PCB Design Guidelines
-
In line with our design guidelines, your data package should consist of the following:
- Clear demarcations for all the copper layers.
- Distinguishable layers of solder mask and legend.
- Board Outline, SMD Paste Layer, Carbon Layers, Peel-Off Layers, etc.
- File Format: All the files should be provided in Gerber RS274-X format with the drill file made available in ExcelloAll the files should be provided in Gerber RS274-X format with the drill file made available in Excellon-1 or 2 formats enlisted with the set of required tools. Do not use obsolete format standards like Gerber RS274-D. If that is the only format you can send, ensure you provide adequate aperture files alongside specific apertures used throughout your design.
- Data Exclusions: Unless you believe that it is essential to do so, we do not recommend you send the original CAD data, Graphicode GWK files, or files in Word, PDF, and Excel format. We do not seek information on the parts list, placement, or assembly either.
- Data Accuracy Standards: Carefully examine the generated output for Gerber and Excellon with a dedicated Gerber Viewing Tool before you send such files to us. Once the process is in production, it would be economically impossible to pause or turn it around by adding high costs to the order. Highlight all the necessary instructions and fabrication inputs needed for your Gerber and Excellon files.
- File Naming Standards: Use accessible, short, and industry-standard file names. The PCB Power team strongly recommends ensuring that the layer function is legible in the file name. You can also provide a complementary readme file with the necessary identification codes.
- Data Ratio: All the data made available must be provided in a 1:1 ratio.
- Sizes & Dimensions: The Gerber files and Excellon data should not have any 0.00 mm or 0 mils apertures to meet our design guidelines.
- Uniformity: Make sure you use the same offset for all Gerber layers and Excellon drill data. We strongly recommend you use zero offsets. We also recommend you to match the units as available in your CAD PCB Design Software with your Gerber and Excellon output data to eliminate conversion and rounding errors. Ensure that you use the same grid resolution for Gerber and Excellon data to enable precise match.
- Sequence: The data must be made available from the top layer of the PCB to the deepest layer. Do not mirror any data layer, image, or drill. Industry standards dictate a top-to-bottom view of the Gerber data for the PCB to ensure the text on the board (copper, solder mask, and legend) is legible, and the text at the bottom (copper, solder mask, and legend) is not.
- Drill Hole Overlap: Ensure that the drill holes do not overlap each other. Do not use overlapping drill holes to define slots. Such design issues lead to broken metal pieces and voids, which then lead to suboptimal performance.
- Drill Size Range: Ensure that your drill sizes are within 0.05mm or 2 mils of distance. This increases the manufacturability of your design.
- PTH and NPTH Holes: Provide separate files for plated (PTH) and non-plated (NPTH) holes. If you cannot provide different files, enlist the tools required for the hole variants with clear demarcations. Do not allow overlapping NPTH holes around the contour or outline. These holes are meant to be a part of the outline. Hence, ensure that you follow professional and precise design practices for outlining. In the end, ensure that the PTH holes are on the board's edge and are identifiable on the mechanical layer.
- Flashes: Use flashes for pads and avoid using pads filled with small draws.
- Using Copper Areas: Do not use copper planes with small draws. We strongly recommend you use contours and polygons to construct areas and planes in your design, in line with the standards defined in Extended Gerber Output (RS-274X).
- Outline: Ensure that the board outline is a part of the copper layers and is accurately aligned to avoid offsets. Make sure that you include the board outline in a separate Gerber Mechanical Plan.
- Copper Pads: Remove every copper pad from NPTH holes in case they serve no utility. Ensure that the copper pattern is distant from the board's edge, in line with specific recommendations provided by our team. If you have to extend the copper plane to the edge of the board or plate the board’s edge, highlight this fact in the mechanical layer.
- Labelling and Omissions: Label each Gerber Layer with text towards the right from the top angle. This would help in avoiding mirror board production. Make sure that you have no peelable and same net space errors in the design files. The PCB Power team strongly recommends using full copper instead of hatched patterns on the copper planes.
- Multilayer Boards: Provide and highlight the sequence of layers for a multi-layered board. We recommend you use numbered sequencing for the same. For instance, you can use 1 to denote the layer at the top, 2 for the first inner layer, 3 for the second inner layer, and so on.
- Spacing and Thermal Isolation:Provide a spacing of at least 0.2 mm or 08 mils between isolated pads if you have copper or silver between two pads. This would support resistance and re-depositing. Ensure that your design avoids thermal isolation.
- Thermal Relief Pads:Define each thermal relief pad and ensure that the definition complies with the industry requirements for Annual Rings, Track Widths (Thermal Segment Width), and Gaps. We recommend a Gap of 0.25 mm or 10 mils for Thermal and a Thermal Segment Width of 0.2 mm or 08 mils.
- Redundant Layers: Incorporate redundant layers to avoid bows & twists while adding symmetry to the central layer. Ensure that the number and weight of the additional copper layers add symmetry to the central layer as they are all stacked together. Use stacked up plane layers for minimizing warpage risks.
- Low Pressure:Do not use a low-pressure area since it restricts airflow through the laminated panel for resins and creates micro-voids in multilayer boards. This might even lead to a delamination issue. Add a vent or copper pattern in the inner layers and balance the distribution of pressure.
- Growth Opening: Add an opening in the solder mask of at least 0.1 mm or 04 mils to ensure enough room for registration error. Ensure that the dam value for the solder mask is at least 0.1 mm or matches the track size of the solder mask. Any value beneath the prescribed minimum would lead to an unwanted lift for the PCB surface.
- Non-Green Masks:Such masks often require wider openings and mask dams than conventional solder masks.
- Legend Printing Guideline: Font size and height are critical for the legend's legibility. Any font size less than 1 mm in height would be illegible post-printing. Ensure that the legend print does not overlap the solder mask layer or cover the pad. Following this practice simplifies the soldering process. Maintain the font's width to 0.1 mm and remove all the lines smaller than this prescribed minimum. If you are not using a solder mask layer, clip the legend around the subsequent copper layer or the drill layer, whichever is conveniently available. We recommend keeping a distance of at least 0.2 mm between elements in the legend and the copper image.
- Sizes and Dimensions:Describe the board outlines and dimensions in mm or inches. Precisely mention the details on the positions and sizes of every element included in the internal milling, slots, and cut-outs. When defining the dimensions, use the center of the contour lines as the directive line for the board's outline, irrespective of its thickness.
- Mechanical Plan: Ensure that you provide the following information in the mechanical plan:
- A reference hole with X & Y distances from the PCB outline. It will be important when NPTH elements are drilled without copper pads.
- Use symbols of varying sizes as necessary in the drill map to indicate the position of all the drills.
- Distinguish the PTH and NPTH categories for slots and holes.
- Provide accurate indications for break-routing or V-Cut scoring when you provide the panelized data.
- A build-up drawing or a sequential order of layers must be provided for all the copper layers, solder masks, and layers containing legends. All the additional layers, such as the peel-off or carbon layer, must be sequentially arranged from the top-to-bottom angle. Make sure the file names reflect the same sequence.
- If you request the PCBs to be delivered as arrays, make sure you provide the mechanical illustrations for the arrays.
- Side Preferences: Provide clear descriptions of the PCB sides where you want the carbon application. You can have the carbon layer on either or both of the sides. Provide a distinguishable sequential layer within the mechanical layer and ensure that positions are well-indicated in the file name. Make sure that you include board outlines in the carbon layers for all the generated output.
- Carbon Design Specifications: Please adhere to these specifications:
- Minimum Carbon Line Width: 0.3 mm or 12 mils
- Minimum Carbon to Carbon Spacing: 0.254 mm or 10 mils
- Carbon Pad Relative Sizes: The carbon pad should be 0.15 mm or 6 mils bigger than the copper pad.
- Mask Pad Dimensions: It should be 0.15 mm bigger than copper pads and have the same carbon pads.
- Side Preferences: The peel-off mask is applied only to the bottom side of the PCB. If you need the peel-off layer on both sides or the upper side of the PCB, highlight this fact in the necessary file name and provide a sequential layer in the mechanical layers. Include the board outline in the peel-off layer.
- Small Peel-Off Areas: Do not use such areas randomly across the PCB design. Use large peel-off areas as much as possible. You can aggregate and connect several peel-off areas to have a sizable peel-off area in your design. Having larger peel-off areas makes it easier to remove them post the soldering process is successfully executed.
-
We recommend these peel-off design rule specifications:
- Minimum Width of Any Peel-Off Element (P): 0.5 mm (20 mils)
- Maximum Coverable Hole End-Size (H): 6.00 mm (0.236 inches)
- Minimum Overlap on Copper Pattern (V): 0.254 mm (10 mils)
- Minimum Clearance to Free Copper (W): 0.254 mm (10 mils)
- Minimum Distance from the PCB Outline: 0.5 mm (20 mils)
- Tolerance for the Position: +/- 0.3 mm (12 mils)
- Completely Closed Via Holes: Such holes can be achieved only by using Via Holes.
- Via Hole Dimensions: The maximum end size for completely closed holes is 0.25 mm (10 mils).
- Via Fill:The via pads and holes are covered with an additional solder mask layer during this process. Ensure that you provide the Via Fill data in the Gerber File with only the via pads that require filling along with the board outline. Make sure that the Via Fill layer includes the board outline. Please take a note that the Via Fill can be applied to any single side of the PCB, based upon your design specifications. Hence, make sure that you mention the PCB side where you want the Via Fill to be applied. Like other specifications, make sure that the mechanical layer's file name and layer sequencing reflect the same.
- We recommend you provide a readme file alongside the design files. This readme file should contain an answer to questions like:
- What are the exact file names and their descriptions?
- Where are the essential details of the Gerber Format in the Gerber-d Files?
- Where are the details on the PTH/NPTH Holes?
- Are there any special requirements in this particular PCB design?
- Are the non-functional pads in the inner layers supposed to be removed?
- Should we add copper thieving for better plating?
- Are there any restrictions on the placement of the logo?
- Are there any teardrops to be added at the intersections of the traces and the pads?
-
In line with our design guidelines, your data package should consist of the following:
- Clear demarcations for all the copper layers.
- Distinguishable layers of solder mask and legend.
- Board Outline, SMD Paste Layer, Carbon Layers, Peel-Off Layers, etc.
- File Format: All the files should be provided in Gerber RS274-X format with the drill file made available in ExcelloAll the files should be provided in Gerber RS274-X format with the drill file made available in Excellon-1 or 2 formats enlisted with the set of required tools. Do not use obsolete format standards like Gerber RS274-D. If that is the only format you can send, ensure you provide adequate aperture files alongside specific apertures used throughout your design.
- Data Exclusions: Unless you believe that it is essential to do so, we do not recommend you send the original CAD data, Graphicode GWK files, or files in Word, PDF, and Excel format. We do not seek information on the parts list, placement, or assembly either.
- Data Accuracy Standards: Carefully examine the generated output for Gerber and Excellon with a dedicated Gerber Viewing Tool before you send such files to us. Once the process is in production, it would be economically impossible to pause or turn it around by adding high costs to the order. Highlight all the necessary instructions and fabrication inputs needed for your Gerber and Excellon files.
- File Naming Standards: Use accessible, short, and industry-standard file names. The PCB Power team strongly recommends ensuring that the layer function is legible in the file name. You can also provide a complementary readme file with the necessary identification codes.
- Data Ratio: All the data made available must be provided in a 1:1 ratio.
- Sizes & Dimensions: The Gerber files and Excellon data should not have any 0.00 mm or 0 mils apertures to meet our design guidelines.
- Uniformity: Make sure you use the same offset for all Gerber layers and Excellon drill data. We strongly recommend you use zero offsets. We also recommend you to match the units as available in your CAD PCB Design Software with your Gerber and Excellon output data to eliminate conversion and rounding errors. Ensure that you use the same grid resolution for Gerber and Excellon data to enable precise match.
- Sequence: The data must be made available from the top layer of the PCB to the deepest layer. Do not mirror any data layer, image, or drill. Industry standards dictate a top-to-bottom view of the Gerber data for the PCB to ensure the text on the board (copper, solder mask, and legend) is legible, and the text at the bottom (copper, solder mask, and legend) is not.
- Drill Hole Overlap: Ensure that the drill holes do not overlap each other. Do not use overlapping drill holes to define slots. Such design issues lead to broken metal pieces and voids, which then lead to suboptimal performance.
- Drill Size Range: Ensure that your drill sizes are within 0.05mm or 2 mils of distance. This increases the manufacturability of your design.
- PTH and NPTH Holes: Provide separate files for plated (PTH) and non-plated (NPTH) holes. If you cannot provide different files, enlist the tools required for the hole variants with clear demarcations. Do not allow overlapping NPTH holes around the contour or outline. These holes are meant to be a part of the outline. Hence, ensure that you follow professional and precise design practices for outlining. In the end, ensure that the PTH holes are on the board's edge and are identifiable on the mechanical layer.
- Flashes: Use flashes for pads and avoid using pads filled with small draws.
- Using Copper Areas: Do not use copper planes with small draws. We strongly recommend you use contours and polygons to construct areas and planes in your design, in line with the standards defined in Extended Gerber Output (RS-274X).
- Outline: Ensure that the board outline is a part of the copper layers and is accurately aligned to avoid offsets. Make sure that you include the board outline in a separate Gerber Mechanical Plan.
- Copper Pads: Remove every copper pad from NPTH holes in case they serve no utility. Ensure that the copper pattern is distant from the board's edge, in line with specific recommendations provided by our team. If you have to extend the copper plane to the edge of the board or plate the board’s edge, highlight this fact in the mechanical layer.
- Labelling and Omissions: Label each Gerber Layer with text towards the right from the top angle. This would help in avoiding mirror board production. Make sure that you have no peelable and same net space errors in the design files. The PCB Power team strongly recommends using full copper instead of hatched patterns on the copper planes.
- Multilayer Boards: Provide and highlight the sequence of layers for a multi-layered board. We recommend you use numbered sequencing for the same. For instance, you can use 1 to denote the layer at the top, 2 for the first inner layer, 3 for the second inner layer, and so on.
- Spacing and Thermal Isolation:Provide a spacing of at least 0.2 mm or 08 mils between isolated pads if you have copper or silver between two pads. This would support resistance and re-depositing. Ensure that your design avoids thermal isolation.
- Thermal Relief Pads:Define each thermal relief pad and ensure that the definition complies with the industry requirements for Annual Rings, Track Widths (Thermal Segment Width), and Gaps. We recommend a Gap of 0.25 mm or 10 mils for Thermal and a Thermal Segment Width of 0.2 mm or 08 mils.
- Redundant Layers: Incorporate redundant layers to avoid bows & twists while adding symmetry to the central layer. Ensure that the number and weight of the additional copper layers add symmetry to the central layer as they are all stacked together. Use stacked up plane layers for minimizing warpage risks.
- Low Pressure:Do not use a low-pressure area since it restricts airflow through the laminated panel for resins and creates micro-voids in multilayer boards. This might even lead to a delamination issue. Add a vent or copper pattern in the inner layers and balance the distribution of pressure.
- Growth Opening: Add an opening in the solder mask of at least 0.1 mm or 04 mils to ensure enough room for registration error. Ensure that the dam value for the solder mask is at least 0.1 mm or matches the track size of the solder mask. Any value beneath the prescribed minimum would lead to an unwanted lift for the PCB surface.
- Non-Green Masks:Such masks often require wider openings and mask dams than conventional solder masks.
- Legend Printing Guideline: Font size and height are critical for the legend's legibility. Any font size less than 1 mm in height would be illegible post-printing. Ensure that the legend print does not overlap the solder mask layer or cover the pad. Following this practice simplifies the soldering process. Maintain the font's width to 0.1 mm and remove all the lines smaller than this prescribed minimum. If you are not using a solder mask layer, clip the legend around the subsequent copper layer or the drill layer, whichever is conveniently available. We recommend keeping a distance of at least 0.2 mm between elements in the legend and the copper image.
- Sizes and Dimensions:Describe the board outlines and dimensions in mm or inches. Precisely mention the details on the positions and sizes of every element included in the internal milling, slots, and cut-outs. When defining the dimensions, use the center of the contour lines as the directive line for the board's outline, irrespective of its thickness.
- Mechanical Plan: Ensure that you provide the following information in the mechanical plan:
- A reference hole with X & Y distances from the PCB outline. It will be important when NPTH elements are drilled without copper pads.
- Use symbols of varying sizes as necessary in the drill map to indicate the position of all the drills.
- Distinguish the PTH and NPTH categories for slots and holes.
- Provide accurate indications for break-routing or V-Cut scoring when you provide the panelized data.
- A build-up drawing or a sequential order of layers must be provided for all the copper layers, solder masks, and layers containing legends. All the additional layers, such as the peel-off or carbon layer, must be sequentially arranged from the top-to-bottom angle. Make sure the file names reflect the same sequence.
- If you request the PCBs to be delivered as arrays, make sure you provide the mechanical illustrations for the arrays.
- Side Preferences: Provide clear descriptions of the PCB sides where you want the carbon application. You can have the carbon layer on either or both of the sides. Provide a distinguishable sequential layer within the mechanical layer and ensure that positions are well-indicated in the file name. Make sure that you include board outlines in the carbon layers for all the generated output.
- Carbon Design Specifications: Please adhere to these specifications:
- Minimum Carbon Line Width: 0.3 mm or 12 mils
- Minimum Carbon to Carbon Spacing: 0.254 mm or 10 mils
- Carbon Pad Relative Sizes: The carbon pad should be 0.15 mm or 6 mils bigger than the copper pad.
- Mask Pad Dimensions: It should be 0.15 mm bigger than copper pads and have the same carbon pads.
- Side Preferences: The peel-off mask is applied only to the bottom side of the PCB. If you need the peel-off layer on both sides or the upper side of the PCB, highlight this fact in the necessary file name and provide a sequential layer in the mechanical layers. Include the board outline in the peel-off layer.
- Small Peel-Off Areas: Do not use such areas randomly across the PCB design. Use large peel-off areas as much as possible. You can aggregate and connect several peel-off areas to have a sizable peel-off area in your design. Having larger peel-off areas makes it easier to remove them post the soldering process is successfully executed.
-
We recommend these peel-off design rule specifications:
- Minimum Width of Any Peel-Off Element (P): 0.5 mm (20 mils)
- Maximum Coverable Hole End-Size (H): 6.00 mm (0.236 inches)
- Minimum Overlap on Copper Pattern (V): 0.254 mm (10 mils)
- Minimum Clearance to Free Copper (W): 0.254 mm (10 mils)
- Minimum Distance from the PCB Outline: 0.5 mm (20 mils)
- Tolerance for the Position: +/- 0.3 mm (12 mils)
- Completely Closed Via Holes: Such holes can be achieved only by using Via Holes.
- Via Hole Dimensions: The maximum end size for completely closed holes is 0.25 mm (10 mils).
- Via Fill:The via pads and holes are covered with an additional solder mask layer during this process. Ensure that you provide the Via Fill data in the Gerber File with only the via pads that require filling along with the board outline. Make sure that the Via Fill layer includes the board outline. Please take a note that the Via Fill can be applied to any single side of the PCB, based upon your design specifications. Hence, make sure that you mention the PCB side where you want the Via Fill to be applied. Like other specifications, make sure that the mechanical layer's file name and layer sequencing reflect the same.
- We recommend you provide a readme file alongside the design files. This readme file should contain an answer to questions like:
- What are the exact file names and their descriptions?
- Where are the essential details of the Gerber Format in the Gerber-d Files?
- Where are the details on the PTH/NPTH Holes?
- Are there any special requirements in this particular PCB design?
- Are the non-functional pads in the inner layers supposed to be removed?
- Should we add copper thieving for better plating?
- Are there any restrictions on the placement of the logo?
- Are there any teardrops to be added at the intersections of the traces and the pads?
