Design PCBs to Better Take Advantage of PCBCart's Manufacturing Capabilities

As a company serving for more than a decade in PCB industry, PCBCart is fully aware of the significance of time cost and efficiency for our customers. To minimize time intervals from design files to final products, we've summarized a full list containing confirmation items that'll be implemented by our technical engineers. Sufficient preparations definitely help ensure you a smooth and rapid PCB order.


Prior to sending your PCB design files to us, it's necessary for you to check the following items one by one. NOTE: a summary list of table will be provided at the end of this article for engineers with little time to check images and details.


PCB Design Software Version


PCB design software features different versions that naturally generate different PCB design files holding distinctions between each other in some aspects. To cut your time and ensure the accuracy of your design files, we suggest you tell us your software version in Notes when you submitting the order. Naturally, the OPTIMAL selection is to provide Gerber files.


Holes


a. Hole Plating


For single-layer PCBs, all the holes should be unplated. For circuit boards with over 2 layers, holes without annular ring in the file should be unplated whereas those with annular ring in the file should be plated.


Holes with or without annular ring | PCBCart


b. Circles as Holes


Circles in the mechanical layer or outline layer without copper and have no corresponding holes in the Excellon file will normally be ignored. If you want them to be drilled as holes, please make a note in your PCB design file.


Circles without copper on PCBs | PCBCart


c. Overlapped Holes


There are two types of overlapped holes: 1). When a small hole is inside a bigger hole, they are called totally overlapped holes. The small one should be removed as it is unnecessary when the big one is drilled. 2). When a small hole is crossed with a bigger hole, they are called partially overlapped holes that should be drilled according to the file design.


Overlapped Holes on PCBs | PCBCart


d. Slot Holes


Two holes in the same pad need to be plated, which is classified into two possibilities: 1). When it comes to two holes in the same copper pad with clearance, spacing of at least 20mil should be left between those holes. Moreover, the two holes should be separately drilled as is indicated in the left image below. 2). When it comes to two slot holes with no clearance between them, they should be shaped as an oval once they are drilled, as is indicated in the right image below.


Slot Holes on PCBs | PCBCart


NOTE: when it comes to holes designed at graphic layer, special mark should be used to highlight them and size, angle and depth should be clarified.


PCB Mark Design


PCB marks should be appropriately designed and design rules can be learnt from article Design Requirement of SMT PCBs Part Four: Mark.


V-cut Design


V-cut depth should be reasonably designed. Normally it's one third of the board thickness. Mechanical line should be drawn on PCB design file to indicate where to carry out V-cut.


Copper Annular Ring


Size of copper annular ring can be figured out by a simple calculation of the diameter of the copper pad minus the diameter of the hole size divided by two. The minimum size of copper annular ring should be 6mil with copper thickness at least 1oz, otherwise it will be broken after completion. The image below is an example in which the annular ring on the left and right of these holes will be broken after completion.


Copper Annular Ring on PCBs | PCBCart


Spacing between Copper/Trace/Pad and Board Edge


For boards whose edge goes through milling, the spacing should be at least 0.2mm while for boards whose edge goes through v-cut, the spacing should be at least 0.4mm. The image below demonstrates a situation in which the spacing between copper and board edge is out of the safe range. This design may result in the copper being exposed on the edge of the board.


Copper too close to the edge of PCB | PCBCart


Spacing between Hole/Via Edge and Board Edge


For routing outline, safe spacing between hole edge and board edge is 0.4mm while safe spacing between via edge and board edge is 0.2mm.


For v-scoring/v-grooving outline, safe spacing between hole to board edge is 0.8mm while safe distance between via and board edge is 0.4mm.


Via Hole Design


Via holes must NOT be designed between bare copper area and non-bare copper area.


Spacing between Via Hole Edge and Pad Edge


Spacing between via hole edge and pad edge should be at least 8mil and covered with solder mask.


Aperture of Mask/Resin Plugged Via


Aperture of mask/resin plugged via should be 16mil at most.


Aperture of Micro Via


Aperture of micro via should be less than 5mil.


Gold Finger Bevel


For gold finger requiring to be designed to be a bevel, the ordinary angle is 35°, 45° or 60°.


Spacing between Positioning Hole Edge and Pad Edge


Spacing between positioning hole edge and pad edge should be at least 0.65mm.


Board Layer


A board must contain pad layer, silkscreen layer and routing layer.


Pads


Multiple pads can never be combined together and they should stay independent from each other.


Spacing between copper pads should be at least 5mil. The image below indicates an example of a design in which spacing between the two copper pads is too small, possibly leading to a short circuit once finished.


Insufficient distance between copper pads on PCBs | PCBCart


Spacing between Copper Grids


Spacing between copper grids should be 10mil*10mil. Take the image below for example, the spacing between copper grids is smaller than demanded. As such, the grids could not be made out properly.


Insufficient distance between copper grids on PCBs | PCBCart


Flower Copper Pad in Inner Layers


As is indicated in the image below, the best flower pad with clearance A should be 12mil and 10mil for both B and C.


Flower Copper Pad in Inner Layers of PCBs | PCBCart


Legend


a. Legend on Copper Layer


Width of legend lines on copper layer should be at least 10mil and width and height of legends should be at least 28mil*40mil. Spacing between legends should be at least 6mil. If copper legends are smaller than required, the finished legends will be fuzzy, as is indicated in the image below.


Copper legends on PCBs | PCBCart


b. Legend on Solder Mask


Width of legend lines on solder mask should be at least 8mil and the width and height of legends should be at least 20mil*30mil. Similar with silkscreen/legend on copper layer, if solder mask legends are smaller than required, the finished legends will be fuzzy as well.


c. Legend on Silkscreen Layer


Width of legend lines on silkscreen layer should be at least 5mil and width and height of legends should be at least 20mil*30mil. Spacing between legends should be at least 4mil. If silkscreen legends are smaller than required, the finished legends will be fuzzy.


d. Silkscreen Legends Cover on Copper Pads


Silkscreen legends covers on copper pads will affect PCB soldering. It's suggested that circuit board should be designed such that silkscreen legends are positioned away from copper pads to avoid overlapping.


e. Silkscreen Legends on Thick Copper


Thick copper refers to anything in excess of 4oz. If the same silkscreen legend covers both copper and substrate material, silkscreen legends will be broken and become unclear due to the step caused by thick copper. We recommend that silkscreen legends are located either on copper or on substrate material but not across them.


Solder Mask


a. Size of Solder Mask Resist Openings


Solder mask resist openings should typically be 2mil to 3mil larger than copper pads and should be the same shape as copper pads that should have solder mask openings on both top and bottom sides.


b. Shifting of Solder Mask


Solder mask resist opening should NOT be shifted from copper pads.


c. Solder Mask Resist Opening for IC Pads or Gold Finger Pads


There are two circumstances available: 1). Openings are separated from each other for IC pads and there'll be a solder mask resist oil bridge between IC pads after circuit board manufacturing is completed, as is indicated in the left image below. 2). Openings are connected to each other for IC pads and there'll be no solder mask resist oil bridge between IC pads once PCB manufacturing is completed.


Solder Mask Resist Opening for IC Pads or Gold Finger Pads | PCBCart


Drilling Holes


Position, size and number of drilling holes should be appropriately designed. If you have some special designs, you can make our engineers informed by taking some notes while making your order.


Others


When it comes to flex-rigid PCB design, circuits should be respectively designed for flexible part and rigid part or a schematic diagram of lamination can be generated to clarify rigid and flexible layers.

Confirmation List Table

To make those principles or rules readable, here is a summarized confirmation list table for PCB design dased on PCBCart circuit board manufacturing capabilitiesthat. Make sure you check this list prior to sending your design files to us.


No. Item General Requirement
1 Software version Should be clarified in your design files or Notes
2 Holes Hole plating Single-layer: unplated;
Double-layer with no annular ring: unplated;
Double-layer with annular ring: plated;
Circles as holes Usually ignored
Overlapped holes Totally overlapped holes: small hole removed;
Partially overlapped holes: drilled;
Slot holes Slot holes with clearance, ≥20mil spacing should be left between;
Slot holes with no clearance, they should be drilled after being shaped as oval;
3 V-cut Depth: one third of board thickness
4 Copper annular ring Size: ≥6mil with copper thickness ≥1oz
5 Spacing Copper/trace/pad & board edge Milling: ≥0.2mm;
V-cut: ≥0.4mm;
Hole edge & board edge Routing outline: ≥0.4mm;
V-scoring/V-grooving: ≥0.8mm;
Via edge & board edge Routing outline: ≥0.2mm;
V-scoring/V-grooving: ≥0.4mm;
Positioning hole edge & pad edge ≥0.65mm
Copper pads ≥5mil
Copper grids 10mil*10mil
6 Via hole NOT between bare copper area and non-bare copper area
7 Aperture Mask/resin plugged via ≤16mil
Micro via <5mil
8 Gold finger bevel Generally 35°, 45° or 60°
9 Board layer Should be complete containing pad layer, silkscreen layer and routing layer
10 Pads Should be isolated from each other
11 Legend On copper layer Width: ≥10mil;
Width and height: at least 28mil*40mil;
Spacing between legends: ≥6mil
On solder mask Width: ≥8mil;
Width and height: at least 20mil*30mil
On silkscreen layer Width: ≥8mil;
Width and height: at least 20mil*30mil;
Spacing between legends: ≥4mil
Silkscreen legends cover on copper pads Silkscreen legends should be positioned away from copper pads
Silkscreen legends on thick copper Silkscreen legends should be located either on copper or on substrate material but not across them
12 Solder mask Size Should be 2mil larger than copper pad
Shifting Should not be shifted from copper pad

The above listed terms belong to ordinary or standard parameter category, which doesn't mean PCBCart is immune to special designs or requirement. As a matter of fact, all your creative designs deserve to be embraced and be spoken highly of. Therefore, if you have some design issues that are not included among the list introduced above or exceed limits regulated above, you can let our technical engineers know by leaving notes when submitting PCB orders online or explain in detail in extra file besides your design files.

Last oneShipping Options of PCBCart

Next articleDesign PCBs to Better Take Advantage of PCBCart's PCB Assembly Capabilities

PCB successfully added to your shopping cart