4 Layer Medium Run Service
Moving to a small production run? Our medium run service will help bridge the gap between prototypes and a full panel.
Pricing
$2 per square inch, 100 square inch minimum. You can have as many different designs as you want, as long as each design is ordered in a multiple of 3 boards.
For example, if you have two 25 square inch designs, you could order 3 of each for a total cost of $300.
100 inches is just the minimum order. You can order as much as you’d like beyond that.
Turn Times
Orders will ship within 12-21 calendar days of ordering.
We do not offer Super Swift Service for 4 layer boards.
For faster options, you may be interested in our Standard 4 Layer Service.
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) |
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) |
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. |
Layer Naming
Most default layer file names are automatically detected and fabricated in the order intended by the design tool.
If your tool 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 |
| Layer 3 | .G3L | Internal layer |
| 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.
