6 Layer Prototype Service


$15 per square inch, which includes three copies of your design.

For example, a 2 square inch board would cost $30 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 9-14 calendar days of ordering.

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

We do not offer Super Swift Service for six layer boards.

We do not offer Medium Run Services on 6 layer boards, but we may be able to discount orders over 100 square inches. Contact [email protected] with your design for more information.

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  


Thickness Layer Tolerance dk df
1mil (0.0254mm)   silkscreen +/-10% (0.2mil,0.00508mm)    
1 mil (0.0254mm)   solder resist +/-10% (0.2mil,0.0051mm)    
1.7 mil (0.0432mm)   1 oz copper clad+plated      
4.36 mil (0.1107mm)   FR408HR 106 75% prepreg +/-10% (0.436mil,0.0111mm) 3.23@1Ghz 0.011
0.68 mil (0.0175mm)   0.5 oz copper clad      
4 mil (0.1016mm)   FR408HR 2113 core +/-10% (0.4mil ,0.0102mm) 3.66@1Ghz 0.009
0.68 mil (0.0175mm)   0.5 oz copper clad      
36.44 mil (0.9256mm)  
  FR408HR core
+/-10% (3.64mil,0.0925mm)    
0.68 mil (0.0175mm)   0.5 oz copper clad      
4 mil (0.1016mm)   FR408HR 2113 core +/-10% (0.4mil ,0.0102mm) 3.66@1Ghz 0.009
0.68 mil (0.0175mm)   0.5 oz copper clad      
4.36 mil (0.1107mm)   FR408HR 106 75% prepreg +/-10% (0.436mil,0.0111mm) 3.23@1Ghz 0.011
1.7 mil (0.0432mm)   1 oz copper clad+plated      
1 mil (0.0254mm)   solder resist +/-10% (0.2mil,0.0051mm)    
1mil (0.0254mm)   silkscreen +/-10% (0.2mil,0.00508mm)    

Material Specs

Spec Value  
Substrate 175Tg FR4 ISOLA FR408-HR Datasheet PDF
Board Thickness 63mil (1.6mm) nominal  
Dielectric See stackup  
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 6  
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)  

Drill Specifications

Spec Value  
Minimum Annular Ring 4mil (0.1016mm)  
Minumum Drill Size 8mil (0.2032mm)  
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.

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 File Extension Layer Placement order
Layer 1 .GTL Top or Front layer
Layer 2 .G2L Internal layer (adjacent to Top)
Layer 3 .G3L Internal layer (top side of core)
Layer 4 .G4L Internal layer (bottom side of core)
Layer 5 .G5L Internal layer (adjacent to Bottom)
Layer 6 .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.