The Guidelines provided below not just help to reduce the cost of your boards but also minimise the risk of manufacturing errors. For details, you may refer to our services overview. In the following section you can get familiar with:
Input Data Format: Accepted data formats for PCB layout data are:
By PCB layout data we mean all the copper layers, soldermask and legend layers, board outline or mechanical layer, SMD pasta layers, carbon layers, peel-off layer, etc. We step up the accuracy and efficiency of tooling by encouraging the designer to output the Gerber file in a RS-274X output and hence relieve the PCB manufacturer from loading apertures during the tooling process. NC data: NC data refers to the drill and profile data with the following accepted formats:
IMPORTANT: Please supply ONLY ASCII-encoded files. These files are man-readable which enable our engineers to check them visually if needed during data preparation. CAD PCB design data is NOT at all accepted by us!
Gerber being clear and unambiguous has since years been the industry-standard format for PCB manufacture. Every PCB design package can output Gerber data. A complete description of the process has been provided in your CAD PCB design package handbook and help-files. You can check the accuracy of the Gerber output data by downloading one of the many free Gerber viewers available on the Internet. We recommend GC-Prevue available as freeware from www.graphicode.com. Input data requirements:
For PCB layout data — Extended Gerbers (RS-274X) For Drilling — Excellon1 + appropriate tool list (ideally embedded)
Example: If you use a 10 mill resolution to draw your board in your CAD PCB design software, then use a 1mil output resolution for your Gerber & Excellon output.
Technical Capabilities: General Board Specifications
Product Specifications :
|Minimum Conductor Width (TW)||5 Mils/ 0.127 mm||4 Mils/ 0.10 mm|
|Minimum Conductor Spacing (PP, TP, TT)||5 Mils/ 0.127 mm||4 Mils/ 0.10 mm|
|Minimum Plated Hole Size||10 Mils/ 0.25 mm||8 Mils/ 0.20 mm|
|Maximum Board Size (Active)||610 Mm X 400 mm||820 Mm X 400 mm|
|Maximum Number Of Layers||18||24|
|Maximum Outer Layer Cu. Thickness||4 Oz (140 Micron)||6 Oz (210 Micron)|
|Maximum Inner Layer Cu. Thickness||2 Oz (70 Micron)||3 Oz (105 Micron)|
|Board Thickness Tolerance||+ / - 10%||+ / - 10%|
|SMD Testing||20 Mils/ 0.50 mm||15 Mils/ 0.38 mm|
|PTH HOLE SIZE||PTH TOLERANCE||NPTH HOLE SIZE||NPTH TOLERANCE|
|0.50-3.50 mm||+/- 0.10 mm||< 3 mm||+/- 0.10 mm|
|>3.50 mm||+/- 0.15mm||> 3 mm||+/- 0.15 mm|
|<150.00 mm||+/- 0.20 mm|
|>150.00 mm||+/- 0.50 mm|
|Thickness of PCB||+/- 10%|
|Tolerance for Track width / spacing||+/- 20%|
|Tolerance for Finished copper thickness (Plating in hole is considered)||> 20 micron|
I) LEAD-FREE FINISHES
II) ELECTOROLYTIC GOLD PLATING
2) SOLDER MASK FINISH
3) PRODUCT RAW MATERIAL
Annular Ring: Annular Ring = 1/2 (Circuit layer pad diameter – PHD) Where PHD = Production Hole diameter or Tool ize = finihed hole size + 0.15 mm for Plated Through Holes = finished hole size + 0.05 mm for Non Plated Through Holes
Minimum Annular ring for Outer layers:0.125 mm Minimum Annular ring for Inner layers:0.125 mm IMPORTANT: Annular Ring calculations are carried out from the production TOOL SIZE for the holes, not from the finished hole ENDSIZE. For connected non-plated (NPTH) holes we recommend a minimum annular ring of 0.50 mm. As NPTH holes have no plated barrel, a smaller annular ring may lift during soldering or break away even during normal operating conditions. Holes:
|MIN. FINISHED HOLE SIZE||MAX. BOARD THICKNESS|
|0.20 mm||1.60 mm|
|0.35 mm||2.00 mm|
|0.40 mm||2.40 mm|
|0.55 mm||3.20 mm|
Minimum drill – drill clearance: 0.15 mm. This is measured edge to edge of the drill TOOLSIZE.Please 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. Note: Please do not use overlapping drill holes to define slots.
1. Tool lists for drill files are ALWAYS read by our CAM systems as finished hole sizes (ENDSIZE).
2. All PCB drills are manufactured in step of 0.05 mm so wherever possible combine the drill sizes that are within 0.05mm with each other. So we convert the drill sizes given in the drill files or tool lists into millimeters and round up to the nearest 0.05mm. For example:
3. If possible, provide separate drill files for plated (PTH) and non-plated (NPTH) holes. Or else, please specify different tools for PTH and NPTH holes and mark clearly which tools are PTH and which tools are NPTH.
4. When no PTH/NPTH info is provided we use the following rules to determine PTH/NPTH: For 0-layer and 1-layer boards: All holes are considered as NPTH by default. For 2-layer and multilayer boards: All holes are considered PTH except the following cases which are considered NPTH:
5. To allow for the plating in the hole we drill holes prior to plating at a larger size (drill over-sizing). The conversion rules from finished hole ENDSIZE to production TOOLSIZE are: TOOLSIZE = ENDSIZE + 0.15mm for Plated Through Holes (PTH) + 0.05mm for Non Plated Through Holes (NPTH)
6. Standard tolerances on drill ENDSIZE diameter. NPTH holes: +/- 0.10mm (for drill size <3.0 mm) +/- 0.15mm (for drill size >3.0 mm) PTH holes: +/- 0.10mm (for drill size <3.5 mm) +/- 0.15mm (for drill size >3.5 mm) In case there are no tolerances specified in your data, we will produce according to our standard tolerances.
7. Drilled holes that overlap the board contour can be, NPTH holes without copper pads: these NPTH holes will be treated as part of the board outline. PTH holes with copper pads: these PTH holes will be considered as plated holes on the board edge.
8. Overlapping drill holes. Please do not overlap drill holes. These cause broken drill bits and small remaining material parts may cause plating voids in production. Copper layer:
Multilayers: When designing multilayers, the following should be considered:
Soldermask & Legend Print: There are minimal concerns when considering solder mask and silk-screen design rules. Our standard process is LPI (Liquid Photo Imageable) which produces the best registration around pad features.
IMPORTANT: Solder mask dam smaller than 0.10 mm will be removed and will be converted to the image below.
General Note: Legend clipping is done with respect to solder mask layer & drill layer as our standard to make sure legend ink doesn’t come on pad for better soldering. Clipping rules:
Design Tip: To avoid your legend being clipped maintain a minimum distance of 0.20mm (8mil) between your legend elements and the copper image. This 0.20mm (8mil) = 0.10mm (4mil) Soldermask Annular Ring + 0.10mm (4mil) Legend Clipping Clearance. Mechanical Layer: A mechanical layer should minimally contain: 1.The exact board outlines, ideally including dimensions (mm or inch). 2.Exact positions and sizes for all inside milling, slots or cutouts, ideally including dimensions (mm or inch). IMPORTANT: When no dimensions are given we will 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:
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. It is important to note that hole sizes should be specified as finished hole sizes. Carbon:
1. Peel-off masks are used to:
2. Generally the peel-off mask is applied ONLY to 1 side of the PCB, usually the bottom side.
5. 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.
IMPORTANT: 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.
|NUMBER OF CIRCUITS PER PANEL||MAXIMUM NUMBER OF REJECTED CIRCUITS|
|02 - 03||1|
|07 - 10||3|
|11 - 15||5|
|16 - 20||7|
The position of the defective PCBs will be clearly marked.
If you need panels which do not include rejected PCBs (X-outs), please order them via the On Demand service and tick the “Panel without cross outs” box.
1. Panelise using menu options: “Power Verified” and “Power On demand” services. Using this service you upload one design and indicate the step and repeat you require. We will automatically construct the panel and add a frame with standard tooling holes and fiducials (optical marks) for assembly machines.
1.1. Manufacturability rules:
1.2. To get a price or place an order.
1.3. Profile and break-out tabs:
Example: “Panel by PCBPower ” with breakrouting
1.4. Detail of panel border :
Example “Panel by PCBPower” – V-cut