Skip to content

Release CheckList

PCB Release Checklist

Directory Setup

  • In Git: Select or create repo for a new design.
  • In Eagle Control Panel (main window), add the repo or Git folder to “Projects” drop down

Project Setup

  • Within the “Projects” drop down of the Control Panel, select desired folder, right-click the folder and select “New Project”. This will create a RED new project folder inside it which designates a project.
  • Double-click the folder to enter into the project (denoted by a GREEN dot next to the folder when it is open) or double-click it again to close it (green light dot turns grey)

Library Setup

  • A set of common / past components is currently stored in the Git under “Archive” -> “Eagle Libraries” -> “GW-devices”; or in the Control Panel under “Libraries” -> “Eagle Libraries”. For KW2-specific parts, there is a library “KW2” in the same directory.

NOTE: Library locations and content should probably be adjusted. Current common parts include a set of SMD resistors, capacitors, inductors, buttons, barrel jacks, several number displays and miscellaneous connectors.

Schematic creation

  • If not already open, double-click on Project folder or right-click -> “Open” in the Control Panel to open the project
  • In Control Panel, “File” -> “New” -> “Schematic” or right-click on Project folder, then “New” -> “Schematic”. This opens a Schematic Editor window.
  • Make sure board and schematic are consistent - ALWAYS have both layers open at the same time in Eagle!

Library creation

  • To create a new part, a schematic symbol (“symbol”), footprint (“package”) and association between the two (“device”) is required.
  • In the top drop down (“Libraries”) of the Control Panel, navigate to or add your library.
  • Double-click to open it, this will generate a new window.
  • To create a schematic symbol, click the gate symbol in the menu bar. Select a current symbol to edit or create a new one. This will open a further new window where a symbol can be drawn.
  • Draw & place pins, rename pins by datasheet / function if desired
  • To create a footprint, click the chip symbol in the menu bar. Select an existing or create a new footprint in the same manner as above.
    • Name pads by datasheet / function if desired
  • To associate the symbol with the footprint, click the button with 4 gates in the menu bar. Either enter a new device name or select an existing one.

    • Add schematic symbol via the gate button on the left menu panel (under the wrench button) and place it at the origin marker unless otherwise required.
    • Attach a footprint by selecting the “New” button at the bottom of the right panel.
    • Click “Connect” in the same panel to associate footprint pads with symbol pins
    • The part can now be used in schematic creation.
    • Layout creation
  • Once a schematic is completed, convert it to a layout. “File” -> “Switch to board” (in Schematic Editor) will create a layout file with the same name in the project in the Layout Editor. If all symbols are part of a correctly created device, the footprints should all be added automatically.

Layer settings

  • Click on the magnifying glass with wires in it (bottom most button on the right column of the left-side menu panel)
  • Select the “Layers” tab and adjust as required. Note: Eagle by default numbers layers starting at 1 for the top layer and 16 for the bottom layer. A 2-layer board thus has top = 1 and bottom = 16, whereas a 4-layer has top = 1, inner1 = 2, inner2 = 15 and bottom = 16. NOTE: The example setup is incorrect; using it will result in a stackup numbered 1,2,3,16 which breaks various other features in Eagle. Ensure your setup is numbered correctly!

DRC settings

  • In the same panel, adjust minimum feature size under “Sizes”, trace / space / board edge clearances under “Clearance” and minimum annular rings for vias and pads under “Restring”. Additionally, in “Misc”, check the “Check angle” box for best results.

Verify a design in Eagle

  • DRC (Design review check) should have no warnings or errors.
  • ERC check should have no warnings or errors.

Exporting a design

  • CAM files accessed via the blue film-reel icon on the top menu or under “File” -> “CAM Processor” of the Layout Editor.
  • Manufacturing files:
    • Gerber files (copper, silk, mask, stencil layers)
    • Codeshelf has CAM files under “Archive” -> “CAM_ULP”
    • For each file, ensure the correct layers and features are checked. Defaults for copper are 1,2,15,16 for 4-layer boards and 1,16 for 2-layer. Adding the board outline to each file is not a bad idea either.
    • For each file, ensure the output directory is correct. By default, the file will be created in the project directory. To change this, each file must be adjusted individually (!)
  • Drill file (holes)
    • Codeshelf does not have a CAM file for drills. Eagle provides one under “CAM Jobs” in the Control Panel (or under “cam” in the Eagle install directory)
  • Centroid
  • BOM (from schematic)

Create a New Library Part

New Library Part Review

  • Schematic symbol corresponds to function / correct number of pins.
  • Use a good naming scheme for the schematic pins.
  • Pins on schematic match pins on package.
  • Package geometric center is the part’s centroid.
  • Correct footprint is attached (e.g schematic and symbol have same number of pins).
  • Footprint has pins in correct order (check layer for mirroring possibilities).
  • Print 1.0 scale version and verify that the footprint matches the part and datasheet.

Release to Manufacturing Checklist

Schematic review:

  • All parts have assigned and CORRECT manufacturers and part numbers (check assigned datasheet vs symbol pin numbers, for instance)
  • Pins on devices labelled as according to datasheets
  • Nets named correctly (by function or pins)

Layout review

  • Fiducials for assembly (3 per side)
  • Check net connectivity
  • Make sure copper pours are present on all layers AND ACTUALLY POURED
  • Check Reference Designators & other labelling are on the correct silkscreen layers
  • Check DRC for correct trace / space and minimum silk screen width according to manufacturer
  • Correct version number applied (out of house do NOT include “P” suffix)
  • All polarized components checked
  • Check the orientation of all connectors
  • Bypass capacitors located close to IC power pins
  • PCB has power rail test points, and test points for important signals, all labeled and accessible
  • Layout PCB so that any rework or repair of a component does not require removal of other components
  • Mounting holes electrically isolated or not
  • Proper mounting hole clearance for hardware
  • SMD pad shapes checked
  • Check for traces running under noisy or sensitive components
  • No vias under metal-film resistors and similar poorly insulated parts
  • Check for traces which may be susceptible to solder bridging if not masked (OFN pins etc)
  • Check for dead-end traces, unless used on purpose
  • Provide multiple vias for high current and/or low impedance traces
  • Component and trace keepout areas observed
  • Ground planes where possible
  • Trace width sufficient for current carried
  • No silkscreen legend text over vias (if vias not soldermasked) or holes
  • All legend text reads in one or two directions
  • Company logo in silkscreen legend
  • Date code on PCB
  • All silkscreen text located to be readable when the board is populated
  • All ICs have pin one clearly marked, visible even when chip is installed
    • Ensure it is in silkscreen layer
  • CAD design rule checking must be turned on
  • High frequency circuitry precautions observed
  • Soldermask does or does not cover vias
  • PCB thickness, material, copper weight noted
  • Thermal reliefs for internal power layers
  • Solder paste mask openings are proper size
  • Blind and buried vias not allowed on multilayer PCB unless required
  • Finished hole sizes are >=10 mils larger than lead
  • All capacitors have been designed with a 50 percent voltage margin.
  • All new components/suppliers must be reviewed for component obsolescence and component availability
  • All PCBA designs must have the revision level released to Document Control and assembly drawing indicating any special assembly/design requirements that violate the standard PCB assembly conventions (i.e. components on the solder side, cuts and jumps, heat-sink assemblies, etc.). - Open question for Calla / Nate
  • All power traces wide enough for anticipated current

Export Production Files

  • BOM
    • Check whether existing columns are:
      • Qty
      • Value
      • Package
      • Parts/Reference Designator
      • MFGN
      • MFGP
      • Notes
    • Gerbers
      • For each file, make sure the right features are selected as well as the board outline
    • Drill file
      • Visual inspection to see if holes line up
    • Centroid

Review Gerber Files

  • Check to see if right files exists
    • Top silk
    • Top mask
    • Top paste
    • Top copper
    • Inner copper 1
    • Inner copper 2
    • Bottom copper
    • Bottom paste
    • Bottom mask
    • Bottom silk
    • Top centroid
    • Board outline
    • DRD (drill file)
  • Open in a gerber file viewer (GerbV, ViewMate)
  • Check to see if each layer contains what you expect (traces, pours, holes)
  • Ensure correct placement of all layers (check whether visually stacks up correctly)


  • Nets named correctly (by function or pins).
  • Lay down ground plane, only after ground traces.
  • Check orientation of mating connectors in associated designs