avoid drawn planes, filling large copper areas or copper planes with small draws (“painting”). Where possible, use contours or polygons to construct areas or planes. Contourized areas or Polygon Area fill are standard features in Extended Gerber output (RS-274X).
- Include the board outline in your copper layers. This will ensure proper alignment of all layers in case of an offset problem. Also include the board outline in a separate Gerber mechanical plan.
- Remove copper pads from NPTH holes if these pads are not used or connected to other copper.
- Keep copper pattern away from the PCB edge as per your manufacturer’s specification.
- If you require a copper area or plane to extend up to the board edge, then clearly indicate this in the mechanical layer.
- If you require the board edge or part of it to be plated, then clearly indicate this in the mechanical layer.
- Use top viewed right-reading text to label every gerber layer to prevent mirror board production.
- Avoid peelables & same net spacing errors.
- Use thieving and copper balancing to the outer layers to ensure even plating.
- Use full copper rather than hatch patterns in copper planes.
- ALWAYS provide the proper layer sequence for a multilayer board. The layer
sequence can be given in several ways: Indicate the layer numbers in the copper
image by placing a logical number in each layer (1 for top layer, 2 for inner1, 3 for
- If the plane layer design leaves strips of copper between isolated pads, a minimum of 0.20mm is required between isolated pads to avoid causing shorts due to resist lifting and redepositing.
- Make sure your thermal relief pads are properly defined and comply with the production requirement for Annular Rings (AR), Track Widths (Thermal Segment Width) and Gaps. Good practice for Thermals is to work with a Gap of 0.25mm (10mil) and a Thermal Segment Width of 0.20mm (8mil).
- To avoid bow and twist problem, board must have a balanced construction. It is good practice to add redundant layers in order to make the board symmetrical from the centre line of the total thickness.
- Number and weight of copper layers should be mirror imaged about the centre of the
- Avoid low pressure area. Due to low pressure area, entrapped air in the laminated panel do not allow flow of air and resin and it causes micro-voids in laminated multilayer boards or may cause delaminating problem. Add venting or copper pattern in inner layers to equalize pressure distribution.
- Typically solder mask should have a minimum of a 0.10 mm “growth/mask opening” around the pad to allow for any mis-registration.
- The minimum solder mask “dam” should be 0.10 mm (a dam is the minimum track size of solder mask). Once the “dam” goes below 0.10 mm, it becomes more difficult to process without the “dam” lifting off the PCB.
- Mask other than green requires wider mask opening and bigger mask dam than green masking.
- For Legend print, the main consideration is font size / height. Font height less than 1 mm is eligible after printing.
- The legend print will ALWAYS be broken – or clipped – against the corresponding solder mask layer to make sure legend ink doesn’t come on pad for better soldering.
- Remove any bits of line smaller than 0.15mm (6mil).
- In absence of a solder mask layer, the legend print is to be clipped against the corresponding copper layer. If there is no copper layer, the legend is to be clipped against the drill layer.
- To avoid legend being clipped maintain a minimum distance of 0.20mm (8mil) between your legend elements and the copper image.
A mechanical layer should minimally contain:
- The exact board outlines, ideally including dimensions (mm or inch).
- Exact positions and sizes for all inside milling, slots or cutouts, ideally including dimensions (mm or inch).
- While giving dimensions, always take the center of the contour lines to be the exact outline of the board, regardless of their thickness.
Additional information that should be included in the mechanical plan when needed:
- A reference hole: the distance from one drill hole in X and Y to the PCB outline. This is particularly important when you only have NPTH holes without copper pads.
- Positional indication of all drills using symbols (=drill map). Use different symbols for each different drill size.
- PTH/NPTH indication for holes and slots.
- If you supply panelized data include proper indications for break-routing and/or scoring (V-cut).
- A clear layer sequence or buildup drawing including all copper layers, soldermask and legend layers, any additional layers like peel-off or carbon, in the correct sequence viewed from top to bottom and with the correct corresponding data file name.
- If the PCBs are to be delivered as an array for assembly, then the mechanical drawing for the array should be included as well. The overall tolerances for mechanical dimensions are +/- 0.25mm.
- Always clearly indicate on which side of the PCB carbon is to be applied. This can be on one side or on both sides. Indicate the position by proper file naming and a clear buildup or layer sequence description in the mechanical layer.
- When generating output include the board outline in your carbon layer(s).
- Overall carbon design rule specifications:
Minimum carbon line width: 0.30 mm
Minimum carbon – carbon spacing: 0.25 mm
Carbon pad should be 0.15 mm bigger than circuit pad.
Mask pad should be 0.15 mm bigger than circuit pads.
Means Mask pad = Carbon pad.
- Generally the peel-off mask is applied ONLY to 1 side of the PCB, usually the bottom side.
- If you require Peel-off on the top side of the PCB or on both sides, please CLEARLY indicate this by means of proper file naming and clear buildup or layer sequence description in the mechanical layer.
- When generating output include the board outline in your peel-off layer(s).
- Avoid using many different small peel-off areas randomly placed on your PCB. Make the peel-off area as large as possible by connecting the separate peel-off areas wherever practical. This will make it easier to remove the peel-off after soldering.
- Overall peel-off design rule specifications:
Minimum width of any Peel-off element (P): 0.500mm
Maximum coverable hole ENDSIZE (H): 6.00mm
Minimum overlap on copper pattern (V): 0.254mm
Minimum clearance to free copper (W): 0.254mm
Minimum distance from PCB outline: 0.500mm
Tolerance on position: +/-0.300mm
- Completely closed via holes can only be guaranteed by using Via Fill.
- The maximum via hole ENDSIZE that can be completely closed is 0.25mm.
- Via Fill is done by covering the via pad and via hole with a second layer of solder mask.
- Via Fill data should be provided as a Gerber file containing only the via pads that need to be filled and the PCB board outline.
- Do not forget to include the board outline in your ViaFill layer.
- Typically Via Fill is applied ONLY to 1 side of the PCB. Which side is dependent on the board design.
- CLEARLY indicate on which side of the PCB (top or bottom) the ViaFill should be applied. Use proper file naming and clear buildup or layer sequence description in the mechanical layer
You can avoid annoying questions by just attaching one readme file with the following details:
- List of file identification
- Detail for the gerber format in case of gerber-d files
- Detail of PTH / NPTH holes
- Details for any other special requirements
Also add answers to frequently asked questions:
- May we remove of non functional pads in inner layers?
- Adding copper thieving for better plating is allowed?
- Is there any logo placement restrictions?
- May we add “teardrop” at trace and pad intersections?
- May we rim void if a land appears where a non-plated through-hole is placed?
- May we give gang opening to the fine pitch SMT packages if spacing does not permit for solder mask dam?
- If hole size tolerances are not called out, may we use +/- 0.075 mm?
- If PCB thickness tolerances are not called out, may we use +/- 10%?
- If PCB size tolerance is not called out, may we use +/- 0.25 mm?
- Check your manufacturer’s technical specifications and refer their updates regularly.
- Latest PCB Power’s technical specifications are as given below.
|For finished copper thickness of 2.0 Oz.||0.15 mm
|For finished copper thickness of 3.0 Oz.||0.175 mm
|Min. finished via hole size||0.15 mm
|Min. finished via pad size||0.50 mm
|Drill to track clearance for Inner layers (upto 6 layer)||0.275 mm
|Min. drill size for plated holes on board edge||0.80 mm
|Min. drill to drill clearance for plated holes on board edge||0.80 mm
Masking and Scoring:
|Mask opening||Other than Green||0.12 mm
|Min. soldermask web width between pads||Other than Green||0.12 mm
|Scoring||Continuous + Jump Scoring
/* Feedback Form on Page */
/* End Feedback Form on Page */
/* Chat Widget */
/* End Chat Widget */