Bay Area Circuits Manufacturing Specifications

Bay Area Circuits Forum page
Post Reply
Message
Author
BayAreaCircuits
Posts: 9
Joined: 12 Feb 2015, 11:09

Bay Area Circuits Manufacturing Specifications

#1 Post by BayAreaCircuits » 21 Feb 2018, 20:15

We, at Bay Area Circuits, thought it would be helpful to share the manufacturing specifications we use to fabricate PCB orders submitted to us directly through DipTrace:

Maximum Board Size
Maximum board size must be less than 22.5 inches in height and 16.5 inches in width (maximum manufacturing capability).

Minimum Board Size
Minimum dimension in height or width is 0.35 inches. Total board area must be greater than 0.4 square inches (i.e. smallest square board allowed is 0.64 x 0.64 inches).

Minimum Trace and Space
Etching resolution is 0.005” minimum trace width, 0.005” minimum space width.

Inner Layers
2-Layer Design: N/A. There are no inner layers for this product.
4-Layer Design: The two inner layers may be solid copper planes, signal layers, or a mix of solid copper and signal traces. Through-hole pads can either be connected to or isolated from these layers. It’s recommended that the inner layers have roughly the same distribution of copper features to prevent warpage. The planes are inset 0.025” from each edge of the board.
6-Layer Design: The four inner layers may be solid copper planes, signal layers, or a mix of solid copper and signal traces. Through-hole pads can either be connected to or isolated from these layers. It’s recommended that layers 2 and 5 have roughly the same distribution of copper features to prevent warpage. For the same reason, layers 3 and 4 should also have roughly the same distribution of copper. The planes are inset 0.025” from each edge of the board.

Soldermask
Color = Green

Silkscreen
Color = White

Surface Finish
HASL (Lead)

Soldermask Pad Tolerance
Pads on the soldermask layers are grown by 0.003” on all sides. As a result, very fine pitch surface mount components may not include any soldermask between the pins.

Material
2-Layer Design: Dielectric material is FR-4 with a glass transition temperature of 135 degrees Celsius. Outer layers begin with 0.5 ounces of copper, then during through hole plating, up to 1 ounce of copper may be added to the outer layers. Thus, the total outer layer copper is between 0.0017" and 0.0021". If the board is 1 layer or does not have plated through holes, then the outer layer copper may be as low as 0.0014”, since less plating is required. The total board thickness will be 0.062".
4-Layer/6-Layer Design: Dielectric material is FR-4 with a glass transition temperature of 180 degrees Celsius. Inner layer copper is 1 ounce (0.0014") thick. Outer layers begin with 0.5 ounces of copper, then during through hole plating, up to 1 ounce of copper may be added to the outer layers. Thus, the total outer layer copper is between 0.0017" and 0.0021". The total board thickness will be 0.062".


Dielectric Constant
2-Layer Design: The dielectric spacing 0.057” with a dielectric constant of 4.58 +/-0.2.
4-Layer Design: The dielectric spacing between the top layer and the first inner layer is 0.008” with a dielectric constant of 4.2 +/-0.2. The dielectric spacing between the bottom layer and the second inner layer in 0.008” with a dielectric constant of 4.2 +/-0.2. The dielectric spacing between the inner layers in 0.040” with a dielectric constant of 4.2 +/-0.2.
6-Layer Design: The dielectric constant is 4.2 +/-0.2. For dielectric spacing, please see our .062 / 6 Layer stackup: https://bayareacircuits.com/multi-layer-stackups/

Annular Ring
Minimum annular ring must be at 0.005” or greater. Calculate annular ring by subtracting the diameter of the via hole from the diameter of the via pad and dividing by two.

Plated Holes
2-Layer Design: Boards are manufactured with 2 (or 1) copper layers. All holes with copper pads on the top and bottom are plated through, while holes without a copper pad on the top or bottom layer are non-plated.
4-Layer / 6-Layer Design: Boards are manufactured with 4 (or 6) copper layers. All holes with copper pads on the top and bottom are plated through, while holes without a copper pad on the top or bottom layer are non-plated.

Hole Sizes & Quantity
All hole sizes between and including 0.010” and 0.247” are available, up to tolerance. Limit number of holes to less than 50 per square inch.

Hole Tolerance
These sizes are the finished hole diameters after plating. Holes 0.014” or smaller may be filled with solder and can only be used as via. The tolerance of 0.015” to 0.020” holes is +0.003 / -0.005. The tolerance for the other hole sizes are +/-0.003”.

Hole Location Tolerance
Hole location tolerance is +/-0.003”.

Minimum Hole Distance
The distance between plated holes of different nets is dictated by annular rings and trace/space. Plated holes of the same net and non-plated holes should be at least 0.005” apart.

Internal Slots and Cutouts
Not Allowed

Perimeter Slots
Board perimeters are cut to shape using a 0.078” router bit. Slots in the perimeter must be 0.100” or wider. Narrower slots may not be cut correctly.

Perimeter Routing
The edges of the board are cut with an accuracy of +/-0.010”. A minimum of 0.020” blank space is recommended between the perimeter and all features on the board. Copper features, vias, and any other design element placed closer than 0.010” to the board’s edge may be routed off.

Temperature
All boards can survive standard reflow. The maximum operating temperature is 125 degrees C.

Other
Arrays (Tab Rout, Breakaway Tabs, Mouse Bites, etc), Beveled Edges, Blind/Buried Vias, Castellated Edges, Countersinks/Counterbores, Controlled Impedance, Edge Plating, and Scoring are NOT included in standard pricing and would require a custom quote.

Questions? Email us: support@bacircuits.com
Bay Area Circuits
support @ bacircuits.com
510-933-9000
Silicon Valley, CA

Post Reply