Overall Dimensions

A minimum width and height of .5 inches (12.7mm) is generally required. Minimum billable area is 1 square inch.


Please do not attempt to make arrays - our system considers each order as a single design, and it may not function correctly if you attempt an array. Arrays are not supported.

Copper Related

Clearance from board edge, outer layers: 10 mil

Clearance from board edge, inner layers: 20 mil

Minimum Annular Ring, Vias: 5 mil

Minimum Annular Ring, Plated Holes: 8 mil

Minimum Drill-Copper clearance: 8 mil

Minimum Trace width: 4 mil

Minimum Space (between copper features): 4 mil

Castellated Holes

Castellated Holes are not officially supported, but will be produced with best effort only. Note that depending upon your design, castellated holes may produce unwanted results such as left over burrs and other debris:

We suggest that if your design has castellated holes, to make the drill hits as large as possible, using a pad size that's as close to our plated hole limits, below, as possible.

Drill Related - Vias, Slots, Holes

Buried, Blind or Embedded Vias

Not currently supported.

Excessive Drill Hits

Drill hits amounting to more than 15 per square inch may be considered excessive, and if so, your job may either be delayed or cancelled. In practice, we try our best not to adhere to this rule. But hey, we're not going to let you make perfboard, OK?

Vias and Holes: Not Quite The Same Thing

In short, if you're using an aperture in your board for mechanical purposes, it's a hole. If you're using it for electrical connectivity, it's a via.


Vias are plated holes that are used solely to connect different layers of a board. Thus, a via is subject to tolerances such that the size may be slightly off from what you specified. This will, in no way, affect the functionality of your board. But it may not be suitable for mechanical purposes, such as inserting components.

Our minimum via specs are an 8 mil drill hit, with a 5 mil annular ring, as per this illustration:

Minimum Drill Size: 8 mil

Smallest Via: 18 mil - see illustration


Holes may be plated or unplated; they're suitable for mechanical purposes, and are drilled to higher tolerance. However, they require an 8 mil annular ring for plated holes, and 8 mil clearance for unplated holes. Thus, the smallest hole possible would be 24 mil:

Minimum Drill Size: 8 mil
Smallest Hole: 24 mil - see illustration

How We Distinguish between Holes and Vias
  • Any unplated hole will be considered, well, a hole, and will require an 8 mil clearance from any copper, or the board outline.
  • Any plated drill hit with an annular ring of 5 mil to < 8 mil will be treated as a via.
  • Any plated drill hit with an annular ring of 8 mil or larger will be treated as a hole.

So - if you require holes that you're fitting something else into - through-hole components, mounting hardware - you must have at least an 8 mil annular ring or clearance.


Cutouts are fine, as long as your outline file shows the shape of the board that you're looking to produce.

Slots are not officially supported. We'll try to accommodate as best we can, but no promises. We strongly suggest that you use a plated hole instead - it'll work just fine if you set the diameter to what the length of the slot would have been. In any event, slots and cutout that are less than 31 mil wide will be ignored.

Overlapping Drill Hits/Drilled Slots

Overlapping drill hits are not supported. Drilled Slots (i.e., G85 commands) are not supported. If we see them, we'll try to do the right thing, but this is not guaranteed.

Mask Related

Minimum Thickness and Clearance: 4 mil

This means that there must be 4 mil clearance between copper and mask, and 4 mil clearance between masked areas, too.

Non-conforming solder mask layers will be adjusted.

If having 4 mil of mask thickness causes clearance issues, create a gang solder mask window:

Paste Related

Hybrid Components

We'll put solder paste anywhere that your paste layer indicates - if we can. But in order to apply paste, we require a minimum surface dimension of .5mm or 20mil, or we will not do so.

Essentially, that means that if your pad or other area is at least 20mil wide or tall, we're fine. But paste for certain components needs special attention.

For example, there are many surface mount connectors that have through-hole retaining features. Here's a suggested land pattern for a vertical USB port:

The manufacturer suggests four plated holes with annular ring, with a .7mm diameter (roughly 28 mil). In order for PCB:NG to properly apply paste, we require at least some part of the ring or pad to have a 20 mil minimum dimension. 

This hole/pad combination would work well, and still adheres to our plated hole constraints, too:

So a corrected land pattern would appear like this:

Board Shapes


Angles sharper (more acute) than 45˚ will trigger a manual review.


The Outline layer should simply be the perimeter of your board - the outside edge. Do not include cutouts, drill holes, etc. They'll either be ignored, or in some cases, cause your design to be rejected. 


If you require cutouts, here's how to make it happen:

  • If you're using an EDA package that supports honest-to-goodness milling/routing features, contact support, and we'll instruct you how to create a correct routing layer that adds such features.
  • If you're using something else (KiCad, Eagle, DipTrace, etc.) that doesn't have this capability:
    • Prepare a layer that has your cutout,
    • Include it in your zip file during initial board upload, and...
    • Our system automatically opens a support ticket for each order placed. Respond to the ticket with your requirements, and either inform us as to the layer name to use for a cutout, or simply attached it to the ticket.

Inside Corners

Due to the nature of how circuit boards are fabricated, inside corners can only be approximated - they'll be rounded to some degree. For example, here's a detail showing a design with inside corners, and the routing path, in gray, that would be used to create the board:

So, for best results with inside corners, and by best, we mean predictable, assume a 2mm milling radius. For example, instead of this:

... you might want to try this:

This is really for folks that are looking to insert their PCBs into enclosures with tight tolerances; if that's not you, don't worry about milling radii and the like.

Silk Related

Minimum line width: 6 mil. Non-conforming will be adjusted (i.e., too-thin lines will be fattened up)