4 Layer Super Swift Service

Pricing

$20 per square inch, which includes three copies of your design.

For example, a 2 square inch board would cost $40 and you’d get three copies of your board. You can order as many copies as you want, as long as they’re in multiples of three.

Turn Times

Orders will ship within 5-6 business days of ordering.

You can get a quote, approve a design, and pay for an order at OSH Park.

Need more than 100 square inches of boards? Our 4 Layer Medium Run Service is a less expensive option for larger orders.

Common Specs

These specs apply to all our PCB services.

Spec Value  
Manufactured in the United States Yes  
Lead Free compatible Yes  
RoHS Compliant Yes  
High Temp Yes, 175 Tg or higher (see Material Specs)  
PCB Finish ENIG (Gold), compliant with IPC-4552  
Soldermask Type SMOBC (Soldermask Over Bare Copper), both sides  
Silkscreen Type High Res DLP, both sides  

Stackup

Thickness Layer Tolerance dk
1mil (0.0254mm)   silkscreen +/-0.2mil (0.00508mm)  
1 mil (0.0254mm)   solder resist +/-0.2mil (0.0051mm)  
1.7 mil (0.0432mm)   1 oz copper clad+plated    
7.96 mil (0.2021mm)   FR408HR 2113 prepreg +/-.796mil (0.0202mm) 3.61 at 1GHz
0.68 mil (0.0175mm)   0.5 oz copper clad    
39 mil (0.9906mm)  
  FR408HR core
 
+/-3.9mil (0.0991mm)  
0.68 mil (0.0175mm)   0.5 oz copper clad    
7.96 mil (0.2021mm)   FR408HR 2113 prepreg +/-.796mil (0.0202mm) 3.61 at 1GHz
1.7 mil (0.0432mm)   1 oz copper clad+plated    
1 mil (0.0254mm)   solder resist +/-0.2mil (0.0051mm)  
1mil (0.0254mm)   silkscreen +/-0.2mil (0.00508mm)  

Complete construction diagram

Impedence Constraint Table

Material Specs

Spec Value  
Substrate 190Tg FR408-HR ISOLA FR408-HR Datasheet PDF
Board Thickness 63mil (1.6mm) nominal  
Dielectric 3.61 at 1GHz  
Soldermask Color Purple Mask Datasheet
Minimum soldermask web 4 mil (0.1016mm)  
Maximum soldermask alignment 3mil (0.0762mm) Covers retraction, expansion, and shift
Silkscreen minimum line width 5 mil (0.127mm) (recommended minimum)
3 mil (0.0762mm) (short lines, text, graphics)
Silkscreen Datasheet
Maximum board size 16in (406.4mm) by 22in (558.8mm)  
Minimum board size 0.25in (6.35mm) by 0.25in (6.35mm)  

Copper Specifications

Spec Value  
Copper Layers 4  
Copper Weight 1oz outer
1/2oz inner
 
Trace Spacing 5mil (0.127mm)  
Trace Width 5mil (0.127mm)  
Annular Ring 4mil (0.1016mm)  
Board Edge Keepout 15mil (0.381) from nominal board edge  
Via Plating Thickness 1mil (0.0254mm)  
Plated Drill to Internal Layer Copper Clearance 10mil (0.254mm)  

Drill Specifications

Spec Value  
Minimum Annular Ring 4mil (0.1016mm)  
Minumum Drill Size 10mil (0.254mm)  
Minimum Slot Size 20mil (0.508mm) (drill slot only) Additional information on slots
Drill Size tolerance Max: +/- 2.5mil (0.0635mm)
Typical: +/- 1.0mil (0.0254)
 
Drill Positional Tolerance Max: 2mil (0.0508mm)
Typical: <1mil (0.0254mm)
 
Via Tenting Yes (filled hole and flat surface not guaranteed)  
Buried Via No  
Blind Via No  
Filled+Plated Vias (via-in-pad) No  
Overlapping drills Allowed, but not guaranteed. May result in missing or slotted holes.
5 mil (0.127mm) clearance is recommended between holes.
 
Castellations Allowed, but not guaranteed Details and recommendations
Maximum Drill Size None Drill sizes above 250mil (6.35mm) will be fabbed, but with larger milling tolerances.
Plated Drill to Internal Layer Copper Clearance 10mil (0.254mm)  

Layer Naming

We automatically detect intended layer order from many tools, using common naming conventions and meta-data formats like Gerber X2. In most cases, renaming files should not be needed, and you can use your default export settings.

If your tool or files requires configuration or manual renaming of layers, we suggest this pattern to ensure your layer order is interpreted correctly.

Layer Suggested File Extension  
Layer 1 .GTL Top or Front layer
Layer 2 .G2L Internal layer (adjacent to Top)
Layer 3 .G3L Internal layer (adjacent to Bottom)
Layer 4 .GBL Bottom or Back layer

For additional info or other layers, see our Suggested Naming Pattern

Internal Plane Polarity

When submitting gerbers, we need the “positive” internal planes, meaning that lines represent copper, not the absence of copper.

Some CAD tools will generate the internal planes as power planes with “negative” polarity so the lines indicate where copper should be removed. To work around this, declare the internal planes as signal layers and use a copper pour to define the power plane.

Take a look at our [Positive and Negative Gerbers][invertedgerbers] page for more information.

Drill Internal Layer Clearance

Some tools will often suppress annular rings on vias that do not connect to internal layers. However, this may not accurately capture required production specs, leading to inadvertent spec violations. While these violations do not always result in issues, they can lead to surprising defects and yield issues.

This DRC requirement is not always obvious inside design tools, with some tools defaulting to a violation, and not providing clear warnings. Care should be taken to ensure compliance. Tools handle this differently, but one of the following methods should help:

  • Configuring the tool to always include annular rings, regardless of net connections
  • Increasing ground plane clearance on internal layer copper pours
  • Configuring custom net rules to increase isolation on internal layer copper pours.

Your design tool’s documentation will assist with these steps.

Examples of drill configurations that comply with specs

Examples of drill configurations that violate specs