PCB Stackup, Drill Table, and Gerber Output Settings Explained

This article covers the documentation and output settings that connect a PCB design database to fabrication: the stackup description and table, the drill table and symbol conventions, and the NC drill and Gerber output parameters. These items are not administrative extras. They define how the fabricator reads layer order, copper and dielectric thickness, hole sizes, and aperture data. A mismatch between the design and the output package can cause wrong layer sequencing, missing pads, incorrect hole sizes, or ambiguous apertures. The article explains how to prepare the stackup text and table, how to assign drill symbols, how to set drill units and precision, and how to configure Gerber format and options for positive and negative layers.

Highlights:

The stackup text and stackup table must align, and the table must define copper plating thickness and interlayer thickness for every electrical layer.
Drill symbols must be legible and unique; holes of the same size use the same symbol, while profiled holes must not share a symbol.
Drill and Gerber units must match the PCB design, and RS274X is required when real Flash pads must be reproduced without a separate D-code aperture file.

Stackup Documentation

Stackup Text and Stackup Table

The stackup text describes the type and order of each electrical layer.
The stackup table describes the material of each electrical layer, the interlayer material, and the thickness parameters.
The stackup text and the stackup table must be aligned, as shown in Figure 79.

Figure 79 | Stackup table

The alignment is not cosmetic. A reader must be able to move from a layer name in the text to the corresponding row in the table without ambiguity, because the two parts serve different purposes. The text establishes layer type and sequence; the table supplies the material and thickness data used to build the board.

Layer Thickness

In the stackup table, describe the copper plating thickness of every electrical layer and the thickness between layers (Thickness), as shown in Figure 79. The fabricator uses these values to build the copper and dielectric structure, so each layer interface should be stated clearly rather than left implicit.

Drill Table

The drill table converts the hole requirements of the design into a fabrication chart. It assigns a symbol to each drill size and provides the data needed to read the drill drawing. Two rules matter most: symbol legibility and symbol uniqueness.

Drill Symbols

Drill symbols in the table must not be too small; the specification is 100mil x 100mil.
Drill symbols must not be repeated. Different drill sizes must not use the same drill symbol.

Drill Sizes

Holes of the same size must use the same drill symbol. Profiled holes are the exception: they must not share the same drill symbol. This keeps a profiled hole from being interpreted as a round hole of the same nominal size and makes the tooling intent clear to the fabricator.

Drill Tape and Gerber Output Settings

The drill tape and Gerber output settings determine whether the fabrication data is interpreted in the same units and with the same precision as the PCB design. Unit consistency and precision should be checked before the output package is released.

Drill Units

The drill unit must match the PCB design unit, as shown by Output Units in Figure 80.

Figure 80 | Drill parameter settings; units must be consistent with the PCB design units, as shown in Output Units in the figure above

Drill Accuracy

When drill accuracy has a specific requirement, increase the drill accuracy. The default is 2.3, as shown by Format. For a PCB designed in metric units, the drill accuracy must be increased to 2.5.

Gerber Format

Gerber format selection determines how apertures and graphic data are delivered to the fabricator.

The common Gerber format is Gerber 6x00, which is RS-274-D. In this format, the D-code aperture file and the Gerber file are separate. Neither file is meaningful on its own.
If the PCB design uses real Flash components, select Gerber RS274X to reproduce the Flash effect in the Gerber output. This format includes the D-code aperture parameters and the Gerber graphic information, so no separate D-code aperture file is required. Figure 81 shows the Gerber format selection.

Figure 81 | Gerber format

When RS-274-X format is selected, the sublayers contained in a negative Gerber layer must not include any Anti-Etch sublayer.

Gerber Options

Gerber output units must match the PCB design units. The default Gerber output accuracy is 5.3. For metric units, or when higher accuracy is required, set the accuracy to 5.5.

The Gerber layer options have the following meanings:

Undefined line width: For lines with zero line width, this sets the line width generated in the Gerber. The minimum setting is 5mil.
Shape Bounding box: Valid for negative film. It defines the width by which the board-edge Anti etch is extended outward. It can be left unset.
Plot mode: The layer attribute, either positive or negative.
Film mirrored: Selects whether the Gerber is mirrored. Bottom-layer Gerber should have this option checked.
Full contact thermal-reliefs: Fully connects thermal pads on negative layers and ignores their thermal-relief parameters.
Suppress unconnected pads: Does not generate unconnected positive inner-layer pads, as shown in Figure 82.

Figure 82 | Example of the Suppress unconnected pads option

Draw missing pad apertures: Draws pads that have no corresponding D-code aperture with lines. This option is needed for devices that have been rotated through non-standard angles.
Use aperture rotation: Uses rotated D-code apertures. This is usually not selected.
Suppress shape fill: Fills areas that have no Anti etch. It is valid for negative layers.
Vector based pad behavior: Valid when the Gerber format is RS274X. It describes apertures with vectors, which produces a smaller file. It is recommended. After composite layers of negative layers are merged, it prevents circular pad rings. Figure 83 Vector based pad behavior illustrates the result.

Figure 83 | Example of the Vector based pad behavior option. Note: By default, set the Gerber line width to 0, layer attributes, Film mirrored, and Suppress shapefill. For Gerber using the RS274X format, each negative layer must not contain

Note: By default, set the undefined line width, the layer attribute, Film mirrored, and Suppress shape fill. For Gerber output in RS274X format, each negative layer must not contain any Anti-etch sublayer.

D-Code File

When generating a D-code file, the units must match the PCB units and the Gerber units. Click the Auto button and select Without Rotation to generate the D-code, as shown in Figure 84.

Figure 84 | D-code generation options

These output settings are applied together at release. The stackup text and table define the layer build; the drill table and drill parameters define hole tooling and coordinates; the Gerber format and options define pad and aperture data. Before releasing the package, confirm that the stackup text matches the table, that drill symbols are unique and correctly sized, that drill and Gerber units match the design, that the required precision is set for the unit system, and that negative layers do not contain Anti-etch sublayers. These checks keep the fabrication data readable and prevent errors in layer order, hole size, pad shape, and aperture definition.

Related Reading: